Cyclic Modal Analysis Constraint Equation Errors 1

[anants]

Hi

This seems to be my week for asking questions and I do apologize if this one is embarrassingly simple. I've looked in the manual though and trawled through a bunch of archives and I haven't found the solution so would like to know if any of you have faced the same problem.

I'm trying to carry out a cyclic modal analysis in ANSYS and everything goes great until I execute SOLVE. At this point I get a whole host of error messages, saying broadly that 'Constraint Equation #xyz has set all nodes/dof to zero and is being deleted'.

The funny part is I've run a modal analysis at least once before and didnt have this problem and I don't remember doing anything different. I've tried the cyclic analysis with a very simple test problem and I get the same issue. I'm following the usual order - define geometry, issue CYCLIC, mesh, define loads, define analysis type, SOLVE.

Would anyone have any ideas on this?

Thanks

Anant Sudarshan
Stanford Linear Accelerator Center
Stanford University

 

[cloche]

My idea is that ANSYS has mis-interpreted your cyclic sector.
Have you used "automatic" cyclic or did you define it "manually" by setting the coupled components you wanted? I personally never let the program do it by itself. For example, here's what I do in these cases: mesh "low-component" face with unsolved planar MESH200 elems; create the "low-component" as CYCLIC_M01L"; copy the mesh to "high-component" face, and create "CYCLIC_M01H"; define the cyclic analysis; mesh the model with the solid elems (the last two operations can be reversed, I believe).

 

[anants]

Thanks. I will try and do it manually then especially since the constraints it has a problem with are all those ANSYS generated itself.

Hopefully that should work.

 

[cloche]

Another thing that could possibly help: rotate the nodal coord system to be the same you use for cyclic coupling. Also assign elem csys to be the same. In that way you will have max coherence in the calculation.

 

[iker]

Check the following:
When you apply Cyclic Symmetry automatically, ANSYS creates constraint equations automatically between low and high component nodes during solution (first creates them and after checks them).

If any adjacent areas to cyclic ones have any displacement restraint, boundary nodes, shared by cyclic and adjacent areas are displacement restrained too.

Automatically, if any restraint is detected on any node with constraint equation applied (these cyclic constraint equations are created automatically during solution) ANSYS will ignore the constraint equation and reports WARNING for that.

So, check if adjacent areas to cyclic ones have any restraint, verify if that areas must have that restraint, and if they are neccessary, then just change limit warning and error message number allowed by ANSYS before aborting any solution (/NERR command) because cumulative warnings could your analysis to fail.

Hope this fix your problem

Regards