General Mechanical

General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

Bend Force

    • Thomsen93

      Hello Dear Sir,

      We need to calculate of bending force and sheet metal's elastic deformation that dependent on top tool's displacement on the -y direction.

      The thickness of sheet metal is 8mm. Also the tools geometry has been defined on the model.

      We have assumed non-linearities that multi linear plastic deformation for sheet metal. We increased young modulus of top and bottom tools for behave like rigid body. And we need to see weak springs effect that occurs after the bending process on the sheet.

      I used size mesh for contact surfaces and had created 2 steps in analys settings. In the first step top tool move -15 mm on -y direction and in 2th step top tool has to get retain position that it started.

      We have encountered some errors about weakspring and solver suddenly stopped.

      Bottom tool is fixed from bot surface, Sheet metal standing on the bot tool and top tool bending it while moving -15mm for -y direction.

      The given hand would be appreciated deeply from our youth spirit

      You can increase top and bottom tool's young's modulus multiplying with 10000.


      Sheet Metal Multilinear Isotropic Hardening Properties.

      MPa                 STRAIN (Young's Modulus 72450MPa Poisson Ration: 0,33)

      250                   0

      269,1                0,003714

      307,05              0,01172

      331,2                0,02052

      348,45              0,03131

      358,8                0,04047

      376,05              0,06199

      386,4                0,07985

      396,75              0,10254

      414                   0,15427


    • peteroznewman

      Hello Thomsen,

      One defect in your model is you need many elements, at least 8, through the thickness of the sheet. One element is impossible to compute.

      I recommend you convert this to a 2D Plane Strain model. To do that, you need surfaces in the XY plane (Z=0). You must also set the Properties of the Geometry cell in Workbench to 2D before you open the Model in Mechanical.

      At this amount of bending, the Total Strain is over 30% while the plasticity model you provided only goes up to 15%

      What is the Elongation at Break for the Aluminum alloy?  Perhaps it has already cracked by this point.

    • Thomsen93
      Hello again Could you update your properties like this?, I have increased plastic linear strain on materials so we don't want to see any cracks on material. The root cause of this fault we have taken these vaules from analys example.
      Can you share your wpz file? Additionally we need to see minimum bending force that get this form on the sheet Metal. Does it consist to use 2d simplification when we re look for force and plastic deformation?

      Sheet Metal Multilinear Isotropic Hardening Properties.

      MPa STRAIN (Young's Modulus 72450MPa Poisson Ration: 0,33)

      250 - - - - 0

      269,1 - - - - 0,003714

      307,05 - - - - 0,01172

      331,2 - - - - 0,02052

      348,45 - - - - 0,03131

      358,8 - - - - 0,1047

      376,05 - - - - 0,1519

      386,4 - - - - 0,2185

      396,75 - - - - 0,2725

      414 - - - - 0,4042
    • peteroznewman

      What version of ANSYS are you using? I did my example in 2019 R3 and have attached the archive. You can't open it if you are on an older version.

      You can update the material and run the model.  Is the data for plasticity in terms of Engineering Stress and Strain or True Stress and True Strain?  It must be in the latter. Here is an example of the conversion process.

      A plane strain model can compute with a plasticity material and has results per unit depth, so for a model in mm, the force is per mm of depth.

    • Thomsen93

      Dear sir,

      I' much preciated for your kindness but when I opened your  wbpz file, model wanted to upload itself. When I did this, your meshes style, restrains all of were gone.

    • peteroznewman

      Not sure what you are seeing. I just downloaded and opened the attached archive. It has a Fixed Support, a Displacement and two Frictional Contacts.  The results are not included. You have to clear generated data on the Solution branch and solve again.

    • Thomsen93
      Hello Peter How s going on?
      I m trying to solve it, while using Web digitiliazer to get plastic multi linear curves from st44 graph that taken from instron machine.
      I don't like to write large paragraph, I will share my result on upcoming days.

    • Thomsen93


      Hello sir,

      I'm considerind about why did you use command notes ?

    • peteroznewman

      NEQIT,100 tells the solver to keep iterating to search for convergence for up to 100 iterations. The default is 26 iterations. When convergence is not found, a bisection occurs, which means the load increment is cut in half and the solver tries to converge again.  Sometimes, when watching the force convergence plot that is updated while the solution is being computed, you can see the two curves, force convergence and force criteria, converging and they just need a few more iterations for the curves to cross, but it is getting close to 26 iterations since the last convergence, that is when you want NEQIT,100.

Viewing 8 reply threads
  • You must be logged in to reply to this topic.