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Fix Creo assembly constraints so legacy Mate/Align contraints work

Fix Creo assembly constraints so legacy Mate/Align contraints work

Currently, all legacy Mate/Align interface constraints are always reversed in Creo Parametric.

This causes the user to have to flip them every time they are used.

To work around this, companies are forced to modify hundreds of thousands of files, changing the mate/align interfaces to the new coincident/offset ones, or users are required to make tens of thousands of extra operations flipping everything.  Additionally, there is no differentiation between coincident constraints, so there is no way to tell which "coincident" applies to what feature.

PTC, please fix the new coincident/offset constraints so that legacy mate/align interfaces still work.


I got clarification oh how the coincident constraint work by default:

"The default coincident constraint is to mate faces.  If you flip them, then they are aligned.  It picks the part rotation using the face orientations. 

This can be seen by creating an assembly and assembling two blocks.  Coincident faces will mate, if you flip, then they are aligned."

Still, it seems like it would have been really easy, and in fact required, to add some code for converting the old, straightforward constraints to the new, vague ones.


Why on earth do we need to vote for this?

This is a serious bug, involving the most commonly used constraints. The software should never have been released without thorough regression testing,

Please fix this problem without further delay!.

Sapphire I

This has been out here for over a year, and like Dave said, we should not need a Community vote to fix a major bug!

Challenge to PTC program manager in charge of constraints: Give us users documentation that shows how the flipping of constraints when renamed by YOUR software meets the design spec that was written for the constraint manager.

At least provide an update on when PTC will provide a fix in Creo3 and tell us that Creo4 does NOT have this same issue. We will be migrating to a late version of Creo3 or maybe Creo4 after we do our Windchill 11 upgrade later this year.


I can't accept the justification from PTC's R&D.
Finally the component interface explicitely has been defined as either "Mate" or "Align".
This means I want to have it "Mate" or "Align" and nothing else!
If R&D decides to provide a new "Fit smart" option as third choice, this is ok. But don't change the existing behaviour!

If this behaviour really was an intented change in the product specification, I ask you (PTC):
Why has the option to choose between "Mate" and "Align" not been removed in the definition of the component interface, as it is useless now?
Why haven't you added a third choice like "Fit smart", as I wrote before?

When I look at these facts, in my opinion the claim of R&D, that this was an intended change in product specification, is only a pretence.

An interface usually is used to (pre)define expected behaviour!
This requirement is not fulfilled anymore at component interfaces using the specialization of "Mate" or "Align".


"Why has the option to choose between "Mate" and "Align" not been removed in the definition of the component interface, as it is useless now?"

Exactly my point.  The component interface should have been updated so it worked regardless of what the interfaces were called.


The Document - CS219399 shows a config option that may calm down the need to flip constraints. One of my users was getting this flip issue when using the replace command. Introduced in Creo 2 M150 place_comp_use_mate_align_type to yes.

I am not certain if this is the full fix but it may help.


Good advice, ian blackie. At a glance it seems to work!

Maybe someone else can test and confirm this?!


I set the option to yes and here's what I get in the assembly constraints now:



It doesn't appear to change the default behavior of Creo, but at least now we can see what the constraint is.


I still haven't had a chance to test the Interface constraints, in the footer of models, to see if they work correctly.

Community Manager
Status changed to: Acknowledged

I finally got around to fully testing the placement by interface and it seems to be functioning correctly now.

When I choose and INSERT-MATE interface, I get a Coincident and Coincident (Mate).

When I select the corresponding assembly references, the component assembles in the correct orientation.


"Insert" and "align axis" are still just called Coincident, so that's kind of annoying, but if the interface has been named in the order of operation, it should be easy to understand what needs to be selected.

I still need to test more of these legacy interfaces before I'll call this fixed, but it looks like, as of Creo 5, the behavior is as I expect it should be.