Data Preparation
Articles related to this topic.
The Layer Matrix menu
To change e.g. the order of layers, you have to open the "Layer Matrix" menu, which can either be directly accessed through right-clicking in the layer panel and selecting "Open Matrix" or selecting "Fabrication » Matrix" in the main menu. There you are able to i.a. add new layers, load predefined standard stack ups, and even print a report of your stack up or export it as CSV.
In addition to the order of the individual layers every other information like default stackup, layer type, hights, layer attributes, material, colour, etc. can also be adjusted to fully fit your needs. Once every configuration is in order the printed curcuit board can thoroughly be inspected by selecting one or more layers (by simply clicking on them) for visual representation. By default, each layer is assigned a specific colour so that it can quickly be identified which parts and layers are belonging together. Related colours and layers can be found between the checkbox and the layer name. Should the colours not meet your preferences, they can also be adjusted either seperately through right-clicking on the concerning layer and selecting "Set Color of Layer" or globally through "Start » Setup Colours".
For example, you can choose a standard stackup for your pcb. To do so, right-click on "File" in the upper left corner of the menu. There, you have the option to choose one of the default stackups.
Color Group
You can get to Colour Group via Developer » Color Group.
- Groups by number
The Groups by number tab creates colour groups on the basis of the first number of the component reference meaning if the refernce is "R123" it would be 1. Usually components belonging together are grouped by their reference number during circuit diagram creation. The colour coding thus allows you to recognize with one glance how the individual functions have been distributed throughout the curcuit board, for example, having all components belonging to the power supply coloured in a deep yellow. - Groups by char
Grouping by char is very similar to grouping by number with the sole difference being that group by char depends on the first char of the component reference rather than the first number whereby the first char in turn usually is dependent on the type of components (R for resistance, C for capacitor, L for coil, etc.). - Group by attributes
Grouping all components with the same attribute. This can be a attribute or an property, you can use e.g. the PACKAGE_GROUP property to mark all Chips, SOPs, QFNs, ... in the same color.
In both cases the colour scheme can of course be customised to fit your preferences.
Here is an example how it can look for package group coloring:

Component Heights
Component height is an important component property that is deeply attached to it. In earlier versions of ODB++ this property was just a number without unit. Since PCB-Investigator needs a unit for certain features like the 3D visualisation it assumes the unit "mils" by default. The Change Component Heights dialog which can be reached by Developer » Component Heights is a fail-safe that allows you to change the unit if it is falsely assumed by the program. Please note that this option only affects the component height property.
With the Filter option you can handle components only on active layers, only selected components or all components.
Generate Net List
The netlist is an integral part of the inner workings of PCB-Investigator and thus the Generate Netlist function is of utmost importance and is needed especially in two main cases:
- Editing the netlist by adding, deleting, dividing, shifting,... destroys the logical links between parts which actually belong together. Generating the netlist anew remedies this by running through all elements of your PCB, identifying which parts are connected and issuing new net names (in case a net name already exists the first net name remains).
- File formats like Gerber have no netlists and no net names. Generate Netlist recognizes, which parts are connected and assigns index based names to them and therefore allows you to use all selection methods of PCB-Investigator even those which are based on net names.
Note: You need correct stackup and drill information to generate the net list correct.
Net Groups
The NetGroup Wizard can be used to create net groups and to add or remove nets to them.
Open the NetGroup Wizard with clicking the "Net Groups" button.
The following dialog will show up.

1. The two important tabs contain the following options.

The net groups are always stored within the ODB design. Sometimes, you want to import net groups from another design. Prior to that, export the current net group to have a backup of them. In the import you can select between different file formats (xml, txt, dcf, dcfx, csv, rulf) to add net groups from other software (e.g. Xpedition or Zuken) or if you select xml from other PCB-Investigator exports.
Import Format List:


The "Tools" tab has three important functions.
- Analyse (see next chapter): Clicking the analyse control, a new dialog will open.
- The PCB Stack-up Calculator is a calculator for the PCB stack-up.
- Generate Net Groups: If you want to generate net groups automatically, you can use the "Generate Net Groups" contol. Clicking this option, will open the following dialog.
To create net groups, the net names will be used. The number is the number of letters to be tapped. All nets with the same beginning will then be added to the net group. The net groups names depend on the tapped letters.
2. The summary of controls allow you the following operations:
- Select: The "Select" control can be used to focus the selected net group.
- Unselect: If you selected multiple net groups, you can deselect one or more net groups to isolate the net groups you want to inspect.
- Activate Layer: This allows you to see the layers nets of the net groups when selecting a group.
- Include Components: "Include Components" also shows you the connected components to net nets of the net groups that you are selecting.
- Apply all Colors: If the net group has been colored, the "Apply all Colors" button allow you to color all nets with the same color.
- Optimize View: With this option you can zoom to the area of the net group and all included nets.
3. The button "Create Group" allows you to create you own groups with the desired group name.
4. This control contains all net groups which are deposited in the ODB dataset. More options to edit net groups can be found by right clicking on a net group.
- Rename: Here, you can rename the net group
- Add Description: You can add text that will be shown behind the group name in the extra tab.
- Assign Color to Group(s): Using this functionality, you can assign a color to the group within the list. It won´t assign color to the nets on the design.
- Apply Color in PCB-Investigator: If you assigned a color to the group, you can now assign this color to the nets included in the net group. Now, the nets will be shown in the design with the same color.
- Zoom to the Net Group: Here, you can zoom the net group. If you double left click a net group entry, you will also zoom to the net group.
- Remove Color Assignment: Use this function to remove color assignments.
- Delete/ Delete All: You can either delete the selected net group or all by using either "Delete" or "Delete All".
5. Every net of the net group will be shown here, if a group in the group view (4) is selected. To remove a net of the net group, right click the net you want to remove and click remove.

6. If y net group (4) is selected, you can add single nets to the net group with clicking a net in the view with the number 6 and clicking the add button. There are two different add buttons:
- The upper add button will just add nets which are selected on the design. If no net is selected, the button can´t be used.
- The button below adds the nets you select in the bottom right net list.
For more details have a look to this short video:
Panel Builder
By clicking on the Panel Builder symbol, the following dialog will open:
1. Clicking on "Add a new Step" enables you to create an additional step.
2. "Import Step" allows you to import a new design / step from another file.
3. "Create Panel (Simple)" is described separatly and in detail under the post "Create Panel (Simple)".
4. "Create Panel (Intelligent Nesting)" is also explicitly described in an extra post.
5. "Edit Step" is an additional functionality to be used to individually place the origin.
6. The "Drag and Drop" option allows you to manually place the steps on your panel. Clicking on it, the following dialog will open:
- Minimum Distance: Minimum Distance to another step that should not be deceeded.
- Distance to Profile: Minimum Distance to the profile.
- Show Measure Lines: Measure lines for a better handling of drag & drop.
- Use Orientation Elements: Orientation elements for facilitating drag & drop.
7. Clicking on a step in the list, you can transform the selected step by rotating it or moving it in individually set intervals.
- Minimum Distance: Minimum Distance to another step that should not be deceeded.
- Distance to Profile: Minimum Distance to the profile.
8. This list shows all steps currently placed on the relevant panel with its most important information.
9. Clicking on "Set Fiducials" allows you to define markers on your panel. The following dialog will therefore open:
- You can either use the values from the panel border or from the origin of the border.
- If you want to place markers, you can select the starting point (left-top, right-top, left-bot, right-bot) from which they are to be placed and - if needed - the interval (X offset) that defines the spacing of the placement.
- You have the choice between four default marker symbols; you can also load another symbol out of the default options or choose an own symbol from a library if needed.
- You can also choose to add a mask opening; the size of this opening can be adjusted individually in mm. This also gives you the option to oversize the symbol.
- You also have the option to add components. To do this, you just need to select one from your Package Library.
- Before setting the fiducial markers (Click on "Set Fiducials"), you have to select the appropriate layer/s where you want or need to place the markers.
10. "Add Routing" is used to define the routing for your panel. Clicking on "Add Routing" will open the following dialog:
- On the top of the dialog, there are four symbols to be further explained (from the left to the right):
- 1. Symbol: For checking for components placed nearby.
- 2. Symbol: Use for multiply cutouts.
- 3 Symbol: Use to clean double cutouts.
- Routing Layer: Choose the layer you want to use for routing.
- Routing Size: Select the size of the routing.
- Cutout Length: Adjust the length of your routing cutout/opening.
- Reduce Size for Intersecting: It is possible to change the routing diameter for small gaps or near child steps.
- Clear Route Layer: Remove all existing routings for new calculation.
- Ignore Holes: Create Routing only for outline elmenents.
- Optimize Routway: Check for overlapping with near child step routings and remove double routings.
- Only in Panel Profile: Depending on your edge handling this can help to place less routings and remove all routings outside of the panel.
- Direct Routing: Place the routing lines direct on the outline of child steps, for some export formats the routing can be handled with shifting (left or right) to get the correct result.
- Only in Vshears: Check Vshear lines on the selected layer, for some cases the routing should be only in some areas.
- Components Outside: Use an oversize for overlapping components, this is needed for assemble in panel.
- After the creation of the routing layer, you can "Use Mouse Click" to define a cutout for each mouse click. You just have to click on the intended routing part to set a cutout.
In the File menu you find an extra dialog "cutout editor" see here
11. For defining holes on your panel, click on "Set Holes". The following dialog will be opened:
- Like described in "9. Set Fiducials", this dialog works practically analogously.
- There is the possibility to decide for the hole shape for each position (left-top, right-top, left-bot, right-bot) by clicking on
: You can either decide for an oval form or a round shape.
- You can define the diameter of the holes to be set in mm.
- To set the holes like defined before, just click on "Set Holes".
12. "Set Profile" allows you to define the profile of your panel. The following dialog will be opened when clicking on it:
- You have the option between setting the contour according to a rectangle or a manufacturing edge: Depending on your choice you have to set different parameters.
- Rectangle: You have to define the x and y axis as well as the width and height of your profile in mm. If needed, you can select to use rounded corners (you therefore have to define a suitable radius)
- Manufacturing Edge: You have to define the size of left, right, top and bottom of your profile in mm. You can also decide for rounded corners.
- By clicking on "Accept", the current size of all active layers will be calculated. If there is no active layer, all loaded layers will be used instead
- By clicking on "Set by all Outlines/Objects", all loaded objects will be used for the calculation.
13. Here, you can add another step on your current panel by choosing the step out of the provided list options. You are able to select each step that has been defined for this design.
14. Clicking on "Apply" applies all changes made by you on your currently opened design.
Test Setup

- With this button, you are able to create a new test session which will be added to the list "Test Runs".
- This list shows all existing test sessions. By using the right mouse button, you can delete, copy or rename them. By a simple click, the session is loaded and shown on the right side.
- If your design has multiple steps (e.g. single board + panel), here you can select the step where probes should be added or managed. You can e.g. add probes to the single board, but export the panel afterwards (the probes of the single board will be reproduced).
- These buttons allow to import/export the current test setup options from/to other layouts.
- Settings for automatic creation of probes, vary on tester type (fixture/fixtureless). Options will be described later.
- Once probes are created, you can define their visibility for the two sides here.
- Save button to save the current session and Export button to export the session to one of the available tester machines.
Fixture Parameters:
Tester Type:
Tester Type to use for the automatic probe creation
Probe Side:
Search probes on this/these side(s)
Exclude Single-Pin Net:
Exclude No/Single-Pin Net, all no-pin and single-pin net entries will not create probe entries.
Use max. Test Resources from Net Setup:
If yes, only the given number of Probes are created. If no, all Probes are created
Search Tasks (Top):
Defines the tasks and the order for searching probes on top side
Search Tasks (Bot):
Defines the tasks and the order for searching probes on bot side
Available Needles:
All allowed needles for fixture probes. Will be used beginning with the largest one. Here also the needed distances to components are defined per needle definition
Standard min. Distance to Components:
If no special distance is defined for the given needle, this is the standard min. distance from probe center to surrounding components
Minimum Distance between Probes:
The minimum distance between Probes, measured from outline to outline (taking diameter of the Needle Definition into account)
TP Reference Filter List:
Comma separated reference filter list (e.g. \"TP, P\"). TP Components must start with one of these entries.
TP Pad Recognition:
Recognize test points by the '.test_point' attribute on copper pads.
Minimum pad size to use as probe (Top):
Minimum copper pad size to create a probe for top side.
Minimum pad size to use as probe (Bot):
Minimum copper pad size to create a probe for bot side.
Enable Solder Mask Analysis:
Enable Solder Mask Analysis, only round pads with openings in solder mask are used if this setting is active.
Minimum pad size to use as probe (Top):
Minimum pad size to create a probe for top side.
Minimum pad size to use as probe (Bot):
Minimum pad size to create a probe for bot side.
Maximum drill diameter to use as probe:
Maximum drill diameter to create a via probe.
Enable Solder Mask Analysis:
Enable Solder Mask Analysis, only round pads with openings in solder mask are used if this setting is active.
Minimum pad size to use as probe (Top):
Minimum pad size to create a probe for top side.
Minimum pad size to use as probe (Bot):
Minimum pad size to create a probe for bot side.
Minimum annular ring to use as probe (Top):
Minimum annular ring to create a probe for top side.
Minimum annular ring to use as probe (Bot):
Minimum annular ring to create a probe for bot side.
Fixtureless parameters:
Tester Type:
Tester Type to use for the automatic probe creation
Probe Side:
Search probes on this/these side(s)
Exclude Single-Pin Net:
Exclude No/Single-Pin Net, all no-pin and single-pin net entries will not create probe entries.
Use max. Test Resources from Net Setup:
If yes, only the given number of Probes are created. If no, all Probes are created
Exposed Copper - Exposed Copper:
The minimum distance between exposed copper areas to not be reported in the Short Analysis (0=deactivated)
Copper - Copper:
The minimum distance between any copper areas to not be reported in the Short Analysis (0=deactivated)
Drill - Drill:
The minimum distance between plated drills to not be reported in the Short Analysis (0=deactivated)
Only Nets with Components:
Only nets with components are checked
Search Tasks (Top):
Defines the tasks and the order for searching probes on top side
Search Tasks (Bot):
Defines the tasks and the order for searching probes on bot side
Minimum distance to Board Outline (Upper Side):
Minimum distance from fixtureless access point center to upper board outline
Minimum distance to Board Outline (Lower Side):
Minimum distance from fixtureless access point center to lower board outline
TP Reference Filter List:
Comma separated reference filter list (e.g. \"TP, P\"). TP Components must start with one of these entries.
TP Pad Recognition:
Recognize test points by the '.test_point' attribute on copper pads.
Minimum pad size to use as probe (Top):
Minimum copper pad size to create a probe for top side.
Minimum pad size to use as probe (Bot):
Minimum copper pad size to create a probe for bot side.
Enable Solder Mask Analysis:
Enable Solder Mask Analysis, only round pads with openings in solder mask are used if this setting is active.
Minimum pad size to use as probe (Top):
Minimum pad size to create a probe for top side.
Minimum pad size to use as probe (Bot):
Minimum pad size to create a probe for bot side.
Maximum drill diameter to use as probe:
Maximum drill diameter to create a via probe.
Enable Solder Mask Analysis:
Enable Solder Mask Analysis, only round pads with openings in solder mask are used if this setting is active.
Minimum pad size to use as probe (Top):
Minimum pad size to create a probe for top side.
Minimum pad size to use as probe (Bot):
Minimum pad size to create a probe for bot side.
Minimum annular ring to use as probe (Top):
Minimum annular ring to create a probe for top side.
Minimum annular ring to use as probe (Bot):
Minimum annular ring to create a probe for bot side.
Offset for the Probe Placement (%):
This parameter is used, if Probes are set to Pins where no TESTPROBE_KEEPOUT but a MPN Package Outline exists. The probe is placed on x % of the distance from the outer edge of the pin to the edge of the MPN Package Outline (also see next parameters). If a keepout is defined, the probe will be placed to the middle of the remaining pin contact area. If no MPN Package Outline is defined, 'Offset Limit for the Probe Placement' is used for the offset.
Offset Limit for the Probe Placement:
This parameter is used, if Probes are set to Pins where no TESTPROBE_KEEPOUT exists. The offset distance calculated with 'Offset for the Probe Placement (%)' is limited to this value, so the offset will not be larger as this value. If no MPN Package Outline exists, this value is used for the offset.
Minimum needed Offset for the Probe Placement:
This parameter is used, if Probes are set to Pins where no TESTPROBE_KEEPOUT but a MPN Package Outline exists. If the offset distance calculated with 'Offset for the Probe Placement (%)' is smaller than this value, no Probe will be placed.
Minimum Pin Size:
Minimum Pin size to be used for the Probe Placement (width and height must be larger/equal
Component Setup

