General Mechanical

General Mechanical

Solving VM250 in Workbench

    • Theliban
      Subscriber


      Hi all, 


         I am the new learner to Ansys, doing my Masters in Engineering Design field. I am doing the VM250 to get some knowledge in Non- Linear Analysis. While solving the problem, I am getting the error as shown in the figure. By decoding the APDL code, I did the procedures and applied the BC. But continuously I get the error message. What should I do to have the converge solutions? Please help me to decode the APDL code. 


      Thanks.

    • peteroznewman
      Subscriber

      I would expect to see the fixed support on the underside of the bottom block (the -Y face). I can't see what kind of connection you have between the two blocks. Please use File, Archive... in Workbench to create a .wbpz file and attach that file to your reply.

    • Theliban
      Subscriber

      With this reply, I attached the Gasket_VM250. Thanks for your support. Please find the attachment

    • peteroznewman
      Subscriber

      I made a change in DesignModeler, picking the three bodies and right clicking to select Form New Part. That results in the two shared faces sharing nodes, eliminating the need to use bonded contact in the model.



      The changes to the model were in the Supports, you see there is now three Displacement supports, one for each axis set to zero. I made a smaller mesh since the result is a uniform pressure. I changed the analysis settings to do 20 substeps on as the pressure increases and 20 substeps as the pressure decreases in load step 2.


      Attached ANSYS 19.0 archive.

    • Theliban
      Subscriber

      Dear Peter, 


                Thanks for your support, I somewhat understood where I went wrong!


      An inference from your modifications:


      1) The contact bodies, make inconvenience in the model.


      2) Understood the boundary conditions


      Doubt:


      1) In this model, you arrest the face of the Gasket also, is it physically possible? (While compression, it tends to squeeze out right?)


      2) Through my coursework, I can visualize the Newton Raphson Method, but I am unable to understand WHAT IS SUB-STEPS? Where Can I learn it. 


       


      Thanks!!! 

    • peteroznewman
      Subscriber

      Gasket Material and Squeeze Out
      A gasket material model and associated element is different from solid continuum materials and elements and is made for the special use-case of gasket compression. There is only ever one element through the thickness of the gasket solid and there is no midside node. The material model has only one input, which is the closure distance. The gasket material is not designed to model the "squeeze out" of excess material.


      The nodes on the face of the block that are held by the displacement BC are shared by the gasket. The gasket element has no midside node, so you could say the gasket is attached to the block and is not controlled by the displacement BC.


      If you want to model the "squeeze out" effect of some hyperelastic solid, you can use a hyperelastic material model, put many elements through the thickness and see that effect.


      If you did hyperelastic material and many elements, the displacement BCs on the X and Z faces represent a symmetry BC so you could imagine that this model represents 1/4 of the full size block and hyperelastic material would squeeze out on the two free sides.  If you did not want to represent a 1/4 symmetry model, you would have to change the support on the bottom to a fixed support, then you could see the material squeeze out on all four sides and you could also put a shear force on the top block and see side movement. 


      A gasket material model has no ability to support shear forces so you could not have just a fixed support on the bottom block, you would also need some way to support the X and Z motion of the top block.


      Newton-Raphson Method and Substeps
      When you have a load step with no substeps, the solver uses Newton-Raphson (NR) searching to find equilibrium for the system of equations. This is good if the solver is successful in its iterative search and if you don't want a plot of a result quantity along the way to the full load. Sometimes the solver fails to find equilibrium or the user want to see the history of a result quantity along the way to full load. In either of those cases, substeps are required. If a user requests 5 substeps, the solver takes the full load and divides it by 5 and applies 1/5 of the full load and begins NR searching for equilibrium. When it finds it, the solver writes out the results, then increments the load by 1/5 and begins searching for the next equilibrium starting with the last equilibrium. If the solver fails to find equilibrium at that increment, it will automatically bisect the load and apply a 1/10 increment instead and try again to find equilibrium.

Viewing 5 reply threads
  • You must be logged in to reply to this topic.