Learning Forum

[javat33489]

Hi guys.

I have a problem with flex sheet. I am using bilinear kinematic hardening.

After the sheet is bent and the press comes back, the sheet flies 5000 mm.

Contacts are all friction. I think the problem is in the contact between the press and the plate.

Help me please. I have attached animation and pictures.

[peteroznewman]

This analysis might solve correctly by specifying a large number such as 100 for the Minimum Substeps in Analysis Settings, Step Controls.

[javat33489]

I have a minimum number of sub-stages of 2000 in one direction and 2000 in the other direction

[peteroznewman]

The Minimum Substeps is not the reason for the failure since it is already a large number.

Putting a small radius on the bottom corner of the sheet body might help. That way there will be a small curve touching the line of the die instead of a single node touching the die as the punch retracts. This might prevent the failure you see.

[javat33489]

Okay, I'll try! Could there be a problem in the contacts that I showed in the pictures?

[javat33489]

>>"That way there will be a small curve touching the line of the die instead of a single node touching the die as the punch retracts."

yes, but the punch does not reach the corner, it compresses the sheet to the corner and returns back

 

[peteroznewman]

 

I’m talking about the contact between the sheet and the die. That sharp corner.

Is this a 2D model or a 3D model?

If it is a 3D model, is the flex sheet a solid body or a surface body mesh with shell elements?

 

[javat33489]

>>I’m talking about the contact between the sheet and the die. That sharp corner.

I tried it, it didn't help

>>Is this a 2D model or a 3D model? If it is a 3D model, is the flex sheet a solid body or a surface body mesh with shell elements?

this is a 3d model and solids (rigid and solid)

 

[peteroznewman]

A single solid element through the thickness of a sheet that will experience plasticity is unacceptable. Four quadratic elements or 8 linear elements through the thickness are a minimum for accurate computation of plastic strain.

Try remeshing with 8 linear elements and see if you have the same problem during the solution.

You haven't tried the rounded corner I suggested. That would require opening the solid body in the geometry editor and adding a blend to the edge of the solid body that makes contact with the die on the way up.  That may not be needed after you increase the number of elements through the thickness.

[javat33489]

>>You haven't tried the rounded corner I suggested.

 

I tried it, but I failed when I had one element per sheet thickness

thanks for the advice, I will increase the number of elements, if it does not help, I will make rounding on the edges of the sheets

[peteroznewman]

It will be much faster to solve this problem as a 2D Plane Strain model.

[javat33489]

I made a 2d setting and twisted the plate. But now, after bending, the plate follows the punch. And the problem is solved only if Normal Lagrange is used.

[peteroznewman]

Try turning on Standard Earth Gravity, that might help the part from rising up out of the die.

Also, turn off weak springs if they were turned on under Analysis Settings.

 

[javat33489]

Weak springs are off. I tried gravity. Nothing helps. Perhaps you need to solve the problem in dynamics and not in statics

[peteroznewman]

What is the goal of the analysis? If it was to determine the springback of the sheet after the die retracts, you have that. The rigid body motion after contact is lost can be subtracted off the deformation result.

You could add a small pressure load to the top surface of the sheet. Leave that pressure load on until the punch retracts, then ramp the pressure to zero in the next load step. Then gravity may be able to hold the part against the die.

You could try Transient Structural, but depending on the speed of the punch, the part may to want to launch itself toward the punch due to the springback. You will then have to let it fall back under a Gravity load until it settles in the die, but it might not be sitting level at the end time.

[javat33489]

>>You could add a small pressure load to the top surface of the sheet. Leave that pressure load on until the punch retracts, then ramp the pressure to zero in the next load step. Then gravity may be able to hold the part against the die.

not worked

>>You could try Transient Structural, but depending on the speed of the punch, the part may to want to launch itself toward the punch due to the springback. You will then have to let it fall back under a Gravity load until it settles in the die, but it might not be sitting level at the end time.

Transient Structural has the same problem

>>What is the goal of the analysis? If it was to determine the springback of the sheet after the die retracts, you have that. The rigid body motion after contact is lost can be subtracted off the deformation result.

i want to see the permanent deformation under different load also my goal is to get a residual two-formation of 2 mm, find out what kind of load is needed

[peteroznewman]

The model you have shows the permanent deformation with some rigid body motion. You could export the deformation of the sheet at the end of the simulation, obtain the directional Y deformation of one "pilot" node, and subtract that value from all nodes. The "pilot" node will always have a Y deformation of 0. In that way you can superimpose the offset nodal data to look at differences in permanent deformation between loads.

[peteroznewman]

I expect if you keep increasing the pressure load, eventually, the part will stay in the die as the punch retracts.

I also expect if you simulate a Transient Structural for a long enough time, gravity (or a large acceleration load) will eventually pull the part down to rest in the die.

[javat33489]

When I apply force or pressure to the sheet to press it, the calculation stops with an error while the punch tries to separate from the sheet.

[peteroznewman]

I would be curious to see the model if you would be willing to share the .wbpz archive file on a file sharing site such as Google Drive, Dropbox or Jumpshare, which is what I use. If you use Google Drive, make sure to mark the file so it will download for anyone who has the link.

[javat33489]

ok it's google drive

ARCHIVE

[peteroznewman]

Thanks! I will take a look at this on the weekend.

[peteroznewman]

The archive you shared is not a 2D plane strain model.  It is a 3D model.  See where it says Analysis Type 3D.  That would say 2D if you had a 2D model.  Just having sheet bodies in the XY plane is not sufficient to get to a 2D model.

Once you have built the model in 3D, that analysis can’t be switched to 2D later. You have to start over with a new analysis and set it to 2D before you open the Model cell.

If I start a new analysis, I can link to the Geometry cell, but in the new analysis, I set it to 2D.  Then when I open the Model cell, I can specify what type of 2D analysis I want. In this case it is Plane Strain.

The solution is easier and faster if you take advantage of half symmetry. Here is the result:

It is difficult for the contact algorithm to have the punch separate from the sheet. I used Contact Step control to soften the contact after step 1, then move the punch up to the point just before contact separation, then I made the contact “Dead” in the next step and finally moved the punch up some more.

Here is the ANSYS 2022 R2 archive: https://jmp.sh/kboP9lt

[javat33489]

Thanks a lot!!! I will look into my mistakes!

[javat33489]

Excuse me for my impudence. Do you have time to look at another problem that I have been trying to solve for several months now. It's the lack of chips in LS-Dyna.

I have attached the animation here:

ANIMATION

Issue archive here:

ARCHIVE

[peteroznewman]

Sorry, I don't know LS-Dyna at all.