- This button fills the “Device” column in the list from the value of the DESCRIPTION Property of the components (if exististing).
- The list shows all components of this data step and allows you to add additional information to each component.
- In the context menu some important functions are easily accessible or the “Edit” (4) dialog can be opened.
- In the “Edit” dialog, you can correct the “Mounting Type” if it was not available in the imported layout data, you can define whether a component is really placed or if it is not in the BOM (“Ignore in Output = true”), and you can force or prohibit the probe generation for single pins. It’s also possible to define if 4-wire measurement is needed and the test model(s) for each single component, although it is recommended to do this in the “Test Model Setup” Tab (C) for all components of the same part number at once.
- This list gives you an overview of how the pins of the selected components are wired. This information may help to define test models, especially when it comes to define the pin types of Diodes (Anode/Cathode) or Transistors and others.
- With this button you can add own columns to the list by stating a property name, e.g. “MPN” for the material part number or “Manufacturer”. Of course, those properties must exist in the layout data.
Test Model Setup

- The list shows all different part numbers of this data step and allows you to define the test model(s) for each part.
- In the context menu some important functions are easily accessible (e.g. copy/paste of test models) or the “Edit” (3) dialog can be opened.
- In the “Edit” dialog, you can define test models for this part. It is possible to add multiple test models (e.g. 4 Capacitor test models for a Capacitor Array).
- Each available test model has different parameters that describe the test. Depending on the export type (e.g. Seica/Takaya/i3070) all or parts of this information is needed/used. One of the most important information is the pin mapping, so e.g. which pin number is the Anode and which is the Cathode of a Diode.
Following test models are available: See appendix.
Net Setup

- The list shows all different nets of this data step and allows you to define the type and the number of probes per net.
- In the context menu some important functions are easily accessible (e.g. Select Net) or the “Edit Net(s)” (3) dialog can be opened.
- In the “Edit” dialog, you can define the type of a net (power/ground/signal) and the needed number of test resources (probes). In the “Test Setup” (A) this number is used for the probe creation (“Use max. Test Resources from Net Setup”).
Probe Setup

- This button creates the probes according to the rules defined in the Test Setup (A). If probes already exist, you’ll be asked if you want to keep and only supplement them, or if you want to delete all probes that are not fixed bevor creating new ones.
Additional Rules:
- The first probe per net will be given “Probe Access = Forced”
- If more than one probe is needed for a net (see “Net Setup (D)”), those probes will have “Probe Access” set to “Alternative”
- If “Use max. Test Resources” is set to false in Test Setup (A), probes that go beyond the needed number will have “Probe Access” set to “No”
- If a component in the net needs 4-Wire-Measurement (“Component Setup (B)”) and only one probe is possible in this net, there will be a second probe created at the same location as the first one
- If a fixture probe location is too close to a component, the next smaller needle size is used. If the smallest needle is still too close to a neighbor component, no probe will be created.
- The probe type depends e.g. on the component type (SMD/THT of the “Component Setup (B)”) or the Component Reference name (“TP Reference Filter List” in “Test Setup (A)”)
- Pad and hole sizes are taken from the layout
- The list shows all probes with their nets, locations and properties.
- In the context menu some important functions are easily accessible (e.g. Delete) or the “Edit” (4) dialog can be opened.
- In the “Edit” dialog, you can change following properties of the selected probe(s).
- Location: Board location of the Probe
- Probe Designator: Probe Designator (e.g. TP100) to which this probe belongs
- Access Type: Access Type (Fixture/Fixtureless)
- Accessible Side(s): Accessible Side(s) for this probe (Top/Bot/Both)
- Probe Side: Probe Side (Top/Bot)
- Probe Type: Probe Type (TestPoint, THT, VIA, SMD, …)
- Probe Access: Probe Access Type (Forces/Alternative/No)
- Fixed: Probe location is fixed and Probe will be kept if probes are recreated
- Needle Definition Name: Name of definition of the needle. Must match a value in the 'Available Needles' section of the Test Setup (A)
- Probe Pad Size: Pad Size of this Probe
- Probe Hole Size: Hole Size of this Probe
- The "Check Probe Distances" button checks the distance between the probes in the list according to the “Minimum Distance between Probes” parameter of the “Test Setup (A)”. Rule violations will be highlighted in red color and additional information in the “Violation” column of the list. The "Optimize Needle Sizes" button trys to find the best possible needle sizes, therefore the "Minimum Distance between Probes" parameter of the “Test Setup (A)” is used. The algorithm trys to keep the largest possible needles, e.g. by setting two close needles both to 75mil instead of one to 100mil and the other to 50mil.
- Visualization options to highlight pins with probe access or select/jump to selected probes
- Clear the list and delete all probes
Access Overview

- Update Button to force update of list entries and statistics
- Statistics for the net access via probes
- List of the accessible nets with probes
- List of nets without access including information about unused test points
- List of unused test points with net information
- In the context menu some important functions are easily accessible (e.g. Select net) or the “Show Details” (7) dialog can be opened.
- This dialog shows the probes and pins for the selected net.
- It’s possible to add manual probes to certain pins by setting this pin to “ForceProbe” in the “Probe Setting” of the “Component Setup (B)”.
Short Analysis

- Button to run the short analysis according to the rules defined in the “Test Setup (A)”.
- List of all found shorts. By selecting a line, the short is shown graphically in PCB-Investigator.
- The context menu offers the possibility to delete single short measurements before starting the export.
Short measurements will be added in different ways to the exported files:
I3070:
Shorts are not used, as this is a “Fixture” test system
Seica:
Short measurements are exported to the “.shi” file, together with shorts measurements from Pin2Pin test models. Redundancies will be removed first.
Takaya:
Short measurements are exported as Resistor Tests (@K OP). Redundancies with Pin2Pin test models are removed first.
Seica Export
The Seica export creates a package of files (.alf/.inf/.nod/.par/.sha/.shi) that contain all available component and net information to easily create the test program in the VIVA Software of Seica.
Following export settings are possible:

- Additional Channel Offset: If a channel is set by AutoSetChannels or TryToParseChannelNumberFromComment, this channel will be incremented by this offset (e.g. AdditionalChannelOffset=1 => Channel 100 will be exported as 101)
- Auto Set Channels: Set a unique channel number per Forced/Alternative Probe (if TryToParseChannelNumberFromComment=false)
- Try to Parse Channel Number from Comment: If the channel number is stated in the comment of the probes, this number will be used in the Seica export. (AutoSetChannels will not be used!)
- Side Switch: If true, the PCB will be checked from bottom up
- Rotation: If >0, the PCB will be rotated clockwise by this angle (e.g. 90°) after applying the SideSwitch command (if SideSwitch=true)
- Resistor Macro Name: Macro name for Resistor (Value from Property: %PROP_NAME%)
- Capacitor Macro Name: Macro name for Capacitor (Value from Property: %PROP_NAME%)
- Inductor Macro Name: Macro name for Inductor (Value from Property: %PROP_NAME%)
- Diode Macro Name: Macro name for Diode (Value from Property: %PROP_NAME%)
- LED Macro Name: Macro name for LED (Value from Property: %PROP_NAME%)
- Zener Macro Name: Macro name for Zener (Value from Property: %PROP_NAME%)
- Transistor (NPN) Macro Name: Macro name for NPN Transistors (Value from Property: %PROP_NAME%)
- Transistor (PNP) Macro Name: Macro name for PNP Transistors (Value from Property: %PROP_NAME%)
- Mosfets (N) Macro Name: Macro name for N-Channel Mosfets (Value from Property: %PROP_NAME%)
- Mosfets (P) Macro Name: Macro name for P-Channel Mosfets (Value from Property: %PROP_NAME%)
- Jumper (Open) Macro Name: Macro name for Open Jumper (Value from Property: %PROP_NAME%)
- Jumper (Closed) Macro Name: Macro name for Closed Jumper (Value from Property: %PROP_NAME%)
- Switch (Open) Macro Name: Macro name for Open Switch (Value from Property: %PROP_NAME%)
- Switch (Closed) Macro Name: Macro name for Closed Switch (Value from Property: %PROP_NAME%)
- Potentiometer Macro Name: Macro name for Potentiometer (Value from Property: %PROP_NAME%)
- Fuse Macro Name: Macro name for Fuse (Value from Property: %PROP_NAME%)
- Opto Photo Coupler Macro Name: Macro name for Opto Photo Coupler (Value from Property: %PROP_NAME%)
- ICOpen Macro Name: Macro name for ICOpen (Value from Property: %PROP_NAME%)
- Pin2GND Macro Name: Macro name for Pin2GND (Value from Property: %PROP_NAME%)
- Pin2GND+ICOpen Macro Name: Macro name for Pin2GND AND ICOpen (Value from Property: %PROP_NAME%)
- Standard Macro Name: Macro name for Components without Test Models (Value from Property: %PROP_NAME%)
- Standard Device Name: Device name for Components without Test Models (Value from Property: %PROP_NAME%)
- Multi Model Macro Name: Macro name for Components with more than one Test Model (Value from Property: %PROP_NAME%)
- Multi Model Device Name: Device name for Components with more than one Test Model (Value from Property: %PROP_NAME%)
- Not mounted Macro Name: Macro name for Components that are 'ignored in output' (Value from Property: %PROP_NAME%)
- Not mounted Device Name: Device name for Components that are 'ignored in output' (Value from Property: %PROP_NAME%)
- Special Macro/Device Rules: Rules to define the Macro and Device according to a property value. Overrides all other Macro/Device settings
- Pin2Pin Max Distance (MM): Maximum distance for pins of different nets to be tested for short circuit (µm)
- Standard Diode Test Value (mV): Test value for standard diodes in mV
- Standard Diode Tolerance: Tolerance for standard diodes (%)
- Schottky Diode Test Value (mV): Test value for schottky diodes in mV
- Schottky Diode Tolerance: Tolerance for schottky diodes (%)
- LED Diode Test Value (mV): Test value for LED diodes in mV
- LED Diode Tolerance: Tolerance for LED diodes (%)
- Inductor Tolerance Addition (%): Inductor Tolerance Addition in %
- Resistor Tolerance Addition (%): Resistor Tolerance Addition in %
- Capacitor Tolerance Addition (%): Capacitor Tolerance Addition in %
Takaya Export
The Takaya export creates a “.ca9” file containing a whole test program. This includes a wire analysis where parallel and serial Resistors/Capacitors/Inductors are merged if there are not enough probes to test them separately. For small value components, that get lost in the tolerance of the overall circuit, additional Vision Tests are created.
The export can be done for one-sided Takaya machines as well as for two-sided ones (4 fingers on one side, 2 on the other).
Following export settings are possible:

- Machine Type: Machine Type (Double Sided / Single Sided)
- Minimum Component Height (MM): Min. Component Height to export as High-Fly Zone
- Maximum Component Height (MM): Max. Component Height to export as High-Fly Zone
- Additional Safety Distance (MM): Additional Safety Distance added on the Component Height
- Side Switch: If true, the PCB will be checked from bottom up
- Rotation: If >0, the PCB will be rotated clockwise by this angle (e.g. 90°) after applying the SideSwitch command (if SideSwitch=true)
- Short Measuring Time: Short Measuring Time (@MT) (<0 => Not used)
- Resistor Measuring Time: Resistor Measuring Time (@MT) (<0 => Not used)
- Diode Measuring Time: Diode Measuring Time (@MT) (<0 => Not used)
- Zener Measuring Time: Zener Measuring Time (@MT) (<0 => Not used)
- Photo Coupler Measuring Time: Photo Coupler Measuring Time (@MT) (<0 => Not used)
- Diode Measuring Range: Diode Measuring Range (@MI) (<0 => Not used)
- Upper Limit for 0-Ohm Resistor (Ohm): Upper Limit for 0-Ohm Resistor in Ohms (@MR)
- Lower Limit for ignored Resistor (MOhm): Lower Limit for ignored Resistor in MOhm (@MR)
- Upper Limit for ignored Capacitor (pF): Upper Limit for ignored Capacitor in pF (@MR)
- Lower Limit for ignored Diodes (V): Lower Limit for ignored Diodes in V (@MR)
- Diode Tolerance Plus: Diode Tolerance Plus (@T)
- Diode Tolerance Minus: Diode Tolerance Minus (@T)
- ICOpen Forced: Export ICOpen Test, also if Component is too small
- ICOpen Tolerance Plus: ICOpen Tolerance Plus (@T)
- ICOpen Tolerance Minus: ICOpen Tolerance Minus (@T)
- ICOpen Sensor Diameter (MM): ICOpen Sensor Diameter (in Millimeter)
- Pin2Pin Max Distance SMT (MM): Pin2Pin Test: Maximum distance for SMT pins of different nets to be tested for short circuit (µm)
- Pin2Pin Max Distance THT (MM): Pin2Pin Test: Maximum distance for THT pins of different nets to be tested for short circuit (µm)
- Conveyor Margin (@Y): Conveyor Margin (µm) (<0 => Not used)
- Probe Speed for TEST_POINT: Probe Speed per Land Figure (@PS)
- Probe Speed for THD*: Probe Speed per Land Figure (@PS)
- Probe Speed for SMD_SMALL: Probe Speed per Land Figure (@PS)
- Probe Speed for SMD_MEDIUM: Probe Speed per Land Figure (@PS)
- Probe Speed for SMD_LARGE: Probe Speed per Land Figure (@PS)
- Probe Speed for CONNECTOR: Probe Speed per Land Figure (@PS)
- Probe Speed for DIP: Probe Speed per Land Figure (@PS)
- Probe Speed for PAD: Probe Speed per Land Figure (@PS)
- Create LED Color Test: Create Dummy LED Color Test Entry (Location=CT)
- Create Vision Test: Create Vision Test for Components without TestModels (@V5)
- Export @VO Option: Export @VO option (Offset for THTs)
- Export @W Option: Export @W option (board width/height) in the CA9 Header
- Ignore NC Pin at ICOpen: Ignore NotConnected Pins at ICOpen TestModels
- Ignore NC Pin at Pin2GND: Ignore NotConnected Pins at Pin2GND TestModels
- Unique Test Step Names: Each Test Step should have a unique name instead of the PartName (except Pin2Pin, Pin2GND and ICOpen)
- Use Testprobe-Keepout as Highfly: Use the TESTPROBE_KEEPOUT instead of the REAL_BODY_OUTLINE as Highfly-Area
- Inductor Tolerance Addition (%): Inductor Tolerance Addition in %
- Resistor Tolerance Addition (%): Resistor Tolerance Addition in %
- Capacitor Tolerance Addition (%): Capacitor Tolerance Addition in %
i3070 Export
The i3070 export creates a “board” and “board_xy” file that contain all available component and net information to easily create the test program with the native machine software.
Following export settings are possible:

