is it possible to sew sheets to automatically fix the gaps (in given tollerence) 1

[vasinka]

Surface given to me by the client always is imperfect and has multiple gaps.
I am using NX 8.0

I am using client's surface to trim my solid.
First i sew the surface, sometimes decreasing the tolerence, and it sews, but gaps are still in the surface, which i dont care about, as long as I can use the surface trim my solid. But these gaps give me an error saying "not complete intersection" even if i decrease the tollerence in the trim settings.

IS THERE A WAY TO SEW THE SOLID TO AUTOMATICALLY CLOSE THE GAPS WITH IN THE SPECIFIED TOLERENCE?

I will later delete the faces and simply the surface because I dont need the details, thats why I dont care which way gap will be cloused.

For me its easier to work with the faces of the solids and simplify, rahther than with sheets.

any advise on how its possible to trim my solid with inperfect sheets.

 

[JohnRBaker]

Sewing surfaces together in NX, irrespective of the tolerance that you needed to use to get a result, will in NO way "close the gaps". Even if the result is a single sheet with no apparent 'holes' or 'gaps' they still technically exist.

All that NX has done is create a multi-faced sheets body where each face will be using an edge from ONE of the original surfaces which were adjacent to each other. This is what's known as 'tolerant modeling'. NX is simply being 'Tolerant' of the gaps, in essence acting as if ONE of the 'edges' no longer exists and that the edge that does exist is shared by the adjoining faces. Now this is generally NOT an issue when the tolerance needed to accomplish a successful 'Sew' operation is significantly less than what would be expected to be used during any downstream manufacturing task, however, if you find that the only tolerance that's large enough to get the job done is approaching or exceeding the anticipated tolerances which will used for manufacturing then you may be creating more problems than you've solved. It's very possible that the NC toolpaths will either give very poor results in terms of quality or worse yet, the toolpaths may look good but the finished parts may be worthless since they will not be close enough to the original 'math data' so as to usable.

If you're finding yourself having to use inappropriate Modeling Tolerances to get an 'successful' Sew operation to complete, then that's an indication that you're either going to have to try and find better data to start with or else you're going to have to do some manual cleanup and fixing of gaps yourself. But even if you do manage to 'close-up' the gaps yourself, you are in essence 'changing the model' and you will need to make sure that these 'changes' do not render the final model unusable since it deviates from the original data sufficiently that could be considered 'out-of-spec'.

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.

 

[vasinka]

Thanks for detailed response.

What I was basically saying is that I dont care about tollerences in this case. All I am trying to do is find a way to 'fix the surface' enough for NX to allow me to use the surface to trmim a solid with that surface.

Maybe there is a different command or a way that would automatically clouse multimple gaps by creating little surfaces or extending edges or whatever it will do.. as long as the gaps that are less than specified tollerence are cloused.and gaps that are bigger than specified tollerence, I will manually fix. So that when I trim a solid with that surface i will not get an error that tool doesn not make complete intersection.

 

[cowski]

What type of file are you getting from your client? If it is IGES, ask if they can send a parasolid or STEP file; you may have better luck with one of those.

Also, you can try the "heal geometry" function; it may help to do some cleanup.

www.nxjournaling.com

 

[SDETERS]

Do you have the Edit surface toolbar? You can do an enlarge surface. This is a very nice feature. If you need to extend your surface past a point you could use this tool. Then you could use these commands in this edit surface tool bar to get your surface to look like you want.

 

[Toost]

As John says, the tolerance when sewing will allow adjacent faces share the same edge. It means that increasing the tolerance will tolerate larger gaps, but it will still not fill the gaps. Looking at a sewn model in shaded mode can / will fool the eye since the graphics will look as if the gaps where gone. Static Wireframe display mode does not "hide" the gaps.

Regards,
Tomas

 

[vasinka]

"It means that increasing the tolerance will tolerate larger gaps, but it will still not fill the gaps."

IS THERE AN OPTION THAT WILL ACTUALLY FILL THESE GAPS AUTOMATICALLY??

I know I can do it using methods like 'extrude' and 'trim' and 'n-sided surface' and 'through curve mesh' and others... but all of that takes too much time to find the gap and fix it. I am looking for a a command like "heal surface" or "optimize face" that would fix the surface automatically and report how many edges/gaps were altered.

That option probably doesnt exist, but maybe it does and I just dont know about it.

NX should create a command "fix surfase gaps" where it will allow you to set the tollerence. EX: 'close all gaps less than .001 inch' that would be magical
Is this worth going on a suggetion list to include in next NX update?

 

[cowski]

Also, you can try the "heal geometry" function; it may help to do some cleanup.

Have you tried "heal geometry" yet?

www.nxjournaling.com

 

[Xwheelguy]

Welcome to the wonderful world of model intergrity! Unfortunately, here isn't a magic command that will fix your gaps. The gaps are either there or they aren't, as simple as that. If you really think about it, how would one even approach fixing a gap when you consider the different continuities that might exist between surfaces? Which of the two surfaces would change, because they'd have to change to fix the gap. How far from the edge would the surface be allowed to change and by how much? See what I'm getting at - it's a domino effect of sorts.

If you have the proper licensing, take a look at the Edit Surface commands and play around with Change Edge and/or Match Edge. Keep in ming that using these WILL change the surface topology (maybe slightly, maybe alot).

Tim Flater
NX Designer
NX 7.5.4.4 MP8
WinXP Pro x64 SP2
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[JohnRBaker]

OK, try this:

Set your Modeling Tolerance to some reasonable value, perhaps something that will catch 80% of the edge/edge conditions and then sew the sheets together into a single surface (it's important that the result actually be a SINGLE surface). Now run this part file through the 'Heal Geometry' utility which will try to fix the remaining 'gaps' in your model (you may wish to run a 'before & after' check using the 'Examine Geometry' tool noting that 'Heal Geometry' will create a COPY of your original part file so that's the one the 'after' check needs to be done on).

You have to at least get some sort of initial sewn sheet body created before you can use the 'Heal Geometry' utility since it doesn't know what to do with totally disjoint (i.e. unsewn) sheet bodies, even if their edges were within the Modeling Tolerance distance of each other. What it's doing is trying to 'heal' an existing BODY, it's NOT trying to make separate sheet bodies more compatible with each other so that they can be sewn together.

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.