1 sketch, 2 extrusion lengths

[napanorton]

Hi, I'm trying to build a simple assembly up. Basically its a frame made out of 1" square tubing. I'd like to create one file that is the cross section geometry of the tubing, then place it in the assembly 4 times. The catch is I need two different lengths for the width and height. How do you do something like this in NX? I can figure it out if I make two part files, one for each length of tubing, then adding two of each to the assembly. The problem with this is I have to redraw the tubing cross section each time. And what about when I want to make a more complex structure out of 1" tubing?? Thanks!

 

[JohnRBaker]

While the name may be counterintuitive, this can be done using a 'Deformable Part' where the 'variable' is the length of the extrusion.

That being said, if you DID decide to create two part files why do you say that you have to create the cross section TWICE. Just create one part with the length set to the first value, save it, then edit the length to the second value and do a save as. Now you have two parts each with a different length but you only had to create one model.

Now if the length of the tubing is going to be predetermined sizes, say 10", 12", 14", 16", etc., you could do this with a Family Table where you create a parametric model with the length as a variable and create your table filling in all of the possible lengths that you will need. Then when you need to add a tube to your assembly you simply add the part and select the needed length from a list of available lengths that has been predefined in the family table.

What version of NX are you using?

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.

 

[napanorton]

Wow, thanks for a quick reply. I'm using NX 6. The reason I didn't want to do a Save As because the first part is already referenced in the assembly. If you do a Save As, NX wants to help and update the assembly somehow - which I don't really understand at this point. I won't have stock sizes, so the Family Table approach probably won't work. I'm also realizing I may have 3 sections that are 36" long, but they might have different miters trims on the ends, Does this mean I have to make part files for each variation?

 

[JohnRBaker]

Why have the assembly open when you're performing the 'Save-As'? Just do it when it's the only file open.

Attached is an assembly made up of 4 components which have all come from the same master part. The master part is a 'Deformable Part' where you can control the length and the angle of the beveled end.

Anyway, give it a try see what you think.

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.

 

[eex23]

Hi John,

I opened your example (with nx8) and tried to make some constraints. try to deform red tube, and you will see strange results for yellow tube.
As far as I can remember, deformable parts always messed my assembly and I decided not to use them at all.

 

[Walterke]

2 question:
1) what if one would want tubes of different length to have different part names?
Would you have to put the deformable part inside the different partname-part?
2) when I deform the vertical tube to 35inches, the one connected to it moves away and the constraint is bugged. See attached screenshot. What am I missing?


NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[eex23]

As I mentioned in my previous post, deformable parts always messed my assembly, if you constrained some other parts to it. I have never tried to use wave links with deformamble parts, but I think I will test it

 

[napanorton]

So its sounds like unless I'm willing to use the deformable parts approach, I will be forced to make a new part for each version of tubing I need. For example, I would need to make a separate part file for each (assuming all the same tubing cross-section):
36" Long, 45 on one end
36" Long, 45 on both ends
42.22" long, 90 on both ends
6.2" long, 45 on both ends
etc....

Somehow this seems like the wrong approach. What other strategies can be used?

-- Thanks, David

 

[cowski]

If you are building one frame assembly, it may be overkill. But if you think in terms of mass production where multiple people and/or machines are cutting the tubes to length and you are controlling inventory, having an individual part number for each tube part doesn't seem so "wrong".

As an alternative, you can build the entire frame in a single file, simply reusing your sketch as needed. It will take a bit more work to generate a BOM from this file if one is needed.

You might also try promotions and/or interpart modeling. The pros/cons depend on what your goals and expectations are.

http://www.nxjournaling.com

 

[JohnRBaker]

If you're going to be doing a lot of this, perhaps you may wish to look at our Mechanical Routing package which while it was originally intended for things like piping and tubing, it can be adapted to 'route' any shaped defined using a 2D profile. It provides many additional tools like generation of BOM's, 'cut lists', support for standard stock length so that you can optimize the material used to reduce scrape and so on.

For more information, go to:

http://www.plm.automation.siemens.com/en_us/products/nx/design/mechanical/routed.shtml

You will also find a link on this page to download a .pdf document which goes into much more detail about what you can do with the Mechanical Routing package and what many of the features and capabilities of this product.

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.

 

[eex23]

John, so whats about deformable parts and assembly constraints?

 

[JohnRBaker]

...try to deform red tube, and you will see strange results for yellow tube.

It worked fine using NX 8.0.2.2 (see attached video) so perhaps there was something which has been 'adjusted' in the latest MR, which should be ready for primetime later this week.

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.

 

[eex23]

Hi John,
Thanks for your post. Please take a look at the attached video. This is again nx8, but as you can see, then the lenght of the deformable component is reduced, the constraints seem ok. and the the lenght is increased - constraints fail.
So could you check this in nx8.0.2.2?

 

[napanorton]

All - thanks for the help!

cowski - I think you're tip was the key for my problem. I was able to figure out how to reuse the sketch repeatedly within one part file. Now all I have to do is figure out if you need to also copy the datum coordinate system each time you copy the sketch as well. I haven't exactly figured out copy/pasting just the sketch.

-- David

 

[JohnRBaker]

I followed you exact same sequence of dimension changes using NX 8.0.2.2 and it worked fine.

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.