- Side Switch: If true, the PCB will be checked from bottom up
- Rotation: If >0, the PCB will be rotated clockwise by this angle (e.g. 90°) after applying the SideSwitch command (if SideSwitch=true)
- Fixture Type: Fixture Type
- Fixture Size: FULL, BANK1, BANK2
- Top Probes Allowed: ON/OFF
- Heavy Probe Force: Heavy Probe Force
- Light Probe Force: Light Probe Force
- Mechanical Density Threshold: Mechanical Density Threshold
- Vacuum Density Threshold: Vacuum Density Threshold
- Autofile: Autofile
- Test Strategy: COMBINATIONAL, EDGE CONNECTOR ONLY
- Wire Wrapping: MANUAL, AUTO, WIRELESS, SEMI AUTO
- Metric Units: ON/OFF
- Common Lead Resistance (Ohm): 0.1m ohm to 100 ohms.
- Common Lead Inductance (µH): 0.1n Henry to 1m Henry
- Capacitance Compensation: Capacitance Compensation
- IPG Digital Resistance Threshold (Ohm): IPG Digital Resistance Threshold, Value in ohms
- Preconditioning Levels: Preconditioning Levels
- Additional Board Voltage: 0-100
- Use Agilent DriveThru Test: Use Agilent DriveThru Test
- DriveThru Impedance Threshold (Ohm): DriveThru Impedance Threshold
- Boundary Scan Overdrive: ON/OFF
- Boundary Scan Disable: ON/OFF
- Boundary Scan Chain Override: ON/OFF
- Ground Bounce Suppression: ON/OFF
- Powered Shorts Shorting Radius (mils): 1-250
- Tolerance Multiplier: 0.1 - 10
- Remote Sensing: ON/OFF
- Fuse Threshold: Fuse Threshold
- Diode Current (A): Diode Current
- Zener Current (A): Zener Current
- Adjust: NONE, FAST, ACCURATE
- Upstream Disable: ON/OFF
- Upstream Condition: ON/OFF
- Test Strategy Cover Extend: BSCAN, HYBRID, HYBRIDGUARD, BSCANGUARD
- Family Options: Family Options contain a list of different family options with settings e.g. for TTL/ECL/LVC...
- Library Options: Library Options contain a list of library paths e.g. './custom_lib'
- Inductor Series-R (Ohm): Inductor Series-R Standard Value
- Transistor High Beta (V): Transistor High Beta Value (If value=0 in test model)
- Transistor Low Beta (V): Transistor Low Beta Value (If value=0 in test model)
- FET High Resistance Limit (Ohm): FET High Resistance Limit (0.1 Ohm - 1 MOhm)
- FET Low Resistance Limit (Ohm): FET Low Resistance Limit (0.1 Ohm - 1 MOhm)
- FET Enhancement Gate Voltage (V): FET Enhancement Gate Voltage (0-9V)
- Fuse Max Current (A): Fuse Max Current
- Failure Message: Failure Message (Value from Property: %PROP_NAME%)
- Failure Message (NOPOP): Failure Message for NOPOP components (Value from Property: %PROP_NAME%)
- Part number field: Part number field value (Value from Property: %PROP_NAME%)
- Part number field (NOPOP): Part number field value for NOPOP components (optional if not PIN LIBRARY) (Value from Property: %PROP_NAME%)
- Special Partname Rules: Rules to rename parts according their original name
- Export Component Outline: Export Component Outline in XY File (DEVICE Section)
- Merge all NC Nets: Merge all NC nets into a single NC net
- Export Transistor as PinLibrary: Export Transistor Model as PinLibrary
- Export FET as PinLibrary: Export FET Model as PinLibrary
- Export Diode as PinLibrary: Export Diode Model as PinLibrary
- Export LED as PinLibrary: Export LED Model as PinLibrary
- Export Zener as PinLibrary: Export Zener Model as PinLibrary
- Export Fuse as Jumper: Export Fuse Model as Jumper Close
- Export Inductor as Jumper: Export Inductor Model as Jumper Close
- Export Switch as Jumper: Export Switch Model as Jumper Close
- Probe Reference Prefix: Reference prefix for dummy components at probe locations
- Suppress Needle Sizes: Suppress Needle Sizes in XY-File (39MIL/50MIL)
- Export PartNumber and FailureString: Export Partnumber and Failure String for all components. If false, Partnumber and Failure String is exported only for PinLibrary components.
- Inductor Tolerance Addition (%): Inductor Tolerance Addition in %
- Resistor Tolerance Addition (%): Resistor Tolerance Addition in %
- Capacitor Tolerance Addition (%): Capacitor Tolerance Addition in %
Appendix - Test Models
| Model | Parameter | Used for Seica | Used for Takaya | Used for i3070 | Used for Elowerk | Used for Spea |
| Resistor | Type | √ | √ | √ | √ (or OTHER if #Pins <> 2) | √ |
| Value | √ | √ | √ | √ | √ | |
| Tolerance | √ | √ | √ | √ | √ | |
| Pins | × | √ | × | √ | × | |
| Capacitor | Type | √ | √ | √ | √ (or OTHER if #Pins <> 2) | √ |
| Value | √ | √ | √ | √ | √ | |
| Tolerance | √ | √ | √ | √ | √ | |
| Pins | × | √ | × | √ | × | |
| Inductor | Type | √ | √ | √ | √ (or OTHER if #Pins <> 2) | √ |
| Value | √ | √ | √ | √ | √ | |
| Tolerance | √ | √ | √ | √ | √ | |
| Pins | × | √ | × | √ | × | |
| Potentiometer | Type | √ | √ (2xResistor) | √ | √ (2xResistor) | √ |
| Value | × | √ | √ | √ | × | |
| Tolerance | × | √ | √ | √ | × | |
| Pins | × | √ | √ | √ | √ | |
| Diode | Type | √ | √ | √ | √ | √ |
| Diode Type | √ | × | × | × | × | |
| Forward Bias | × | × | √ | √ | × | |
| Test Current | × | × | × | √ | × | |
| Pins | × | √ | √ | √ | √ | |
| LED | Type | √ | √ (as Diode) | √ (as Diode) | √ | √ |
| Color | × | √ (2nd Diode Test) | × | × | × | |
| Forward Bias | × | × | √ | √ | × | |
| Test Current | × | × | × | √ | × | |
| Pins | × | √ | √ | √ | √ | |
| Zener | Type | √ | √ (Zener+Diode) | √ | √ | √ |
| Value | √ | √ | √ | √ | × | |
| Tolerance | √ | √ | √ | √ | × | |
| Test Current | × | × | × | √ | × | |
| Pins | × | √ | √ | √ | √ | |
| Transistor | Type | √ | √ (Transistor + 2xDiode) | √ | √ | √ |
| Transistor Type | √ | √ | √ | √ | √ | |
| Pins | × | √ | √ | √ | √ | |
| FET | Type | √ | √ (FET + Diode) | √ | √ | √ |
| FET Mode/Type | √ (only Type) | √ | √ | √ | √ (only Type) | |
| Pins | × | √ | √ | √ | √ | |
| Fuse | Type | √ | √ (4-Wire if possible) | √ | √ (or OTHER if #Pins <> 2) | √ |
| Pins | × | √ | × | √ | × | |
| Jumper | Type | √ | √ (Resistor) | √ | √ (Switch or Resistor) | √ |
| State | √ | √ | √ | √ (Switch) | × | |
| Pins | × | √ | × | √ | × | |
| Switch | Type | √ | √ (Resistor) | √ | √ | √ |
| State | √ | √ | √ | √ | × | |
| Pins | × | √ | √ | √ | × | |
| PhotoCoupler | Type | √ | √ (PhotoCoupler + Diode + Resistor) | √ (PinLibrary) | √ | √ |
| Pins | × | √ | × | √ | × | |
| Seica: Special Model | DIGITAL | √ | × | × | × | × |
| OPENTIC | √ | × | × | × | × | |
| OPENFIX | √ | × | × | × | × | |
| AUTIC | √ | × | × | × | × | |
| VOLTAGEREGULATOR | √ | × | × | × | × | |
| OPAMP | √ | × | × | × | × | |
| COMPARATOR | √ | × | × | × | × | |
| TRIAC | √ | × | × | × | × | |
| SHORTTEST | √ (in the .shi file) | × | × | × | × | |
| Takaya: Special Model | ICOpen | × | √ | × | × | × |
| Pin2Ground | × | √ (Diode Tests) | × | × | × | |
| Pin2Pin | × | √ (Resistor Tests) | × | × | × | |
| i3070: Special Model | PinLibrary | × | × | √ | × | × |
| Connector | × | × | √ | × | × | |
| Elowerk: Special Model | All Types | × | × | × | √ | × |
| Spea: Special Model | All Types | × | × | × | × | √ |
Exceptional cases:
1. If NO model exists
- Seica: Macro is set to "$DIGITAL", Device/Macro can be customized.
- Takaya: No electrical test, optionally a Vision Test is created.
- i3070: Exported as "Undefined", "Connector" or "PinLibrary" according to setting.
- Elowerk: Exported as "OTHER".
- Spea: Exported as "Analog Device" or "Test Point" (if component reference is a TP according to setting).
2. If >1 model exists
- Seica: Macro is set to "$DIGITAL", Device/Macro can be customized.
- Takaya: Each model is generated independently.
- i3070: Exported as "PinLibrary".
- Elowerk: Exported as "Cluster" with all single models included.
- Spea: Exported as Array (if there are only Resistor OR Capacitor OR Inductor OR Diode models) or "Analog Device".
3. "Not in BOM" is true
- Seica: Macro is set to "$NOTMOUNTED", Device/Macro can be customized.
- Takaya:
-
General:
- Comment is set to "NOPOP".
- Values are set to "*". -
Special:
- Zener: @K is set to F, @MR can be defined, no Zener Test.
- LED: @K is set to F, @MR can be defined, no color test.
- Transistor: @K is set to JP, no Diode Tests.
- FET: @K is set to JP.
- Switch, Jumper, Fuse: @K is set to OP.
- Resistor, Diode, Pin2Ground, Potentionmeter: @K is set to F, @MR can be defined.
- Capacitor: @K is set to E, @MR can be defined.
- Inductor: Esported as Resistor with @K is set to OP, @MR can be defined.
- PhotoCoupler: @K is set to JP/F(Diode)/OP(Resistor).
- ICOpen: @K is set to JP.
-
- i3070:
-
General:
- PartNumber is set to "NOPOP". -
Special:
- Resistor is exported as Open Jumper.
- Capacitor is exported with 0.1pF.
- Inductor is exported as Open Jumper.
- Transistor is exported with 0.002/0.001V.
- FET is exported with 99999 Ohm.
- Diode/LED is exported with 0.002/0.001V.
- Zener is exported with 0.001V.
- Fuse is exported as Open Jumper.
- Jumper is exported as Open Jumper.
- Potentiometer is exported with 100MOhm.
- Switch is exported "Off".
-
- Elowerk:
-
General:
- PartNumber is created with export option "Part number field (NOPOP)".
- All test models are ignored and the component is exported as "OTHER".
-
- Spea:
-
General:
- In the "Part List" section, the "Mounting Side" is set to "P" (not mounted top) or "M" (not mounted bottom). - Special:
- Resistor is exported fixed value 100k +/- 0.01%
- Capacitor is exported fixed value 0.1p +/- 0.01%
- Inductor is exported fixed value 0.1n +/- 0.01%
- Potentiometer is exported fixed value 100k +/- 0.01%
- Zener is exported fixed value 1V +/- 0.01%
-
Edit Dimensionings
1) After you have adjusted the settings for the next dimensionings you want to add, you can press "Add".
Then, move to the graphic interface to choose two points on your printed circuit board you want to select for measuring their distance. PCB-Investigator thereby helps you with reference points to easily mark e.g. the edge or centre of a component. To set a marker for dimensioning use a right-click. A double-click allows you to change the location of the set marker by entering new values for x and y. You can also easily relocate the connecting line and its associated text information with holding the right mouse botton and shifting the line in its wanted position.
2) Here, you can adjust the settings for the layer, the text and the type of the new dimensioning you want to add.
- Layer: You can only choose between the currently activated layers. It´s also possible to choose "all layers". Dimensionings with this categorization will be visible no matter of the layers being activated.
- Text: This setting allows you to configure which information about the dimensioning you want to be displayed. %DIS% %UNIT% displays both, the distance and the unit used. If you use the same unit for all dimensions (see 7), you can only use %DIS%. It´s also possible to use any other text by entering the propriate information.
- Type: There are four different types of dimensioning you can use: cross, vertical, horizontal or text.
- Cross, vertical, horizontal indicate the direction of the connecting lines. The rotation can also be changed afterwards.
- Text allows you to add additional information or notes to you printed circuit board (e.g. marking drillings). You can duplicate text marker points by holding STRG while right-clicking. A double-click will eliminate the duplicate. A text type can´t be switched into a direction type once defined.
3) There are three more options you can adjust before adding a new dimensioning: text size, text rotation and font.
- text size: This allows you to determine the size of the text that should be displayed.
- text rotation: Here, you can choose the rotation of text which should be used for the next dimensioning. Using -1 will adapt the text parallel dimensioning line. You can also rotate the text by double-clicking on the appropriate text information in the graphic interface.
- font: Choose the font you want to use for the text.
4) You can also determine the colors that should be used for the visualization of the dimensioning: line color, text color, back color.
- line color: Color of the connecting line between the two points selected for dimensioning.
- text color: Color of the text used to describe the dimensioning information.
- back color: Background color of the text.
5) Clicking on "Apply" allows you to subsequently change the settings of (3) and (4) for all dimensionings you have determined so far at once.
6) In this list, you will find a overview of all dimensionings you have determined with all their relevant information. You can also adjust the settings by double-clicking on the intended configuration. A right-click on a dimensioning will highlight the appropriate dimensioning in the graphic interface.
7) Here, you can choose the unit you want to use for your dimensionings. Selecting "auto" will apply an automatically choosen unit (most practical solution) for each dimensioning. To avoid misunderstandings using "auto", you should indicate the unit for each of your dimensionings (2).
8) "Set Bounds Dimensionings" sets the dimensionings for your overall printed circuit board (lenght, width).
Example for dimensionings on a design:
View Dimensionings:
To display or hide your dimensionings, click on the framed symbol which can be found under "View".
Symbol Library
Symbols / Objects are stored in the symbol library. You can either access it when e.g. adding or editing objects or you can directly open the symbol library.
By clicking on the tab “Symbol Library” which can be found under the ribbon “Fabrication”, the following window will open.

1. Under “Loaded Library”, you have three different types of libraries to choose from:
- Job: You will see all symbols that are used in the currently open design or on the corresponding panel
- XML Library
- PCB-I 365: Only if you have registered for.
To get access to the symbols of one of these symbols, you have to open the subcategories of the corresponding library.
2. Then, you will see a list with all symbols and their properties stored in this library.
3. Selecting one of these symbols in the list, will visualize them on the right side of the list.
4. Clicking on the green plus at the bottom left corner of the dialog will open the following dialog:

Here, you have the choice between different ODB++ symbols that can be adjusted according to your needs by defining their parameters. Clicking on “Accept” will then add the newly defined symbol to the currently opened Library.
5. Clicking the “X” when you have selected a list item, allows you to extinguish this symbol in your library.
6. Clicking on the pen symbol will open up the “Symbol Property Editor”.

The Symbol Property Editor allows you to change the name of the symbol and create a new property by entering a new property name and by choosing a new value type for the symbol.
You can´t delete or edit the properties of a symbol that is a regular feature of your design. When you have selected one of these symbols, the two buttons will be greyed out.
7. If you have selected the currently opened Job as a Library, you have the option to pick any of the symbols on your design in the graphic interface and the corresponding symbol in the list will be highlighted.
There are two more options when you have selected an XML or 365 Library to work with. The dialog for these libraries will also look a bit different:

When choosing either an XML or PCB-I 365 library, you can click on
to open another dialog for adjusting the settings of the library.

This editor allows you to create, edit, remove, import and export a (new) library. When adding a new library (click on “Create”), you have to enter a new name for the library and you have to select the propriate path for the library file you want to choose.
If you want to remove a symbol library in the setting dialog by selecting it and clicking on “Remove”.
You can also edit the parameters of an already existing object or add a new symbol from the current selection. Clicking on
or double-clicking on a symbol in the list will open a new window of PCB-Investigator allowing you to adjust the currently selected symbol in the list to gain a special symbol that’s not contained in any of the libraries.

To configure this symbol, you can then click on “Add”. This allows you to compile a special symbol. How to add symbols or objects is described under “Add Objects”. If you have completed the compilation of your special symbol, you can click on “Save” or “Save and Close” on the upper right corner of the window and you will get back to the main Symbol Library dialog.
OIB Server Manager
When you open the "SIPLACE OIB Connector" (in the 'Machine Export' menu) the first time, you have to first enter your OIB server settings by clicking on the gear button (1):

Following dialog will open:

In this server manager, you can organize multiple OIB servers. To create a new one, please press on the little green "+" button and enter a name.
Afterwards you'll have to specify the OIB server adress by entering an IP/Hostname + Port, or directly enter the 'net.tcp://...' adress (1).
When this is done, you'll have to specify two server directories by clicking on the small browse button (2):
- "Component Main Path": This is the OIB directory, where your part library is located. Parts in this directory are only read, but never written or changed.
- "Component User Path": This is the OIB directory, where parts, that do not exist in the main path yet, are created by PCB-Investigator. The user has to complete the information of those parts in the SIPLACE Software and can then move them to the main path later.
Click "Save" and close the dialog to preceeed.
Placement List Creator
To start, please select a server and click "Connect" (1).
With the "Placement List Creator" tab, you can create placement list elements for each component side on the OIB server.

To start, you have to do a few settings in block (2):
- 'Current Step': Select the board step, for which placement lists should be created
- 'Group Components by': Choose whether to use the internal 'Part Number' or any other Property in your CAD data to get the list of part numbers. These part numbers are the 'key' to search for parts on the OIB server.
- 'Component Type Filter': You can filter components by the '.comp_mount_type' attribute, e.g. to get only SMT components
Always when you change settings in (2), you will have to 'Refresh' the list and 'Match Parts via OIB' again (3).
When the matching process is done, you will see all your filtered parts in the list (4), including an overlay of the matching OIB part definition on the selected server. Found OIB parts are centered on the CAD package center. Details of the found OIB part and the fitting state are listed on the bottom side (5).
The 'Status' column indicates, whether a OIB part was found or not, and if the found part fits onto the CAD package. The condition for fitting is, that the pin definition of the OIB part must at least partly overlap the CAD package pin.
If the found part does not fit, you have the possibility to shift its position or to rotate it until it fits (6). With the two buttons in this block on the right, you can open the property dialog of the CAD component or zoom to it.
If the OIB part has a polarity definition, this polarity marker is visualized in red. The fitting alorithm then also uses the polarity information, to recognize if the component is correctly rotated (CAD polarity pin is same as OIB polarity pin).
Example of the fitting process (6) (by rotating 90° clockwise):
=> 
When clicking the 'Create Placement List via OIB' button (7), you are asked to select a folder on the OIB server and enter the name for the placement list(s) for top and/or bottom side. Afterwards, the placement lists are created via OIB. Missing parts, that where not found during the matching process, are automatically created in the 'Component User Path' (see 'OIB Server Manager'). Those created parts are dummy parts without any real outlines or pin definitions. Their information must be completed by the user in the SIPLACE Software afterwards. Components that have the ".comp_ignore" attribute are marked as 'omitted' in the placement list.
Here is a screenshot of the result in the SIPLACE Software:

Board Creator
After having created the placement list of the single board(s), you can create the panel data with the "Board Creator" tab.

