Centerline extraction at a system level in NX

[jrhagen]

I have been struggling for a couple of days with a task and was hoping someone on the forums could help out. I am a contract designer with an aerospace company working on an APU. I have been tasked with doing some nodal analysis for a fuel supply system using NX and NX advanced simulation package. The tubes in the fuel supply system were created with mechanical routing. I have worked out a way to extract the mechanical routing centerlines by exporting thru IGES. That process works great for a single part, however it does not work at an assembly level? The person who I am working for does not want to use the solid models for nodal analysis directly. They want to extract the centerlines for tubes and clamping locations and build up the solids/mesh using the 1D idealized elements in NX advanced sim.

Does anyone know how to extract centerlines at an assembly level from tubes using mechanical routing tools? The end result is to have all tube centerlines and profile of clamping locations contained in a single file. Thanks in advance for any help.

 

[cowski]

I'm not familiar with the mechanical routing package, but I assume the tubes are created based on the same method in modeling. If so, there should be a defining centerline in the tube part file. If the tube is a component in the assembly you should be able to create a reference set in the tube file that contains the defining centerline spline. At the assembly level, change the tube file's reference set and the centerline should show up in the assembly.

www.nxjournaling.com

 

[jrhagen]

Yes that was basically my process for single tubes. I exported to IGES and made sure coordiante systems and curves where checked on for the export. I just exported the tube model and left the nuts and sleeves off. I then just put a fix constraint on every node on the bottom of my tubes where they would be coupled to the nut.

My issue is trying to get that same behaviour when exporting an assembly of tubes. I made sure the reference set was set to entire part at the top level and all sub assembly levels before exporting. If I have coordinate systems and curves checked on I get nothing when I export. If I turn on solids I do get a dumb solid assembly as would be expected, unfortunately a dumb solid meshed model is not my deliverable. They want an idealized 1D element model using the predefined beam, clamp, fastener, and other elements.

I should mention we are on NX 7.5.3 (the .3 may be .5 I forget which one we are on now) and are using Teamcenter. I have exported everything to a native instance of NX and have confirmed all models and the top level assembly open good using only native NX.

 

[jrhagen]

One last thing. The tube centerlines seem to behave a bit differently than standard curves. They are all made with links and ports to external references in the assembly. I did of course break links and isolated the elements before exporting. I was able to open each tube model on its own and they were not missing links after isolating everything.

 

[cowski]

When you open an individual tube model, is there a spline that drives the shape, or is it all driven by the links and ports at a higher level?

www.nxjournaling.com

 

[jrhagen]

When I open just the individual tube model yes there is a centerline that drives the shape of the tube. I made all the control points non-associative before bringing them local. Single tubes work great, its just an assembly of tubes in my global APU coordinates that is giving me issues. I did try to add a commmon coodinate system to each model and activated that as the WCS before trying to bring everything over as an assembly that didnt seem to help either. That was when i was going to try and do each tube individually and reassemble them in space. They still all came in right around the orgin because that is how they were modeled. Adding the common coodinate system seemed to do nothing, it continues to just drop everything for all parts right at the orgin both as an assembly and as an exported dumb solid multi-body part.

 

[JohnRBaker]

Try giving the attached NX Open program a try (after downloading the file, edit the file extension from '.zipper' to '.zip' before attempting to extract the files).

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.

 

[jrhagen]

I do not have too much experience running NX Open files. I tried to launch it and got the error:

Failed to load image - see log file for details

File name Cocuments and Settings\myusername\Desktop\Cable_centerline1\Cable_centerline1.dll

Function name: ufusr


After looking at the log files it basically says the exact same thing as the error. I ran it while in modeling, do I need to switch to another NX application before running it? I tried running it from the Desktop and out of our NXOPEN folder in our installation.

 

[jpetach]

Jrhagen,

If your version NX is 64 bit and the dll is for 32 bit NX it could produce that message.

HTH,

Joe

 

[jrhagen]

Yup we are on 64 bit.

 

[jpetach]

Jrhagen,

Here's a 64 bit version for NX 7.5.

HTH, Joe

 

[cowski]

If the centerlines already exist in the model files and all you need is to have them at the assembly level, you should be able to use the "entire part" reference set in your assembly (or create your own new reference set in each part that contains the centerline). Unless there is another requirement I have missed?

www.nxjournaling.com

 

[Toost]

I'm late into this discussion but, I still don't understand why you are exporting the Iges files.
You have the model in NX and intend to run the simulation in NX , correct ?

When working with NX routing, the tubes can, depending on the setup in your company, either be assembly components ( "Stock As Components" =SAC ) or "Assembly level features" ( "Legacy Stock" =LS)
If they reside in separate files, using the reference set "Entire Part" on that component should display the centerline ( the "Path" in Routing terminology)
If they reside in a sub assembly (LS in that part) Then again Ref Set entire part on that subassembly should display the path.
If they reside in the top assy ( LS) and invisible, the layer containing the "path" is invisible.

The "Routing Path" is regular curves such as lines/arcs/splines but with added Routing functionality. They should be usable directly as curves in another application.

Regards,
Tomas

 

[NXsupport]

Is there a executable to work with NX6.0.5.3.. We are behind the crowd in upgrade of NX..
Both the executables from John Baker and Jpetach gave the error message

Failed to load image - see log file for details

File name Cocuments and Settings\myusername\Desktop\Cable_centerline1\Cable_centerline1.dll

Function name: ufusr

We are on Windows 7 and 64bit..

Appreciate if I can get any help on this

 

[FrankSwinks]

I wrote the original program quite a while ago. It does not work for the application under consideration for several reasons. The first is that it was written specifically for the case when the tube/blend/extrude was a b-surface. This is the case only when these faces have been imported or extracted as a b-surface. Therefore if the face is not a standard b-surface the program will error out. The second reason is that the original program has not been signed.

I don't have routing but if you want a program to create centrelines for tubes I think I can do this. Let me know.

Frank Swinkels

 

[NXsupport]

Hi Frank,

Yes please I would appreciate if you can get me a program which when run on tube or circular profile sept along a spline in 3D and this body got exported a parasolid or something which is not having any parameters , will give me the central line .. This would be of great help as there is no option in NX to achieve this..

 

[FrankSwinks]

NXsupport

Attached is a zip file which contains a journal for testing. Just change the .txt to .vb. This journal works for several cases. If the original is a sheet body (as is the case of tubes) then the program works fine. If the case is a body with a number of faces (say the example of an extruded circle but is a solid body and not a sheet body) you need to use Insert->Associative Copy->Extract Body. You need the type as Face and the surface type as Polynomial Cubic. The program also work for blends when the blend face is also copied as above.

Frank Swinkels

 

[jrhagen]

Just to give a follow up, I ended up recreating the centerlines using points, lines and bridge curves to use for my 1D elements in advanced sim. The customer really wants to use a dumb solid model and just do 1D analysis from the centerlines so there are not tons of links in TC going back and forth between the analysis effort and the actual tube models. IE it may be required to release the tubes ahead of the analysis so we can start building them. If I did the analysis to the actual models in TC I would not have been able to release them due to customer release rules within Teamcenter.

 

[NXsupport]

Thanks FrankSwinks .. That works like a charm..