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ENGINEERINGXYZ8-Gravel
8-Gravel
November 15, 2023
Question

Inquiring About a Feature in Creo Similar to SolidWorks

  • November 15, 2023
  • 4 replies
  • 2123 views

I'm currently exploring the capabilities of Creo and was wondering if it offers a functionality similar to one I've used in SolidWorks. In SolidWorks, there's a feature that's particularly useful when working on complex designs. As you know, when you modify a part repeatedly, it can result in a multitude of features, making the design appear cluttered and complicated. SolidWorks has this great function that allows you to recreate the same part with far fewer features, significantly cleaning up the step-by-step process and making the design more manageable.

Does Creo have an equivalent or similar feature? If so, could you please provide some insights into how it works? This feature would be incredibly helpful for maintaining the simplicity and clarity of designs as they evolve.

 

Edited: 

I used to save the SW file into a non editable format, then using the following function to recreate a new part.

https://help.solidworks.com/2019/english/SolidWorks/fworks/t_recognizing_features_automatically.htm

4 replies

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
November 15, 2023

Do you know the name of the function?  It is hard to determine if there is an equivalent without seeing how it works.

There is always more to learn.
E
ENGINEERINGXYZ8-GravelAuthor
8-Gravel
November 15, 2023

I used to save the SW file into a non editable format, then using the following function to recreate a new part.

 

https://help.solidworks.com/2019/english/SolidWorks/fworks/t_recognizing_features_automatically.htm

kdirth
21-Topaz I
kdirth21-Topaz I
21-Topaz I
November 15, 2023

There is a Creo Reverse Engineering Extension that may be able to do what you are looking for.  I have never used it and it is an add-on that you will have to pay more for.  $$$

 

I always try to incorporate changes into the model as far up the tree as appropriate to avoid the bloat.

There is always more to learn.
M
16-Pearl
Michael16-Pearl
16-Pearl
November 15, 2023

You can collapse a set of features into one generic feature but it’s permanent. You can create groups to organize better. You may also like inseparable assemblies. Also use the new quilt body evolution tree. 

Patriot_1776
Patriot_177622-Sapphire II
22-Sapphire II
November 16, 2023

You can export the Creo model as a STEP file, suppress all the features in the model tree, then import that STEP back into the model as a SOLID, higher up in the model tree right after the (default?) CSYS used to export it.  If you need to change the model, suppress the STEP file feature, make changes, and then repeat the process ending by resuming the STEP import after you've redefined it to use the new version of the STEP file.  This way the model retains all it's features, but in a vastly compacted form, yet still retains the ability to make changes to the native features and keep making new STEPS as needed.  You can use the same name for the STEP file over and over, and simply redefine the "Source File" (Important!) of the STEP feature to use the newest version.

 

You know, I'm glad you prompted me to think about this, I think this technique could be used for ALL files in large assemblies to speed things up.  You could make it a 2-instance family table part, and swap out the instances as needed if you needed to change the model.  Further, if you did this to all files in your database, it would probably speed Windchill up significantly as well also.  Step files are drastically smaller and less complicated.  Hmmmm.....

 

As a side note, I've found that simply suppressing all the features and then saving the file results in a file DRASTICALLY smaller than a STEP file for times when the recipient (via e-mail, etc.) ALSO has Creo.  If they use SolidQuirks or Tormentor, then you might be stuck sending a STEP.

 

EDIT:  Well, it sorta worked.  The original file was 1,140KB, the STEP file generated was 381KB, but suppressing all the native features and importing the STEP brought the file size back up to 1,044KB.  So, it reduced the file size by maybe 8.5%.  Not as much as I'd have liked (or thought) but it DID work.  And for REALLY large assemblies or large assemblies of much more complicated parts (big IM plastic parts, large castings, etc.), this might just be a thing.  Caveat emptor....

Chris3
Chris321-Topaz I
21-Topaz I
November 16, 2023

As @Michael said you can use the collapse feature to turn all of the features into un-editable features. The advantage of using the collapse feature over stepping it out is that all of the surface IDs are retained so any assembly references to surfaces are retained.

https://youtu.be/ekvVg3M3_F8?t=141 

 

 

From there, you can use flexible modeling to recognize features and continue editing them.

https://www.youtube.com/watch?v=h8sUwGKOf6Y 

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