Redefining the Default Coordinate System in Creo - 11.0.4.0

[AV_13191284]

Good day,

I’m trying to redefine the default coordinate system that Creo assigns to a part or assembly.

Background:
I have a main assembly representing a vehicle, which is divided into multiple subassemblies — each assigned to a different designer. A recurring issue arises when a designer does not use a skeleton model: the parts or subassemblies do not assemble correctly when using the “Default” constraint in the main assembly.

With a large top-level assembly, it becomes quite time-consuming if every designer has to manually constrain each part or subassembly to the correct position.

Workaround Tried:
One approach I’ve used is to create a new coordinate system in the desired position, export the part/assembly as a STEP file, customize the export to use this new coordinate system as the default, and then reimport it. This works, allowing me to use the “Default” constraint correctly — but it’s not an efficient process.

Question:
Is there a more direct or recommended way in Creo to redefine or replace the default/main coordinate system of a part or assembly — essentially assigning a custom coordinate system as the new default?

Thank you in advance for any suggestions or best practices.

Kind regards,

[ArnoldCollett]

I'm not sure if there's an easy way to do that.

You can create a skeleton with the main locating csys and a local csys for each different section. That way the piece parts can be assembled to each section, then the sections can be assembled in the top level assembly.

You wouldn't really want every part built in place of a large top level assy. That throws the default csys of a small part way out of the way when trying to create the drawing.

Hope this helps.

[tbraxton · Accepted solution]

I would not bother pursuing changes to the default csys of models that have already been created. In practice I have found the best way to deal with the issue you face is to create a new csys in the models such that you can assemble components using csys to higher level assemblies.

This is readily done through the use of the Analysis measurement of csys transform matrix. 

To Generate a Transformation Matrix

You can save the measure results to a .trf file that can be used to create a new csys by reading from the .trf file.

You can assemble components by default to an assembly, if it is not aligned correctly then create an analysis using transform matrix to determine where a new assembly reference csys is required in the component model. Do this by measuring from the component default csys to the assembly default csys in the context of the target assembly. Save the results to a .trf file. Read that .trf file into the component model when creating a new csys from file. You can then assemble the component using the newly created csys aligned to the default csys of the target assembly.

You save the .trf file by opening the information window and then saving the results file (*.trf).

[BH_12246893]

This is pretty much what I used to do when I worked in automotive decades ago and then we would assemble by coordinate system instead of default.

[pausob]

@AV_13191284 , for sake of completeness, I wanted to also point out another way of generating the coordinate system which might be quicker than what I think @tbraxton is describing.

This is a kind of an easter-egg type of Creo UI quirk, so maybe hard to follow but hopefully these screenshots capture the idea:

Example situation:

Modeled component, when placed in the assembly "by default", but it is in the wrong place (red).  So we have positioned it in the correct location, using whatever whatever methods/constraints (green one):

How to define a coordinate system in this model such that when it is placed with this new coordinate system coincident to the assembly coordinate system, it will result in the correct location?  Here is the procedure:

1) activate the "green" component and start defining a coordinate system:

2) first, select the assembly coordinate system:

3) then, the very next step is to select the part's default coordinate system:

Notice the system makes the new CS0 reference the (2nd selected) PRT_CSYS_DEF but will populate the UI with the offsets and rotations that makes it be coincident with the (1st selected) assembly ASM_DEF_CSYS.

Now this component can be placed by a single coincident constraint and be in the green place:

[ArnoldCollett]

You beat me to it. This is how I do it, also. It's also easy to create a mapkey to do most of this, other than your picks.

[pausob]

If one were able to redefine the default csys, wouldn't that mean that this "default csys" was defined in terms of another (i.e. parent) coordinate system?

But the default csys is the parent.

Anyway, I understand the end goal is to be able to place the already constructed model using the Default constraint and have the result be "in the right place".  So in theory one should be able to just replace the references and direct the model's features to use the "correct" csys instead of the default one:

In practice, though, Creo does not let you replace the default coordinate system references because you can't put features above it (and you can only use the Replace References tool with features that are older).  So one is then forced to edit the references of the children which is more tedious.

So long story short, it isn't easy.  And it gets worse if you have annotations and if you have user defined views, etc...

I would tend to agree with what others in the thread have already said.

Insisting that part be designed around some top-level assembly or skeleton default coordinate system seems inflexible.

Specifying the "placement coordinate system" in the model (or in its parent assembly) and avoiding the use of the "default" constraint is the way to go.

It is only a couple of extra clicks to place such a part using the Coincident constraint.