NX5 threads

[jerry1423]

I am running NX5.0.2.2.
We do our drawings using master modeling.

I am having a problem with my threads showing up correctly in a drawing view. The tap drill shows up fine, but the threads do not. We us "ANSI simplified" to show our threads.

I have made sure that the thread curves are in the reference set, and they are in the proper layer, but they still do not show up in the view. They show up fine in the model, but without silhouette curves.

Any suggestions would be appreciated.

 

[JohnRBaker]

I have no problems at all getting a properly displayed threaded hole in a master model drawing, as seen in the attached image, using NX 5, true it's NX 5.0.5.2, but it does work.

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/

 

[hudson888]

Jerry,

It shouldn't matter whether the thread curves are in the reference set or not. I don't know why you think silhouette curves have any bearing.

There are two ways you can apply a thread in modeling Symbolic and Detailed, they're both under the same dialog. You're describing using the symbolic method which visually appears in modeling as a dash circle at either end of the thread describing its root diameter and length. The detailed method creates faithful 3D modeling feature of the helical thread form, in other words it looks like a thread, but it doesn't serve as well for the symbolic methods used in drafting.

There are ways of showing threads in drafting also and they are found in the View Style under the Threads tab. So if your problem is in drafting then you may have it set to none.

For testing purposes create a block with a hole and a symbolic thread and then in the same file go into drafting add a top and side view then going into the View Style Thread tab cycle through the options. Compare that with the part where you found the problem and you ought to be able to diagnose the problem.

Also if you're using linked geometry threads to not get wave linked they need to be re-applied.

Best regards

Hudson

 

[JohnRBaker]

Hudson,

Starting with NX 5.0.2.2, the preferred way to model a threaded hole is to now use the Threaded Hole option which is part of the new Advanced Hole Feature.

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/

 

[hudson888]

Good Point John,

Yes I prefer that method too.

For the purposes of my explanation above the threaded hole option in NX-5 produces a symbolic thread. So that Ben ought still be able to experiment in the same way should he use that method and come to an understanding about what his problem involves.

Ben,

I was getting to the point of just describing the possibilities because the question itself seems to need some other piece of missing information that you may only be able to provide by experimentation. It sounds to me like something really specific is missing, and I wouldn't mind if you posted some pictures of what is wrong and what you expected. Let us know if similar geometry works differently for you in earlier versions of NX.

Cheers

Hudson

 

[JohnRBaker]

For the record, as mentioned by Hudson, the arcs that you see when looking at a model with threaded holes, be they the older legacy Hole + Thread feature or the new NX 5.0.2.2 Threaded Hole, are of value only as a symbolic marker for the model. When you create a drawing, the software is keying off the 'feature' data itself that is part of the hole feature, either appended by adding the symbolic thread feature to a legacy hole, or as part of a Threaded Hole feature itself and therefore does not NEED to see the 'arc' when in the drawing file. That why Master Model works despite the fact that the arcs got left behind in the original piece part file.

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/

 

[ewh]

While it is reassuring to know that NX "knows" where a threaded hole is, it would be helpful if it were always shown as such on the screen.
Several times I have created arrays of threaded holes in NX5, and only the first hole(s) show the symbolic thread curves. This can be disconcerting when you are used to wysiwyg.
I have also seen this occur when using multiples of the same component in an assy drawing (master model).

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[jerry1423]

These threaded holes were done using the latest and greatest NX5 method.
I think the problem is what ewh mentioned: the threads were arrayed, and the curves for them (except the parent) needed to be forced into the reference set.
The reason I mentioned the silhouette curves is because I never had a problem with them showing up in the model, until now.

I just lived with the threads as they were, and view dependently added the thread silhouette curves, like back in pre-solid days.

 

[JohnRBaker]

I still don't understand what the problem is. Attached is an image of a part which was created using the new NX 5 threaded hole feature which I then arrayed and then I explicitly removed the arcs from the Reference Set and then created my Master Model drawing and everything still looks correct. As I said, drafting is supposed to KNOW what a Threaded Hole looks like and does not depend on anything other then the data included in the feature itself.

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/

 

[hudson888]

Jerry,

What thread standard do you use. I am beginning to wonder and in which view relative to the hole are you looking when it fails to work. If you take a view from above the hole so that the hole would appear as a circle then the ISO thread standard shows the thread as a thin line with one gap section. If you use the ANSI thread standard then the hole would appear with a thin dashed line shown approximating the OD of the thread. Now since the dashed lines indicating a symbolic thread in modeling approximate the ANSI representation used in drafting, are you confusing the two?

Best Regards

Hudson

 

[ewh]

Here is an example of what I am seeing. Both sections were taken at different angles thru the same block at the axis of the threaded hole. This one appears as expected.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[ewh]

This one is missing the thread curves in the block. Same parts, same axis, different angle about axis.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

OK, this might be it. Check the Style -> Section of each view and make sure that you have NOT toggled on the 'Hidden Line Hatching'. Note that 'Hidden Line Hatching' is not intended for orthographic views, but rather when creating isometric break-out section views in which case threads are not intended to be rendered anyway.

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/

 

[ewh]

Hidden Line Hatching is toggled off in both views.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

OK, remove the screw and see if anything changes.

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/

 

[ewh]

I removed the screw, double checked that the section was indeed through the hole axis, and updated the view. Still no thread curves.

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

Can you send/post the part file?

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/

 

[ewh]

John,
I don't think management would appreciate it. I did however try to recreate the problem by exporting the parts in question as new parts and re-assembling them, and the problem went away. I'm going to go back and double check the constraints I used in the initial assy.
While this problem is looking like a red herring, I am still puzzled over the threaded hole array problem. Unfortunately, it's been a couple of weeks since I have experienced it and will have to research just what part(s) I was having trouble with.
Thanks for your time!

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]

 

[JohnRBaker]

One last thing to try, which shouldn't make a difference but I do see that you two views that you sent images of did have a slight difference. The view that worked had the 'Background' option toggled ON, while the one that didn't looked like it was toggled OFF. This shouldn't make a difference, but it's the last thing I can think of.

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/

 

[ewh]

I don't think it should make a difference, either, but it did. They show up with the background toggled "on" (as does much unwanted geometry).

Believe it if you need it or leave it if you dare. - [small]Robert Hunter[/small]