Creepage Analysis can be found in the "Analysis" tab. The following picture shows the main view after clicking the "Creepage Analysis" button. As you can see, there are three different tabs.

1. Net to Net
2. Net Group to Net Group
3. To Outline

1. Net to Net creepage analysis is used to detect creepage issues between two single nets.
2. Net Group to Net Group creepage analysis has to be used to detect issues between any net of the first group to any net of the second group (Note: You have to create Net Groups first. To create Net Groups use the button of the following image. Creating net groups can be found in "Net Groups", shown below)
3. There is also an option to detect issues between a single net, or any net of a group to the board outline of the PCB

On top of the "Net to Net" view, you can find two drop down menus to select two nets, which have to be analysed. The buttons on the right side of the drop down menu may be used to automatically fill the drop down menu with corresponding nets you are currently selecting on the board design.

If you are using the button in the "Net Group to Net Group" tab, the button click will set the net group name (the net has to be included in a net group).

The options "outer/inner distance" and "Allow creepage flow via the board outline/ routings" (below) are the most important ones.

Allow creepage flow via the board outline/ routings

This option allows the calculation to consider the board outline and routings. So using this option, it allows to check inter layer distances as well.

NOTE: This option is the main difference to the "Net Groups" calculation, where only distances between nets for each layer separately are calculated.

Outer Distance & Inner Distance (max values)

To decide the proper distance, you have to consider the important parameters for the calculation. 

These parameters are:

• Voltage of the net
• Material Group
• Pollution degree

To connect these parameters there are several tables in the internet. The following image shows an example table.

Using tables like this, it is much easier to decide the proper distances for your cases.

For example:

Known

• The net has max. 400V.

Assumption

• Pollution degree = 1 on the inner layer
• Pollution degree = 3 material group II on the outer layers

With these three parameters, it is easy to get the "Inner Distance" of 1.0 mm and the "Outer Distance" of 5.6 mm.

As shown in the picture above, the corresponding DIN Standard in this example is DIN EN 60664-1.

At the bottom of the main view image there are further options.

Outline Calculation Precision

If a creepage flow is possible using the board outline, it has to be calculated in small iterations. A line or arc could be mathematically described in nearly infinite points connected by small lines. We have to limit the amount of points, so that the calculation for the shortest way can be finished within an acceptable time. In order to determine the amount of points (granularity), there are the parameters "Tolerance Lines" and "Tolerance Arc", after which distance lines and arcs are to be divided into points. The figure below illustrates this procedure.

Maximum creepage flow steps

The "maximum creepage flow steps" option allows you to influence the calculation directly. This number defines the number of steps the creepage flow is allowed to do.

For example:

You want to measure between Net/Group A and Net/Group B with a minimum acceptable distance of 5.00 mm.
With e.g. 2 allowed creepage flow steps, you allow the creepage current to go from the Net/Group A to the Net/Group B via an independent Net/Group C.
The flow distance inside the Net/Group C is not counting to the total distance, as the Net/Group C is a conducting surface. In this way, the creepage distance might be reduced compared to the direct distance between Net/Group A and Net/Group B.

So, you allow the calculation to make the creepage flow look like this:

Moves from    a Net of Group A    over   a Net of Group C    to    a Net of Group B

In this example the creepage distance between Group A and Group B is reduced from 5mm to 4mm when going over Group C elements!

Result

The image below shows a possible result of the calculation.

The following is a detailed analysis of the red marked entries. These two entries are calculated with the "Maximum creepage flow steps" of 2.

1. The first attribute of the entries shows the calculated distance. In this case it´s 3.823 mm.
2. As explained above, the calculation was done with a maximum creepage flow step count of two. The second parameter shows you the distance the creepage flow has to travel on the outer layer, combined with the percentage of this distance to the distance under test.
3. The third parameter is identical to the second parameter. The only difference is that they handle different layers. The third parameter refers only to the inner layer.
4. If the creepage flow used the PCB edge to move further, it will be shown in parameter four. Parameter four has an identical structure as the second and third parameter.
5. Parameter five visualizes the total percentage of the covered distance (this is a combined percentage of the allowed distances on outer and inner layers).
6. The following parameters are the "Net Names" and the "Layer". They will contain every net name of each net the creepage flow has used. The "Layer" parameter shows you the start layer of the creepage flow and the end.

(The following description shows just the difference to the "Net to Net" tab)

The difference of the drop down menus lies in the fact that nets are replaced by net groups. 

If the "Net Group" drop down menu in the "Net Group to Net Group" tab is disabled, there is no net group to use. So, you have to create net groups first. This can be done in the "Net Groups" dialog.

Rules

1. The first button allows you to import an external ruleset file.
2. With the second button, it is possible to choose or create a ruleset, if there is no ruleset deposited. The dialog which is going to open was also used in the "Net Group Wizard" (-> Tool -> Analyze -> Edit Rules). Information about how to create a ruleset can be found in the "Net Group Wizard" manual.
3. The third button is doing almost the same as the calculate button below. The difference is that the third button is completely ignoring the chosen net groups above, using every net group and checking to all other net groups with the given rules.

Important: If a ruleset is set, the current "Inner/ Outer Distances" shown on the view will be ignored, if distances are set in the rules themselves.

To generate net groups see here

(The following description shows the difference to the "Net to Net" tab)

"To Outline" can be used to check the distance of a "Net Group" or a "Net" to the outline of the PCB.

1. It is possible to check the distance of a "Net Group" or a "Net".
2. The second number shows you the value which will be the reference for the check. If the calculated distance is smaller than the set value, the corresponding net will be reported.
3. If the third option is set, the chosen net or net group will be checked only to the PCB outline. If you uncheck the third option, the net or net group will also be checked to routing layers and unplated drills (Note: If the "Maximum Creepage flow steps" is set to two or higher and "Drills and routing layers" are not ignored, the net or net group will check the distance to different layers as well.).
4. "Run All" conducts like the calculate button below. The only difference is that "Run All" checks every net group to the outline instead of just one.

5. If a netgroup is selected in the control field, it checks whether there is a rule that contains the selected rule group for the netgroup selected above. If such a rule exists, the distances which are stored in the rule are used for the calculation. If a net is selected instead of a netgroup in point "1", the system first checks whether the net belongs to a netgroup. If this is the case, the procedure is identical to the sequence with a netgroup. If the net is not in a netgroup, the entered distance is used for the calculation.

2D View and 3D View

2D View

After the calculation is finished, the result may look like this:

Selecting one of the results will show you the area with a resulting line in 2D. It also shows the name of both nets, which cause the result entry.

Sometimes it can be hard to detect the issue on 2D. For this reason, it is possible to present it on 3D.

To show the result 3D, follow the instruction below.

1. Creating a separate window

   3D View

   

   Now a new window opens with the current design (it may take a few seconds).

2. Activate important options

On bottom left of the new created window, there are several options.

Enable the green bordered ones.

Use the result window for the following steps.

1. Select a result entry.
2. Click the 3D button and synchronize the selected result to the separate window.
3. Right-click the selected entry. The following dialog will pop up.

Click the "Select Nets" to activate nets in the separate window. Now the 3D view should be ready to inspect. It may look like the following image.