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Cannot not cut.

Genius
Genius

Hi All.

 

In need of more help.

 

I have a model part that was made from an assembly.  For some reason I cannot use cut to remove material from some areas of the model.

I have tried revolve cut, extrude cut, revolve cut and hole.

I converted it to a .stp and opened as a .prt and even as a .asm, and still cannot mdify the model.

 

Any ideas?

10 REPLIES

Re: Cannot not cut.

Phenom
Phenom

In the design tree, is there anything that says "design body" or "construction body" If so, which.

Another question.....the original part which you translated.....was it an .stl file?

Solid Edge 2019
Windows 7 Professional
Nvidia K2200 & Intel Xeon
"You're doing it wrong"

Re: Cannot not cut.

Genius
Genius

Hi Nominus.

 

The original was a .par file that was converted from a .asm file.  I do not have access to the original assembly.

 

What I am trying to do is remove parts that will have made up the assembly. (i.e. cover plate, screws)

 

It seems that the cover plate  I am trying to remove is Ø430.  I can cut out Ø429.99, but this leaves an edge that I cannot remove.

Re: Cannot not cut.

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

A picture or file upload is worth a thousand words. Give or take.

Bruce Shand
ST10 MP10 - Insight - Win10 - K4200

Re: Cannot not cut.

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

HI @Dazzie

 

 

a picture, an example file, everything what let us be able to work with

 

regards
Wolfgang

Re: Cannot not cut.

Phenom
Phenom

Have you tried thee delete face command?

Solid Edge 2019
Windows 7 Professional
Nvidia K2200 & Intel Xeon
"You're doing it wrong"

Re: Cannot not cut.

Gears Phenom Gears Phenom
Gears Phenom

sees like you are most likely dealing with a mixture of design and Construction (surface) bodies.

 

and probably seeing boolean errors.

 

do you have features in the PF?  can you select by feature instead of graphically?

 

a picture or model upload would help us, help you.

 


Matt Johnson
Solid Edge Certified Professional (ST7 & ST8)
Solid Edge ST9 (SEEC) - Production
SE2019 Pre-Production Testing
NX11 (Tc Integration) Pre-Production Testing
Teamcenter 10.1.7

Re: Cannot not cut.

Genius
Genius

Hi Everyone.

 

I will try explain. (i did manage to make it work).

 

On the attached file.

Image 1: I want to cut back from the face with the small bore 26.5mm.

Image 2: The diameter is Ø430mm, same as the model diameter.

Image 3: I changed cut diameter to Ø429.99mm.  As you can see I can cut.

Image 4: I changed the diameter to Ø430.001mm.  As you can see I can cut.

 

It seems the issue is i cannot cut using the same diameter as Ø430mm.

 

Is it that solid edge just cannot do it or am I missing something?

 

Re: Cannot not cut.

Gears Esteemed Contributor Gears Esteemed Contributor
Gears Esteemed Contributor

Hi @Dazzie

 

 

 

OK, now everything is clear.

 

This is the typical situation for the old fashioned "Non-Manifold Situation"

At least this is my idea when seeing Your pictures.

If I have the part, man could test it directly.

So at the moment I only assume this.

 

If You try to cut the 430mm diameter then there will be a tangent to another cylindar situation where volume with a singualarity will be created.

And this is something what Parasolid modeler can not achieve.

By the way also every real part will break at the same place.

 

So I suppose, that a situation which can't be in reallity will prevent You from creating this hole.

 

Think about possibility and gibe the answer

 

regards
Wolfgang

Re: Cannot not cut.

Phenom
Phenom

Yes, as @hawcad said, you are attempting to make a non-manifold body. This occurs when the area being cut leaves a small area that is infinitely small at that location. There is both material there and no material there, which cannot be. You could turn it into a multi body part, or do like what you did and make sure there's some material left when you cut it.

Solid Edge 2019
Windows 7 Professional
Nvidia K2200 & Intel Xeon
"You're doing it wrong"