Parts shifting unexpectedly

[JVAero]

Hi,
I'm using v5 r15, and am having trouble with parts changing. The assembly has about 400 parts, and I need to convert to step file to transfer to the draftsman for detail drawings. The problem is that the parts keep shifting slightly, with the result that the bolt holes don't line up, or parts interfere with each other, or parts come out of alignment. In addition to the step file having problems, I also have the problem in CATIA in that parts go out of alignment after applying all the constraints.
What should I be trying to fix in the CATIA assembly / parts to correct this?
My guess is to make sure all the sketches are iso constrained. Is there a search technique to locate sketches that are non iso constrained?
Any suggestions on other aspects that should be reviewed, checked, corrected?

John

 

[bradmac65]

If parts are shifting around after applying the constraints, it sounds to me as though some of the constraints are incorrect. If the parts are in the correct position when loading the file, I would personally delete any assembly constraints to start with so the parts won't move due to the constraint update.

Another possible reason parts may shift out of place is if they were created with contextual links to another file, thus driving the design of the individual part. If the part itself needs an update when the file is loaded, it will look to the parent geometry for the update and this may also cause the part to shift or holes to not line up depending exactly how things were created initially. You could isolate the parts that are contextually designed (if this is in fact what is needed) and the link would be broken between the part in question and the part with the parent geometry.

There is no way that I am aware of to search for sketches that are not iso constrained.

Since you say that all you need to do is convert to a step file, the first suggestion is what I would try - parts load up in correct position, delete constraints and save as step.

Brad

 

[jackk]

You can check CATParts for non-iso constrained sketches by using the Tools + Parameterization Analysis and change the filter to "under-constrained sketches"

 

[jackk]

Parts don't just shift and go out of alignment on their own. Something made them change.

Could be contextual links that inadvertantly changed the wrong parts, as Bradmac suggested. But, when used correctly, contextual links should force mating parts to always have mathcing features.

Was it the parts themselves that shifted? Or was it features within the parts that shifted?

I suspect bad or missing constraints. Either Sketch constraints that are missing and allowing features to shift slightly when the sketch is being edited. Or Assembly contraints that are missing or broken that allowing the parts to shift out of alignment.

Another possibility is Search Order. If many people or working on different parts, are you opening the latest version of each part?

 

[JVAero]

Brad:

I will try deleting all the constraints before next iteration with draftsman (today or tomorrow).

Jack:

Thanks for the lead. Is there a way to quickly use parameterization analysis on an assembly. Maybe a vba macro that loops through all the parts.
I'm doing all the modeling. The shifting does appear to be related to incompatable constraints. THe parts themseleves change slightly. Can an under constrained sketch be changed by applying assembly constraints?

 

[bradmac65]

A sketch would not be changed by an assembly constraint.