General Mechanical

General Mechanical

Problem with Contact Simulation in Mechanical APDL

    • Franzanstein
      Subscriber

      Hello Forum!

      I have a problem with my contact simulation in Ansys APDL. Basically I am simulating Spur gear contact in a way that one gear is held in place on its inner diameter while on the inner diameter of the other gear torque is applied. The two tooth flanks that are in contact are defined as Contact174 and Target170 surfaces. I have the Problem that when I simulate this Model one surface penetrates the other as in the attached Picture (It seems contact is only detected at one node, probably the one initially in contact, the rest of the contact area is ignored). But when I use the Large deflection effects setting (NLGEOM) this problem does not seem to occur and the simulation seems to work fine. I dont understand why this setting would help me with the simulation though, as the contact is initially closed and the deformation of the elements is minimal.

      What are some settings that would make this simulation run correctly (or is NLGEOM a valid setting for this and why)? I have tried a lot of different settings (Pinball region, ...) but it seems none have really worked

      Other settings I use: Solid186 elements, symmetric contact pair, pure lagrange multiplier, auto time step.

      Thanks

    • peteroznewman
      Subscriber

      NLGEOM is a valid setting for this becuase it creates a solution process with multiple solve iterations.  Without NLGEOM, a single solution using the nodes that are initally in contact gives you the local deformation.  With NLGEOM, the nodal posititions are updated, and the contact status is reevaluated and new nodes are found to have come into contact. The second solve spreads out the contact patch.  The nodal positions are updated again, and the contact search is repeated to look for new nodes that have come into (or out of) contact. The iteration continues until there are no more changes in contact status.

      If you have a very fine mesh around the contact point, you will get many iterations and a very smooth contact pressure patch that covers many elements and has the pressure highest at the center of the patch and tapering off to the edges of the patch.  Your mesh is too coarse to see this effect. Consider refining the mesh at the contat point.

      I see you are working in APDL. I don’t know the command in APDL, but in Workbench, an Advanced configuration of the contact is to Update Stiffness on Each Iteration. 

      • Franzanstein
        Subscriber

        Hi Peter!

        Thanks a lot for the fast reply! I was wondering if there is a different way to achieve the updating of nodal positions or if NLGEOM is the best way to handle the simulation? (Also do you maybe know where I can find detailed documentation of the NLGEOM setting? I couldnt find much in the contact guide except for some information on how NLGEOM influences the pinball region).

        I have tried updating the stiffness at each iteration (Keyoption 10=2) but again the simulation and this setting only work when NLGEOM is activated.

    • peteroznewman
      Subscriber

      Hi Franz,

      NLGEOM is the bedrock of the entire nonlinear structural solution process. It is the best way to handle this simulation.

      Regards,

      Peter

Viewing 2 reply threads
  • You must be logged in to reply to this topic.