SW Sim09 Meshing Help

[Kriegen]

Hello Gents,
I am attempting to create a stronger wire basket. I would like to use simulation to find the stress points for said basket. However I cannot get the program to mesh the model. I have created the model as one solid part. I have merged all bodies into one solid body. After the comp attempts to mesh the body, it tells me that the surface mesh is successful but the volume mesh has failed and that I should try a smaller element size for meshing. I have scaled the model up to four times where the larger wire diameter is now 1.250in and the element size is .00186in and yet the program still asks for a smaller element size. Is there any thing I can maybe do different?

 

[corus]

For this kind of model you really need to use beam elements. not solid elements.

corus

 

[Kriegen]

Well, now I have tried that and have actually gotten it to mesh, however the joints and connections are weird. Is there a way to modify joints and connections in SW Sim09??

 

[Kriegen]

Here is a picture of the mesh I get with beam elements. The differences in the picture will show you that the mesh thinks there are many connections that are not really there.

 

[Kriegen]

Does anyone know how to fix this problem? Everyone I talk seems to be blown away by this. It is ok to admit when we don't know the answer, but I would at least like to know that this is not an easy solution.

Foofire
CSWP

 

[macPT]

Hi Foofire

AFAIK there is no way to directly control joints and connections.

You can have some control over them by changing joint clearence value (the same for all joints, so not much of a control). It will be a trial and error work until you have the model that pleases you.

You can also delete joints from de Result window, which adds more control.

Joints between 2 members are represented by violet spheres. Beams ends are rpresented by greyed green spheres. You must check if colors are according to model or if you dont have a sphere where it was suppose to be and vice-versa. If one of these erros occours, you need to adjust the joint clearence.

Smaller joint clearence values have the effect of missing joints. Bigger joint clearence have the effect of considering some joints of smaller menbers as one. So I guess that you must have the smaller joint clearence that provides you a good model.

One trick: in order to have a correct rebuild of the
model between 2 joint clearences, meke a dumb joint clearence with a big value in the middle.

I hope this hepls you.

Regards

 

[kellnerp]

This is not a problem for solid elements. You use beam elements, find the location of peak stress and then, perhaps, submodel that location in solids.

What result are you after? Stress in the spot welds? Deflection? Possible yielding of the wire?

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[drbooshkit]

Agreed, beams are most appropriate. However, if you insist up going down the solid route (use symmetry of course), then you can probably work around the mesh error.

"surface mesh is successful but the volume mesh has failed" indicates that the mesh tolerance was high enough to cause volume elements to collapse. You can try:
1. Decrease global element size
2. Decrease tolerance (even to .000001 to see if it will work).
3. Try curvature-based mesher.

You'll need a bit of RAM to do this one!

 

[Kriegen]

Well, I have decided that beam mesh is the way to go, however I just have lots of joint issues.

Foofire
CSWP

 

[kellnerp]

Just curious, but what is the goal of the analysis?

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[Kriegen]

Preferrably I would like to get a stress map for the model

Foofire
CSWP

 

[kellnerp]

Why not break the problem into small parts?

Model the bottom of the basket and look at the effect of loading patterns.

Take the reactions from the bottom and apply them to the sides. And model just the sides.

Then apply the side reactions to the support frame.

Use symmetry to reduce the problem size.

You might also consider finding an equivalent shell thickness and replace the wire with shells? When FEA first started this was done alot.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[Kriegen]

Well that would be fine to begin with, however I am going to have to do this for 50 parts. I would like to find out how to do this for the one parts in complete form then reproduce for all others.

Foofire
CSWP

 

[kellnerp]

Then figure out an equivalent shell thickness and use shell elements. You aren't concerned with individual wires.

Any plates and shells book will probably do an approximation of a shell with beam elements. You would just be working backwards.

TOP
CSWP
BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[Trevorjjj]

It strikes me that this meshing problem needs a little more input, rather than telling the user to change what they want from the simulation.

This software is not some mickey mouse product, and the meshing problems are global, not limited to wire baskets.

The help is pathetic.

 

[kellnerp]

...rather than telling the user to change what they want from the simulation.

The responses here are valid responses from experienced FE users. I hold Advanced certification in the software he is using. I have been doing FE since 1987. Some of the others that responded also have such qualifications. Make no mistake, these experienced users are not telling him to change the engineering result, but rather how to get that result in a robust and expeditious manner.

This is a case of trying to let the software dictate how to solve the problem. The developers of Simulation have chosen to limit the tools to what the masses can understand rather than give the wide choice of elements and options that more complete FE software contains. However, Cosmos/M is included with Simulation, is a complete FE solution and can be used to create a beam mesh at the expense of requiring the user to understand the problem to a greater extent than Simulation.

The reason the experienced FE users are pointing the OP away from proceeding down the path of solid meshing is that it creates a HUGE model that is difficult to mesh, takes a long time to solve, if it will mesh and solve at all. A beam mesh on the other hand will take considerable less time to solve and will give just as good an answer. The same is true of an equivalent shell mesh.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."