To start, you have to select the panel step that should be created (1). It is also possible to create panels in panels (recursive), when the most outer panel is selected.
For the given panel, the included single board(s) is/are listed unter (2). Here an already existing placement list on the OIB server must be selected per board and side. If the placement lists where created before in this session with the "Placement List Creator", the information is already prefilled. If not, you can click the small browse button and select the right placement list.
In the block (3), there are different options available:
- "Export Board Outline": if checked, the complex board outline of the CAD data is exported. This may need some time. If not checked, the bounding box is used
- "Export Fiducials": if you want to export objects with ".pad_usage=gfiducial/lfiducial", please check this box and select a fiducial type from the OIB server by clicking on the little browse button
- "Export Inkspots": if you want to export objects with ".board_mark=bbm" (Bad Board Marker), please check this box and select a fiducial type from the OIB server by clicking on the little browse button
- "Requires trace information": This field on the OIB server can be set or not here
- "Requires PCB barcode verification": This field on the OIB server can be set or not here
- "Default processing orientation": 0/90/180/270° for Top or Bot (sets the corresponding fields on the OIB server)
In the block (4), you can choose which CAD layers should be exported and imported in OIB for this board per side. It is mainly thought for paste/mask layers.
When clicking the 'Create Board via OIB' button (5), you are asked to select a folder on the OIB server and enter the name for the board entry. Afterwards, the board is created via OIB.
Here is a screenshot of the result in the SIPLACE Software:



SIPLACE QD/XLSX Exporter
Use the SIPLACE QD/XLSX Exporter in Machine-Export to export a loaded board or panel from PCB-Investigator. The dialog offers two outputs: structured .qd files for SIPLACE/ASM and a placement table in .xlsx or .csv format. Both use the selected component filters, rotation corrections, rotation direction and insert point.

The numbered areas show preparation (1), component checks (2), rotation tools (3), optional Gerber export (4), export settings (5), table export (6) and QD export (7).
Prepare the board or panel (1)
- Open a design and start SIPLACE QD/XLSX Exporter. In Step to Export, select the single-board or panel step to export. For a complete panel, select the panel rather than one of its child boards.
- Choose the Part Number Identifier: Part Number uses the CAD part name; Property uses the selected component property. Choose the identifier that matches the part names in the destination system. A component without the selected property has an empty exported part identifier; check the list before exporting.
- Set Component Type Filter: All, SMT, THT or Pressfit. Type filtering uses the component's mount-type attribute, falling back to its package attribute. Components without a matching type can be omitted by a specific filter. Components without pins are excluded.
- Set Ignore Unplaced as required. This filter excludes components marked with
.comp_ignore. Check how non-populated parts are marked in the imported design; other non-population attributes do not have the same effect on this filter. - Click Refresh List after changing the identifier, its property or component filters. This applies the settings and rebuilds the component list.
Check component orientation (2–3)
The list shows Package Name, Part Numbers, References, User Confirmed and Step. Entries group components of the same package and existing rotation correction within a step. One entry can therefore represent several references and part numbers.
- Select an entry and compare the package preview, pin numbering and orientation with the part definition used on the ASM machine. The preview also shows the reference, package, CAD body size and ASM Delta Rotation.
- In Rotate Part, enter the required increment in degrees and use the rotation arrows until the package matches the machine definition. The correction applies to all components represented by the selected entry, not only the displayed reference. Reset Transform removes their stored rotation correction.
- Check User Confirmed after inspecting the entry. Use F3 and F4 to move to the previous or next entry. The property button opens the displayed component's properties; the magnifying-glass button selects and zooms to it in the design.
Note: Rotation corrections are stored on the components and are used by both export formats. They are not just preview changes. Save the design if you want to retain these corrections. Components Checked by User counts represented components, not list rows. Unconfirmed entries are not automatically excluded and do not disable export; complete the checks before releasing production data.
If a warning reports the same part number with different package definitions, check the selected part identifier and the underlying data before proceeding.
Optional Gerber export (4)
Enable Export Gerber Layers and check the required layers separately under Top Side and Bot Side. The counters show how many layers are selected. QD export writes one .ger file per selected layer beside the corresponding side's QD file. Bottom-side Gerbers are already transformed for that side; an extra mirror in SIPLACE is normally unnecessary. Gerber selection has no effect on XLSX/CSV export.
Common export settings (5)
- Task — Export Top Side / Export Bottom Side: select at least one side. QD creates separate side files; XLSX/CSV puts all selected sides in one table.
- Rotation direction — Clockwise / Counter-Clockwise: selects the exported angle convention for both outputs. Angles are normalized to a range from 0° up to, but excluding, 360°. Match the destination's convention.
- Project name: supply a non-empty valid name. It determines the QD output names and the proposed table filename.
- PCB Height: board thickness for QD, in the displayed unit. The current dialog shows mm. This value is not a column in the placement table.
- Comment: exported with the QD structure. It is not included in the placement table.
Optional panel and board fiducials
- Export Panel Fiducials … as: includes fiducials on panel steps.
- Export Board Fiducials … as: includes fiducials on the single-board steps.
- For each enabled option, enter the fiducial path/name used in SIPLACE, for example
fiducials/14. The number in parentheses shows the detected count.
Fiducials are detected from pad or surface objects on the relevant outer copper layers whose .pad_usage value identifies a fiducial, such as g_fiducial or l_fiducial. Enabling an option does not create missing fiducials. These settings apply to QD; they do not add fiducial rows to XLSX/CSV.
Choose the insert point
Insert Point determines which point of each package is exported as its placement position. It affects the X/Y coordinates in both QD and XLSX/CSV. It does not change the chosen part number. Match this selection to the placement reference expected by the machine library or the downstream table importer.
| Selection | Point used | When to choose it |
|---|---|---|
| Middle of Component | Centre of the overall package bounding rectangle, including its component geometry. | Use when the destination expects the centre of the complete component footprint. Protruding or asymmetric geometry can move this point away from the body centre. |
| Middle of Body | Centre of the package body bounding rectangle. | Use when placement is referenced to the housing centre. Inspect the body definition first: asymmetric pin layouts can make this differ substantially from the centre of the complete component. |
| Middle of Pins | Centre of the bounding rectangle covering the package pins. | Use when the destination references the centre of the pin pattern. This is the centre of the enclosing rectangle, not the arithmetic average of individual pin centres. |
| Middle of Pin 1 | Centre of the first pin geometry's bounding rectangle. | Use for a workflow referenced to pin 1. Verify that the first pin in the imported package definition is the intended pin 1; the exporter uses the first pin geometry rather than searching for a pin named “1”. |
| Package Origin | The local package origin, at package coordinates 0,0. | Use when the destination library follows the CAD package origin. The origin need not coincide with the body centre, pin-pattern centre or pin 1. |
The centre methods use bounding rectangles; they are not area-weighted centres of gravity. Insert Point is one setting for the export, applied to every component through its own package geometry. It is not selected separately for each list row.
How to select and verify the point
- Check which reference the destination system expects. Choose the corresponding method rather than assuming all centre methods give the same result.
- Inspect a representative package in the preview, including an asymmetric package and a bottom-side component. Changing Insert Point updates the preview.
- Check the rotation correction separately. The selected package point is transformed with the component's correction and placement; panel placement is also accounted for. Changing the point can therefore shift both exported X and Y for a rotated component.
- Export a table and compare a known reference against the expected coordinates, angle and side. For example, if an asymmetric connector has a body centre 1 mm from its overall package centre, selecting the other method changes its exported placement point; after rotation this offset need not lie along the board X axis.
Warning: A suitable insert point does not by itself establish the correct ASM orientation. Verify both the reference point and the rotation convention before importing production data.
Export an XLSX or CSV placement list (6)
Use this output for spreadsheet review or a downstream system that accepts a placement table. It contains one row for each included component instance. Both selected sides are written into the same file. For panels, child-board instances are expanded into panel coordinates, including their offsets and rotations; repeated references receive a board-instance suffix when multiple boards are present.
- Prepare the selected board or panel, component filters, part identifier, rotation corrections, Rotation direction and Insert Point as described above.
- Choose Export Top Side, Export Bottom Side, or both.
- Click Export CSV/XLSX File (6).
- In Export Pick & Place List, choose Excel File (.xlsx) or CSV File (.csv), enter a filename and select the destination. The proposed name is
<Project name>_PickAndPlace.xlsx. Connected storage destinations are available according to the configured file providers. - Save and open the result. Excel output contains the worksheet
PickAndPlace; CSV contains the same table and uses PCB-Investigator's configured CSV separator.
| Column | Meaning |
|---|---|
ID | Sequential row number. |
Reference | Component reference; with a board-instance suffix for a multi-board panel, for example R1_1 and R1_2. |
Part | Part name or property value selected in Part Number Identifier. |
Package | CAD package name. |
X (mm), Y (mm) | Coordinates of the selected insert point after component and panel transformations. This dialog exports the table in mm, independently of the viewer's unit setting. Bottom-side X coordinates are mirrored. |
Rotation | Corrected angle in degrees using the selected rotation direction, including panel-instance rotation. |
Side | Top or Bot. |
In BOM | No for components marked with .comp_ignore, otherwise Yes. BOM means bill of materials. This field is not a general evaluation of all possible non-population attributes. |
With Ignore Unplaced enabled, components marked with .comp_ignore are omitted instead of appearing as In BOM = No. XLSX/CSV does not contain the hierarchical QD board structure, board thickness, QD comments, fiducial definitions or Gerber files. Export QD separately if you need those outputs.
Export QD files for SIPLACE/ASM (7)
QD export creates machine-oriented board and placement data. It includes the board dimensions and thickness, selected-side components, part identifiers, references, corrected placement coordinates and angles, and optional fiducials.
Boards and panels
Select either a single board or a panel in Step to Export. QD supports panel structures, including nested child steps, repeated board instances, offsets and rotations. Board definitions are referenced within the exported structure rather than converted into one flat placement table. A panel containing exactly one unrotated, unrepeated single board is handled as a single-board export with its offset accounted for.
Bottom-side component coordinates are mirrored by the exporter. Panel placements are also transformed for the bottom side. Check the imported result against a known component and fiducial instead of applying an additional mirror automatically.
Create and check the output
- Complete the common preparation, orientation check and insert-point selection. Configure fiducials and Gerbers if required.
- Click Export QD File(s) (7) and select an output folder.
- Check the completion message and generated files. Import the selected side into SIPLACE and verify the board/panel structure, part mapping, known component positions, rotations and fiducials.
For a project named Example, the selected output folder contains:
Leiterplatten/
Example_T.la/
Example_A.qd
Example_B.la/
Example_B.qd
Only selected sides are written. Top uses the _T.la folder and _A.qd filename; bottom uses _B.la and _B.qd. Optional Gerber files are stored in the respective side folder. Existing QD output at the same path is replaced; use a separate destination when you need to retain an earlier export.
Note: If unplaced components are retained, QD can mark them as blocked rather than placeable. It recognizes non-population markings including no_pop with yes, loaded with false, and comp_ignore. The Ignore Unplaced filter specifically excludes components with .comp_ignore; review other markings in the result.
Troubleshooting and final checks
| Symptom | What to check |
|---|---|
| Both export buttons are disabled. | Click Refresh List after changes to the identifier or filters. Select at least one export side, enter a non-empty valid Project name, and fill in the panel-fiducial name if that option is enabled. Both buttons share these checks, including the panel-fiducial field even when you intend to export a table. |
| The confirmed count is below the total. | Inspect the remaining entries and mark them User Confirmed. This count does not itself block either export. |
| Components or part identifiers are missing. | Check mount types, pin definitions, Ignore Unplaced and the chosen property. Click Refresh List after changing filters or identifier selection. Text filters in the check list help locate entries; they do not replace the export's component-type and unplaced filters. |
| Coordinates are offset or angles differ from the machine. | Check Insert Point, package geometry/origin, correction and Rotation direction. For a panel, also verify the selected step and board-instance placement. Check bottom-side mirroring before adding further transforms. |
| QD was created, but a Gerber warning appears. | The QD files may already exist. Check selected layers, destination access and whether existing Gerbers can be replaced. Correct the issue and repeat the export. |
| No fiducials appear. | Check the detected counts, selected panel/board options, relevant copper layers and fiducial attributes. Verify the entered names against the SIPLACE library. |
Before using the exported data in production, verify at least one known component on each selected side and representative repeated/rotated boards. Check the file's units, part mapping, placement point and rotation against the receiving system.
Example results in SIPLACE
The following SIPLACE screenshots illustrate the imported result.



Assign Testpoint Attribute
You can find the Testpoint Assign Tool under Plugin >> Assign Testpoint Attribute.
This tool helps to find and mark testpoints in a layout which could be defined via multiple non standardized attributes. Marking them with this tool then helps to standardize this and prepare the layout for following tools (for example the DFT Preperation).
On the top left you can switch between using the current selection or a set rule to find the testpoints and assign the test_point value.
When choosing rules you can add another rule by checking the checkbox of the lowest row in the current listview and then fill out which attribute should be tested and what value needs to be set in said attribute.
All attributes are listed in a simple drop down menu. The Filter Value then has to represent the value of the attribute. Wildcards are allowed when searching for attribute values. The image shows for example all ways to search for "tp" in the "geometry" attribute:
- The first rows searches for all geometry attributes that have exacly the value "tp".
- The second row seraches for all geometry attributes that end with "tp"
- The third row searches for all geometry attributes that start with "tp"
- The fourth row searches for all geometry attributes that have "tp" anywhere in their value
Also it is possible to search for multiple values of the same attribute as shown in the last row. Simply seperate the values with a semicolon.
Boolean attributes do not need any value since their existance already means they are set.
To remove a rule simply select the whole row by clicking on the left most column of the row you want to delete (left of Use Rule) and press the "delete" key on your keyboard.
Checking a rule will select all found possible testpoints of the job (the checkboxes Assign Top and Assign Bottom change the selection depending on the check state of them)
On the top right side there is an information panel showing:
- The currently already set testpoints of the loaded job for the top layer and the bottom layer
- A button to open this help page
- A button to select all currently set testpoints of the loaded job
Export Rules exports the currently set rules to a xml file on selected location on the machine or in a cloud
Import Rules imports rules from a file either from the machine or from a cloud
Remove all Testpoint Attributes removes the "test_point" attribute from all pads of the job
Assign Testpoint Attribute adds the "test_point" attribute to either the currently selected pads or the pads found by the selected rule (handled by the radiobuttons "using Selction" and "using Rule")
Assign Top is a checkbox that when unchecked the "test_point" attribute will not be set for the pads on the top layer
Assign Bottom is a checkbox that when unchecked the "test_point" attribute will not be set for the pads on the bottom layer
To find possible testpoints the attribute histogram is a good way to start.
Elowerk Export
The Elowerk export creates a “xCAM” file that contain all available component and net information to easily create the test program with the native machine software. Optionally also Excellon2 files to create the adapter can be exported.
Following export settings are possible:

- Part number field: Part number field value (Value from Property: %PROP_NAME%)
- Part number field (NOPOP): Part number field value for NOPOP components (Value from Property: %PROP_NAME%)
- Inductor Tolerance Addition (%): Inductor Tolerance Addition in %
- Resistor Tolerance Addition (%): Resistor Tolerance Addition in %
- Capacitor Tolerance Addition (%): Capacitor Tolerance Addition in %
- Export FUSE as RESISTOR: Export FUSE Models as RESISTOR with fix Value (100mOhm/10%)
- Export JUMPER as RESISTOR: Export JUMPER Models as RESISTOR with fix Value (100mOhm/10%), or as SWITCH
- Export SWITCH with Open State: Export SWITCH Models always with Open State
- NAIL Start Index: Start Index for FIXTURE Nails
- Special Partname Rules: Rules to rename parts according their original name
- Export TOP Probes (.ex2): Export TOP Probes as Excellon2
- Export BOT Probes (.ex2): Export BOT Probes as Excellon2
- Export Tooling Drills (.ex2): Export Tooling Drills as Excellon2 with 1.0mm Diameter
- Use Metric Unit (Excellon2): Use metric (true) or imperial (false) unit for excellons
- Export Probes (.xlsx): Export Probes as XLSX
- Set ProbeID in Comment: Changes the current session and sets the Probe ID (Channel) to the Comment column of each Probe
Spea Export
The Spea export creates a “CAD” file that contain all available component and net information to easily create the test program with the native machine software.
Following export settings are possible:

- Side Switch: If true, the PCB will be checked from bottom up
- Rotation: If >0, the PCB will be rotated clockwise by this angle (e.g. 90°) after applying the SideSwitch command (if SideSwitch=true)
- Part number field: Part number field value (Value from Property: %PROP_NAME%)
- Merge all NC Nets: Merge all NC nets into a single NC net
- Inductor Tolerance Addition (%): Inductor Tolerance Addition in %
- ResistorTolerance Addition (%): ResistorTolerance Addition in %
- CapacitorTolerance Addition (%): CapacitorTolerance Addition in %
- Part Device Name: Device name for all parts (Value from Property: %PROP_NAME%)
- Use Value as Device Name (RCL): Use the value as device name for all RCL parts
- Probe Reference Prefix: Reference prefix for dummy components at probe locations
- Export PACKAGE_PINS: Export 'PACKAGE_PINS' Block
- Special Partname Rules: Rules to rename parts according their original name
Stencil Generator

The Stencil Generator uses all zones defined by the Stencil Area Editor. If there are no zones the outline will be used as main zone. Use default rules for your company. Setting a package group, enables the Wizard to set the rules regarding it. SOICs, Chips, BGAs and any definition needed. The Wizard is delivered with predefined settings. To adjust all data preparation to your product you can setup own data preparation Scripts to adjust to your equipment.
Set Package Group is only necessary if your data don’t contain a proper information. Customers with EPL (“Easylogix Part Library”) can resolve trusted data from EPL. The Wizard also process layouts with multiple mask layers in the stack-up. Set “Keepouts for Chips” is only available if you have MPN packaged defined. It will handle the usable area for you. You also can set plugged drills as free usable area.
Check stencil by using current rules
Rule preview
You have the possibility to set rules by package, set extra rules for components in defines zones or to set a rule for each component.
To set another rule to your component, select one in the given list.

