ANSYS Workbench contact metal stamping problem

[JoelHenrik]

I have a problem that requires me to do a simple simulation of a sheet metal stamping. I have access to Ansys Workbench v12 Academic version, and have familiarized myself with the program and tried to read up on its features and limitations.

The simulation is selected as a static structural.

The boundary conditions are set as:
* The lower die-tool underside is set with a Fixed Support
* The upper die-tool vertical sides are set with Frictionless support, to allow a movement in the vertical direction.
* The sheet metal plate´s long sides are also set with Frictionless support, to prevent a possible Rigid-body motion, but still allow a vertical press movement.
* The upper tool is applied with a displacement towards the second tool.
* There is a initial contact between the platesurfaces and the tool's pressure surfaces.
* There a two sets of contacts. First, the upper tool´s whole stamping-area and the surface of the plate that it intersects with. Second, the lower tool´s surface and the bottom surface of the plate.

My problem occurs when I am applying the contact conditions for the contact area. Ansys choice is initially a bonded contact, and simulations can be done. However, this does not simulate the reality as we do not allow room to stretch and slide the plate. I would therefore choose a Frictional contact and puts friction to about 0.3, just to test out. Then the simulation would not converge, and the upper tool glides right through the plate without being aware of when a contact occurs.
Could it be that Workbench is not allocated for this type of simulation, or do I choose the wrong settings?
Would any kind person be able to explain if this is not possible, and if so, what restrictions of the program that causes this?
J-H

 

[minger]

That is a difficult problem to solve, as it encompasses many "advanced" ANSYS features. It seems that you are still relatively new to ANSYS, seeing as how this involves contact and possibly large deformations of the middle piece, it's certainly jumping in head first.

One thing you'll find: Contact elements are a [insert favorite derogatory word].

What I'll recommend is to seriously learn ANSYS Classic (or Mechanical APDL for v12 users). It allows users, particularly in complex analyses such as these, more control over the solution.

Especially when it comes to contacts, it really helps to be able to manually create the elements so you can make sure the element normals are facing the right direction, the formulation is how you want it, etc, etc.

If you insist on staying in Workbench, you'll probably need to play around with the contact settings (there are a TON). They will all mess with convergence and performance, so read up. In classic, you specify them via real constants when you create the elements. In workbench, you'll have to go through the output file, find which real sets they belong to, and manually change then via a /PREP7 command snippet.

 

[Mech_Engineer]

This problem can be solved in Workbench, but you'll need to make sure you've got your settings right. There's a LOT to be taken into account here, so I'll try to cover a few tips at a time because otherwise my post will be a mile long:

1. Pay Close attention to your mesh density in the sheet metal being bent, as well as in the contact conditions that are moving it. The mesh should be of similar size on both sides of the contact, you can use a "contact condition mesh refinement" to make sure this happens.
2. Make sure you use an "Augmented Lagrange" formulation for the contacts between the sheet metal and press. This formulation will work best with sliding conditions.
3. As a start, make the contact condition between the sheet metal and press frictionless. Once you get it to converge, then you can think about considering friction.
4. Make sure your contact condition forces update every substep, and split your problem into MANY substeps (on the order of 100).
5. Make sure you have accurate material data for your sheet metal, especially into the plastic deformation region which you'll be probing specifically.
6. Remove the "frictionless supports" which are nonlinear boundary conditions that I suspect will cause you undue grief, and replace them with fixed displacement conditions (0 displacement in axis perpendicular to surface).

That's a good start anyway... I'm not sure of your limitations using ANSYS Academic (the mesh is limited to what, 10K nodes or something?), but hopefully this will start getting you in the ballpark.

 

[nvn]

Perhaps ensure you are selecting options such as large displacement, nonlinear. Ensure you are using a small step size, have a small-enough element size, and good mesh quality. If it continues to fail, perhaps try Solution controls > Advanced NL > Arc-length method (?). If it continues to fail, ensure the academic version allows advanced analyses.

 

[JoelHenrik]

Sorry for not following up on this right away! Mech_Engineer's work really good, and the simulation went trough after some testing, thank you!

But I did encounter a new problem that I am not sure can be handle within WB. After I have pressed(stamped) my plate to the right geometry and released the die&tool so the plate wouldn't suffer from any elastic deformation, I would want to continue my analysis.
Basically I want to subject my deformed plate(with built-in tension and plastic deformation) to another load environment. My first thought was to have two loadsteps and in the first one going trough my stamping process, and in the second one deactivate/suppress certain bodies and connections and activate some new bodies and contact connections.

In this way I would have two setups with bodies(and the contacts that would be needed), and I would be able to perform a two-step simulation?

Is that possible?
Best regards Henrik

 

[jmart157]

Reviving an old thread because I need help with something similar!

PM me!

 

[Mech_Engineer]

Reviving an old thread because I need help with something similar!

PM me!

Why don't you just post your problem in here so EVERYONE can help?

 

[jmart157]

https://www.physicsforums.com/showthread.php?p=3445330#post3445330

I thought I did last night. Different forum, my mistake!

 

[tomahawk7]

Hi, I have similar problems, I'm modeling with ansys wb 12.1..I searched all over the guides but couldn't find, even in the contact technological guide, a guide which clarifies the 1000 options in the contact windows(formulation, interface treatment, offset...)
Can you help me?where I should look, I really cannot continue to randomly change things :)
thank you!

(i'm using a transient structural (ansys) analysis )