Posts tagged with 'Analysis'

Rule File Manager

With the help of the "Rule File Manager" different rule sets can be created and managed.

DRC Rule File Manager

New:
Create a new rule set with a user defined name.
Save:
Save changes in the currently selected rule set.
Delete:
Delete the currently selected rule set.
Import:
Import a new rule set out of a xml file.
Export:
Export the current rule set to a xml file.
Tolerance:
Tolerance for all check values. All check values will be reduced by e.g. 1% to not show false errors (e.g. when checking for 150µm spacing, a distance of 49.9 µm can be ignored in this way).
Unit Converter:
Small tool to convert numbers between µm and mils.
Compare:
Opens a new window where two rules can be compared in a table view.

 

Single check rules:

 

        • Outer Signal Rules
          DRC Minimum Spacing Minimum spacing between copper areas of same or different nets on outer layers
          DRC Minimum Trace Minimum copper trace width on outer layers
          DRC Acute Angle Minimum angle in copper areas on outer layers
          DRC Missing Thermal Pad If active, all SMD pads with soldermask opening and component pin are reported, if they are located completely inside a copper area (no thermal reliefs)
          Ignore Thermal Pads Do not report missing thermal pads, which are located completely under a component body and have a size larger as this value (e.g. cooling pads)
          DRC Mask Clearance SMD Minimum needed solder mask clearance arround SMD pads (.smd Attribute)
          DRC Mask Clearance Testpoint Minimum needed solder mask clearance arround test point pads (.test_point Attribute)
        • Inner Signal Rules
          DRC Minimum Spacing Minimum spacing between copper areas of same or different nets on inner layers
          DRC Minimum Trace Minimum copper trace width on inner layers
          DRC Acute Angle Minimum angle in copper areas on inner layers
        • Solder Mask Rules
          DRC Distance to Copper Minimum distance from the solder mask opening to surrounding copper
          DRC Minimum Space Minimum spacing between solder mask clearances (=smallest solder resist fillet)
          DRC Minimum Trace Minimum width of solder mask clearances
          DRC Minimum Angle Minimum angle in solder mask clearances
        • Silkscreen Rules
          DRC Minimum Mask Distance Minimum distance to any solder mask opening
          DRC Minimum Component Distance Minimum distance to any component
          DRC text primitives Check only text primitives (.nomenclature attribute) for a minimum distance to components, or all primitives
          DRC Minimum Space Minimum spacing between silkscreen printings
          DRC Minimum Size Minimum size of silkscreen primitives
          DRC Minimum Angle Minimum angle in silk screen printing
        • PTH Rules
          DRC Mask Clearance PTH Minimum needed solder mask clearance for plated through holes
          DRC Mask Clearance PTH Pads Minimum needed solder mask clearance for plated through hole copper pads
          DRC Masks smaller as PTH Pad If active, mask clearances which are smaller than the PTH-Pad are not reported
          DRC Annular Ring outer Layers Minimum annular ring for the drill on outer signal layers
          DRC Annular Ring Inner Layers Minimum annular ring for the drill on inner signal layers
          DRC Missing Pads Inner Layers If active, missing copper pads on inner signal layers will not be reported
          DRC Distance to Copper Minimum distance to surrounding copper on inner layers, if missing pads are accepted
          DRC Missing Thermal Pads THT If active, all THT copper pads are reported, if they are located completely inside a copper area (no thermal reliefs)
          DRC Minimum Diameter Minimum diameter of plated through holes
          DRC Minimum Drill Distance Minimum Distance to any other Drill
        • NPTH Rules
          DRC Mask Clearance NPTH Minimum needed solder mask clearance for unplated through holes
          DRC Distance to Copper Outer Layers Minimum distance to surrounding copper on outer signal layers
          DRC Distance to Copper Inner Layers Minimum distance to surrounding copper on inner signal layers
          DRC Minimum Diameter Minimum diameter of unplated through holes
          DRC Minimum Drill Distance Minimum Distance to any other Drill
        • MicroVia Rules
          DRC Mask Clearance VIA Minimum needed solder mask clearance for laser drills
          DRC Missing Mask If active, missing solder mask openings for laser drills will not be reported
          DRC Annular Ring Minimum annular ring for the laser drill on all affected signal layers
          DRC Minimum Diameter Minimum diameter of laser drills
          DRC Minimum Drill Distance Minimum Distance to any other Drill
        • Buried Drill Rules
          DRC Annular Ring Outer Layers Minimum annular ring for the drill on outer signal layers
          DRC Annular Ring Inner Layers Minimum annular ring for the drill on inner signal layers
          DRC Missing Pads Inner Layers If active, missing copper pads on inner signal layers will not be reported
          DRC Distance to Copper Minimum distance to surrounding copper on inner layers, if missing pads are accepted
          DRC Minimum Diameter Minimum diameter of plated through holes
          DRC Minimum Drill Distance Minimum distance to any other Drill
        • Copper Foil Rules
          Foil Thickness Maximum Foil thickness for this rule
          Minimum Space Outers Minimum spacing between copper areas of same or different nets on outer layers with this foil
          Minimum Trace Outer Minimum copper trace width on outer layers with this foil
          Minimum Space Inner Minimum spacing between copper areas of same or different nets on inner layers with this foil
          Minimum Trace Inner Minimum copper trace width on inner layers with this foil

Result Explanations

The result explanations help you to easily interpret the check results reported by PCB-Investigator`s Design Rule Check.

