General Mechanical

General Mechanical

Problems with rotating assembly and loads

    • Frenwa1
      Subscriber

      I'm trying to analyse a mechanism with a very specific load pattern depending on where it is along it's rotation.


      After messing around with contacts and joints for a long time I believe I got a pretty stable configuration, using exclusively joints.


      I am now trying to get the whole mechanism turning with specific loads applied at each degree of rotation.


      Some solutions have converged, but for some reason, when I apply loads to the turning mechanism, it starts to expand into space. This happened while using Static structural and Transient Structural.


      Should I use a different type of analysis? Or is it simply my set up who is at fault?


       


      Loads and rotation on the mechanismLoads on the blade at each degree of rotation


      Here is what my results looks like :https://gph.is/2PX6pdg 

    • peteroznewman
      Subscriber

      Under Analysis Settings, you must have Large Deflection set to On.  Was this Off?

    • Frenwa1
      Subscriber

      It is off, when I set it to On the solution fails to converge. It stops after a few minutes after I start it.

    • peteroznewman
      Subscriber

      Is this the Static Structural model? There are several steps needed to make a nonlinear model converge.


      Under Analysis Settings, you must have Large Deflection set to On. 


      On the Solution Information folder, request 4 or more Newton-Raphson Force Residual Plots.


      Under Analysis Settings, turn Auto Time Stepping On


      Set the Initial Substeps to 100, Minimum Substeps to 10 and Maximum Substeps to 500


      Click Solve. 


      In your reply, insert a screen snapshot of the Force Convergence Plot found in the Details of the Solution Information.


      In the Solver Output, find the Error and copy the text of the error to show that.


      Under the Solution Information folder will be four NR Force Residual plots. Look at each one and turn on the Max flag. Take a screen snapshot of each one.


      The corrective action is to add mesh controls to reduce the element size around the Maximum of the NR Force Residual plot. There are several discussions that show this process. Here is one that includes videos.

    • Frenwa1
      Subscriber

      Hello,


      I ran the simulation with the settings you proposed. Here's the error I got shortly after.


      Last time I ran the simulation with Large Deflection turned ON, I got the highly distorted error as well, although it was on another piece.


      Could this be caused by some sharp edges in my geometry (a keyway in my case)?


    • peteroznewman
      Subscriber

      Please show the Force Convergence Plot. Did any substeps converge or did no substeps converge?


      Please show the NR Force Residual Plot, where is the Maximum force residual?


      You can create a Named Selection of Element 113112 so you can see where that element is on the Body.


      After you look at this data, you improve the mesh where the problem area was. You might have to do this several times in a row. This is the normal work to get a nonlinear analysis to solve.


      It could also be unreasonable inputs. On the graph below, the red curve shows you are requesting a sudden change from zero to some large value. It would be better to ramp up to that large value.  Which input is the red curve?  Is that on the same part that has the excessive distortion. Maybe that is the reason for the failure to converge. But maybe it's the blue curve. I can't see the inputs and everything on that plot is scaled by the maximum value so actually the blue input could be larger than the red.


      Loads on the blade at each degree of rotation


      It looks like at T=90 s the red and blue curves both start at zero and increase. That is probably a better point to have at T=0 so that convergence can begin with the inputs at zero. 


      If you want more help, please attach a Workbench Project Archive .wbpz file after you post a rely and state which release of ANSYS you are using.


      Regards,
      Peter

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