load definition on surface

[Anonymous]

Hi,

I attached a model. In the center is a surface that I would like to apply a bearing load to. This can not be done right now in Inventor Nastran (only cylindrical surfaces). So I apply a Force load and select the middle surface and run the simulation and get around 38ksi max stress. I then try and 'split' the middle surface using the 'xy' plane and apply the same load only to the bottom half of the middle surface. This nets me around 55 ksi max stress. I don't understand how this load should be applied. When I think of a force I think of a 'point' load. But when you apply a force to a surface does Nastran distribute the load like a pressure? Is the 'bottom half' loading case the correct way? And why such a difference in stresses for the two ways?

See attached

[John_Holtz]

Hi @Anonymous 

• When I run your model with the force applied to the bottom surface the maximum von Mises stress is 51,870 psi.
• When I run your model with the force applied to the bottom and top surfaces, the maximum von Mises stress is 52,410 psi.

Is it possible that you were looking at a different stress result (such as X-Normal stress or something) for one of the cases? Or is the difference because you had a different mesh after you split the surfaces?

Note that the maximum stress in this model is almost certainly a stress singularity. The results will approach infinity as the mesh is made smaller and smaller. Singularities are locations where the stress is inaccurate because of the sudden change from fully, rigidly constrained to having no constraints on the adjacent element. That is just the nature of the mathematics. You need to ignore the results at these locations.

The answer to your other question about how the force is applied is yes ... almost. The force applied to a face (a surface) is converted to a pressure. Technically, the pressure is then multiplied by the area of the face, and then the force is applied as point forces to the nodes on the face.

Which load is more accurate (applied to the bottom face versus bottom and top faces) is not making a big difference that I can see. Otherwise, the load that is more like the real situation is the one that you should use.

[Anonymous]

Thanks for the reply John,

Wondering did you re-mesh before/after split of the middle surface? I noticed when I did that (re-mesh) I got drastically different results (as noted in original post)... If I don't re-mesh I get the same results similar to yours... 

[John_Holtz · Accepted solution]

Hi,

I did not remove the split feature and remesh the model because the goal was to compare the results when the loading was changed. That is, what is the difference when the load is applied to the bottom half versus applied to the top and bottom halves.

I know that the mesh is too coarse to give accurate answers, so it is natural that changing the mesh (even slightly) will change the results. If you want accurate results, you need to start refining the mesh and look at results in an area of the model that is not affected by the constraints. Once the mesh size becomes "small enough", the results will settle down to an accurate answer.

But as indicated in my previous post, the "maximum" result which occurs right at the location where the constraints end is not a location that can be calculated accurately by simulation. The result will always change at that location. Since the fillet in the shoulder could be an area of concern, I would suggest the following:

1. Split the end of the shaft X inches away from the fillet.
2. Apply the constraints so that the stress singularity will not be X inches away from the fillet.
3. Ignore the stress result that occurs at the stress singularity. Instead, concentrate on the stress in the fillet and in the center of the pin.

[Anonymous]

I followed the advice and you are correct,the max stress goes up with the number of elements. I adjusted the constrained surface on the trunnions to start 3/8" away from the faces. I probed the stress levels around the center and fillet. I think they are acceptable if I go with A572-50 material. I need a factor of safety of 3.