There is a focus on illustrating the technical background as well as on giving a understanding of the unavoidable tolerances during the PCB manufacturing process.

  • Bottlenecks and spacing
    DRC_results_bottlenecks_and_spacing

    Small distances in copper, as well as thin copper areas might not be producible due to physical etching restrictions.

    A chosen technology e.g. IPC Class II should be applied everywhere on the board, as only a single violation forces the PCB supplier to switch to finer production parameters (e.g. IPC Class I) for the whole board.

    The finer the structures, the more expensive the board will be.

  • Solder resist webs and spacing
    DRC_results_solder_resist_webs_spacing

    Solder resist webs with a width of less than app. 70µm are hardly producible with standard technology.

    There is always the risk, that those small pieces will detach and adhere somewhere else, which can lead to solder problems and failures.

    Smaller distances and webs might only be producible with an expensive special solder resists and less resist height, which influences the isolation quality.

    To avoid unnecessary costs, PCB-Investigator reports all those violations.

  • Coverages and exposures
    DRC_results_coverages_and_exposures_CAD CAD data
    DRC_results_coverages_exposures With allowed displacement

    As there will always be a slight displacement between the solder resist and the conductive pattern, surrounding copper should have a minimum distance of the allowed displacement from the solder resist opening. If not, there is the risk that the surrounding copper will also be exposed, which can lead to electric shorts by e.g. solder bridges.

    The allowed displacement is app. 75µm, also 50µm is possible, but more expensive.

  • Soldering and testing
    DRC_results_soldering_testing_CAD CAD data
    DRC_results_soldering_testing With allowed displacement

    The displacement can also have negative impact on the solderability of SMD pads or testability of test points.

    To ensure further processability, there should be a solder resist opening with an oversize of the maximum allowed displacement (e.g. 75µm) for all SMD pads and test points.

    So, the copper will always be completely solderable/testable.

  • Drilling and cleanliness
    DRC_results_drilling_cleanliness_wrong_mask

    Each drill should have a solder resist opening, which ensures that the drill is free of solder resist despite the combined displacement of the solder resist and of the drill itself.

    A partly covered drill or solder resist in the drill sleeve can detach and adhere somewhere else during the cleaning process. This can lead to solder problems and failures and contaminates the chemical baths of the PCB supplier. It also effects the EMC behavior.

    DRC_results_drilling_cleanliness_missing_mask

    A completely covered drill without any solder resist opening on one side can´t be cleaned and therefore contaminates the chemical baths.

    If covered on both sides, the enclosed air in the drill could break the solder resist cover when expanding due to heat. The result is unwanted dirt on the board.

  • Drill size and distance
    DRC_results_drill_size_and_distance

    The drill diameter and the drill distance are very important factors for the price calculation.

    Very thin drills have a short life period and must often be replaced. They are also less long, which forces the PCB supplier to drill only 1-2 panels at the same time instead of drilling e.g. 5 panels in a package.

    Small distances between two drills increase the risk the drill is breaking or the two holes are merging to one undefined shape.

    Two holes at the same location can also lead to broken drills or an undefined hole shape.

  • Copper connection
    DRC_results_copper_connection

    To achieve a clearly defined connection between layers, the copper pads for the single drills must be large enough, so that a drill displaced within the allowed tolerances is still located completely within the pad.

    If not, this can have a strong impact on the EMC behavior and lead to failures due to a loose or broken contact.

    Small annular rings and therefore narrow tolerances in the drilling process might still be producible, but force the PCB supplier to use high-end drilling machines and to drill only one Panel at the same time instead of e.g. 5 panels in a package. This has a very strong influence on the PCB costs.

  • Distance to surrounding copper
    DRC_results_distance_surrounding_copper

    In this case we must differ between plated and un-plated drills.

    For plated drills, the distance to surrounding copper is important on inner layers, when the copper pad is omitted. Due to the production tolerances, the displacement of the drill could lead to broken connections or shorts, if surrounding copper is too close.

    DRC_results_distance_surrounding_copper

    For unplated drills, the distance is needed for tenting the hole during the plating process to avoid copper in the hole. When the un-plated drill could not be securely tented, a second drill process after the plating process is needed instead. This raises the costs enormously.

