Showing results for 
Search instead for 
Do you mean 
Reply
Solved! Go to solution

NX Nastran for plastic deformation in profile bending

Hello,

 

I am currently learning to use Abaqus to simulate a bending process. I have an aluminium profile which will be bent with permanent deformations to achieve an angle. In the current setup I am using two stationary rollers at the bottom, and one above the profile which will move downwards unti the correct angle has been achieved.

 

To my (limited) experience Abaqus is very well suited for the task either using dynamic implicit or dynamic explicit solver. However, Abaqus is very difficult to use, as it is not at all user friendly.

 

So my questions are therefore: 

1.) Does anyone have experience using NX for plastic deformations? Compared to Abaqus?

2.) Can NX10 run both dynamic implicit and dynamic explicit?  Which solver?

3.) Can anyone point me in the direction of some tutorials/examples/videos(youtube) which go through the process of creating and running such a type of simulation?

 

Keeping my fingers crossed. 

 

-Andreas-

13 REPLIES
Solution
Solution
Accepted by topic author AndreasMH
‎06-14-2016 04:54 AM

Re: NX Nastran for plastic deformation in profile bending

Don't bother attempting such type of analysis with NX nastran.

ABAQUS is one of the best tool for that sort of analysis and I have never heard that it is difficutl to learn! With ABAQUS.CAE creating the model and setting up the analysis is (very) easy. It's been a while since I have used it but difficult is not a word I can remember (and I was slef taught!). The type of analysis you are trying to do might be difficult but that's another issue

Production: NX9.0.3.4, NX10.0.2.6
Development: VB.NET (amateur level !)

Re: NX Nastran for plastic deformation in profile bending

Thanks a lot. 

 

I have sort of come to the same conclusion after speaking with other FEA-guys. It's just that the licensing scheme for NX is far better than for Abaqus (and ANSYS also), because I can use as many cpu cores for parallell processing as I have available on my workstation.

 

Anyaway, I have reached a point where my simulations seem to run(in Abaqus), though with some warnings etc. 

 

Have you ever tried the program Deform 3D before for plastic deformation? Excellent software.

 

 

Re: NX Nastran for plastic deformation in profile bending

NX Nastran Advanced Nonlinear solutions can be used to perform this simulation. SOL 601,106 is an implicit nonlinear static solution. SOL 601,129 is an implicit nonlinear transient solution and SOL 701 is an explicit solution.

 

For the analysis you describe, SOL 601,106 would be sufficient. It allows multi-linear plasticity and 3D contact.

 

For more information, see:

 

Re: NX Nastran for plastic deformation in profile bending

How do I define the materials to be elastic and plastic. I don't know if I made myself clear but I wanted to define the aproximation between Elastic and Plastic behaviour, the slopes of the stress-strain like in this picture:

 

http://www1.us.elsevierhealth.com/books.elsevier/companionsites/JenkinsKhanna/mmd/yieldpoint/Image16...

 

Thank you

Re: NX Nastran for plastic deformation in profile bending

NX Nastran Advanced NL (SOL 601/701) would fare just as well as Abaqus.  But if all you have is SOL 106, then life might not be entirely festive, as selex_ct pointed out.

 

As for SMP, I don't think SOL106 would do much better with multi-cores, so the licensing advantage would probably not help as SOL106 wouldn't scale with cores like Abaqus would...  SOL601 probab;y would.

Re: NX Nastran for plastic deformation in profile bending

Yes, I am able to use SOL 601,106 and 601,129. I will need the transient solution because I will be simulating a crash with an acceleration function. My question is: how do I create a material and introduce plastic behaviour? What are the steps?

Re: NX Nastran for plastic deformation in profile bending

Isotropic plasticity is defined via a combination of MAT1 and MATS1 cards. If the MATS1 card is present, the solver will automatically use the material data at runtime.

 

See section 3.4.1 of the Advanced Nonlinear Theory and Modeling Guide

Re: NX Nastran for plastic deformation in profile bending

[ Edited ]

Thanks for the reply.

However, most of the materials I am using is custom, therefore I wanted to know what to write in their properties. Just a quick question just  to know If what I am doing is correct so far: Initial Yield Point (LIMIT1) is when it changes from elastic to plastic and Stress-Strain (H) is the slope of the plastic part of the stress-strain function, right?

Re: NX Nastran for plastic deformation in profile bending

Yes, for a bilinear curve, E is the slope of the linear segment, LIMIT1 is the inflection point and H is the slope of the plastic segment.

 

For multilinear, the first point in the stress-strain data table is the inflection point. Note that the software will compare the slope between (0,0) and the first data point to the specified value of E and report a warning if they are not equal (within a tolerance).