(NX5) Problems sewing surfaces to make a solid

[speedster29]

I am trying to create a solid body by sewing surfaces together. It seems to work OK with simple surfaces like bounded planes, but I am having problems when I try sewing an N-sided surface. The sew operation leaves a couple of orange-highlighted edges; I assume this means they did not sew properly. How can I fix this? The documentation is no help.

 

[speedster29]

Nevermind, the problem was that the default sew tolerance was too tight. I changed it to 0.1 and now it works fine.

 

[JohnRBaker]

Be careful with making the sew tolerance too large. Contrary to what your model may look like after the sew operation is complete, making the tolerance larger does not actually cause the 'gaps' between sheet bodies to disappear. All that it does is tell the system that you're willing to accept a larger 'gap' in the final model.

When you sew two sheet bodies together and the edges don't match 100% but their gap(s) are within the modeling tolerance, the edges are NOT modified so that they do match. What happens is that the model uses ONE of the edges from ONE of the sheet bodies as the new 'shared' edge of the sewn body (since to be topologically valid, two adjacent faces of a body must share a SINGLE 'common' edge). What this means is that the face representing the sheet body whose edge was NOT used will now act as if the edge that was used is also the edge of its face, which works OK except that mathematically the 'gap' between the old edge and new assumed edge still exists in the model. It's just that NX has been designed so that as long as any downstream applications, be they modeling or some other application like machining or meshing, does not attempt to create any data object smaller than this gap.

Let's give you an example:

Say you have two sheet bodies with a gap of 1 mm and so you set the tolerance to 2 mm and 'sew' the sheet bodies together, which will technically work and it will look like the 'gap' has gone away. However, you may discover later that you will NOT be able to create say a blend or chamfer which approaches 1 mm in size since that would require the code to actually find points on the true faces of the model, but remember those 'gaps' still exist in the data representing the individual faces. However, as long as you don't attempt to create anything near 1 mm in size the depends on either the sewn edge or the faces near the edge.

This scheme, where the models, when sewn, uses one or other of the edges to define the common face edges but which does NOT alter the actual date used to define a model, is referred to as 'Tolerant Modeling', and it's a very powerful capability, as long as it's not abused by using too large a tolerance so as to overcome poorly modeled geometry.

Anyway, just keep all this in mind as you decide between changing the tolerance or redoing a model in order to get it to perform as expected.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[speedster29]

John, I follow what you are saying but don't see where I have any other choice. The N-sided sheet was created using the edges of the adjacent sheet, so the error should theroetically be zero. Apparently the surface trimming operation generates gaps greater than .0254mm.

 

[JohnRBaker]

I was just trying to make sure that everyone understands what's happening when you sew sheets together and what changing the tolerance is actually doing. True, there are times when we have to do what we have to do (after all, that's why we developed the code to work in the manner that it does) but even then we need to be aware of what compromises I may have just made.

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[hudson888]

I'm also not happy if you're using a sew tolerance of 0.1, but for different reasons. Usually we want to sew using tolerances between 0.01 and 0.0254 depending on the job and the client's requirements.

I just don't trust the use of N-Sided surfaces to patch holes in the manner that you're describing. I'm concerned that you're probably trying to solve a problem using the wrong tool or without realising that there are other things that probably ought to be fixed first.

I'd like to see you post a model of the sheets surrounding the N-Sided surface and perhaps the surface that you created.

N-sided surfaces are often used to fill holes of three or five sides seemingly quickly and easily. But there's a price to pay in that they work to a tolerance. So either you look at your tolerances when creating the N-Sided surface to try and tighten them, or you fix the surfaces more thoroughly in other ways.

Surfaces are basically four sided meshes so using odd numbers of sides will involve the application of tolerances. That said the number of sides doesn't necessarily mean the equivalent of the number of edges because two edges that are continuous may chain to form one side of the surface. In fact two edges that are continuous do not work well to represent separate sides because you actually need a corner on occasions where the surface mesh would be expected to cross over in opposite directions. Meanwhile on the other hand you may have what you assumed was a continuous edge which is actually not technically meeting the tolerance for tangency such that the system applies its own tolerance to arrive at an approximate result not quite meeting the selected edge. If you're doing either of those kinds of things to create your N-Sided surface then it will likely be the sort of surface that you really don't want to have in your model and which you need to replace with something else. N-Sided surfaces seem like a quick easy fix but unless you're experienced with surfacing you could be unaware that you're creating more problems than solutions.

