Autodesk Simulation Mechanical and Multiphysics

[#1]

Hi,

to understand the plate model better I am running a study on the twisting coefficient ratio and how it affects the result.

Therefore I used a plate model with the same parameters and varying coefficients from 1 to 0.0000001. My five load cases were forces in x and z-direction and moments in all 3 directions.

After each analysis I compared the results for max principal stress, and max. displacement for each load case / type of force: The values only vary between 0.159% and 4%.

However, my min/max stiffness increased with each step of 10^(-1) for 10x. For example a step from 1 to 0.1 in artificial stiffness caused a max/min stiffness warning from 1.53E13 to 1.53E14.

All in all thus I would assume that the coefficient of 1 would fit my analysis, but then I also checked the reaction forces. While the forces are fine in all case, the reaction moments do not deliver a good result in any case (not for a ratio of 1, nor for 0.0000001). Even if I inquire all nodes (so if the parts are partially constraints one should see the reactions at other points of the model) the result does not get any better.

So my question is now: Did the loads disappear because the coefficient is still too high or is it simply not possible to inquire the reaction moments on a plate model?

By the way: the stress- and displacement results itself seem to be realistic.

[#2]

I do not remember all of the details, but I have only seen one case where a customer needed to adjust the twisting coefficient ratio. So except for special cases, I think it is not necessary to change the value. Perhaps one reason to change it would be if the default setting resulted in a max/min stiffness warning that could be eliminated by changing the value.

For the reactions, you will probably need to attach an archive of the model to a reply. See "Create, Post, or Provide an Archive of your model". If all of your analyses had max/min stiffness warnings, then I can understand how the results may be inaccurate. But if you have some cases with no warnings, I would expect the reactions to be accurate.

[#3]

Speaking of things disappearing (loads), I thought for a while that I had lost my mind! I distinctly remember replying that to calculate the overall moment in Simulation results, you would need to do a spreadsheet calculation to get the sum of (force cross distance) plus any moment reactions. It turns out that my reply was to a different thread (Resulting moment at ....), so I may not be losing my mind afterall.

KlnKai provided his model through a method other than this discussion board. For explanation purposes, think of a three dimensional plate element model, restrained in many places with general constraints (boundary conditions) and 1D springs (elastic boundary elements). The model has one moment applied about the Y direction with a magnitude of 1.7E8. So by using the following equation, saving the appropriate reaction forces/moments to a file, and using a spreadsheet to do the math (see attached), here are the results:

Moment about Y = sum(Rx * Z) + sum(Rz * X) + sum(My)

  = (-0.274) + (1.7E8 + 2387) + (-2156)

  = 1.7E8 + 234

where Rx and Rz are the reaction forces, Z and X are the coordinates of each reaction, and My is the reaction moment about the Y vector.

The result is essentially the same as the applied moment of 1.7E8 -- 234 units higher than 1.7E8 is nothing. So the reactions do equal the applied loads, and everything looks good.

[#4]

Thank you John. I really appreciate it!

I would like to add (just for everyones knowledge) that you have to take care for +/-. In this case,

Moment about Y =  sum(Rx * Z) - sum(Rz * X) + sum(My).

It somehow confused me when I calculated Mz, but then I realized that x rotates in negative direction (in case of Mz).

In this case here, it just wasnt obvious because I did not take care for the +/- sign of the result

However, neither the twisting coefficient ratio nor the rigid elements' stiffness seem to be very sensitive in this case.