ZERO JACOBIAN ERROR!!!!...COSMOSWORKS

[jose2112]

Hi...i'm performing a static analysis to the rear suspension elements of our vehicle using cosmoworks; but a "zero jacobian" error pops out when a execute the analysis...do you guys know why is this happening? where can i find info who help me to solve this problem?

Thanks!!!

[jose2112]

Hi...i'm performing a static analysis to the rear suspension elements of our vehicle using cosmoworks; but a "zero jacobian" error pops out when a execute the analysis...do you guys know why is this happening? where can i find info who help me to solve this problem?

Thanks!!!

[The AFX Master]

Are you analyzing wishbones or rockers?. If you're doing wishbones, the zone where the tubes meet a ball joint housing generate weird mesh patterns, Jacobian is a measure of the distortion of the tetrahedral elements that you're using for mesh. When an element have a negative Jacobian Ratio that means that you have a highly distorted element, that is ussually common on sharp corners or inner edges.
Try to apply a mesh control on those edges.

In a few words, some tetrahedral elements collapsed as triangles. As the Jacobian is an indirect measure of the element volume, zero jacobian means an element with zero volume

Or, the easy way:

If you're analyzing wishbones, I think that solid TETRA-10 elements aren't the way to go. you'll have a insanely high count of elements on each tube due to the aspect ratio of a tube (way longer than thicker at the wall). I can suggest using beam elements (plain simple and fast) or mixed mesh of solids (for the ball-joint housing) and shells (for the pipes).
Remember that cosmos static analysis DO NOT consider buckling.. and your very first failure mode in a lower wishbone will be... buckling. Do some hand calcs to check for buckling.

a good intro to CosmosWorks here (http://www.owlnet.rice.edu/%7Emech403/HelpFiles/IntroducingCW.pdf)

[Composites Guy]

I used a two-force member approximation for susension loads. For example, I modled each a-arm in Solidworks as two "pencils". I mated all the "pencils" of the suspension up in an assembly and then loaded them with appropriate forces in cosmos-motion (the Adams solver not the FEA part). That output the forces in each member, and I just did hand calcs for buckling and tension/compression strength.

CosmosWorks FEA is pretty unlimited in terms of model size. If you have a lot of RAM it can support INSANE amounts of elements. I have a million node shell model of my entire frame (just for kicks, I used another program 'Ansys' with beam elements in the end). Modelling a suspension corner with shell elements should be no problem.

Is it all one part? Do your boundary conditions eleminate all 6 rigid body rotations and translations? Have you tried the alternate solver? Is it a shell or solid mesh? Could you post a picture of your model?

Just as a note for The AFX Master the version of CosmosWorks FEA that is available free to most FSAE teams does not include tetrahederal meshing (yet.) Unless you guys have something that I don't.

[The AFX Master]

We have both the student edition and the fully licensed one.
Student edition does have tetrahedral elements, when you create a new study, the dialog box let you to select between tetrahedral solid mesh, shell mesh with mid surfaces, mixed mesh and beam mesh.
Also you can select the element on the mesh creation options dialog box as quadratic (TETRA 10?) or linear (4 nodes) element order.

I think alternate solver will not solve the problem since is caused by a bad mesh. but the alternate mesher could do the job.
Also bad boundary conditions will result in a singular stiffness matrix (the program will say so or ask you to activate the inertial relief option).
So the problem is a mesh problem. Jose, post pics of the problem.

[pablo180]

What is the error number?
Doing a search though the Cosmos Knowledge base could give you some guidance as to what is wrong and how to go about fixing the problem.

http://66.223.111.93/cgi-bin/search.cgi