Sew Sheets - how to find the gap? 1

[carlharr]

Good morning,

We have a user who has created a model from sheets, and attempted to sew them together into a block.

The sew appears to have worked but has not generated a solid body, so we think there is probably a gap or other discrepancy.

My plan is to rewind his part and re-build it step by step, to see if I can find the problem.

Does anyone know another good method to locate a gap in such a part, other than measuring edge deviations (because there's lots of edges)?

Thanks in advance,

Carl

 

[stevethb]

Hi Carlharr

There is a simple way to check it.

Go to Analysis - Examine Geometry -> select Sheet Boundaries and select your sew sheet body and click Examine Geometry. Select Highlight Results. Result shows you where the gaps are.

Regards

 

[carlharr]

Thank you very much Steve, that's worked perfectly and saved me quite a bit of time! I found the gap with no trouble once I'd used this method.

Thanks for your help! Carl.

 

[jerry1423]

Also go into Preferences -> Modeling
and change the distance tolerance to a greater number

 

[carlharr]

Thanks Jerry, in this case the gap turned out to be a gaping chasm (just well hidden), but its worth knowing the tolerance setting for a later date!
Carl

 

[JohnRBaker]

I would be a little cautious about increasing the Modeling Tolerance until you get a 'successful' result.

You have to understand that while it looks like the sewing operation 'joined' two edges so that they are now the same. Actually that's not how it works. What happens is that shape of surface and its edges are NOT modified even if there was gap less than the Modeling Tolerance. What happens in a case like that is that ONE of the edges becames the common and the other edge is 'removed' and the visual 'appearance' corrected so that it LOOKS like there's only ONE common edge. But in reality the 'gaps' are still there, it's just that the code simply ignores them and acts AS IF the gaps didn't exist. Now under normal conditions all the NX applications will work just fine with this, however, there are limitations because even if you could open-up the Modeling Tolerance enough to get a result, you're potentially creating what someday might be seen as a very poor model if and when it's discovered that the edges of the model faces are not as well behaved as they might appear. After all, even with a piece software like NX, it's still generally 'impossible to make a silk purse out of a sow's ear'.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

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

 

[capnhook]

Use the tolerance setting at your own peril, though.........too tolerant a value might sew you a "valid" solid, but if you go to machine it you may have difficulty with some of the surface machining operations, sofar as them getting confused and lifting and repositioning near "ragg-ed" face edges.

Proud Member of the Reality-Based Community..

[green]To the Toolmaker, your nice little cartoon drawing of your glass looks cool, but your solid model sucks. Do you want me to fix it, or are you going to take all week to get it back to me so I can get some work done?[/green]

 

[jerry1423]

Now that you found the gap, closing it can be a bit of an issue.
Here is something that I do to close up something like that.
Create a Face Blend between the two surfaces, just big enough to get the task done. Have the Sew all Faces option checked on, also have the Trim Input Faces to Blend faces option checked on.
Delete the face of that blend using Syncronous Modeling.
The original two faces will trim together.
Remove the parameters if desired.