Consecutive nonlinear analysis

[bocchiardoje]

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?

Thanks!!!

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.

 

[ThomasH]

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

Thomas

 

[bocchiardoje]

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

I solve the problem!

Like "jbrackin(Structural)" said in post:

http://www.eng-tips.com/viewthread.cfm?qid=345267)

--------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
"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

 

[bocchiardoje]

I send to you the second and third consecutive nonlinear analyzes *.dat

 

[bocchiardoje]

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!

 

[ThomasH]

Hi

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.

Thomas

 

[RealSaladsamurai]

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

 

[bocchiardoje]

Thanks to both of you! ThomasH & RealSaladsamurai