Preprocessing

Preprocessing

Incorrect Number of Nodes for Beam188

    • JSmith
      Subscriber

      Hello.  I am having an issue with getting ANSYS Mechanical ADPL to create a linear mesh.  I have created a 5 cm long extracted beam in SpaceClaim and imported it into Mechanical ADPL using Workbench.  I have changed the mesh settings to have a Linear Element Order and large size to get 1 element.  However, when I mesh, the statistics show 1 element and 3 nodes.  When I add the node numbers I only see 2 nodes, but the program will run as a quadratic element.  I've tried to restart and run the model again, and I get the same results.  I am unsure what needs to be changed in the program to get the correct number of nodes.  Any assistance that you can provide would be greatly appreciated.


    • JSmith
      Subscriber

      Additional note: I have tried changing to a truss element as well and get the same node error.  I will get linear results then, but I would like to still understand why there are 3 nodes instead of 2.

    • peteroznewman
      Subscriber

      What evidence do you have that a model with a Linear mesh will run as a Quadratic element?


      Is it because you see an extra node in the mesh Statistics as shown below?



      That doesn't imply the element runs as quadratic.  After this model solves, I can look in the Solution output and see that one linear element BEAM188 was used.



      If I change to a Quadratic mesh...



      then I get one Quadratic BEAM189 element in the Solution output.



      You might ask, "Why is there an extra node?"  I expect it is used to orient the beam cross-section.


      If this post answers your question, please click the Is Solution link below (when logged in) to mark this discussion Solved.

    • JSmith
      Subscriber

      I know that it is running as quadratic due to the results. I am comparing to a known solution from custom software to the output of ANSYS.  The linear choice in ANSYS gives a quadratic solution.  And the quadratic choice gives a cubic solution.  I think it is associated with the additional node.  

    • peteroznewman
      Subscriber

      The terminology used by ANSYS and every other Finite Element program is that a linear beam element has two nodes with a quadratic displacement function, while a quadratic beam element has three nodes and a cubic displacement function.


      Two nodes can deliver quadratic displacements because each node has rotation degrees of freedom as well as translation degrees of freedom.


      The benefit of a quadratic beam element is that it can represent curved geometry, while a linear beam element can only represent geometry that is initially straight.


      You seem to be looking for a two node element that has a linear displacement function. That is called a truss element, which NASTRAN calls a ROD and ANSYS calls a Link Element, or LINK180.  That has only translation degrees of freedom and no rotation degrees of freedom, so the displacement function is linear.  In the Details of the Line body under Geometry, you can change a Beam to a Link.

    • JSmith
      Subscriber

      Thanks for that assistance.  One last question.  Where do I find this third node? It appears for both the beam and the link element.  Thanks!

    • peteroznewman
      Subscriber

      When you click on the Solution branch in Mechanical, you can Write Input File.  I attached an example text file. It is listed in there. I don't know how you find it graphically in Workbench.  I expect you can see it graphically in the Mechanical APDL program.


      If your question is answered, please click the Is Solution link below the post that best answered it to mark this discussion Solved.

Viewing 6 reply threads
  • You must be logged in to reply to this topic.