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T_F16-Pearl
16-Pearl
December 13, 2020
Question

Feature fails after regenerate a part

  • December 13, 2020
  • 1 reply
  • 2659 views

I,

I'm having problems while open some parts, that wer drawn in context of an assembly. When I open the master assembly it runs ok. But when I open the isolated part, there is a lot of features that fails, after regeneration task. The ones that fails are some reference patterns, and features that have been created in context of the master assembly. I think it fails, because they aren't loaded.

 

But I need to send this file (only this file) to a collegue, and I need him to open it, and do some work on it. How can i do it, without any problem with regeneration? Any config option?

 

See video.

1 reply

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
December 14, 2020

If you are in a bind and must use the file as it is now you could try this.

 

1) Regenerate the part model in assembly mode

2) Set all features up to the last assembly feature as read only (this will prevent their regeneration when set, it is reversible).

3) Save the part

4) Delete all items from session and then open the part of interest. You should see that all of the assembly features exist and are not failing regen.

5) Provide this model for additional work to be done on it.

 

The read only status may affect the ability to use a feature as a reference for other features. I have not tested this with assembly features so you will need to consider that.

 

Assembly features should be avoided at all costs. There are times when they actually capture design intent but I have rarely seen when it is actually the best way to capture design intent within Creo. 

T
T_F16-PearlAuthor
16-Pearl
December 14, 2020

So it means that you don't make patterns using points from a sketch from other part? Or extruding using a sketch from other part?

tbraxton
22-Sapphire II
tbraxton22-Sapphire II
22-Sapphire II
December 14, 2020

It is possible to implement both of your examples using the top down design tools and not assembly features. Using assembly features for both of your examples is not generally considered to be best practice in Creo modeling.

 

If I have geometry that needs to be used in two or more models I would use a parent model and then pass that geometry to the two derivative models using merge, external copy geometry, etc. For assemblies, skeleton models can address many scenarios for managing intent. Notebook (layout) is also useful for controlling locations or pattern instances among models among other things.

 

Using assembly features can cause many issues. A prime (some would say extreme) example is that of needing to have an assembly in session to locate an axis for a shared hole among parts. If that assembly consists of 100,000 parts then it is not the best way to create that shared geometry in assembly mode as a feature (hole/cut). If your user has to load 100,000 parts in Creo to modify a model, that is not an efficient use of labor or hardware. This is one reason why the top down design tools were developed.

 

With Creo 7 multibody functionality you also now have that tool to capture/manage design intent shared among models. Multibody behind the scenes it is still leveraging the top down design functionality to share common data among parts controlled in a single "master" model.

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