All Rules explained below
Add own rules to your stencil automation
You can add your own rules by clicking on the setting symbol.
Panel
| Send the stencil data in your preferred format to your supplier |
Result of the rule-base stencil wizard |
Before and after |
Stencil pad details |
Here is a short video to show special cases in one of our demo designs:
Stencil Area Editor
Edit base settings for each area
Context Menu
side, or description, as well as setting a color for the zone. Additionally, you can export
the file as a list or HTML and such much more opti
Set Area around Selection with cutouts
Add zones by predefined drawings
Edit the Shape
Add a new zone by drawing a rectangle
Note: For high quality, it is recommended not to cut pin pads. You can combine areas e.g. from different parts to get ideal areas.
Zone function
Add new zone with cutting out a previous tone by drawing a rectangle
Combine different zones to one zone
Combining by bounds or intersecting available, depending on the zone size maybe the form has to be an rectangle or it is possible to set special area outlines.
Manage zone settings
-->Zone settings can be saved in ODB attributes, exported as xml and imported from xml.
Part Matcher
For the matching process the mostly unique part number (MPN) is used, but can be extended by the manufacturer to avoid confusion if several manufacturers use the same MPN.
This following picture shows how to match components of the board with part libraries.
1. Select Manufacturer Part No: You can choose between "Part Number", which shows a fixed attribute of the part, or "Property", where you can select any property which contains the value for the MPN. This setting is used to match parts in the selected libraries.
2. Select Manufacturer Part No: Additionally, the manufacturer can (but does not have to) be included in the search (selection of an attribute of the component in which the manufacturer is located). This setting is used to match parts in the selected libraries.
"+" -add new library "-" -delete last library to search
4. Components List of all components in the current design with selected values for Manufacturer Part Number and Manufacturer. Highlighted components does not have values for the selected Manufacturer Part Number and Manufacturer property and can not be searched by the Part Matcher. The checkbox can be used to select the components which should be matched by the Part Matcher.
8) User Credentials
User Credentials to log in or change user
Solder Frames
The Production Tool Editor to define solder frames:

The solder frame definition based on an single PCB with fixing elements as well as down holder with routings for spcial cases like THT components.
Coating Carrier
The Coating Carrier function allows users to create and configure production carriers for conformal coating processes. A coating carrier is used to securely hold one or multiple PCBs in a defined position inside a coating machine, allowing them to be processed together.
PCB-Investigator simplifies the creation of coating carriers and helps optimize the available space within the coating machine. Predefined frame templates can include the machine's working area, allowing users to arrange PCBs efficiently within the available space. These templates and working areas can also be customized and maintained by the customer to match their specific production equipment.
The editor provides tools for defining carrier frames, adding fixing and supporting elements, generating routing geometries and checking coating keepout areas.

Basic Settings
The Basic Settings section defines the PCB or panel used for generating the coating carrier.
- Basic Step: Selects the PCB or panel step used as the basis for the carrier.
- Define Extra Material: Allows users to configure additional elements such as stoppers, fixing elements and supports.
- Create Coating Elements: Generates a separate step containing the coating elements for a single assembly, which can be used to create the complete carrier frame.
Coating Machine
The coating machine settings allow users to adapt the carrier to the equipment used in production.
- Select Coating Machine: Selects a predefined coating machine.
- Configure Coating Machines: Opens the configuration dialog for managing coating machines.
- Coating Machine Info: Displays additional information about the selected machine.
- Edit Coating Keepout Zones: Opens the editor for defining areas that must remain free of coating material.
Depending on the configured extra material, openings for the coating machine heads can be generated automatically.
Routing Options
The Rout Option section provides tools for creating and modifying routing geometries around the PCBs.
- Oversize (mm): Defines the additional clearance around the routed elements.
- Create Routing: Automatically generates routing around the individual PCBs in the coating frame.
- Add Routing Element: Allows additional routing geometry to be inserted manually.
- Clean Routings for Export: Cleans corners and overlapping routing segments to prepare the geometry for export.
After manually modifying routing elements, use Clean Routings for Export to ensure that the routing geometry is prepared correctly.
Coating Panel Frame
This section allows users to generate the complete coating carrier frame and verify its supporting structures.
- Bridge Size (mm): Defines the size or distance of the connecting bridges in the frame.
- Create Coating Panel Frame: Generates the complete carrier frame, including the configured sub-elements.
- Check Bridge Sizes: Checks frame bridge clearances based on the estimated PCB weight.
- Top View / Bottom View: Activates the relevant layers for inspecting the corresponding PCB side.
Coating Areas
The Coating Areas section allows users to check whether the defined coating keepout zones comply with the required clearance rules.
- Distance Rule Routing (mm): Defines the minimum distance between coating areas and routing geometry.
- Distance Rule Panel (mm): Defines the minimum distance between coating areas and panel edges.
- Check Coating Keepout Area: Checks the defined keepout zones against the configured distance rules.
- Create Coating Areas for Components: Generates coating areas on additional layers based on component information. This function is hidden by default.
Detected violations are displayed in a result list containing the following information:
| Column | Description |
|---|---|
| Coating Errors | Description of the detected issue. |
| From | First affected object. |
| To | Second affected object. |
| Layer | Layer containing the issue. |
Double-click a result to navigate to the corresponding location in the PCB graphical view.
Recommended Workflow
- Open the Production Tool Editor and select the Coating Carrier tab.
- Select the required Basic Step.
- Configure the fixing and supporting elements under Define Extra Material.
- Click Create Coating Elements to generate the individual carrier elements.
- Select and configure the required Coating Machine.
- Define the necessary Coating Keepout Zones.
- Set the routing Oversize and click Create Routing.
- Define the Bridge Size and generate the frame using Create Coating Panel Frame.
- Verify the frame with Check Bridge Sizes.
- Configure the clearance rules and click Check Coating Keepout Area.
- Review and correct any reported violations.
- Clean the routing geometry and export the finished carrier using the Export tab.
Result
The generated coating carrier contains the configured frame geometry, fixing and supporting elements, routing structures and coating keepout definitions.
The carrier can be inspected in the PCB-Investigator graphical view and exported for further processing in compatible production and manufacturing systems.
Workpiece Carrier
The Production Tool Editor to define workpiece carrier:

The Workpiece Carrier function allows users to create customized transport frames for PCBs during the manufacturing process. These frames help securely position and hold the PCB in place while it moves through different production stages.
Additional elements, routing paths and hold-down features can be defined to adapt the carrier to the specific PCB geometry and production requirements.
This makes it possible to prepare workpiece carriers that support stable handling and positioning throughout the manufacturing process.
Supporting Plate
The Production Tool Editor to define supporting plates:

The Supporting Plate function allows users to design customized support plates for press-fit operations during PCB manufacturing. These plates provide mechanical support to the PCB and help prevent bending or damage when pressure is applied during component insertion.
Users can define routing paths and additional geometries to adapt the supporting plate to the PCB layout and specific production requirements.
The resulting design data can be exported for manufacturing and documentation, helping ensure accurate positioning and reliable support throughout the press-fit process.
Test Adapter Since v17.1
The Production Tool Editor to define adapter definitions:

The adapter definition is the most complex production tool, it contains all standard cases for special testing routines e.g. high voltage checks or vacuum systems. Special handling for connectors, LED Checks, switches or press buttons included.
You can handle stops and fixing elements as well as routings for high components and down holder or supporting stamps. After defining all important elements it is possible to add an example adapter panel to export the adapter package for one DFT Session.
The export contains additional files to create 3D models like this:

(3D view contains PCB, models for fixing pins, extra electronic and the adapter case)
Export routing data as a single STEP file.

It is now possible to combine complete plate stacks for one side in one step file, you get different depth values in the plate for each routing level. You can use the export for 3D printing or import it in other tools. The new stackup definition system is more flexible and gives user better options to define the routing depth.
Video Tutorial
Watch our PCB-Investigator - DFT Preperation Video here:
Tutorial: DFT Preperation & Machine Export:
Cutout Editor
The Cutout Editor helps you to create additional elmenets and modify the cutouts:

1) List of all cutouts, they have an running ID and a Location X/Y for special cutouts there is also and End X/Y and an repeat Index (for each child step).
2) Edit area for the cutouts, you can modify the Location.
3) Additional Element Area, here you can define what you need on different layers
4) Auxilary Drills is special, you can generate mousebites for one or both sides.
For setting mouse bite drills we have a second video:
Package Library Manager
The Package Library Manager handle all libraries for packages, this could be e.g. an 365 library, an lite DB or an xml library and customized libraries:

You can edit the packages here and change properties.
Here is a short video to show how you can add your own library:
Part Library Manager
The part library manager gives you options to edit your list of part libraries:

With some options to copy/delete/add new parts you can manage your libraries here and manage the available libraries in the settings dialog:

The library types containing data from the open Job/Design, local types like xml or lite DB and online types like API Part Libraries, REST Libraries and out 365 Libraries:

With the context menu you have options to copy or edit the part, you can export the library list and search for specific information:

Here is an short video how to bring parts in your library:
Edit Properties
use the pencil button to edit package properties in an seperate dialog:

Depending on the library type there are different properties available, with 365 libraries you can manage your properties in admin area or in xml library you can directly change the available properties.
Edit Properties
use the pencil button to edit part properties in an seperate dialog:

Depending on the library type there are different properties available, with 365 libraries you can manage your properties in admin area or in xml library you can directly change the available properties.
Net Groups
All Nets can have net attributes, if you set an Net Group it will be handled in some plugins together.
To find out how you can set this net groups read this page
Settings

There are some basic settings to match the packages.
Pin Positions are always used, but you can change the Height information of your CAD Data to tolerance value based on the component height or ignore it complete.
Overwrite package and step information defaul by "Ask", this mean there comes a dialog with checkboxes.
How To Use
How to use the Package Expert firt time?
Here is a short video how to ask Library for all components and set 3D settings:
Main Dialog
Open BOM Expert from the PCB-Investigator plugin menu. The dialog works with the current design and active step.
Part Match Library
Select the library used to search for matching parts and package information. A library must be selected before BOM or AVL data can be imported.
Settings
Settings
The settings control the available BOM and AVL importers, property names written during Apply, not-populated and component-ignore behavior, copying of library properties, the review library used for reported parts, and an optional action executed after applying the result.
Status Message
The status message is displayed in the Status column of the upper component list in the BOM Expert main dialog. It shows the current result of the reference, part, and package matching for each component entry.
| Status | Meaning |
|---|---|
Unknown |
No detailed matching result is available. |
ReferenceNotInAVL |
The component exists in the layout but not in the imported AVL data. |
ReferenceNotInDesign |
The imported reference does not exist in the current design. |
NoPartAvailable |
The AVL entry contains no usable part candidate. |
NoPartSelected |
Candidates are available, but no part is selected. |
NotFoundInLib |
The selected MPN was not found in the active library. |
OKUnverified |
A part is assigned, but package or pin compatibility was not fully verified. |
OK |
The selected part and CAD package are considered compatible. |
SelectedPartDoesNotMatch |
The selected library package does not match the CAD package sufficiently. |
Stencil Creation Script
To automate your custom stencil scripts, it is necessary to use the StencilCreationScript interface.
Here is a link to see all details for your implemention manual.
You have to set public porperties to give user options to change in the property grid, there is also a method to create the preview and the pads. You should fill the corde with all calculation you need e.g.
public bool CreatePads(IPCBIWindow parent, IStep step, IODBLayer StencilLayerOutput, InterfaceCMPObject BasicObjects, List<IPolyClass> UsedPinPads, List<IPolyClass> MaskForCheck, List<IPolyClass> Drills, double ThicknessPaste)
{
if (StencilLayerOutput == null || BasicObjects == null || UsedPinPads.Count == 0)
return false;
bool IntersectWithMask = false;
CreateRectangleElement(StencilLayerOutput, UsedPinPads, MaskForCheck, Drills, BasicObjects, out IntersectWithMask);
return true;
}

In the options area (1) you can add your custom developed scripts (2).
Stencil Rule Donut
Donut Creation for Stencil Pads
In stencil design, a donut shape is used to define a circular opening with a central void (hole), commonly used for thermal reliefs or annular ring designs. The donut is generated around a pad center based on several configurable parameters.
Donut Properties
| Property | Type | Description |
|---|---|---|
InnerDiameter |
double | Defines the inner diameter of the donut. This is the size of the central hole that will not be cut into the stencil. |
OuterDiameter |
double | Specifies the outer diameter of the donut, representing the total size of the stencil opening. |
AngleStep |
double | Angle between each arc segment when constructing the donut shape. A smaller step creates a smoother circle. |
OffsetX |
double | Offset in X-direction from the pad center, applied to reposition the donut shape. |
OffsetY |
double | Offset in Y-direction from the pad center. |
Rotation |
double | Applies a rotation (in degrees) to the donut shape around the pad center. |

Usage
These properties are used by the StencilScriptDonut class to calculate and render the donut shape on stencil pads. The donut is typically composed of an outer arc (outer diameter) and an inner arc (inner diameter), combined with connecting lines to form a closed shape.
Ensure that InnerDiameter is less than OuterDiameter to create a valid donut. Adjust AngleStep based on performance vs. accuracy needs.
Stencil Rule Array
Array creation is used to replicate pad openings in a structured pattern. This is especially useful for components like QFP or QFNs,
where cooling pads are very big and replaced by array formation. The array is defined using specific rules and transformation parameters, it gives you an easy way to define an array of similar (rounded) rectangles.
Array (Fix) Properties
| Property | Type | Description |
|---|---|---|
Array Field Count in X direction |
int | Fix Array Rule only: Array pads count in X direction. |
Array Field Count in Y direction |
int | Fix Array Rule only: Array pads count in Y direction. |
Corner Radius (MM) |
double | Corner radius for rounded elements in MM. |
Utilization Array Area (%) |
double | Utilization of avalable area in percent (only used if no fix size is used and value >0). This option will ignore the undersize value and depending to the settings it is possible the values are not exact. |
Minimum Array Field Size (MM) |
double | Array pads has minimum this size, if there is only space for one pad no array created. |
Offset to Center in X direction (MM) |
double | Fix Array Rule only: X offset to shift the array from the pad center. |
Offset to Center in Y direction (MM) |
double | Fix Array Rule only: Move array in Y direction from center of the pin. |
Distance Array Fields (MM) |
double | Array pads has this distance to next pads. |
Undersize Value in MM |
double | This value is only used if no Array size is defined. All other Elements will use this value in mm to generate undersize. |
Ignore Mask Intersecting |
bool | Do not check for mask intersecting (add all array elements without checking mask). |
Array Size Width (MM) |
double | Width for complete array, if it is =0 the original element width is used. |
Array Size Height (MM) |
double | Height for complete array, if it is =0 the original element height is used. |

Usage
These properties are used in the StencilScriptArray class to define how shapes are duplicated and transformed. Each array pattern follows a specific logic:
- check avalable size of array
- check max pad size and gap value
- split area in pads and round the rectangles
Use array rules to easily build consistent and scalable designs for components with repeated pad layouts.
Adjust offset values to fine-tune placement, it also has an utilization property to gives the rule an optimum of area.
Stencil Rule House
The StencilScriptHouse class defines the necessary parameters to create a house structure around a stencil pad for solder paste applications. It is used for automating stencil generation and includes geometry, shape characteristics, and spacing considerations.
Properties
| Property | Type | Description |
|---|---|---|
Corner Radius (MM) |
double | Corner radius for rounded elements in MM. |
Offset to Center (MM) |
double | Move houses to the center of the component. |
Invert Direction |
bool | For smaller elments sometimes the house should be show away from the component. |
Undersize Value (MM) |
double | All Elements will use this value in mm to generate undersize. |
House distance cut size in Percent |
double | Value in percent depending to the height of the pad. |
Utilization House Area (%) |
double | Utilization of avalable area in percent. This option will modify the cut size value to come near to the percent value. Use 0 to ignore this value. |

These parameters help define the geometric and contextual constraints for automatically generating stencil pad protection using a house-shaped perimeter. The house rule is recommended for chip packages, but can be used for all pins with clear directions.
Note: If the pin is under the body the direction cannot be calculated and no house is created.
Stencil Rule Inverted House
Depending to the chip size it is recommended to change from house to inverted house rules.
Inverted House Properties
| Property | Type | Description |
|---|---|---|
Corner Radius (MM) |
double | Rounding on the corners. |
House distance cut size in Percent |
int | Value in percent depending to the height of the pad. |
Invert Direction |
bool | For smaller elements sometimes the house fhould be show away from the component. |
Max Size of one Element (MM) |
double | Each element has maximum width and height, if the size is bigger it is automatically splitted in more elements. The value is in MM! |
Undersize Value (MM) |
double | All elements will use this value in mm to generate undersize pads. |
Offset to Center (MM) |
double | Move houses to the center of the component. |
Step for Big Elements (MM) |
double | If the element is bigger Max Element Size it use this value to split the size in more elements. |

