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How to resolve SOLIDWORKS Non-Matching Internal ID Errors

Article by Scott Durksen, CSWE created/updated April 24, 2013

Perhaps you received a different part file that you need to use in your assembly.  Or maybe your original file was lost and needed to be recreated.  If the new file is saved as the same name as the original file, the next time you open your assembly get ready for some SOLIDWORKS Non-Matching Internal ID Errors.

SOLIDWORKS Non-Matching Internal ID

SOLIDWORKS Non-Matching Internal ID

What is a SOLIDWORKS internal ID code?

When a new file is created, even if the geometry is identical, every face/edge/vertex is assigned a different internal ID code.  Therefore when an assembly picks up the reference to a completely new file, the ID codes will not match.  You can choose to browse for the original file if it has moved and avoid errors.

If you select “Use this file anyway”, mate errors will inevitably be waiting for you.  Mates are assigned to specific IDs so mate errors will occur when these IDs are missing.

Wrist Pin

The Original “Wrist Pin” Component

It can be a daunting task to see the SOLIDWORKS Non-Matching Internal ID error and all the mate errors that need to be corrected, as shown in the screenshot below:

Mate Errors

Mate Errors after the Assembly References a Different “Wrist Pin” File

Using the Replace Components Tool

Instead of replacing the file with the same filename in Windows Explorer, a better method is to use the Replace Components command within SOLIDWORKS.  This will provide graphical prompts showing what mates are missing their ID codes.  The Replace Components command cannot replace a component with the same filename.  It is always best practice to have files with unique filenames to avoid reference errors.  In this example, I am replacing the “Wrist Pin” file with “Wrist Pin v2”.

Expand Menu

Expand Menu

Right-click on the component in the Design Tree and click the arrow at the bottom of the menu to expand.  Select Replace Components to open this command.

Replace Components

Replace Components

With this command, you can browse to the replacement file.  Ensure that the “Re-attach mates” option is enabled.

Re-attach Mates option

Re-attach Mates option

Resolving missing mates

The PropertyManager will list all mates and show a “?” beside any mates that cannot locate the modified face/edge/vertex.  Click on each one to see a graphics window highlighting the face of the original file, then select the face on the new file that has been inserted.

Reassign Mates

Reassign Mates

Continue through the mates until all have a green checkmark:

Reassign Mates Completed

Reassign Mates Completed

Pick OK to finish and the mate error will now be resolved:

No Mate Errors

No Mate Errors

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Scott Durksen, CSWE

Scott is a SOLIDWORKS Elite Applications Engineer and is based in our Dartmouth, Nova Scotia office.

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