  •  Missing Thermal Pads

  

Thermal pads are soldering surfaces of electronic components that are only connected to larger copper surfaces with thin webs.
This cross-sectional reduction prevents the heat from escaping via the copper surface electrically connected to the soldering pads when heating at specific points, as in the case of hand soldering, and thus impairs the soldering process. If the PCB is heated over a large area, for example in machine soldering where the entire PCB is heated uniformly, no thermal pads are necessary, but they do not normally interfere.
 

Summary

Performing the Design Rule Check (DRC) of PCB-Investigator is the first step to avoid unneeded costs and to increase the reliability of your PCB.

Although in some cases the standard rules must be violated to fulfill some requirements (e.g. Space requirements), there is always a potential to save money and increase the reliability with a few minor layout changes.

AOI Analysis 2D

By using the 'AOI check' button the following window appears:

 

 

    Open a PCB design first and then start the ‚AOI check‘.
  1. First you have to decide, if you want to analyze your design with a 2D or 3D inspection. However, the following section deals only with 2D inspection. If you need information about the 3D inspection, use the 3D AOI description.
  2. Enter the angle of your future automated optical inspection for the camera angle. Tolerances can be calculated using’ additional distance’. By default, this value is set to 0.00. As 2-pin components often aren´t relevant or, due to their shape, difficult to analyze , they can be excluded here. Occasionally components with very large pins are used. These pins often do not need to be checked due to their size. For this reason, enter an area in the’ Value of an area to hide huge pins’ input field that meets your requirements. You can also select the two options’ Create an aoi check layer’ and’ Color pins’. If you want an additional layer, on which the direction of inspection per pin is marked, activate ’Create an aoi check layer’.With the use of the ’Color pins’ option, the pins in the diagram displayed in color are also colored in the design.
  3. After you have adapted all values to your requirements, you can start the inspection.
  4. The inspected components and their pins are now displayed and can be sorted using the riders. The result list contains one line per pin. It contains the following information:
    • ID: Identification Number
    • Layer: Contains on which side the pin can be found
    • Component: Component name
    • Pin: Pin number
    • Shadow Component: Component that is too close to the pin
    • Distance: Shows the calculated distance
    • Checkdistance: Shows the required distance
    • Shadowcomp. Height: Shadow component height
  5. The diagram illustrates the result of the inspection.
  6. The inspection can now be saved using the ’Export Result’ option. When using the import result, an old inspection result can be loaded.
  7. If you move the mouse over the ’Help’ icon, the following picture will be displayed to explain how 2D inspection works.
  8. Ignore components: At this point you have the option exclude components that are not relevant for the later AOI analysis. Depending on your design, you can do this by using the properties, the package name or by individually selecting the components in the tool itself.

 

 

Example:

Doubleclick an entry shows the component J1 and the corresponding pin 8 (red colored) with too small distance to the component LDR after the 2D inspection.
aoi_2d_list_entry_on_board

AOI Analysis 3D

By using the 'AOI check' button and switching to 3D AOI the following window appears:

Open a PCB design start, then the ‚AOI‘.

  1. First you have to decide,if you want to analyze your design with a 2D or 3D inspection. However, the following section deals only with 3D inspection. If you need information about the 2D inspection, use the 2D AOI description.
  2. First replace the’ laser angle’ arranged between the laser and the camera with its actual laser angle. Since the direction the laser head moves in differs during the 3D inspection, it can also be adjusted with ’horizontal’ and ’vertical’. The colouring of the affected components can be selected as required. It is also possible to graphically display the overlapping of the shadow with other components in separate layers using the’ create shadow layers’ option. So the layers show the shadow of a component in both test directions and are shown as follows.

 

aoi_3d_additional_layer

3. After you have adapted all values and selection options to your requirements, you can start the inspection

4. The inspected components and their pins are now displayed and can be sorted using the riders. The result list contains one line per pin. It contains the following information:

    • ID: Identification Number
    • Layer: Contains on which side the pin can be found
    • Component: Component name
    • Shadow on: Identifier whether the shadow falls on a component body or the corresponding pin
    • Package: Package name
    • Shadow Components: Shows the component names of the components affected by the shadow

5. The diagram illustrates the result of the inspection.

6. The inspection can now be saved using the ’Export Result’ option. When using the import result, a past inspection result can be loaded.

7. If you move the mouse over the ’Help’ icon, the following picture will be displayed to explain how 2D inspection works.

8. Ignore components: At this point you have the option exclude components that are not relevant for the later AOI analysis. Depending on your design, you can do this by using the properties, the package name or by individually selecting the components in the tool itself.

Example:
Doubleclick an entry shows the component J1 and the corresponding pin 8 (red colored) with too small distance to the component LDR after the 2D inspection.
aoi_3d_list_entry_on_board

Hazard Analysis

In addition to the distance calculation, an area calculation following the risk assessement tool of ZVEI is also supported.

