Why there is no tolerance option for "Trim Body" feature? 2

[opetrenko1]

Isert -> Trim -> Trim Body
The feature sometimes fails and I would like to losen the tolerance, instead of patching tiny gaps, but tolerance option is not available.
Thanks

 

[cowski]

I believe it is controlled by your general modeling tolerance.

I'm not sure what you mean by "tiny gaps". Does the trimming object have gaps, or does the resulting trim create gaps? It sounds like there is a problem that will not be solved by loosening the default tolerance. Can you upload a pic and/or small demonstration part?

www.nxjournaling.com

 

[JohnRBaker]

Only Modeling functions where the tolerance value is included as part of the definition, and therefore has some relevancy for that feature, will the dialog include an option to change the default tolerance for THAT particular feature. Generally speaking, if you don't see an entry widget for a 'Tolerance' value, then it's probably irrelevant for this particular feature type.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[opetrenko1]

Thank you for the reply.

The Trim Body feature fails, while Trimmed Sheet feature works after loosesning tolerance down to 0.001".
I'm timming a sheet by a duct sewn together of dosens of sheets. Unfortunately Trimmed Sheet feature is not robust, and the kept and discarded regions interchange several times as I move the sheet to be trimmed along the duct.
Trimmed sheet is used to measure x-sectional flow area of the duct.

Thanks

 

[opetrenko1]

Then what separates Trim Body feature from similar Trimmed Sheet and others?
Thanks

 

[opetrenko1]

I have a hinch.
I guess multiface sheet bodies have only ONE edge for two neighbouring sheets, (not two, that would mean there is a gap within ug accuracy). So if I sew sheets with higher resolution, there is a chance of a gap between sheets, which edges within the tolerance distance from each other.
Conclusion: sew with lower resolution to avoid gaps? Will try it next time I run into the problem.

Would be nice to hear from someone with knowlege of UG engine...

 

[JohnRBaker]

OK, NX uses something called 'Tolerant Modeling' when it comes to stuff like sewing sheet bodies together, either into a solid or into a larger sheet body. If the adjoining edges of two sheet bodies do NOT match exactly BUT they're within the Modeling Tolerance, when they are sewn together the system will choose ONE of the edges as the NEW edge representing the 'seam' between what are now two faces of the new 'body', and the other edge will be permanently hidden. What this means is that theoretically there is STILL a gap between the faces since the actual shape of the sheet bodies have NOT been modified. However, NX will TREAT the body AS IF THERE WAS NO GAP for all downstream operations. This is why it's called 'TOLERANT Modeling' since the NX operations are 'tolerant' of this condition.

Now if the 'gap' between the sheet bodies is greater than the Modeling Tolerance and there were more than two sheet bodies being sewn together, you might get a result showing a single body but there could still be actual gaps between some of the sheets. To see if this is the case, after the sewing operation, go to...

Analysis -> Examine Geometry...

...and make sure that the 'Sheet Boundaries' check in toggled ON. When you hit the 'Examine Geometry' button look for highlighted 'edges'. Now if the only highlights edges are around the perimeter of the new sheet body, then that's OK. However, if you see some highlighted edges between faces of the new body then there are gaps, which probably meant that the mismatch between the original sheets bodies was greater than the 'Modeling Tolerance'. Now you can do one of two things, either use a larger modeing tolerance or try cleaning up the sheet bodies so that they match better. If you choose to increase the Modeling Tolerance be aware that eventually this could result in downstream problems if the hidden 'gaps' are so large that they are close to the size of whatever downstream operation that you're performing is based on. For example, if you're going at a blend or chamfer one of these edges sewn with a large modeling tolerance and the they are close to the size of the tolerance used they couls fail. The same holds true for toolpaths with small step-overs or FEM meshes with small element sizes.

Also note that once a feature which depends on the Modeling Tolerance is created, changing the default Modeling Tolerance will have NO effect whatsoever on any of these features when the model is subsequently updated. In order to change the Tolerance used by a feature you have to actually edit that feature and change the Tolerance parameter in the Feature's dialog.

Anyway, I hope that helps.


John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[Xwheelguy]

While on the subject at hand, is it still "recommended" or "preferred practice" to not change the Modeling Tolerance (under Preferences -> Modeling) as features are created in a single part file? Does this hold the same for those features which DO have the tolerance available in the feature's dialog (as you're creating them)? Granted, I know that not every situation is going to follow the unwritten rule book for modeling, but generally speaking, would the above be true?

As with many things, I seem to recall at some point in time that someone relayed to me that it is recommended we set the tolerance and leave it alone - I just cannot recall from whom or when I heard it.

Tim Flater
NX Designer
NX 7.5.4.4 MP2
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

Generally speaking, one should leave the out-of-the-box tolerance as is. But of course, if we had NEVER wanted you to change it we would NOT have given you the option to do so ;-)

That being said, except for something like the scenario discussed earlier in this thread where someone was trying to sew together some 'poorly-modeled' sheet bodies, you should only consider changing the modeling tolerance if you're going to be creating 'very large' or 'very small' models. By 'very large', we might think of something like a ship or submarine, and for something 'very small', perhaps a watch movement or dental appliances. In situations like these it might prove to be beneficial in terms of performance and/or reliable model updates to adjust the modeling tolerance. For example, in the case of the 'very large' category, I would loosen the Modeling Tolerance by a single decimal place, changing the default from 0.0254mm (0.001in) to 0.254mm (0.01in). Conversely, for the 'very small' category, I would tighten the Modeling Tolerance by a single decimal place, changing the default from 0.0254mm (0.001in) to 0.00254mm (0.0001in).

Note that these are just 'rules-of-thumb' and that you should do your own testing and validation if you feel that you may fall into some other unique category.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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