Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


Consecutive nonlinear analysis

Consecutive nonlinear analysis

Consecutive nonlinear analysis

Hello to all!
A little introduction of me: My name is Jorge, I´m aeronautical engineer from Argentina, but now I'm working in Brazil with FEMAP /NASTRAN for 5 years.

And now, the question/problem: I want to make 2 consecutive nonlinear analysis in the same model.

The FEM is the typically specimen used to make a traction test, but this one have a hole in the middle, made on aluminium. Please see the attached file!

In the first analysis, I need to deform plastically the model simulating an expansion of the hole using a special tool (Coldworking fastener holes, http://coldwork.com/about/coldwork ). I simulate this using enforced displacement in radial direction with a cylindrical coordinate system. Some part of the model will stay deform (with residual stress?) and other will back to zero displacements.

In the second analysis, I have to start from the previous deformed model but with the residual stress state, not only with the displacements (I know how to use this tools: CUSTOM TOOLS > POSTPROCESSING > Nodes Move by Deform with Options, from this previous forum: http://www.eng-tips.com/viewthread.cfm?qid=345267, but I don’t want/need to use that).

I don’t want to combine both load cases and make one nonlinear analysis, because I want to simulate the process, so I think that I need to create “subcases” but I never have done that yet.

I don´t have problem to run each analysis. They converge and I get the expected results.

Someone can help me?


My mother tongue is spanish, I know portuguesse, and and I try to speak (or write) in english, So feel free to answer in any language.

RE: Consecutive nonlinear analysis

What version of Nastran are you using (MSC/NX/NEi(Autodesk))?

Normally for a nonlinear solution it goes like this.

First subcase you add 100 N. So you use the load 100 N.

Second subcase you add 200 N. Then there are two options, either you go from subcase 1 and increase load from 100 N (including the deformations and stresses) up to 200 N. Or you can go from 0 to 200 N.

In NEi Nastran there is a parameter NLSUBCREINIT that controls the sequence. For the other options I'm not sure.

But I think that the normal for Nastran is that nonlinear subcases are accumulated. Meaning 0 N to 100 N to 200 N.

It should be easy to test by plotting the deformations.

Good luck


RE: Consecutive nonlinear analysis

Hello ThomasH! Thanks!
I'm using Femap with NX Nastran.

I solve the problem!

Like "jbrackin(Structural)" said in post:
"If you really just desire to apply a loading history with different loads being added or subtracted as you continue the analysis, then you just need to create subcases in the nonlinear solution. Each subcase should completely define the loads desired for that subcase, in other words, do not add an "incremental" load, apply the total load desired for that particular subcase. Nastran will automatically find the "delta" load by comparing to the previous subcase.
subcase 1 = preload only
subcase 2 = preload + mechanical load
subcase 3 = preload + mechanical load + thermal load"

My problem was that I have different boundary condition, so I couldn´t do the simulation in that way. I solved the problem doing the next:

1) First analysis: Nonlinear analysis of hole expansion with enforced radial displacements (I have to set constraints in that direction to work properly).
2) Then I took the results of the previous analysis and I create a new load set, but with forces. Replacing the enforced displacements by loads in the hole (causing the same displacements). I used this tool: MODEL>LOAD>FROM OUTPUT>NODAL FORCES>CONSTRAINT FORCES & MOMENTS
2) My second analysis was with that new load set, but with the same boundary condition that I will gonna use in the next consecutive analysis. (The result was the same, of course)
3) Third analysis: the same previous load set (expansion of the hole with forces) + plus the set to traction the specimen!

And that's it! work :D

RE: Consecutive nonlinear analysis

Maybe the best and fast way to perform this both analysis, is using "restart" option.
But I can't figure out how to do it yet!
If some know how to do it, I'll be glad!

RE: Consecutive nonlinear analysis


Good to know that if worked out.

Regarding "restarts". I don't use them often but I know that when I did there were some good tutorials avaiable. But I don't rememder is they were for NEi or MSC. I'm pretty sure it wasn't NX.


RE: Consecutive nonlinear analysis

Hi bocchiardoje! I am very new to FEMAP, so I am not sure if this will help you. But, under HELP > EXAMPLES if you navigate to "Example 16 Modal Frequency Analysis of the Hinge Model" they explain how to do a modal analysis and then use "restarts" to expedite the frequency response analysis. I believe that they are assuming that you are using NX Nastran, but I am not positive. It may or may not be useful for you!

Best of Luck!

NX7.5.5.4 - Teamcenter 8
ANSYS Workbench 14.5

RE: Consecutive nonlinear analysis

Thanks to both of you! ThomasH & RealSaladsamurai

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members! Already a Member? Login


eBook - 10 Reasons to Choose CATIA on the Cloud
To compete in today’s fast-paced and competitive market, smaller and newer firms need a powerful platform that will enable them to compete with bigger players, without the heavy investments needed in computer hardware, software and personnel. Download Now
White Paper - Smart Manufacturing for Electronics
This white paper describes a transformative approach to electronics manufacturing made possible by the addition of Mentor Graphics to the Siemens family. It describes a completely digitalized strategy that supports both printed circuit board (PCB) and mechanical design and manufacturing, uniting the entire product lifecycle – from idea and production to customers and back. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close