Settings

Important type of test (Calculate Distance):

Examining, it is necessary to distinguish, which areas should be examined together.  The two types of simulating shown here differ mainly in the speed of test and their accuracy (number of results found).

1. Choosing "Exposed Copper", the non-lacquered (omitted), conductive copper pads and copper lines are compared directly to each other. This type of simulation takes a bit longer, but produces significantly more precise results (thin white line).

2. Choosing "Solder Mask Opening", it isn´t the direct copper pads or copper lines that are used for comparison, but the so called solder mask openings, i.e. the surfaces not being covered with varnish. However, these are slightly larger than the copper areas they release (thick white line).

Particle:

The length of the assumed contamination can be parameterized here.

Ignore Options:

1. If the contamination is located between elements of the same net, you can select whether the entries should be ignored or not.

 2. If you select the option "underneath component", results of possible short circuits being completely under components will be hidden.

3. If the option "same component" is activated, possible short circuits between pins of the same component will be hidden.

 4. If nets are connected by contamination and at least one of the nets is a not-used "$NONE$" net, the results can be hidden as well.

5. You can also ignore areas with coating (Top oder Bot side). The coating prevents the occurrence of short circuits. Therefore these areas are not relevant for the analysis.

Filter options:

 

Filter:

If you want to look closer at a certain component or net, you can filter by using the two drop down menus. In this case, the list is filtered to only show the selected net or component (either in the 'from' or the 'to' column).

Example Area Calculation:

 

 

Introduction

The plugin DFM Analysis can be found under the grid "Analysis" respectively "Assembly". If you click on "DFM Analysis", the following window opens.

In the upper left corner you can see the STEP (1).

Below, you will find three options (2) available for performing the DFM analysis: "Selective Soldering", "Fiducial Solder Mark" (AOI verification), "Panel Dimensions" (technical verification of panels).

Selective Soldering

To begin with, the first topic is "Selective Soldering". This checks whether the set THT components will fit at the given location or whether the pins or holes of the THT component may be too close to components on the opposite side. The THT components you want to check can be selected either by the property or by the package name. It is also possible to directly select the THT components (3).

Before you can start the "Connector Analysis" (4), you have to define the settings for the analysis. There is a distinction between "Single Pad" (5), "Multi Pad" (6) and "Multi Pad Row" (7). For each case, you can individually define the settings that will be used for the analysis. The pictures are intended to illustrate these variables. Each variable is determined by two different values, the "favorite" or optimum value and the "acceptable" value up to which manufacturability (according to your specifications) is still guaranteed.

The results of the analysis are then displayed in the table on the right-hand side of the window (8). Right-click to export them in HTML format. You can also use the tool to display the result. Components in the yellow area are located in the range you have defined as still acceptable. If a component is within the red area, the producibility with the current design is not guaranteed or the specifications defined by you are not fulfilled.

The following functionalities are equally integrated in all three options ("Selective Soldering", "Fiducial Solder Mark", "Panel Dimensions"):

It is possible to exclude components from the analysis (9). You can do this either via "Pin Count", "Height" or "Property". Furthermore, a search function via "List" is available, which lists all excluded parts in an overview. Finally, you can export the previously defined settings so that you can reuse them for later analyses. Already saved settings can be imported via the "Import Settings" button (10)

Clicking on the question mark (11), the corresponding page of our online manual will open.

 

Fiducial Solder Mark

The "Fiducial Solder Mark" option allows you to check whether the markers set for the AOI analysis can be implemented according to the selected specifications.

To do this, you must first search for the fiducials in your design (1). Four options, "Pad Usage", "Pad Geometry Name", "Package Name" and direct selection via the tool are provided for this purpose.

You can also check the current fiducials for their manufacturability (2). The different parameters are illustrated in an illustration: CU corresponds to "Copper Diameter", SM to "SolderMask Diameter" and CMP Free to "Component Clearance Diameter". The check is then performed using these settings. Again, the results are displayed in the table on the right (3) or can be viewed directly via the tool.

Panel Dimensions

The "Panel Dimensions" option allows you to check whether your panel meets the specified measurements. In order to be able to start the analysis for the "Panel Dimensions", you must first switch to "panel" in the tool.

 

The settings for the analysis can be defined under "Panel Size" (1). You can also set the "Minimum Distance" between components and the edge of the panel (2). At the same time, you have to choose an optimal value ("favorite") and a boundary value ("acceptable"). If the acceptable value is not reached, the producibility of the panel is endangered. Furthermore, you can decide, which edge of the board should be checked ("check sides").

The results of the analysis are displayed in the window on the right (3). You can also view the analysis results directly in the tool. Problematic components are marked in blue.