You see symptoms of a problems solvable by changing tolerances, but I detect symptoms of geometry that should be corrected.

Cheers

Hudson.

 

[speedster29]

Hudson,

Thanks for the advice. I'm not using the N-sided surface to patch holes or fix problems. I want to create a domed surface for styling reasons; think of a "pillow top" look. Can you suggest a better way to do this?

 

[Xwheelguy]

speedster,

That might depend on what modules you have available. Do you have a Shape Studio license? If so, then a Studio Surface might work nicely.

How about an image of the shape you're wanting to create?

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[speedster29]

No, we don't have shape studio, but I was able to create the shape I wanted using "Through Curves" folowed by "Through Curve Mesh." See the attached picture; first I used Through Curve with three sections in order to create the curved sides. Then to get the pillow top, I extracted all the surfaces except the original flat top, created the Through Curve Mesh using the rails shown, and then sewed all the surfaces back together to get a solid.

Is there any alternative to extracting the surfaces? I come from I-DEAS, and I am used to being able to delete surfaces of a body and then create new ones.

 

[JohnRBaker]

In NX 5 we added a function similar to Ideas 'delete surface of a body'. To use it, go to:

Insert -> Combine Bodies -> Unsew...

Note that after you perform this operation, the 'surfaces' (faces) will still exist so you will probably want to Hide them to get them out of the way (but do NOT attempt to delete them since that will not result in what you want).

John R. Baker, P.E.
Product 'Evangelist'
NX Design
Siemens PLM Software Inc.
Cypress, CA

http://www.siemens.com/plm

http://www.plmworld.org/museum/

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

 

[speedster29]

Unsew does the trick, thanks!

 

[hudson888]

Speedster,

I'm guessing that when you selected the curves for the through curve mesh that the system chained right around the four sides of the feature and created a solid. If I am correct then the solid had a flat to and a flat bottom.

Technically you might be able to create the top surface as a through curve mesh and then patch it on to the solid. However I wouldn't do it that way because I don't necessarily trust the geometry of the original solid yet.

If you have created a solid and using extract faces or unsew your able to get four faces one for each side then fine. but otherwise I would go back to the start and do the following.

Use curve mesh but turn off the chaining but setting the selection method to single rather then connected or tangential etc. Select the three curves top, mid and bottom for each side and create four surfaces. Make the flat surface on the bottom using a bounded place, and the top surface using a curve mesh. Then sew the lot together to create a solid.

This is what I would call the tried and true method as long as your curves are sound you model is pretty much going to be bulletproof.

Cheers

Hudson

 

[speedster29]

I tried setting the selection to single curve with no chaining but it still creates flat top and bottom surfaces.

 

[Xwheelguy]

If you need sewn sheets, you could do one of two things:

1.) Go to Preferences -> Modeling and set the Body Type to Sheet then create your surfaces. This should prevent any Freeform commands from creating solids. Don't forget to change the Body Type back to Solid prior to sewing the sheets into a solid or you will end up with a sewn sheet body.

2.) This looks like a shape that could be mirrored....maybe try creating half of the sides (divide the shape curves by length or the width), mirror, then the TCM for the top and bounded plane for bottom.

Tim Flater
Senior Designer
Enkei America, Inc.

http://www.enkei.com

Some people are like slinkies....they don't really have a purpose, but they still bring a smile to your face when you push them down the stairs.

 

[hudson888]

Are the curves making up the four sides of the pad actually four separate curves for each level, i.e. four top, four mid and four bottom curves? They should not ideally be joined at the corners since any not tangential angle lacks continuity and that can create problems with the surface output.

Best regards

Hudson

 

[speedster29]

So what's tha alternative, leaving a gap and filling it in with a face blend?

 

[hudson888]

No the curves should meet at the corner so that the edges of the surfaces that you create will sew together, but the curves should not be joined across a corner or any other non-tangent point.

This gets into a long technical explanation of surfacing technique that you really need pages of explanation with pictures to explain properly. I'll give you a very much cut down version of the reasons why I'm advising you this way.

It has to do with how the surfaces themselves are created. A good surface has the minimum required number of evenly aligned poles possible to define the shape. Both surfaces and curves are described by poles so that if the curves have uneven poles then the surface will be complex. If the surface maps a break in continuity without recognising the alignment of all the elements across those corners then the surface internals and to some extent the sewn edges might be all over the place. This could lead to all sorts of problems.

Often running examine geometry checks will detect the worst of these problems as surface self intersections, face intersections and consistency errors.

I hope this helps

Best Regards

Hudson