How to create a “Dumb solid” of an assembly in Creo?

[SpencerZeedyk]

Need to create a dumb solid of an assembly that contains no
internal features( holes, cavities, parts, etc.), only the external features.

The goal is to unite all the bodies in the assembly and remove
the interior faces.

When we were using Unigraphics NX4, there was a wizard call “Simplify
Assembly” that would do this very well. With this wizard you could plug holes
and fill gaps until all the bodies are united into one and the interior faces
are completely isolated from the exterior faces, The interior faces are then
removed. The result was a single lightweight and airtight solid.

Is there a way to do this in Creo 2?

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[StephenW]

Not as well what you are describing. The method in Creo is to do a save as-shrinkwrap in the assembly. There are several options in the shrinkwrap dialog box. You would want to specify MERGED SOLID and you can use filled holes options. As far as filling the inside surfaces, there is really no equivalent. The QUALITY LEVEL will allows you to specify how much fine detail saves with the shrinkwrap though. You'll have to experiment with that value. If I was you, I would start with a low value and then increase it until you have enough detail, but not too much. The higher the number, the more detail you get and the longer it takes to generate.

[bgruman]

As Stephen Williams suggested,  Shrinkwrap is the way to go if it will give you what you need.

Sometimes it doesn't quite get it done,  so you need to do it the hard way...   It goes something like this...

-Create a new part in your asm.

-Create Copy Geom features...  and using "surf-n-bound" select all the exterior surfaces of all your components.

-Open your part in a separate window.

-Set all your Copy Geom feature to "independent"

-Proceed with curves, fills, extrudes, extends, trims, merges, or whatever else is needed to patch up your quilts.

-Done

  (optionally,  if you want the model as an un-modifiable single feature blob...)

-Export your model as an IGS.

-Import your IGS into a new model.

-Done.

It usually ends up being quite a job (especially if your dealing with complex geometry) but it can be done and does get you what you want.

Good Luck

Bernie

Bernie Gruman

Owner / Designer / Builder

www.GrumanCreations.com

[Patriot_1776]

"Need to create a dumb solid of an assembly..."

....convert it to Solidworks?