boolean operation question in NX12

[Franklin M.]

I have a model that was stepped out of Catia. One side is made of a bunch of surface patches. I need to make some changes to some cross ribs. Synchronous modeling only handles a few of the needed changes. In some areas I've had to extract surfaces, trim them, thicken and then "glue" them in.

This has worked for other areas on the part excepting one. I get the "patch" created but when I do a boolean unite it adds it to the tree but the "patch" is invisible. If I change the thicken by .0005 either under or over it fills the opening.

There isn't enough data to recreate the model so that isn't an option. My method is rather Flintstone-ish I know I couldn't get anything else to work.

Anyone have suggestions on my invisible patch?

Franklin
UG 10,13 & 18
NX 1,2,4,6,11 & 12
NCL502 (yep I love Sequential Mill)

 

[jerry1423]

Is it possible for you to show a picture of this ?
Yes, there is probably a better way to do it.

Jerry J.
UGV5-NX11

 

[Franklin M.]

Thanks for the reply.

These are the model before "tapering", the inside after unite, the outside after unite.

The .0005 difference seems to be controlled by the default tolerance of .004 in the boolean drop down. I changed it to .0001 and then the thicken to .1201 (wall is to be .120) and these pictures show what I have. this is a tough area to edit, as you can see from the outside pic there are 5 surface patches converging.

When I tried to change it via synchronous modeling I get errors regarding a b-surface that won't move to close the gap.

Franklin
UG 10,13 & 18
NX 1,2,4,6,11 & 12
NCL502 (yep I love Sequential Mill)

 

[jerry1423]

On the top picture it looks like all the faces shown below are on the same plane.
Is this the way it is ?

Jerry J.
UGV5-NX11

 

[Franklin M.]

They're not planar, they are moldline, which comes out of Catia as B-surfaces. when you extract and untrim them the edges over lap and only meet at the trimmed edges. The side of the part is the result of several aircraft surfaces being trimmed to tough each other. I know that's not a good description but hopefully you get the idea. The edges beyond the adjacent surface no longer touch.

Franklin
UG 10,13 & 18
NX 1,2,4,6,11 & 12
NCL502 (yep I love Sequential Mill)

 

[NutAce]

Try to make these faces co-planar first

Then see what happens if you split the surface at the blend and then delete the faces (Arrows)

Ronald van den Broek
Senior Application Engineer
Winterthur Gas & Diesel Ltd
NX9 / TC10.1.2

Building new PLM environment from Scratch using NX12 / TC11

 

[Franklin M.]

Ronald,

Your suggestion didn't quite work but you did put me on the path. I used replace face to join some of the common faces, then in the move face dialog, turned on all the features under settings. The face moved and updated.

Thank you and Jerry for your replies and suggestions. Hopefully I'll be able to pay it forward.

Regards, Frank

Franklin
UG 10,13 & 18
NX 1,2,4,6,11 & 12
NCL502 (yep I love Sequential Mill)

 

[cowski]

When importing STEP files, I suggest running "heal geometry" and/or "optimize face" right after the import operation. These commands can help clean up/merge faces, making subsequent work easier.

www.nxjournaling.com

 

[Franklin M.]

Cowski, thanks for the info. I run these on a fresh copy of the part and post the result.

Regards, Frank

Franklin
UG 10,13 & 18
NX 1,2,4,6,11 & 12
NCL502 (yep I love Sequential Mill)

 

[Franklin M.]

Cowski,

I just ran the heal geometry on a part right out the step converted, it fixed a bunch of stuff, over 500 issues on the report. Pretty cold. Unfortunately I'm too far down the road on this one, might try running it on the part I have correction in.

Regards, Frank

Franklin
UG 10,13 & 18
NX 1,2,4,6,11 & 12
NCL502 (yep I love Sequential Mill)

 

[cowski]

Note that these commands will remove parameters from your part. This isn't a big deal on freshly imported files, but may be an issue if you have added features to the part.

www.nxjournaling.com