Usage
These properties are used in the StencilScriptInvertedHouse class to define how shapes (such as stencil pads or vias) are duplicated and transformed. In general this rule is used for Chip Packages.
Note: If the pin is under the body the direction cannot be calculated and no house is created.
Stencil Rule Simple Rectangle
The StencilScriptSimpleSurface class defines the necessary parameters to create a rectangle structure around a stencil pad for solder paste applications. It is used for automating stencil generation and includes helpfull options.
Properties
| Property | Type | Description |
|---|---|---|
Corner Radius (MM) |
double | Corner radius for rounded elements in MM. |
Try Find Direction |
bool | Rotate surfaces depending to the direction of the pin. |
Rotate Bridges 45 Degrees |
bool | All bridges are rotated 45 degrees to obtain diagonal openings. |
Offset to Center X (MM) |
double | Move rectangle in X direction from the center of the pin. Or if you use negative values away from center. |
Offset to Center Y (MM) |
double | Move rectangle in Y direction from the center of the pin. Or if you use negative values away from center. |
Bridge Width (MM) |
double | Use bridges to cut the rectangle with this width. |
Bridge Count X |
int | Use bridges to cut the rectangle with count in X direction. |
Bridge Count Y |
int | Use bridges to cut the rectangle with count in Y direction. |
Offset move away disctance (MM) |
double | Move surface away from center point, this is only for outer pins (not for cooling pins). |
Size Width in MM |
double | Width for this pad. |
Size Height in MM |
double | Height for this pad. |

These parameters help define the geometric and contextual constraints for automatically generating stencil pad protection using a rectangle-based-shaped perimeter.
Note: The simple rectangle rule ignore the mask opening and overprint it!
Stencil Rule Undersize
The StencilScriptUndersize class defines the necessary parameters to create a similar structure around a stencil pad for solder paste applications with smaller size. It is used for automating stencil generation and includes geometry, shape characteristics, and spacing considerations.
Properties
| Property | Type | Description |
|---|---|---|
Undersize Value in Percent |
double | All Elements will use this percent value on the smaller side to generate undersize. |
Undersize Value in MM |
double | All Elements will use this value in mm to generate undersize. |
Corner Radius (MM) |
double | Corner radius for rounded elements in MM. The value is independent of the undersize and can change the earthings with different values. |
Max Size of one Element (MM) |
double | Each element has maximum width and height, if the size is bigger it is automatically splitted in more elements. Value is in MM. |
Steg for Big Elements (MM) |
double | If the element is bigger MaxElementSize it use this value to split the size in more elements. Value is in MM. |

These parameters help define the geometric and contextual constraints for automatically generating stencil pad protection using a smaller-shaped perimeter.
Note: If the undersize values to small no pad will be created, the rule checks the mask layer for intersecting!
Stencil Rule Use Pin intersecting with Mask
The StencilScriptUsePinMinusMask class defines the necessary parameters to create a pin bases structure. It is used for automating stencil generation and includes geometry, shape characteristics, and spacing considerations.
This rule gives you the option to use the pin outline as basis with following options:
Properties
| Property | Type | Description |
|---|---|---|
Undersize Value in Percent |
double | All Elements will use this percent value on the smaller side to generate undersize. |
Undersize Value in MM |
double | All Elements will use this value in mm to generate undersize. |
Overwrite All Pins |
bool | Overwrite all pins regardless of the underlying pads. Set this property to false if you want to change single pins with different rules! |
Corner Radius (MM) |
double | Corner radius for rounded elements in MM. The value is independent of the undersize and can change the earthings with different values. |
Ignore Mask Layer |
bool | Take Pin without Mask Intersecting! This do not check overlappings and openings in the mask layer. |

These parameters help define the geometric and contextual constraints for automatically generating stencil pad protection using the pin definition as basis.
Note: If the undersize values to small no pad will be created, the rule checks the mask layer for intersecting and it is a special handling for Overwrite All Pins to replace all pins with one rule!
Testpoint Foil Export
Export tespoint foil as PDF or print it.

The export looks like this:

All Labels are searchable in the PDF, for panel it counts up after the first PCB.
Component Attribute Import
Import component attributes and properties from csv/excel files:

There are some options to set variants, no pop and comp ignore attributes. Depending to the containing components all others are ignored and/or set no_pop. The variants set/add for all included components so it is easy to handle different placement variants by loading different excel/csv files.
Depending to your attribute file you can connect it via Reference, Part Number, Package or free propertes (e.g. MPN or VPN).
Essemtec Pick & Place Exporter
Essemtec Pick & Place Exporter

The Essemtec Pick & Place Exporter is used to create ePlace recipes from an ODB++ design loaded in PCB-Investigator. The dialog compares the CAD components from the selected ODB++ step with the Essemtec/ePlace component library, allows the user to check and correct package alignment, and finally creates the required recipe structure in ePlace.
The typical workflow is shown by the numbered areas in the dialog. Work through the dialog from top to bottom and from left to right.
-
Open Settings
Before the exporter can communicate with ePlace, the connection to the PCBIEssemtecServer must be configured. Press Settings to open the settings dialog.
Configure the PCBIEssemtecServer connection
In the settings dialog, select whether the server is used as a Local Server or a Remote Server. For a local server, enter the path to the installed PCBIEssemtecServer in Server Path. The server address is typically localhost. The Server Port defines the REST port used by PCB-Investigator.
The PCBIEssemtecServer is installed separately if required (contact support@easylogix.de to get the installation package). It provides a REST server for PCB-Investigator on one side and connects to the ePlace DLLs on the other side. PCB-Investigator communicates only with this server. The server performs the required ePlace library queries and creates the requested ePlace objects.
Press Save to store the settings. The exporter uses these settings when refreshing the list and when creating recipes in ePlace.
-
Select the Step to Export
Select the ODB++ step that should be prepared for export. The selected step defines the board, panel, or sub-panel level that is used to build the component list and recipe structure.
-
Choose how components are grouped
Use Group Components by to define which value is used as the Essemtec/ePlace component name.
Part Number uses the internal ODB++ part number field.
Property allows selecting any existing component property from the ODB++ design. The selected field must contain the component name that also exists in the ePlace library.
Example: If the property EssemtecPart is selected, every component group must contain an Essemtec part name in this property. This name is then used to search the ePlace component library.
-
Set the component filters
The Type Filter controls which components are included in the list according to the ODB++ attribute .comp_mount_type.
Activate Ignore Unplaced if components marked as not placed should be excluded when building the list. Components with ODB++ attributes such as .comp_ignore or .no_pop can be left out this way.
The Property Filter can be used to include or exclude components based on a selected component property and a text value. The filter affects both the displayed list and the export result. Only components that are present in the list are exported to ePlace.
-
Refresh the component list
Press Refresh List after opening the dialog and whenever the selected step, grouping, filters, or settings have changed.
Refresh List builds the component list according to the current filter settings and immediately matches the component groups against the ePlace library. During this step, PCB-Investigator also tries to automatically recognize the correct orientation. Components may be tested in 90 degree rotation steps to find a fitting orientation.
-
Check the component placement list
The main table shows the grouped CAD components and the result of the ePlace library matching. Each row represents one component group.
The table shows the component name, references, ODB++ step, matched Essemtec part, Essemtec processes, status, and description. The status column is the most important column for checking whether the component is ready for export.
-
Understand the status messages
OK means that the Essemtec part was found and the package analysis is valid.
No Essemtec Part Available means that no matching part with this name exists in the ePlace library. The component can still be exported with this part name, but the missing part must then be created later in ePlace, unless an existing component shape is selected before export.
Selected Essemtec Part does not fit means that an Essemtec part is selected, but its package does not match the CAD package. The user must check the component, select another shape if required, or correct rotation and offset.
POLARITY is added as an information marker if the component has a polarity marker. In this case, the user should check the polarity carefully before export.
-
Use the package and pin analysis
The exporter checks whether the package from the ePlace library fits the CAD package. The analysis verifies that the pin count is identical and that every ePlace pin lies inside exactly one CAD pin. Additional orientation checks are also performed.
If polarity information is available, PCB-Investigator also checks whether the polarity marker is located close to CAD pin 1 or the marked polarity pin. If this is not the case, a warning is shown in the pin analysis.
-
Search a component shape for missing parts
If no Essemtec part exists for a component group, right-click the row in the lower component table and select Search Component Shape (F2).
This allows the user to select an existing package or component shape from ePlace. PCB-Investigator can then create a new Essemtec part in ePlace using this selected shape.
PCB-Investigator only creates the new part. Missing component information must be completed later in ePlace by the user.
If no package is assigned, the component is still exported with the part name from the list. In that case, the part does not yet exist in ePlace and must be created later there. ePlace will warn the user about this situation.
-
Review the selected Essemtec part details
The lower table shows the selected Essemtec part or component shape for the currently selected component group. It contains information such as Essemtec name, component shape, comment, size values, processes, and pin analysis result.
-
Use the graphical preview
The preview on the right side overlays the CAD package and the selected Essemtec package or shape. It helps the user visually check body size, pin position, pin numbering, package center, and polarity.
The CAD and Essemtec outlines are shown together so that mismatches can be detected before export. If the Essemtec package is shifted or rotated compared to the CAD package, the component may not fit until the placement transformation is corrected.
-
Move or rotate the selected part
Use Move Part to shift the selected Essemtec part relative to the CAD component. The step width defines the movement distance for each click.
Use Rotate Part to rotate the selected Essemtec part. The rotation value is entered in degrees and is applied clockwise.
Use Reset Transform to remove the manual transformation and return to the automatically recognized position.
-
Enter the project name
The Project name is used as the base name for the created ePlace recipes and optional jobs.
Recipe names are created from the project name, the step name if required, and the side postfix. For the selected step itself, the project name is used unchanged as the base name. For lower-level steps, the step name is appended. The side postfix is then added, for example Top or Bot.
-
Select the export side
Use Top Side and Bottom Side to define which board sides are exported. Only the activated sides are created in ePlace.
The exporter creates separate recipes per side and step. For panels and family boards, the individual board recipes are created first. Panel-level recipes are then created separately and reference the corresponding individual board recipes in ePlace.
-
Select a template recipe
Press the template recipe selection button to select an existing ePlace recipe as a template. The selection dialog lists the available recipes from ePlace.
The selected template can be used to copy ePlace-specific settings into the newly created recipes. These settings are independent from the PCB layout data in PCB-Investigator.
The following template settings can be copied if selected:
-
Machine Settings
-
Process Control
-
Transport Parameters
-
-
Export fiducials
Activate Export Fiducials to export recognized fiducial pads to ePlace.
PCB-Investigator recognizes ODB++ pads on the outer copper layers with the attribute .pad_usage=l_fiducial or .pad_usage=g_fiducial. These pads are exported per step using the selected ePlace fiducial symbol.
The number in brackets shows the number of recognized fiducials that will be exported with the current settings.
-
Export bad board markers
Activate Export Badmarkers to export recognized bad board marker pads to ePlace.
PCB-Investigator recognizes ODB++ pads on the outer copper layers with the attribute .board_mark. The value of the attribute is not relevant. Pads with values such as bbm or gbm are recognized.
The pads are exported per step using the selected ePlace badmarker symbol. The number in brackets shows the number of recognized badmarkers that will be exported with the current settings.
-
Set an additional global rotation
Use Additional Rotation (CW) if the PCB is placed into the machine with an additional rotation.
The entered angle is applied globally to the generated recipe. The value is clockwise.
-
Check the recipe process order
The Recipe Process Order area shows the processes available from ePlace, for example Glue, Solder, and PICKANDPLACE.
The processes shown for each component come from ePlace. The user can select which processes are included and define their order before export.
-
Select the default medium for each process
For each process, select a Default Medium from the list provided by ePlace.
The selected medium is required when the job or recipe is created in ePlace. The available names come from Essemtec/ePlace.
-
Create the recipe or recipes in ePlace
Press Create Recipe(s) in ePlace to create the required ePlace recipes from the current list and settings.
Before the export starts, PCB-Investigator checks whether the required recipe and job names are still available in ePlace. If one or more names already exist, the occupied names are displayed and the user must change the project name or naming settings before exporting.
PCB-Investigator does not delete, edit, or overwrite existing ePlace objects. It only creates new objects.
All components currently shown in the list are written to the recipe. Parts are only newly created in ePlace if they were not found during refresh/matching and if the user assigned an existing package or component shape.
-
Create jobs per side if required
Activate Also create a 'Job' per Side if jobs should be created together with the recipes.
A job is an ePlace object that is based on one or more recipes. If this option is active, PCB-Investigator creates the required jobs after creating the recipes.
Additional information: XML settings
Some naming options can be adjusted manually in the XML settings file:
%LOCALAPPDATA%\EasyLogix\PCB-Investigator\PlugIns\EssemtecExportSetting.xml
The default side postfixes are typically Top and Bot. They can be changed in the XML settings if another naming convention is required.
The name prefixes for exported fiducials and badmarkers can also be configured there. By default, fiducials use the prefix Fid and badmarkers use the prefix Bad. The generated names are therefore created as Fid1, Fid2, Bad1, and so on.
Prepare 3D Print Since v18.0
The Prepare 3D Print function allows users to prepare PCB-related production tools for 3D printing. It provides tools for creating 3D areas, defining multiple plate levels, generating component openings and preparing the required geometry for export.
This workflow is particularly useful for creating customized production fixtures that require precise cutouts and different height levels to accommodate the PCB and its components.
Project Overview
The Project Overview window manages the available 3D printing projects. Existing projects are listed on the left, displaying the project name, type and associated PCB step.

The following actions are available:
- Add Project: Creates a new project.
- Remove Selected Project: Removes the selected project.
- Export Selected Project: Exports the selected project.
Each project contains two main tabs:
- General Data: Contains customer information, project details, quantities, PCB thickness and comments.
- Task: Provides the tools for preparing the 3D printing geometry.
Create 3D Areas
The Create 3D Areas tab defines the geometry and basic export settings for the 3D printing project.
Export Settings
- Export PCB Dummy: Includes a dummy representation of the PCB.
- Export Panel Dummy: Includes a dummy representation of the PCB panel.
- Export Plates: Includes the defined plate geometries.
- Export Layer: Allows an additional layer to be selected for export, including a configurable dimension.
Geometry Preparation
- Create 3D Print Step and Layers: Creates the required PCB-Investigator step and layers for preparing the 3D printing geometry.
- Create manual Cutout Objects for Print Area: Allows manual creation of cutout objects within the print area.
- Create Component Openings: Generates openings for components in the prepared geometry.
Define Outline
The Define Outline section allows users to configure the dimensions of the print area.
- X / Y: Define the position of the outline.
- Width / Height: Define its dimensions.
- Use rounded corners: Enables rounded corners.
- Radius: Defines the corner radius.
Click Create Outline to generate the configured outline.
Define 3D Levels
The Define 3D Levels tab allows users to create multiple plate levels for the top and bottom sides of the PCB. Each plate can be configured independently to define the required geometry at different heights.
Plate Settings
| Parameter | Description |
|---|---|
| Name | Name of the plate level. |
| Distance to PCB (mm) | Distance between the plate level and the PCB. |
| Mill-in from (mm) | Starting height for the milling or cutout region. |
| Routing Step (mm) | Height level associated with the routing geometry. |
| Thickness (mm) | Thickness of the individual plate. |
Top and Bottom Configuration
- Enable Top Side: Activates the plate configuration for the top side.
- Enable Bottom Side: Activates the plate configuration for the bottom side.
- Add Plate: Adds another plate level.
- Remove: Deletes the selected plate level.
- Set Default: Restores the default plate configuration.
- Top View / Bot View: Activates the corresponding view for inspecting the geometry.
The graphical preview displays the individual plate levels in relation to the PCB.
Combine Plates in ONE STEP File
When enabled, this option combines the defined plate levels into a single STEP file instead of handling them as separate plate models.
Recommended Workflow
- Open the Project Overview and create or select a project of type Prepare 3D Print.
- Enter the required information under General Data.
- Switch to Task > Create 3D Areas.
- Configure the required export options.
- Define the print area using Create Outline.
- Click Create 3D Print Step and Layers to generate the necessary geometry structure.
- Create additional cutouts and component openings where required.
- Open Define 3D Levels.
- Enable the required PCB sides and configure the individual plate levels.
- Review the plate arrangement and height settings.
- Select Combine Plates in ONE STEP File if a combined model is required.
- Click Export Selected Project to export the prepared project.
Result
The prepared 3D printing project contains the defined print area, selected plate levels and any generated cutouts or component openings.
These geometries can be exported for further processing in compatible mechanical CAD or 3D manufacturing applications.
Load a Component List and Map Columns
Use Components (CSV) Import to create placed components from a pick-and-place or other tabular component list. Open it through Import > Assembly > Components (CSV) Import. The window title is Import Components.

