imported step files from Pro-E: cylindrical faces divided into 2 faces 1

[FXjohn]

I am having trouble with step files imported into UG from Pro-E having their faces divided into 2 faces. This makes it impossible to do a resize faces and is just annoying in general.
Is anyone else having this problem, and can it be fixed somehow?

 

[NXMold]

How do they come through via other formats? I seem to remember ProE handling cylindrical surfaces that way natively when I worked with it.

NX 5.0.3.2 MoldWizard

 

[FXjohn]

parasolid does the same thing

 

[uwam2ie]

there is a command under the trim operation called join face, select your imported body and use the same face option.
Getting foreign cad data form step there is a special step option in the def file to add :
DO_IMPORT_MERGING_REDUNDANT_TOPOLOGY = On

hp it hlps

 

[FXjohn]

wow, yes that worked perfectly!

 

[BOPdesigner]

Can you put that same option string in the igesimport.def file? Is there a listing of options strings and what they do somewhere? I can't find this string in the online documentation.

 

[FXjohn]

if you can't find it, you can also do a heal geometry operation I found out.

 

[hudson888]

CATIA does the same thing. You can also use delete face, or even replace face in most cases to model away the offending segments. It can be a reasonably time consuming and troublesome process on occasion so I'd start by questioning what is to be gained by it?

Cheers

Hudson

 

[FXjohn]

a couple of reasons, for starters if i want to resize face it won't work, another is that it doesn't look right when smooth edges are on, and you don't extract a full arc from the edge. it's just way cleaner when they aren't divided into two. If it's more than a few faces, just do a heal geometry. fix them !

 

[ameiza]

I've found that if the step is created from revolved cylindrical solid in the foreign CAD system, the import works ok. I'll also try some of the sollutions as suggested above.

 

[hudson888]

You're correct about the first part in my experience also. I don't think any of the translators add extra faces as such, at least I've never seen it from STEP or IGES so I wouldn't worry about it in that account.

Probably just do the delete face thing if you want to get rid of the second half faces.

Cheers

Hudson

 

[FXjohn]

the delete face won't work, but the join face fixes evey face on the body.

 

[hudson888]

What happens and how you should remedy it depends very much on what version of NX you're using. If you're willing to go back to NX-2 then I may stand corrected, about what the translators do.

I have a couple of CATIA parts as exported to STEP and IGES. They each contain a block and a simple hole. Very simple geometry that I obtained to test with.

In NX-2 if you import the STEP file the double up face inside the hole is actually deleted upon importing it in to NX. All later versions plus the iges file and the original inside CATIA do exhibit the two faces inside the hole. So here's a tip to try importing it first to NX-2 perhaps.

NX-2 and NX-3 The Join Faces command works very well for a range of simple examples and can be found under Edit>Face>Join Face. It appears to require only one selection pick in most cases so I can see why it is favoured.

After NX-4 the Join Face command appears to have been discontinued, but delete face does work. It appears that delete face wouldn't work in NX-2 but does in NX-3 onward.

At NX-5 Edit>Face is replaced with new tools under direct modelling. So in either NX-4 or NX-5 you will need to at least pick each of the faces that you wish to remove, using either version of the delete face command.

It seems to me like the join face command was better at least in simple examples, but that for anything more complex it could perhaps have the potential to be difficult to control. I'd like to hear more comment about the relative merits of the changes to this command and the translators over the versions and whether what I'm reporting gels with the versions you are variously posting about.

Best Regards

Hudson

 

[JohnRBaker]

The reason why some systems export models with cylindrical faces which are divided into two sections is because these system do NOT support what is known as a 'Periodic Surface', or one that has 'no beginning and no end'. NX (and Unigraphics before that) has always supported Periodic Surfaces. You will probably also see something similar if you import spheres or tori from these same systems.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[hudson888]

John,

I knew that already but it is nevertheless a good explanation. I was just curious as to why NX-2 imported the STEP file as periodic whereas the later versions, the IGES and indeed the native file in CATIA were all non periodic. I was hoping some obscure setting change in the STEP translator may solve our poster's original problem.

Cheers

Hudson

 

[JohnRBaker]

I think STEP provided a scheme that allowed the conversion whereas IGES did not. As for the Catia translator, I suspect that the developers of this program decided to try and leave the original geometry (and thus its topology) as it was in the authoring system and leaving any 'conversion' the user of the results itself.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

To an Engineer, the glass is twice as big as it needs to be.

 

[DavidTolsma]

Instead of using STEP, try opening the file directly in NX. I think there is a license requirement for this, but could give it a shot.

-Dave Tolsma

http://Tolsnet.com/jobs

http://groups.google.com/group/NX_CAX/

http://groups.google.com/group/plm-exchange/

 

[hudson888]

Yes there is a license requirement for that.

 

[FXjohn]

I tried "opening" the step file and it did indeed join the faces.

 

[hudson888]

FXJohn,

NX-?