Ansys Products

Ansys Products

Discuss installation & licensing of our Ansys Teaching and Research products

How to use ‘moment reaction’ in user defined result

    • Koen Franse

      Hi there,

      I've been trying to automate the computation of rotational stiffness computation, meaning dividing the moment reaction by the prescribed angle. However I cannot find how I can use the prescribed angle in my remote displacement boundary condition, or the moment reaction result in a user defined result, since I cannot assign an ID to these seperate values. Does anyone have a solution/workaround for this?

      I want the rotational stiffness as a specific result so I can use it in a parameter set for designXplorer.

    • mjmiddle
      Ansys Employee

      User defined results are contour results. There are yet no summation (probe) types of User Defined Results. So a user defined result is like an array of data, each item in the array being a node or element value, and the equation is applied at each of these values. So to use any IDs in a User defined result, it has to have matching element/nodes in the array. This means you have to scope to the same geometry to use the ID for one result in another result, and it only works for contour results, not probe results. This means you have three choices, in order of increasing complexity:

      1. Make a typical moment reaction probe in Mechanical. Click the checkbox to promote the outout value to a design parameter. Also promote the angle load for your remote displacement. In the "Parameter Set" in workbench, make a user defined parameter and divide the two numbers to get your stiffness parameter.
      2. Use a command snippet under solution, using FSUM to compute moment. You may have to set summation point with SPOINT. If you name your final variable with prefix "my_" it will show in the Details and you can click the checkbox to make a design parameter. You will also promote the angle for your remote displacement load. In the "Parameter Set" on workbench, you can make a user defined parameter to divide the two numbers to get your stiffness parameter. When communicating with the APDL solver in command snippets, we usually make named selections of the necessary geometry and use CMSEL to get that selection.
      3. Do it all in a command snippet, using *GET to get the applied displacement angle from your remote boundary condition, as well as FSUM to compute the moment, and divide to get your stiffness. Name the final variable beginning with "my_" and you can promote to an output design parameter.

      If you have never done APDL scripting before, you will have to do some learning,

    • Koen Franse

      Okay thanks a lot, I think solution 1 will already be sufficient for now!

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