pressure load in pro mechanica 1

[andymagpie]

hello, i am very new to pro mechanica. I am trying to apply a uniform pressure of about 5 psi to a model. the model is basically a sheet metal plate about 1m^2 that is constrained at longitudenal ribs (x5) equally spaced. The plate is about 2mm thick and made from nickel cobalt. when i run a static analysis the von mises stress is much larger than anticipated. I am applying 34kPa (5 psi) and the max stress is 500 Mpa?
I would really appreciate some help in this matter.
Thanks

 

[prost]

As you know, because you have tried to describe your model and did not give me a picture of it, I am going to have to guess what you are trying to model.

1) Did you increase the degrees of freedom in the mesh by increasing the polynomial level (the 'p-level)? Did you see the max. stress just keep increasing with p-level? Then you have a numerical singularity in which you have fixed a node in a direction it wants to move. This might be a mistake, so you should check that.

2) Even ignoring the max. stress, does the plate deform as you expect? This is a check that you have properly modeled boundary constraints.

I am relatively new to this eng-tips.com. To the vets out there, is there a way for someone to get us a picture of the model with constraints and loads identified?

 

[andymagpie]

Thanks for the reply, I believe i have a problem with the constraint set. the result is definately spurious as when i alter the legend accordingly apart from points near the constraint (very small points i may add)the max stress is more realistic. I think i have a way forward. Regards!

 

[JohnAndrews]

It sounds like it is your constraint which is causing the problem, and you can ignore local stress concentrations around the constraint.

If you can access the PTC Knowledge base, it is worth looking at "Suggested Technique for Identifying and Avoiding Singularities in Pro/MECHANICA Structure":

http://www.ptc.com/cs/cs_25/howto/mst726/mst726.htm

The problem you are having with your constraint is typically because the area constrained is zero, i.e. if you constrain an edge or a point with solid elements - this also applies to loads.

Stress = Force / Area
if Area = 0 , Stress = Infinate (or typically very high values in Mechanica)

 

[prost]

To JohnAndrews comments, you might want to add
As Area goes to zero, Stress goes to infinity (this is sometimes called the Boussinesq problem).
Further, as the stress goes to infinity in this case, the strain energy goes to infinity.

This is a very important result that is almost never discussed in finite element classes or outside of the university. This result addresses the convergence of the numerical solution. It can be shown (Szabo and Babuska, Finite Element Analysis), that the minimization of the potential energy (of which strain energy is a part) is equivalent to finding the exact solution. If you have a situation in which the strain energy (and, potential energy) is infinite, your finite element solution cannot be fully trusted because obtaining a converged finite element solution depends on minimization of the potential energy--you are searching for the exact solution with your finite element analysis; if you cannot minimize the potential energy because the exact solution's strain energy is infinite, then you cannot obtain a converged finite element solution. This is why a so-called "Point Load" or "Point Displacement" constraint is not allowed with the finite element method.

While it appears that this Boussinesq problem is a singularity similar to the singularity of a crack, the key difference is the behavior of the strain energy in the Boussinesq problem, which is infinite, compared to the crack problem, which has finite or bounded strain energy.