deep drawing tutorial

hamit_hushoni

hello everybody..
im studying numisheet 2018 bm2.. can help me tutorial deep drawing..
thank you

Victor

The PipeClip.liml example in the manual and Samples folder might be a place to start. Add plastic material and more parts. The common features with deep drawing are contact and time dependent prescribed displacement.

Beware though that people seem to run into problems with deep drawing. There are limits to how severely you can deform it. In part because the contact sometimes fails at corners, and in part because it doesn't regenerate the mesh as it deforms so elements may become too distorted. Refinement can help to some extent.

Another problem is that it might not be possible to simulate anisotropic plastic behavior with CalculiX or Mecway. You can have anisotropic elasticity with isotropic plasticity but maybe not both.

I've heard that it's better to use hex elements so revolving the mesh from a 2D shape would be a better way to generate it than meshing a STEP file (tet only).

If you already have the geometry, I can help set up the analysis.

hamit_hushoni

thank you mr. victor. i will try it... the geometry same with numisheet 2018 bencmark
2,,

takziawa

Hello.
The blank holder is needed in BM2.
B.H. is controlled with constant load. it's little bit difficult to set up......

Victor

Yes, that's more tricky. I would constrain the stripper with a weak spring to oppose the holding force and ramp up the holding force so that the full 50 kN is not applied until after the contact closes.

hamit_hushoni

mr viktor and mr takziawa thank you so much,
this is the first deep drawing simulation for me, so I still have a lot of confusion and haven't got the examples or tutorials yet. can mr. takziawa or mr.viktor have sample videos for deep drawing, I would be very grateful for that

Victor

Here's some steps to get started. From this, you can solve it and get some kind of solution but it doesn't yet have:

• Holding forces
  
• Plastic material. See manual 14.1 Custom model definition for an example.
  
• Friction. Set it in the contacts. But it's better to start without until you get everything else working otherwise it can be very slow and frustrating.
  

1. Make 2D mesh
   1. File -> Import the two .dxf files from http://numisheet2018.org/Benchmarks/index.html
      
   2. Select the line element boundary of each part and use Mesh tools -> Automesh 2D on each. Quad dominant, Quadratic elements, Maximum element size 20 mm for tooling and 10 mm for sheet.
      
   3. Assign them each to a new component.
      
   4. If any quad elements have exactly one node on the rotation axis, split it into two tri elements (Mesh tools -> Change element shape).
      
2. Make 3D mesh
   1. Edit -> Select elements
      
   2. Edit -> Select all
      
   3. Edit -> Select faces
      
   4. Mesh tools -> Revolve. Axis of revolution +Y, Angle 90 degrees, Number of subdivisions 20.
      
   5. Select all the nodes on the axis and use Mesh tools -> Merge nearby nodes with a tolerance of 0.0001 mm.
      
3. Right click Analysis -> Analysis settings. Solver CCX, Nonlinear Static 3D, Quasi-static, Time period 5 s, Time step 1 s, Automatic time stepping on.
   
4. Edit -> Edge detecting selection. Select the bottom surface of the punch. Right click, Loads & constraints -> New fixed support.
   
5. Select the top surface of the die, Right click, Loads & Constraints -> New displacement, Y, displacement -10*t, Units mm, s.
   
6. Apply a Frictionless support (total of two) to each of the two sets of faces in symmetry planes in the same way.
   
7. Select the contact surface of the punch and add a contact. Select the bottom of the sheet and Edit the contact and set the slave surface to that. The sheet is the slave because it will probably be refined later and it's better for the finer mesh to be the slave.
   
8. Add contacts between the lifter and sheet, die and sheet, and stripper and sheet.
   
9. Add an elastic support to a face on the symmetry plane of each of the floating parts - sheet, stripper, lifter. Set the Tangential stiffness per unit area to something much smaller than E/thickness, I used 1000 Pa/m but you'll need to confirm that it's small enough not to affect the solution. This is to keep them constrained in the axial direction before the contacts close.
   
10. Add a material to each component. Right click it, Assign new material on the first one and Assign material for subsequent components having the same material. I used a simple elastic material with E=200 GPa for now.
    

takziawa

Mr. Victor

I am surprised at the detailed support.
I thank you as one of mecway user, too.


Mr. hamit_hushoni

The dies and punch can be a rigid wall.
In the case of problems involving bending of the sheet, it is necessary to divide the element into about 7 layers in the thickness direction.
Since BM2 has no material anisotropy, it is recommended to analyze it with von Mises first.

hamit_hushoni

thank you so much mr victor. this describe make me very happy.. i cant say nothing about it because your information really helped me to complete my study.
thank you so much mr.takziawa.. your information very important for me. I hope I can meet you two and say thank you in person

hamit_hushoni

Error generating inp file: Node 5673 has a coordinate transform (*TRANSFORM) together with more than one *AMPLITUDE block. This is not allowed by CCX.
whAt must im doing sir if that error show

hamit_hushoni

Victor

The *TRANSFORM is likely because of a frictionless support on a surface not aligned with the 3 global axes. The *AMPLITUDE is likely from a time-dependent force.

If these two things are sharing nodes, change it so they aren't. One way is to replace frictionless support with elastic support and give it a high normal stiffness per unit area and zero tangential stiffness per unit area. Another way is if the frictionless support's surface is supposed to be aligned with the axes, but isn't due to tiny errors in the node coordinates, change it to displacement in the x, y or z direction.

hamit_hushoni

i have tried mr. victor,, its work, thank you so much mr.victor

hamit_hushoni

good afternoon mr,blank returned to its original form after the drawing process, what I have to correct, and i try set plastic properties in material but solve cant running

Victor

hamit, could you post the .liml file?

Sergio

Hi, I have remade the model, also with elastic material works but not with plastic one, even reducing the increment size.

Time 0-1 Stripper preload (and keeped up to time 3)
Time 1-2 Lifter preload (and keeped up to tome 3)
Time 2-3 Punch displacement
Time 3-4 Load and displacements released

I have made a preliminar model with load control preloads, but looks like they are not enough to keep the plate in place to receive the punch displacement, that´s why I change to displacement control to the preloads.

hamit_hushoni

after springback blank come back like sheet normally mr sergio,, i have tried and i want set plastic properties but the simulation cant solve

maybe another friend have solution,

Sergio

Looks like that with a smaller increment (0.001) it works. It's taking a little time (more than one hour with 18 cores) but has passed the point where it fails before

Sergio

These are the results with a simple plastic material. I will do a new run but lifting the stripper more than now to see if then the blank has different behavieur

hamit_hushoni

thank you so much mr sergio,,

prop_design

that's a really cool simulation sergio

Famous_Mortimer

Nice Work

hamit_hushoni

thank you so much everybody,,