Prepare and load the component list
For an existing PCB, open the intended job and step first. Coordinates in the component list must refer to the same origin as the PCB geometry. For a component-only job, use Create new Job on the Settings tab before creating the components.
- Click Load Component List and choose a
.xlsx,.csvor.txtfile. - If the Excel workbook contains several sheets, select the sheet containing the placement table.
- Review the loaded data on Column Mapping. If text data appears in one column or splits incorrectly, check Text Separator on Settings, then reload the file.
- Assign the source columns using the selectors on the left. Verify the proposed assignments against several actual components.
CSV and delimited TXT files use the selected separator. Auto evaluates common separators; aligned fixed-width TXT reports can also be recognized. Warnings about irregular rows require checking the preview before proceeding.
The last successfully loaded file is remembered separately for each saved design. The next selection starts in its directory while that directory is available. Otherwise, the job's user folder is offered when it contains tabular files, followed by the usual file-dialog location. Cancelling the selection does not replace the remembered file.
Assign the source columns
Column letters identify the source data, for example B. Assigned fields appear in parentheses in the preview header, such as B (Reference). Leave an optional selector empty when the list does not contain that information.
| Field | Meaning and checks |
|---|---|
| Reference | Reference designator, such as R46 or U2. Use a unique reference for each placed component. |
| Partname | Part name or part number used for component information and optional part-library lookup. |
| MPN | Manufacturer part number, where supplied by the source list. |
| Package | Source footprint name used to find a suitable package. This name can differ from the final assigned library package. |
| Pos X / Pos Y | Placement coordinates. Map both columns and select their unit on Settings. Rows without valid numerical coordinates cannot be placed. |
| Rotation | Placement angle in degrees. Select the source convention, CW or CCW, under Rotation Direction. |
| Location/Side | Assembly side. Use clear values such as Top and Bottom. An absent or empty side is treated as Top. |
| Mirror X | X-mirroring indicator. The text value true requests mirroring; this field is separate from assembly-side selection. |
| Value | Electrical or descriptive component value. |
| Description | Additional component description. |
| Manufacturer | Component manufacturer. |
Recognized headers and previously used header layouts can propose a mapping. These proposals do not establish that the source coordinates, side or rotation convention are correct. Check those settings each time the input format changes.
Check a representative placement
Choose a component with a recognizable pin 1 or asymmetric footprint. Check its reference, side, coordinates, angle and package name in the preview. After creation, compare the actual pin geometry with the PCB pads. A correct-looking component centre alone is insufficient.
Import Components Settings
Open Import > Assembly > Components (CSV) Import, load the placement list and select Settings. Configure the import before pressing Create Components. The blue callouts below identify the four groups described in this article.

1. Import Options
| Control | Purpose and use |
|---|---|
| Text Separator | Select the delimiter used by CSV or delimited TXT data, or choose Auto. Fixed-width TXT tables are recognized separately. If parsing is wrong, change the setting and reload the component list. |
| Unit | Select the unit of the imported X/Y coordinates, for example mm, inch or mil. This describes the source file, independently of the unit displayed by the PCB view. Check automatically suggested units against the source export. |
| Create new Job | Create and load a new job for the imported components. Leave it unchecked to add components to the current PCB. Existing-board pad checks and geometry-based footprint detection require a loaded board rather than an empty new job. |
| Add Pin Pads | Add pad geometry for the imported component pins. Enable only when additional pin-pad objects are wanted in the job; it is usually unnecessary when suitable board pads are already present. |
| Remove Existing Components | Remove the current step's existing top- and bottom-side components before importing the new list. It is unavailable when creating a new job. |
| Rotation Direction: CW / CCW | Interpret source angles as clockwise or counter-clockwise. Angles are in degrees. Use the convention of the placement-file export and verify it on a component with a recognizable pin 1. |
Warning: Review Remove Existing Components before importing into a populated job. Keep a saved copy of the original design if the existing placement must be preserved.
File metadata or coordinate headers can provide a unit suggestion. If the suggested unit disagrees with the source export, select the correct unit manually before creating components.
2. Libraries
Used Part Library (optional) selects a source of part information. Part names from the component list are matched against this library to enrich component information. A part library supplies part data; the package library in group 3 supplies footprint geometry.
Use MPN Outline for Missing Packages can supply a simplified component outline when no suitable package is resolved and the selected part library provides a usable manufacturer part number (MPN). It requires the optional part-library lookup. Review the resulting outline and pins; an outline fallback is not proof of a complete footprint match.
3. Package Finder
Used Package Library
Select the concrete library containing the footprints to search. Provider headings identify sources and are not selectable package libraries for component creation. The Used Package Library checkbox state and the library choice are retained with the import settings after successful Create Components.
Package Name Compare
- Check for Similar Package Names allows a similar-name search when no exact package-name match is found. Check the resulting geometry before accepting a candidate with a different name.
- Only Exact Matches Allowed restricts name comparison to exact matches. It does not turn off separately configured footprint detection.
These options are mutually exclusive and are restored from the saved import settings.
Package aliases
Use Package Alias Cache reuses saved mappings between source package names and library packages. Suitable aliases are checked before ordinary package-name matching. Successful matches can improve the saved mappings. With the option unchecked, the import does not read or automatically update those aliases.
Manage Alias Cache opens Package Alias Cache – Management. The button is enabled when Use Package Alias Cache is checked. The dialog is described at the end of this Settings article.
Enabled Layer Check
Enable Enabled Layer Check to validate candidate package pins against the PCB's pad geometry. Choose the physical comparison layer separately in Top Layer and Bottom Layer. The selectors use the job's layer colours. Controls for a side without imported components are disabled.
| Pad Check (Layer Type) | Use with |
|---|---|
| Perfect Fit (Copper) | Copper pads: compare the footprint pins with the board's copper pad geometry. |
| Pads Bigger (Mask) | Solder-mask openings: allow the mask openings to be larger than the footprint pads. |
| Smaller Pads (Paste) | Paste apertures: allow paste geometry to be smaller than the footprint pads. |
| Auto | Use the matching rule appropriate to the selected layer's type. Check that the PCB matrix assigns the correct type to that layer. |
This pad check validates library candidates. Group 4 instead detects footprint geometry from board layers; the two functions have separate layer selections.
4. Footprint Detection
Enable Search for Footprints to derive footprint candidates from the loaded PCB geometry and associate them with the imported placements. It is available when working with an existing board.
| Priority | How detected geometry is used |
|---|---|
| High Priority | Prefer a detected footprint over an otherwise resolved package. |
| Medium Priority | Keep a uniquely resolved name or alias match; prefer detected geometry when the ordinary match is not unique. |
| Low Priority | Use detected geometry when the other package search has not resolved a usable package. |
These priorities apply to available detected candidates; they do not guarantee detection for every component.
- Top enabled / Bottom enabled: include the corresponding layer inputs. Bottom layers can also be enabled without bottom-side CSV components, for example to provide the bottom mask for through-hole detection.
- Paste: select the solder-paste layer supplying pin pads for surface-mount detection on each required assembly side.
- Mask: select the solder-mask layers supporting geometry checks and through-hole recognition.
- Silkscreen: optionally select the layer containing component outlines to support grouping and body detection.
- Drill: select a suitable drill layer for through-hole technology (THT). Through-hole detection also requires mask layers on both sides.
For top-side detection, choose the top paste layer. For bottom-side CSV components, enable the bottom side and choose its paste layer. When only supplying bottom mask information for through-hole detection, a bottom paste layer is optional. Confirm the actual layer content rather than relying on its name alone.
Package Alias Cache – Management
On Settings, enable Use Package Alias Cache and click Manage Alias Cache in Package Finder. This dialog lets you review and maintain saved assignments between package names from component files and packages in a selected library.

The cache remembers previous package assignments so later imports can reuse them when Use Package Alias Cache is enabled. An entry relates a CSV Package name to a Library Package within a library and can include an angle correction. Review the resulting footprint on the PCB when the source data or library changes.
Find and inspect entries
- Library: selects the library whose cached assignments are displayed. The list contains libraries represented in the cache.
- Search: filters the displayed entries by text in CSV Package, Library Package or Part Name. Clear the field to show the library's full list again.
- Click a column heading to sort the table; click it again to reverse the order.
| Column | Meaning |
|---|---|
| CSV Package | The package name from the component list that the assignment applies to. |
| Library Package | The corresponding footprint name in the selected package library. |
| Part Name | Associated part information, where available. This field can be empty. |
| Angle Correction | The saved rotation correction in degrees for the package assignment. |
| Score | The stored match score used to compare assignments. It is not a percentage or a guarantee of correct geometry. |
| Last Found | The recorded date and time for the entry. This column is read-only. |
Add, edit and delete assignments
- Add opens a form for a new assignment. Enter the required CSV Package, Library Package and Library Name; supply part information, angle correction and score as needed. Confirm with OK or leave the form with Cancel.
- Edit an existing assignment directly in its table cells. The package names, part name, angle correction and score are editable; Last Found is not. Check that the target package exists in the intended library.
- Delete removes the selected row or rows after confirmation. Check the selection before confirming.
- Save Changes explicitly saves the edits.
- Close, or File > Close, closes the dialog and also saves pending changes. Closing is not a discard action.
Tip: If a newly added entry is not visible, select its library and clear Search.
Import and export cache entries
File > Export… writes all cached entries for the selected Library to an XML file. The Search filter does not restrict this export.
File > Import… loads assignments from an XML cache file and merges them with the existing entries. A completion message reports how many entries were added or updated. Review the resulting list and use Save Changes to save it explicitly.
Create Components and Review Packages
After configuring Import Components, use Create Components to place the imported list and open Results for package review. Open this dialog through Import > Assembly > Components (CSV) Import.
Create the components
- Verify Column Mapping, coordinate units, source rotation direction and assembly sides.
- Review the four groups on Settings, especially Create new Job and Remove Existing Components.
- Click Create Components. The imported placements are processed with the selected package-search and footprint-detection options.
- Review Results and the placed geometry in the PCB view. The two board-view buttons beside Create Components switch the view to the top or bottom side.
Successful component creation saves the import settings and the job. Save the job again after subsequent manual package corrections.

Read the result table
The left table groups components by their assigned package and source package name. Use its column filters and horizontal scrollbar to inspect the relevant groups. One source package name can produce several rows if its placements resolve to different footprints.
| Column | Meaning |
|---|---|
| Package Used | The actual assigned package. An unresolved row can have no resolved package name. |
| Package File | The original package name from the input file. It remains the source identifier when a package is reassigned. |
| Status | Creation or correction result, explained below. |
| Count / References | Number and reference designators of the components represented by that row. |
| Pin Count | Pin count of the assigned package. |
| Size X / Size Y | Package body dimensions, independent of placement rotation. Column headers identify mm or mil according to the current PCB unit. |
| Status | Interpretation and next action |
|---|---|
| Created | Components were created with an assigned package. Verify the geometry and pin orientation. |
| Updated | The package was changed after creation. Recheck the affected placements. |
| Missing | No suitable package was resolved; a placeholder can be present. Assign a valid library package or create one from selected pads. |
| Partially Created | Only part of the source package group was resolved. Inspect the remaining problem rows and references. |
| Bad Placing | Some placements in the source group remain unresolved although others were created. Check side, coordinates, package orientation and comparison-layer selection. |
Green rows identify created or updated results; red rows identify unresolved/problem groups. A green row is not a manufacturing approval. Check pin 1, pad alignment, component side and the number of placed components.
Inspect and compare package candidates
- Select a result row. Ranked alternatives, where available, appear in the package browser on the right.
- Use Selected Library: to browse another available library. The selected library is remembered for later openings.
- Select a package to show its footprint preview over the associated components in the PCB view. Compare its pin arrangement, orientation and body size with the board.
- Double-click a result row to select its components in the PCB view and zoom to them. Enable Sync Selection to highlight result rows when selecting components on the board.
BEST identifies the assigned best entry. Other candidates can show a Score; compare the geometry as well as the ranking. A fitted component angle can differ from the file's angle when the package uses a different local orientation. Judge the placed pins and pin numbering together.
Change Package
Use the Edit Package controls to correct the selected result rows.
- Select one or more result rows, then select one package in the library browser.
- If necessary, use the rotation-arrow buttons and direction-arrow buttons to adjust the preview. The numerical field sets the move increment in the displayed PCB unit, mm or mil. Rotation buttons normally adjust by 90 degrees; a component at a 45-degree orientation can use a 45-degree correction.
- Click Change Package to apply the displayed package correction to the components in all selected rows.
- Inspect the updated placements and save the job.
To replace a package for every occurrence of one source footprint, filter Package File for that name and select its matching rows before clicking Change Package. The source name in Package File remains unchanged.
Create Package from Selection
Use this when a suitable library package is unavailable but the PCB contains its pin-pad geometry.
- Select exactly one result row whose components should receive the new package.
- In the PCB view, select all pin pads for one instance of that component. Selecting the layout component alone does not provide the required geometry.
- Optional lines and arcs can describe the body outline. When pads are selected, these outline objects do not become extra pins.
- Click Create Package from Selection. The generated package is added to the job and assigned to every component represented by the selected row.
- Check all affected placements, including pin numbering and orientation. The board selection is cleared after successful creation; make a fresh pad selection for the next package.
If the selected objects contain exactly one distinct non-empty .string attribute text, that text becomes the reference of the target component nearest the selected geometry. Other references in the row remain unchanged. Leading/trailing spaces are ignored, and repeated texts differing only in case count as one text. Missing or conflicting texts leave the reference unchanged.
Undo or Ctrl+Z reverses this complete package-from-selection action in one step, including its rotation and reference changes. It remains available after closing the dialog. A package created by that action is removed if it is no longer used.
Edit Selected and save reusable settings
Edit Selected opens the standard component editor for components selected in the PCB view. Select the actual components before using it.
Save Setup writes the current import configuration to an XML settings file; Load Setup restores a saved configuration. This is separate from saving the PCB job. Recheck library availability, mappings, units and board layers when applying a setup to another design.
Successful Create Components remembers import preferences, including the Used Package Library checkbox and the Package Name Compare selection. Familiar header layouts can restore previous mappings and options. Always verify the active settings before a new import.
Component CSV Import Troubleshooting
Use these checks when importing a component placement list through Import > Assembly > Components (CSV) Import. Correct the input or active settings, then inspect representative placements before accepting the result.
| Symptom | Checks and correction |
|---|---|
| The preview has one large column or unexpected columns. | Check Text Separator, then reload the file. Confirm the correct Excel worksheet or that the TXT file contains a recognizable aligned table. Inspect any irregular-row warning. |
| Too few components were created. | Verify Reference, Pos X and Pos Y assignments. Check that both coordinate fields contain valid numbers. Compare the source list with Count and References in Results and inspect the application error log. |
| Components are displaced or scaled. | Verify the source coordinate unit and the common origin of the placement file and PCB. Compare several positions across the board, not only one component. |
| Components face the wrong direction or appear on the wrong side. | Check CW/CCW, Location/Side and Mirror X. Verify pin 1 and pad numbering against the assigned package; its local orientation may differ from the original export. |
| Create Components is unavailable. | Load a usable component list and select a concrete package-library entry or the available NO Library option. A library-provider heading is not a valid selection. Also confirm that an existing job or Create new Job is available. |
| Layer controls are disabled. | Check whether the relevant function is enabled, whether Create new Job is selected and whether the imported data contains components on that side. Bottom enabled in Footprint Detection can be used to supply the bottom mask for through-hole detection. |
| Footprint detection does not resolve a component. | Check Search for Footprints, enabled sides, actual paste-layer contents and imported position. Use suitable mask/silkscreen inputs where available. Through-hole detection requires a drill layer and mask layers on both sides. |
| A package remains Missing or has a poor fit. | Check its source name, chosen library, Package Name Compare and pad-check layers. Review aliases if a recurring mapping is unsuitable. Inspect alternatives in Results, use Change Package or create a package from selected pads. |
| Create Package from Selection is unavailable. | Select exactly one result row and the pad geometry for one component instance in the PCB view. Selecting a component object alone is insufficient. |
| Change Package or preview adjustment is unavailable. | Select the result row(s) and one package in the library browser. Preview move/rotation controls require an active package entry. |
| Edit Selected is unavailable. | Select components in the PCB view. |
| A remembered import directory is not offered. | The history belongs to the saved design. Confirm that the same design is open and that the previous file's directory is still reachable; otherwise the normal start-directory selection is used. |
Before running Create Components again: Decide whether the previous components should be retained or replaced. Review Remove Existing Components to avoid either unintended duplicates or unintended removal. Save the corrected job after reviewing the result.
Select Layers and Run Footprint Detection
Open Import > Assembly > Component Footprint Detection with the intended PCB job and step loaded. Use Layer Selection to specify the board geometry from which component suggestions should be created. A component placement file is not required.

