Tolerance problem when trimming an Extruded Solid
Tolerance problem when trimming an Extruded Solid
(OP)
Hi, I am newer to NX first off. I am having a problem that I would so appreciate some help with. I am trying to take a Class A side Styling surface(Automotive Trim Parts),Sew them together, everything good so far. Then take the trim lines(boundry curves ot surface, parting lines} of that surface and project them onto a plane, normal to my Die Direction. Then Extrude those trim lines back through the actual trim lines(along the die line), so I can then trim the Extrude with my Sewn Surface and Shell in my part thickness. The problem I am having is NX won't Trim the Extruded Solid with the Sew Surface, says the two do not intersect at the trim lines and the edge of the extrude. Of course they do though. Even if I loosen the tolerance value in trim body forever, it will not trim it. Are there some Tolerance issues I need to know about or what? I really want this to work. help please!





RE: Tolerance problem when trimming an Extruded Solid
try extrude what you have without the "project to plane" step. - adding this project step will only add to the total deviation.
Make sure that the trimming surfaces oversize. Then trim.
Regards,
Tomas
RE: Tolerance problem when trimming an Extruded Solid
RE: Tolerance problem when trimming an Extruded Solid
You're able to thick a surface via Extrude it boundary curves along any vector. Is the picture shows what you need?
1. The Datum Axis defines a Die Vector
2. Make an Extrude with outermost boundaries along the vector. The result would be a Sheet Body
3. Then copy top face along the Die Vector in order to "cover" the Sheet Body from the bottom
4. Sew both Copied Face and Sheet Body
5. The result should be a Solid
RE: Tolerance problem when trimming an Extruded Solid
After you made a boundary projection onto a plane along a die vector - extrude it with end limit set to Until selected:
Also try to use the Emboss Body feature, it would also helps.
RE: Tolerance problem when trimming an Extruded Solid
Not extending the surfaces beyond what's necessary could be the issue. It's typical best practice to over extend surfaces or bodies the majority of the time, regardless of the software being used. It makes it easier for the system to approximate edges when you go beyond the intended boundary. If you try to fight it, you're going to spend way more time attempting to force it to work than what it's worth.
You can take the existing surfaces, Extract an associative copy of all of them and then extend all the outer edges beyond what's necessary (outside of your Extrude) then Sew the extended surfaces together and Extrude up to the extended sewn surface like Lockdain has shown but if you have more than 1 surface, it won't work - you'll have to Extrude beyond the sewn surfaces and then use Trim Body.
Without seeing the part and what all you're trying to do or a similar part, our responses are going to only be best guesses.
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
RE: Tolerance problem when trimming an Extruded Solid
RE: Tolerance problem when trimming an Extruded Solid
www.nxjournaling.com
RE: Tolerance problem when trimming an Extruded Solid
In an assembly environment, you could use Until Selected/Extended to an external object’s Plane/face/surface with the option of automatically creating Interpart Link (Associative/non- associative).
Optionally to trim face and also when the surface (larger than the extrusion) isn’t intersecting the extrusion, you could use Sync Modelling's Replace Face.
Michael Fernando (CSWE)
www.solidCADworks.com
Tool and Die Designer
Siemens NX V10.0 + PDW
SWX 2013 SP3.0 X64
PDMWorks 2013
Logopress3
FastForm Advance
FormatWorks
RE: Tolerance problem when trimming an Extruded Solid
RE: Tolerance problem when trimming an Extruded Solid
RE: Tolerance problem when trimming an Extruded Solid
www.nxjournaling.com
RE: Tolerance problem when trimming an Extruded Solid
RE: Tolerance problem when trimming an Extruded Solid
RE: Tolerance problem when trimming an Extruded Solid
You can't convert sewn surfaces into a single surface? Sure you can - look at Quilt. Keep in mind, Quilt may not be a 100% 1:1 "conversion" - there might be some tolerancing used to create the resulting single-faced surface. Quilt can be a bit touchy, depending upon the complexity of the starting sewn surfaces. What I usually do is once I get a Quilt to work, extract the isoparametric UV curves of the Quilt surface to create a curve mesh (the UV curves do NOT need to be associative) then create either a Through Curve Mesh surface or Studio Surface using the extracted UV curves. I don't feel it's necessary to keep the "old stuff" around if it's not going to be used.
Don't take offense, but it sounds like you might benefit from some training to get familiar with what NX commands will fit your modeling workflow(s).
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
RE: Tolerance problem when trimming an Extruded Solid
To Lockdain: I may have to try what you're saying. I guess when I get a new A-Side Surface, I could Edit with Rollback on the Sew, and deselect all the Sheets and select all the new Sheets. I'll have to try it.
To MFDO: I'll have to look into what you are saying, but when you say Single Face = plane, are you understanding that I son't have a single face or a plane? I have multiple curved surface Sewn together.
To XWheelguy: I will try the Quilt today, extract the UV parameters and rebuild the surface and see how much it deviates from original surface.
Thanks all very much for suggestions!
RE: Tolerance problem when trimming an Extruded Solid
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Enterprise x64 SP1
Intel Core i7 2.5GHz 16GB RAM
4GB NVIDIA Quadro K3100M
RE: Tolerance problem when trimming an Extruded Solid
www.nxjournaling.com
RE: Tolerance problem when trimming an Extruded Solid
www.CADabout.ru