Tek-Tips is the largest IT community on the Internet today!

Members share and learn making Tek-Tips Forums the best source of peer-reviewed technical information on the Internet!

Register Log in
  • Congratulations TugboatEng on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Axisymmetric model in NX 7.5

Status
Not open for further replies.
mobech

mobech

Mechanical
Joined
Nov 8, 2013
Messages
11
Location
NO
Hi,
I'm going to do an analysis on a threaded connection on a pipe. I would first like to make an axisymmetric model of the threaded section of the pipe so that the analysis do not demand that much computer power. Could you guys give me a few tips on how to make an axisymmetric model? I'm using Siemens NX 7.5.
Thanks!
 
Sort by date Sort by votes
It's easiest if you create the full model of the pipe then cut it in half.

So what do you know about creating models in NX ?
 
Upvote 0 Downvote
Not sure exactly what YOU mean when you say you'd "like to make an axisymmetric model". Could you provide a bit more detail please?

Note that the 'Scale Body' function in NX does provide an option to perform an 'Axisymmetric' scaling of a model, that is the ability to set a different scale factor along one axis of the model as compared to the rest of the model. There's also a 'General' option which lets you input three different scale factors, one for each axis of a model as defined by a selected CSYS.

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.
 
Upvote 0 Downvote
The assignment is to do an finite element analysis of a 4.5" ASI threaded pipe. The radius at the bottom of the thread is about 1.5mm, so I need a very fine mesh to do an accurate analysis. So instead of analyzing a 3D model of the whole threaded pipe, I will do an analysis of a 2D axisymmetric model. I would like to know how I can make this 2D model in NX.
 
Upvote 0 Downvote
There's an excellent video tutorial in NX8.5 help showing the procedure for an axisymmetric structural analysis, do you have similar in NX7.5 ?
 
Upvote 0 Downvote
Hello!,
Yesterdy I wrote a post regarding 2D Axisymmetric analysis with NX Advanced Simulation, here you are the link:

original


Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Thank you, I'll check it out!
 
Upvote 0 Downvote
Your post about axisymmetric models explains very good what it is, but I`m finding it difficult to find the functions and how I`m supposed to make the model in NX.
 
Upvote 0 Downvote
Hello!,
Well, the workflow is very easy and simply:
1. Open the part or assembly.
2. Create the FEM and Simulation.
• Solver = NX NASTRAN
• Analysis Type = Structural
• 2D Solid Option = ZX Plane, Z Axis or XY Plane, X Axis
3. If necessary, position the model so that the axisymmetric portion of the model is on positive half of the axisymmetric plane. Axisymmetric analysis requires that the center of rotation and radial axis of the axisymmetric model be properly aligned to the absolute coordinate system. You can use the Reposition Master command to reposition the idealized part.

For the NX Nastran solver:
• The axisymmetric axis is absolute Z
• The axisymmetric plane is absolute XZ for positive X

This means the model must lie in the +X half of the XZ plane.

4. Make the FEM the work part.
5. Open the idealized environment.
6. Split the body: Use the XZ-plane to split the part in two using Split Body command (Advanced Simulation toolbar, Geometry Preparation Drop-down list)
7. Mesh the axisymmetric faces in the +X half of the XZ plane with 2-D QUAD axisymmetric elements.
8. Define the physical and material properties.
9. Apply loads & boundary conditions, solve and postprocess results.

Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
So I'm not supposed to choose "Axisymmetric Structural" under Analysis Type?
 
Upvote 0 Downvote
Dear mobech,
Axisymmetric analysis is supported in the NX Nastran Structural, Thermal, Axisymmetric Structural, and Axisymmetric Thermal environments, and the NX Multiphysics Thermal environment.
Simply choose Axisymmetric Structural, and you are done.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
OK, thank you. I think I'm doing it right now, but when I'm trying to see the solution I get a warning message that says: "Result not loaded" and "Result File in wrong format". Any idea why?
 
Upvote 0 Downvote
Hello!,
This means that the solution gave error. Open the *.F06 (this is the nx nastran output file in ASCII format) located in the same directory as the *.SIM file and look for the word FATAL, there you will have the description of the error.
Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
I`m getting these two warnings:

*** 17:39:06 ***
WARNING : Skipping load and constraint set spc(1)

*** 17:39:06 ***
WARNING : Skipping load and constraint set Force(1)


Not sure what I`m doing wrong...
 
Upvote 0 Downvote
Hello!,
This content never could be part of the *.F06, you are editing the wrong file *.DIAG, make sure you see properly the extension of the files in Windows Explorer and edit the *.F06, OK?.
Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Hello,
Upload the nastran input deck *.DAT file, if seems that no loading exist:

Code: 
 *** USER INFORMATION MESSAGE 5293 (SSG3A)
    FOR DATA BLOCK KLL     
    LOAD SEQ. NO.             EPSILON              EXTERNAL WORK      EPSILONS LARGER THAN 0.001 ARE FLAGGED WITH ASTERISKS
                1          0.0000000E+00          0.0000000E+00
 ^^^ USER   WARNING MESSAGE 9142 (SESTATIC)  
 ^^^ [b]THE SOLUTION FOR THE RESIDUAL STRUCTURE AND THE APPLIED LOADS FOR THE CURRENT SUBCASE ARE ZERO[/b].

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Hello!,
In fact, not loading exist in the nastran input deck. Simply edit the *.DAT file with a text editor and you can see it:

Code: 
$*
$* LOAD AND CONSTRAINT CARDS
$*
$*  NX Load and Constraint: Fixed(2)
SPC            2      19  123456  0.0000
SPC            2      21  123456  0.0000

Make sure you apply loadings EXCLUSIVELY to the edge of the face that you used to mesh with 2-D axisymmetric elements, only loadings in the edge are translated, any load applied to the other geometry will be ignored, causing a WARNING just as the beginning (written in the screen and in the *.DIAG file).

I suggest to ask for CAE training to your NX VAR or RESELLER, the questions you are possing here are very basic.
Good luck and best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48011 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

S
  • Question Question
Reverse Engineering Surface Modeling from STL in Siemens NX
Replies
0
Views
4K
Sennja
S
Nahid Mubin
  • Question Question
Standard Practice for Drafting in NX
Replies
3
Views
8K
GigaManf
G
Jashe
  • Question Question
Sketch Failure Message in NX
Replies
3
Views
2K
Jashe
Jashe
G
  • Question Question
NX Journal
Replies
15
Views
28K
Toost
Toost
Kenja824
  • Question Question
Model Items Selectable in Drafting View?
Replies
5
Views
670
Kenja824
Kenja824

Part and Inventory Search

Sponsor

Back
Top