Choose the assembly sides and input layers
The left input column is for the top side; the right column is for the bottom side. Enable at least one side. Selecting a layer offers the available job layers, using their matrix colours and contrasting text.
| Control | Selection and purpose |
|---|---|
| Top enabled / Bottom enabled | Include the corresponding assembly side. Its Paste, Mask and Silkscreen inputs become available. Disable a side that should not be processed. |
| Paste | Required for each enabled side in this dialog. Choose the solder-paste layer containing the component pin-pad geometry. |
| Mask | Optional for surface-mount detection. Choose the solder-mask openings for the corresponding side. Mask layers on both sides are required for through-hole detection. |
| Silkscreen | Optional. Choose the corresponding silkscreen layer to provide component outlines that help distinguish adjacent footprints and body boundaries. |
| Drill | Select a suitable drill layer to support through-hole technology (THT) detection. This input spans the full width and applies to the board rather than one assembly side. |
For THT detection, enable both sides and provide their Mask layers and a suitable Drill layer. Satisfy the enabled sides' Paste selections before starting the run.
Note: The layer names in the screenshot are example selections, not a layer assignment to copy to every job. Verify the actual layer content and its matrix type, particularly for the Paste inputs. Hover over a control for its tooltip.
Remembered selections
Layer choices and enabled sides are saved when changed. When the dialog is reopened, a saved layer is selected if its name exists in the current job; otherwise an automatic suggestion can be used. Review these selections when switching designs.
Choose None for an optional input that should not be used. This clears its saved layer name; on a later opening, an available automatic suggestion may be selected again. A required Paste input must contain a usable layer.
Run the detection
- Confirm the active PCB step and the selected top/bottom input layers.
- Click Run. The progress dialog identifies the current stage.
- When the run completes, the dialog switches to Results and the created component suggestions can be inspected in the PCB view.
- Review the grouped results and compare representative components with their source pads before saving the job.
Warning: A new run replaces the displayed result list and can replace existing suggestion layers, including components added or corrected there manually. Save a copy of the job before rerunning if those results must be retained.
Cancel, close and retry
Cancel in the progress dialog requests a stop. The current operation may need to finish first. Components already created remain in the job; cancellation does not automatically undo them. An interrupted run is not displayed as a completed result. Inspect the board before retrying.
Close closes the dialog without reverting component creation or package edits. Save the PCB job to retain the changes. Closing or replacing the loaded job also closes this dialog.
If Run does not start, enable at least one side and select its required Paste layer. If the result is empty or incomplete, verify that the selected layers contain the expected pads, outlines and drills, then inspect the detection report in the application error log for skipped inputs or export failures.
Review and Correct Detected Components
After Run in Import > Assembly > Component Footprint Detection, use Results to inspect the created components and correct their package assignments. The dialog stays open while you select objects in the PCB view.

Read the component groups
The left table groups components by Package Used. A row can represent one component or many components sharing that package; check Count and References before changing an entire row.
| Column | Meaning |
|---|---|
| Package Used | The package currently assigned to the components in the row. Generated names identify detected geometry rather than a verified manufacturer part. |
| Package File | The source package-name field shared with the CSV-import results view. It is empty for results created here without a placement-file import. |
| Status | Created identifies generated components. Updated identifies a package assignment made during review. |
| Count | Number of components represented by the group. |
| References | Reference designators of the grouped components, including automatically generated references such as AUTO_178 in the example. |
| Pin Count | Pin count of the assigned package. |
| Size X / Size Y | Package body dimensions, independent of component placement rotation. The column headers identify mm or mil according to the PCB unit. |
Some columns may require horizontal scrolling. Use column filters to narrow the results. Green Created rows confirm component creation; still verify pin count, pin 1, orientation, side and pad alignment. Groups that could not be created are not available as editable result rows; consult the detection report for failures.
Select components and compare packages
- Double-click a result row to select its components in the PCB view and zoom to them.
- Enable Sync Selection to highlight the corresponding result row when selecting a component on the board.
- Use Selected Library: on the right to choose a package library. The chosen library is remembered for later openings.
- Select a package entry to display its preview over the components in the selected result row(s). Compare its pad arrangement, pin numbering and body dimensions with the actual PCB geometry.
The browser shows package names and available details such as Score, Pin Count and dimensions. BEST, where shown in the alternative list, identifies the assigned best entry. The screenshot illustrates an automatically generated package selected for review.
Correct a library package with Edit Package
| Control | Action |
|---|---|
| Rotation-arrow buttons | Rotate the preview before assignment. The normal increment is 90 degrees; components already at a 45-degree orientation can use a 45-degree correction. |
| Direction-arrow buttons | Move the preview left, right, up or down by the distance in the numerical field. |
| Distance field | Set the move increment. The displayed unit follows the PCB unit: mm for metric or mil for imperial. The initial increment is 0.1 mm or 10 mil, respectively. |
| Change Package | Apply the selected library package and preview corrections to the components in all selected result rows. Check the scope of the selection before clicking. |
| Create Package from Selection | Build a package from selected board pads and assign it to exactly one selected result group. See the before/after correction example. |
| Edit Selected | Open the standard component editor for components selected in the PCB view. Selecting only a result row is not a substitute for selecting the intended board components. |
To replace a detected package, select the target row(s), select one library package, adjust the preview if necessary and click Change Package. Check all affected placements and save the job. A fitted package can have a different local orientation, so inspect the final pins together with the package rather than comparing the component angle alone.
The shared package-browser controls are also described in Create Components and Review Packages.
Add a component that detection missed
Add Component from Selection creates an additional component without another full detection run. It is also available before the first run and does not require a selected result row.
- Switch the PCB view to the intended top or bottom side.
- Select all pin pads for exactly one component. Optional outline geometry may also be included. Selecting a component object alone does not provide the package geometry.
- Click Add Component from Selection. The button is available when suitable geometry is selected and no run is active.
- Inspect the new component, which is selected in the PCB view and added to its package group in Results. Save the job after review.
The new component is created on the current view side's suggestion layer. A matching existing job package can be reused; otherwise a package is created from the selected geometry. Other result rows remain available, and the pad selection is cleared after successful creation.
If selected objects carry one distinct non-empty .string attribute text and that reference is unused in the step, it becomes the new component's reference. Otherwise a free reference is generated automatically. Leading/trailing spaces are ignored and texts differing only in case count as the same text. A later Run can replace these manually added suggestions.
Unavailable actions and saving
- Change Package requires selected result row(s) and one selected package in the library browser.
- Preview move/rotation controls require an active package entry.
- Create Package from Selection requires exactly one result row and selected pad geometry in the PCB view.
- Edit Selected requires components selected on the board.
- Add Component from Selection requires selected geometry and is unavailable during a run.
Component creation and corrections affect the current job immediately. Use the normal PCB-Investigator save command to retain them; Close does not undo the changes.
Create Package from Selection: Before and After
Use Create Package from Selection in the Results tab of Component Footprint Detection when the detected grouping or assigned package does not represent all pads of the intended component. Open the dialog through Import > Assembly > Component Footprint Detection.
Prepare the target and pad selection
- Select exactly one result row whose components should receive the corrected package. Check its Count and References: the operation changes every component represented by that row.
- In the PCB view, select all pin pads for one complete instance of the intended component. Include only the pads belonging to that instance.
- Optionally include outline geometry. When pads are present, selected lines and arcs contribute to the package outline rather than becoming additional pins.
- Click Create Package from Selection in Edit Package. Selecting a layout component alone is insufficient; the actual pad geometry must be selected.
- Verify the resulting pin count, pad positions, body outline and pin numbering on every affected placement. Confirm the result before saving the job.
This action replaces the selected group's package assignment. Use Add Component from Selection instead when an additional component must be created without changing an existing result group.
Before and after the button click

Read this image from bottom to top. The blue arrow points from the state before the button click to the state afterwards.
- Before — lower panel: the board geometry is selected and the Create Package from Selection button is outlined in blue. The existing component is labelled
AUTO_184and its displayed package has two numbered pins, although the selected geometry contains the six pads of the intended component. - After — upper panel: a six-pin package covers the intended pad arrangement and the displayed reference is
J2. The numbered pins and outline can now be checked against the board. The geometry selection has been cleared, so the button is no longer enabled until another suitable selection is made.
The package is created in the current job and assigned to all components in the selected result row. The row changes to Updated and its package details are refreshed. No full detection rerun is required.
Reference text, repeat use and Undo
The reference change shown in the example depends on the selected objects' attributes. If the selection contains one distinct non-empty .string attribute text, that text can become the reference of the target component nearest the selected geometry. It is used only if no other component in the step already has that reference. Other references in the group remain unchanged.
Leading/trailing spaces are ignored and repeated texts differing only in case count as one text. Missing, conflicting or already-used reference texts leave the existing reference unchanged; the package can still be corrected.
Make a fresh pad selection for each subsequent correction. Use Undo or Ctrl+Z to reverse the package-from-selection operation in one step, including its package assignment, rotation and reference changes. This action remains available after closing the dialog. A package newly created by the action is removed when it is no longer used. Save the PCB job after accepting the correction.
Layers & Stackup
Open Signal Integrity Analysis → Layers & Stackup to review the physical build-up used by the analysis. Layer thickness and dielectric properties define the separation and electrical environment of your traces.
1. Default settings and project controls
Default settings… opens the starting values for new SI projects. The separate Save Settings button saves the current project configuration without starting a simulation. Result viewer… opens previously saved runs. These controls remain available outside the workflow pages.
When a design already contains an SI project, opening the analysis restores that project's values. A new project starts from the design's layer data and the configured defaults for missing values.
2. Review and edit the layer stack
The table follows the PCB layer order. Take over from PCB imports the current design stack into the SI configuration. Use it deliberately when you want to replace the SI stack values with the current PCB values; it is not the action for simply saving your edits.
| Column | Meaning and action |
|---|---|
| PCB layer | The original layer name, used to relate the analysis to the PCB. |
| Model layer | The corresponding layer in the simulation stack. |
| Material type | Copper or dielectric material category. |
| Foil / dielectric | Base copper-foil thickness or dielectric thickness, in the unit shown. |
| Plating | Additional copper thickness for a copper layer. |
| Total | The resulting layer thickness, including the configured copper contributions. |
| εr | Relative permittivity of a dielectric layer; use the value for the actual material. |
| tanδ | Dielectric loss tangent. A deliberate zero represents a lossless dielectric in the configured model. |
Edit the required values directly in the table. The table distinguishes foil, plating and total thickness so the combined copper height remains clear. A thickness that differs from the design is subtly highlighted; its cell information identifies the design value. Row heights are fixed.
Check layers checks the sequence and whether the required thicknesses and dielectric properties are present and in a usable range. In particular, review the dielectric separation between copper layers. The check is based on the layers supplied by the design: confirm the complete core/prepreg build-up against your board stackup information.
3. Material starting values and copper properties
Starting material values provides permittivity and loss-tangent values for new layers. The values already shown in the stack table are the values used for those layers; changing a starting value does not replace the existing table entries.
Under Copper model · PEC approximation, copper is treated as ideally conducting. Conductivity is a starting-value field and does not introduce resistive copper loss into this model.
Via wall is the thickness of the metallized wall of a plated hole. It is not the finished bore diameter or the pad diameter. Use the fabrication value for the board. The simulation also needs the actual start and end copper layers and the finished hole size.
For round plated vias, the cell size must resolve at least two cells through the wall and four across the bore. As an example, a 25 µm wall calls for a cell width no greater than 12.5 µm. This can determine the grid even if the trace itself is much wider.
4. Layer preview
The lower preview shows the configured layer sequence and thickness labels. The shapes are schematic rather than a manufacturing cross-section to scale. Use the table values to read the dimensions, and scroll the preview when the stack contains many layers.
Save the configuration
SI edits are stored in the job's user/SiAnalysisSettings.xml. They do not write material values or thicknesses back into the PCB matrix. Use Save Settings at any point, then save the PCB job normally to retain the associated job files.
Lengths follow the PCB-Investigator unit setting. The example uses metric dimensions; always read the unit on your own field before entering a value.
For the associated setup, see preparation and physical-port requirements.
Default Settings
Choose Default settings… at the top of the SI Analysis dialog to define consistent starting values for future projects. Use this dialog for your usual working values, and edit the actual board and connection values in each SI project.
What the defaults affect
The dialog applies to new SI projects only. Saving defaults does not overwrite the stackup, targets, models or simulation settings of an existing project. Project values are saved separately with Save Settings.
| Group | Starting values provided | How to use them |
|---|---|---|
| Material defaults | Relative permittivity, loss tangent and copper conductivity. | Provide usual initial material values; replace them with board-specific values in the layer table where required. |
| Quick Check targets and limits | Impedance target, impedance tolerance, reflection limit, skew limit and eye-height limit. | Choose the starting assessment criteria for new projects. Use the actual connection requirements in each project. |
| Signal and channel preview | Pattern, data rate, amplitude, rise/fall times, source/load resistance and step duration. | Set the initial stimulus and equivalent-line preview parameters. Voltage is in V, resistance in Ω and time in ps. |
| Ports and IBIS models | New-port reference impedance and related model starting values. | Set how newly created ports begin. An existing port retains its project-specific impedance and model. |
| Mesh, frequency and vias | Cell and frequency settings, via wall and calculation-area starting values. | Provide an initial simulation setup, then adapt it to the board's smallest relevant structures and frequency range. |
| Compute device and cell limit | Initial calculation device and cell-count limit. | Choose a practical starting resource configuration for your workstation. |
The category headings are not editable values. Scroll the table to reach the lower groups. An impedance target, a port reference impedance and a driver output resistance are different parameters, even when all three happen to use the same numerical value.
Manage generic model templates
Generic model templates… opens the global library shared with the Generic values… dialog on Ports & Models. A template stores its name, pin role and electrical values together. Loading one into a pin creates that pin's own project copy; later changes to the global template do not update those copies.
Save or cancel
Save defaults stores the values in si_analyse_settings.xml in PCB-Investigator's AppData PlugIns area. Cancel closes the dialog without applying the edited default values.
Template saves and deletions have their own immediate effect in the global library. Closing a pin-model dialog with Cancel does not undo a template operation you already confirmed.
Tip: On Quick Check, Reset to defaults explicitly copies the current saved defaults into that project's Quick Check fields. Use it when you want to reset those fields, rather than expecting a global default change to alter an existing project automatically.
For the associated setup, see project-specific layer settings.
Nets and Reference Nets
Open Signal Integrity Analysis → Nets to choose the connections to investigate and the reference conductors available to their physical ports. The signal list is loaded automatically from the current PCB design.
1. Select active nets in the signal table
| Column | How to use it |
|---|---|
| Active | Check a row to include that net or pair in the analysis. Checked rows have a light-blue background across the row. |
| NetName | Find the actual net name or a formed pair. |
| Pins | Inspect the connected PCB pins, for example R70-2 and J5-15. These come from the layout, before detailed port modelling. |
| Type | Use name-based hints such as Differential, HighSpeed, Clock or Other to locate candidates. A hint does not assign a driver, bit rate or electrical model. |
Type in the filter row below a column heading, or use its filter button. Combine filters to search by net, component pin, type or checked state. Use Remove Filter in the context menu to clear them.
A highlighted row and a checked Active box have different purposes. Highlighting selects a row for an action; the checkbox selects a calculation case. To change several rows, select them with Ctrl/Shift and click a checkbox, or use Space. Filtering does not deactivate hidden checked rows.
Active nets are highlighted in the PCB view without changing their stored object colors. The highlight follows the visible layers. More actions provides actions for clearing checked nets, highlighting in the PCB and resetting PCB colors; clearing the checks does not delete nets from the board.
2. Use the PCB selection
Use PCB selection replaces the active checks with the nets represented by the PCB elements currently selected. A single selected pad or trace element selects its entire net, not just that section of copper. The action also clears the column filters so the resulting selection can be seen.
This is an explicit transfer. Later selection changes in the PCB do not automatically replace the SI checks. With no PCB elements selected, using this action clears the active checks.
3. Find an additional reference net
Type part of the actual net name under Search PCB nets. The candidate list filters immediately. Select the intended result and press Enter, double-click it or use Add selected (Enter).
Typing a name alone does not add it. Only nets that exist in the current design can be selected.
4. Maintain the selected references
Selected reference nets is the approved list of conductors used as references in the SI project. For a new project, names containing gnd or ground are preselected without regard to case. Review this initial list against the circuit; AGND, PGND and GND may have different functions.
Add each required reference from the search list. Select one or more entries and use Remove selected or Delete to remove them. The list is saved with the SI project.
The list makes a conductor available to the model. It does not assign the physical reference of every port. Each port also needs its own Reference layer and Reference net, with real copper at the contact position. New ports use the nearest unambiguous suitable reference where one can be identified.
5. Detect differential pairs
Detect pairs identifies unambiguous matching net names. Check that the two nets really form the intended differential connection and that their positive and negative sides are correctly assigned.
6. Form a pair manually
Use Form pair when you want to combine the intended positive and negative nets explicitly. A pair is one calculation case containing both conductors. Two separately checked single nets remain two separate cases, and their Quick Check rows do not acquire a shared skew value simply from similar names.
For a four-port differential broadband connection, confirm the physical order: P1 input +, P2 input −, P3 output +, P4 output −. The names alone do not establish which endpoints belong together.
Continue with the selected cases
The active selection stays synchronized with Quick Check and Ports & Models. Selecting a case in a later preview only changes the case displayed or edited; it does not uncheck the other active cases.
For the associated setup, see physical reference-conductor requirements.




