convergence analysis using Cosmos

[ozzkoz]

Hi, My company uses Cosmos for sructural analysis and I was hoping someone with some experience can help me assess the convergence.

I am using the adaptive analysis option, p-element. I find that typically after running an analysis it reaches it's stopping criteria and when I check the adaptive convergence plot I have 2 loops with a large change in degrees of freedom and sometimes a large change in max stress, sometimes nearly zero. The nearly zero change probably indicates that the max stress is pretty stable relative to the number of degrees of freedom, but sometimes there is a large change. When this occurs what I would really like is for Cosmos to run at least a third loop so I can see if the stress is linearlly going up toward infinity or if it begins to level off.

I guess the best way to ask my question is, how do I force Cosmos to use enough loops for me to determine the convergence?

Alternitivley, how can I use p-elements and specify the order so I might perform this convergence analysis myself without resorting to h-elements in the area of interest (and using a ton of them).

Thanks

 

[kellnerp]

When the stress keeps going up with mesh refinement you likely are looking at a singularity in a linear static analysis.

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[EngAddict]

Do it manually, create duplicate studies with increasing mesh refinement, then run all studies. Plot your max bending + membrane against mesh size. If you plot levels off the you can stop refining the mesh.
Like kellnerp said if the stress continues to increase infinitely then you have a singularity, so make sure to measure away from any intensification factors because you don't want to plot the peak stress.
This is the problem with the adaptive methods, they are not recommended on geometry that is prone to singularities, since COSMOS will continue to refine the mesh in areas where it is not important.

 

[ozzkoz]

I can do the convergence analysis myself, but I was hoping to be able to specify p-elements (allow for higher order elements while using less number of elements). Is it possible to specify the order without using the adaptive routine?

I didn't realize you could get a separation of the bending and membrane stress. Is this an option in the plot settings somewhere?

 

[EngAddict]

Based on thin shell theory you can pull these off directly, provided you are using shells. If you are using solids and you have the Pressure Vessel module, then you can plot a line across the thickness and it will output, membrane, bending at points 1 and 2, membrane + bending at points 1 and 2, and peak stresses at points 1 and 2.
Otherwise, you will have to probe the nodes across the thickness and probe the average stress on a face away from the discontinuity and then linearize the stress, to calculate the bending and peak stresses. See ASME VIII Div.2 section 5 (I think) or Google stress linearization.

I don't think you can increase the order without using adaptive.

 

[johnhors]

Eng Addict,

"If you are using solids ....... it will output, membrane, bending ......"

How does Cosmos do this? How is it possible?

Just curious!

http://www.Roshaz.com

 

[kellnerp]

It is probably time to ask the question which Cosmos is your company using?

Cosmos/M
CosmosWorks
Simulation

TOP
CSWP, BSSE

http://www.engtran.com

http://www.niswug.org

"Node news is good news."

 

[ozzkoz]

cosmos design star I think.

I'm not a huge fan of it, I liked ANSYS Workbench better, I could scope the results away from singularities and then use the adaptive mesh refinement to get pretty decent results.

 

[EngAddict]

In that case you will have to do it manually. They have stopped deveoping DesignSTAR, I think you will find Simulation much better. The only down side is it runs as an add-in to SolidWorks, rather than a stand alone app.

Ansys and SW Simulation both have almost identical tools for linearizing the stress across the thickness.