Workbench Solver pivot errors with semitrailer analysis

[DavidSimthQC]

Dear all,

I am rather new to ANSYS and am trying to use to analyze a semitrailer structure under various loading cases.
[ol 1]
[li]Starting fro CAD which was a SolidWorks assembly file, I used Anssys SpaceClaim direct modeler to prepare the CAD and solve some problems before meshing it into ANSYS.[/li]

[li]I had to supress three sold parts (400, mirror400 and 506) in order to get it to mesh, I am not sure if this is right or there is a better way to solve the issues with meshing, anyways.[/li]

[li]After suppressing the three aforementioned parts, meshing went through OK, I then applied constraints at the suspension and king pin and added some load (100 N) just to see how things will work.[/li]

[li]I received the following message,"Solver pivot warnings or errors have been encountered during the solution. This is usually a result of an ill conditioned matrix possibly due to unreasonable material properties, an under constrained model, or contact related issues. Check results carefully."[/li]

[li] I looked into the contacts folder and I suppressed all contacts with errors (not sure if this right either), I rerun the analysis and got the same error message again.[/li]

[li]I have archived the whole analysis workbench files and uploaded them. I will appreciate your help on this.[/li]
[/ol]

Many Thanks


David Smith

 

[dwallace1971]

Sounds like you've haven't constrained all rigid-body motion.

"On the human scale, the laws of Newtonian Physics are non-negotiable"

 

[rickfischer51]

What kind of contact? Bonded, frictionless or ? Look at the Solver Output in Solution Information for actual errors. Allso check the .err file. If there are no errors, convert all contact to bonded, turn off weak springs and run it again. Weak springs are not necessary unless there is a component constrained only by sliding friction. Weak springs usualy lead to loe coefficient warnings and affect pivot ratios. IF the warnings go away, turn on weak springs and rerun. If the warnings repaear, is just the weak springs.

Rick Fischer
Principal Engineer
Argonne National Laboratory

 

[DavidSimthQC]

dwallace1971 I think the model is well constrained, I even added another fixed support to the lower surface of the longitudinal beams but still errors.

rickfischer51 thank you for your reply,

All contacts are bonded, I've turned off weak springs and still the simulation will not run "PROBLEM TERMINATED BY INDICATED ERROR(S) OR BY END OF INPUT DATA"

I've attached the error file, and will appreciate your input.

Thank you all


David Smith

 

[rickfischer51]

You have a lot of warnings about pinball may be too large. That means the bonded contact will not bond and something can fly off. Run it as a modal analysis. If there are loose parts, you will get zero frequency modes and you will be able to see the loose parts. To fix it, either change the geometry and get the parts to touch, or manually set a pinball value for each contact item that is at least as lagr as the initial spacing. Also, the last entry talks about UY at node 99994. Go into Mechanical APDL (aka MAPDL, Classic, Blackscreen, real Ansys) and see what component that node is on:

nsel,s,node,,99994
esln,s,0
esel,u,stif,,168,178
*get,enum,elem,0,num,min
*get,typeno,elem,enum,attr,type
esel,s,type,,typeno

Cut and past this into the command line. In Workbench, each part has ia distict type number, so this should select the component.

Rick Fischer
Principal Engineer
Argonne National Laboratory