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Bob_Johnson1-Visitor
1-Visitor
August 13, 2020
Question

Can't extrude through imported geometry

  • August 13, 2020
  • 5 replies
  • 7995 views

I want to extrude away some threads on hardware models that I imported as STEP files. 

When I go to do this the "remove material" option is grayed out. 

 

Questions:

  1. Why can't I extrude cut imported geometry?
  2. Is there an error in the model that needs to be repaired before I can do this?
  3. Is there another way?

Bob_Johnson_0-1597333294850.png

Thanks,

Bob

5 replies

kdirth
kdirth21-Topaz I
21-Topaz I
August 13, 2020

Your imported geometry is surfaces only, no solids.  With no solids in the model, Creo has nothing to cut.  If you switch the feature to a surface, you will be able to cut the surfaces.

 

Solidify the imported surfaces and you will then be able to cut away the threads.  This may be as simple as redefining the import to be a solid, or may require repairing the import.

There is always more to learn.
Mahesh_Sharma
Mahesh_Sharma22-Sapphire I
22-Sapphire I
August 13, 2020

@Bob_Johnson 

 

Is STEP file imported as solid or surface? Surface model is one of the common reason for such issue. 

 

If it is a surface model, try solidify that prior extrude. 

T
Tdaugherty16-Pearl
16-Pearl
August 13, 2020

Hi, 

 

A few things...

 

Your method does work. Can you try to extrude all the way up to the hex head surface? You can extrude to a reference. Add material instead of trying to remove it.

 

I've attached a video of another really cool option. It's the one I teach to users most of the time. Based on what you select, the remove command works differently. If you select all of the surfaces that make up the thread, they will be removed more quickly than what I showed in the video.

 

Ty

P
Pettersson15-Moonstone
15-Moonstone
August 14, 2020

As others have said, most likely your imported model is surface geometry. Generally Creo imports as solids if he can, which means your import probably has some errors. This leaves you with two options:

 

  • If you need the part as a solid, you'll have to repair it using the Import Data Doctor, or remake it yourself (it doesn't look too complicated).
  • If you're ok with a surface model, make your extrude as a surface and then merge the quilts together. With some luck, you might even cut away the bad geometry and be able to solidify the part afterwards.
T
Tdaugherty16-Pearl
16-Pearl
August 14, 2020

Hi, 

 

If you need help solidifying your geometry, there are a few techniques you can use. The first one I normally try is the repair tool in Data Doctor. Here's a quick video I made for somebody else last week on the topic. If this doesn't work, I can suggest some other options.

 

Ty

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