Metal forming simulation tutorial question

[stuartf]

Hi Everyone. I am busy testing Nastran In-Cad and have been working through a few tutorials. I have completed the tutorial labeled "metal forming simulation using nonlinear material and contact". Everything seems fine and behaves as expected but the simulation ends with the punch and die in the closed position. Is it possible to open the forming tool to see what the formed part would like, factoring in "spring back".

[Andrew.Sartorelli]

Hi Stuartf,

Welcome to the Nastran In-CAD forum! It's not possible to run the analysis in reverse, a non-linear static solution can only have a linear ramp for a load curve. So we can get to a maximum but then not decrease back to zero. You could switch the analysis type to Non-linear Transient and you could define a time dependent load curve for the loads. Use the following steps to give this a try:

1. Duplicate the Analysis
2. Edit the new Analysis and change the type to Non-linear Transient Response
3. Edit Dynamics Set Up 1
   • Set Time Step (S) to 0.05
   • Number of Timesteps to 20
4. Edit Damping
   • Uncheck Structural Damping (This isn't ideal, but for the moment lets do it)
5. Edit the Load
   • Click the button next to New Table for Transient Table Data
   • Enter (0,0), (0.5,1), (1,0)
6. Run the analysis

This should cover converting it to a time-dependent solution, although I haven't run the model myself. You can always look at the plastic or permanent strain induced however by looking at SOLID EFFECTIVE STRAIN-PLASTIC/NONLINEAR ELASTIC. Before a model enters permanent deformation it will show the elastic strain, once one element converts to plastic strain by exceeding the yield stress the result vector will reset and show only the plastic strain.

I hope this helps, let me know if you have any questions.

Regards,

Andrew
______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[stuartf]

Hi Andrew

I will try it out during the coarse of the day and let you know what happens.

[stuartf]

Hi Andrew

I have followed your suggestion however when I edit the load I get a pop up stating that Enforced motion loads are not supported in Non-linear Transient Response analysis.

[Andrew.Sartorelli]

Hi @stuartf,

Ah yes that is correct, I forgot that enforced displacements were used in that tutorial. What you can do is capture the force required to push the die during the non-linear static analysis. To do this, right-click on the constraint for the bottom of the die in the model tree and select SPC summation. Then write down  the force for a few times over the course of the analysis to create a load curve. I think the load curve will end up more or less linear.

Now in the non-linear transient analysis create a force instead of enforced motion. Once you get to 100% load (1second), change the load scale factor to  negative values to get the die to move in the negative direction. This should then allow you to model the die stamping the piece and the die retracting. Leaving you with a formed metal piece, I expected it will retain the shape it was stamped into as it us undergoing a large amount of plastic (permanent) deformation.

Regards,

Andrew

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Andrew.Sartorelli]

Hi @stuartf,

Did you have a chance to try my suggestion regarding switching to a force from enforced motion?

Regards,

Andrew

[stuartf]

Hi Andrew. I did try it yesterday but was unsuccessful. The solver ran for a few hours which seemed excessive and then failed. I have no idea why. I have decided to try again but using a different model, one that is closer to my goal. 

Thanks for your assistance.

[Andrew.Sartorelli · Accepted solution]

Hi @stuartf,

I had a chance to work on your model some more today and got a result that I think you'll be pleased with. Attached is an assembly file that you can place in your directory with the part files and it should run OK. Please look at the second analysis in the file. In this I've created a second sub-case with a dummy temperature load (a load is required by the interface) to allow for the open and closing of the die. The results looked pretty good to me! Let me know if you have any questions.

Regards,

Andrew

[stuartf]

Hi Andrew

Wow, thanks for the effort. I actually gave up on it as I got really busy at work.

[Andrew.Sartorelli]

Glad I could help! Feel free to post any other questions you might have as you get familiar with Nastran In-CAD.

Andrew

[g.ceruti]

HI @Andrew.Sartorelli

I'm a little bit confusing...

In a your previous post you say:

" It's not possible to run the analysis in reverse, a non-linear static solution can only have a linear ramp for a load curve. So we can get to a maximum but then not decrease back to zero. You could switch the analysis type to Non-linear Transient and you could define a time dependent load curve for the loads."

but now, in your file you set up a non linear static analysis with two load steps: first a "loading" step with an imposed displacement and then an "unloading" step with only a temperature load.

[shigeaki.k]

Hello @g.ceruti,

I will try to explain what Andrew meant. If you open up the dialog box for Load in nonlinear static analysis, you will notice that you do not have a way to input the load as a time variant i.e. F(t) using table. Instead you enter the final load value. With nonlinear static analysis, the load is applied in a "ramp" form. For example, if you apply a load of 1N, a portion of the load is applies at each time step, until 100% of the load is applied by the end of the analysis. You will see "OUTPUT SET: INCR x, Load=y" in the bottom left of the work area when nonlinear analysis is run, where "x" and "y" represent the increment number and proportion of the load applied, respectively.

So if you want to model releasing of a load (i.e. unloading) in nonlinear analysis, you need to add a second subcase study with that load removed. The analysis will then gradually remove the load in a ramp form in that subcase study. The only problem is, you need a load defined in a study or the analysis will not run and you will get the message "No load exists within a subcase". To get around this issue, Andrew applied dummy thermal load, allowing the "force" load to decrease to zero.

For more information on how load is treated in nonlinear analysis, please refer to the article below for reference.

"How do subcases function in a non-linear solution type in Nastran"

Regards,

Shigeaki K.

-----------------

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!