Static analysis - "ERROR in cascade" with CCX solver (OK with internal solver)

dculpdculp
If the attached test model is analyzed with Mecway's internal solver then the analysis is completed satisfactorily. However, if analyzed with the CCX solver then the analysis aborts with "*ERROR in cascade: the DOF corresponding to node 4 in direction 1 is detected on the dependent side of a MPC and a SPC". (Node 4 is at the interface between the two mating cylinders where the bonded contact occurs.) If I suppress either the bonded contact or the frictionless support on the lateral faces then the analysis finishes (but the results are wrong). This link (https://calculix.discourse.group/t/cyclic-symmetry-error-when-slave-master-contain-some-nodes-from-fixed-surface/440) seems to indicate that there is some conflict between the bonded contacts and constraints at shared nodes. Also see calculix source code -- https://stuff.mit.edu/afs/athena/software/calculix_v2.7/CalculiX/ccx_2.7/src/cascade.c (search for "ERROR in cascade: the DOF").

I need to get the CCX output (.frd file) in order to view the results in Paraview. Therefore, I can't rely just on Mecway's internal solver. However, when the model is saved via Mecway's CCX input deck (attached) and analyzed from a Windows 7 cmd window using either ccx216.exe (2020-01-19) or ccx212.exe (2017-04-04), the same error occurs.

Important -- This test model uses "static" contacts. If elastic contacts are used then this static analysis model runs OK with the CCX solver. However, most of my analyses are modal analysis for which Mecway reports, "Elastic [contact] is not allowed with this analysis type." Therefore, I have to resolve the problem using "static" contacts (unless there is a work-around).

Thanks for any suggestions.

Don C.

Comments

  • VictorVictor
    Yes, it's having constraints on the slave nodes of the bonded contact.

    A workaround it to replace the frictionless supports with elastic supports with eg. 1e15 Pa/m Normal stiffness per area and 0 Tangential stiffness per area.

    I don't know why elastic bonded contact shows an error for modal vibration. It could simply be that I haven't tested it and it's actually OK, or it could be that there was some bug in CCX. I don't see any warning against it in the CCX manual.
  • dculpdculp
    Victor --

    See the attached Mecway error message.

    When I run the modal analysis with the CCX solver (inside Mecway) I get the attached result for one mode. This shows that the elastic contact isn't working. Attached is the liml file for modal analysis.

    image

    image
  • VictorVictor
    Oh, that's funny. It works if you have stress stiffening but not without. It seems like it requires the static *STEP that comes with stress stiffening and then remains active for the subsequent *FREQUENCY step.
  • VictorVictor
    I saw your post on CCX forum so just to clarify in case of misunderstanding, it works for both static and modal with elastic support, not elastic bonded contact.

    In case that's no good, another workaround is to extrude a thin layer at either the slave contact surface or the frictionless support surfaces so there are no common nodes along the edge.
  • dculpdculp
    Victor --

    Thanks, I understand.
Sign In or Register to comment.

Howdy, Stranger!

It looks like you're new here. If you want to get involved, click one of these buttons!

Sign In Register