You are here

Cross Probing is not working in OrCAD Capture CIS - OrCAD PCB Editor flow

Error Message

Intertool communication does not work after netlist creation. When I select a component in Capture, it is not highlighted in PCB Editor, and vice versa. I receive the following warning message:

WARNING (ORCAP-1712): Could not find component X in design to highlight


Definition

This warning message might occur because of any of the following reasons:

  • The Message Passing System (MPS) is OFF in Capture CIS.
  • The board file is not updated.
  • Capture CIS and PCB Editor have different security levels.
  • There is a space used in the design name.
  • There are special characters (:, \, and <) used in hierarchical block names.
  • There is a space used in the user name (for versions prior to release 17.2-2016).


Solution

To resolve this issue, perform the following tasks depending on the cause of the warning message.

Turn ON MPS in Capture CIS

Ensure that MPS system is ON in Capture CIS.

  1. Open Capture and go to Options > Preferences. This will open the Preferences dialog box. 
  2. Go to the Miscellaneous tab. 
  3. Select the Enable Intertool Communication checkbox.


     

Update the board file from the Create Netlist dialog box in Capture

  1. Go to Capture > Tools > Create Netlist.
  2. In the Create Netlist dialog box, select the PCB Editor tab. 
  3. Select the Create or Update PCB Editor Board (Netrev) checkbox.
  4. In the Options section, browse to the the input board file (if present) and specify the name of the output board file.
  5. Under Board Launching Option, select Open Board in PCB Editor option.
  6. Click the OK button. 

 


  1.  

If you perform the above tasks correctly but cross probing is still not working, you should check the following configurations:

  • Ensure that both Capture CIS and PCB Editor have the same security levels. For instance, if PCB Editor is set to "Run as Administrator", Capture CIS must also be started as an administrator. If these two processes are at different security levels, Windows will not allow cross probing to work.
     
  • Ensure that there is no space used in the design name. For example, the design name  "my design.dsn" has a space between "my" and "design". Remove the space from the design name and then try to cross probe.
     
  • In a hierarchical design, if cross probing is not working only on a few parts in the design, presence of special characters in the Name field of a hierarchical block can be the cause of the problem.

    Check for the presence of the characters ":", "\", and "<" in the hierarchical block names. There are special meanings assigned to these characters. Perform the following steps to resolve this issue: 

  1. Select all hierarchical blocks in the schematic.
  2. Right-click the selection and select Edit Properties.
  3. Set the filter to "Current Properties".
  4. Find the Name field.
  5. Remove (or replace with _ ) the characters mentioned above if they are present in the Name field for any of the hierarchical blocks.
  6. Save the design and create PCB Editor Netlist of this modified design.
     
  • Ensure that the user name does not contain a space.

    This issue has been fixed in release 17.2-2016. However, if you cannot install release 17.2-2016, you can use the following workaround:

  1. Start Capture using the following command:

    capture.exe -mpssession <user name with underscore>

    For example, if the user name is cadence 1, you will use the following command:

    capture.exe -mpssession cadence_1
     

  2. Now, netlist and update the board.

Note: Cross probing between Capture and PCb Editor is available only for the Windows version of Capture.