Solid vs Surface - Different results
I simulated a T-joint subjected to a nodally distributed force on its top surface, and fixed at the edge of the web. I simulated the model using both solid elements, and shell elements on the extracted midsurfaces. The stress results are very different. I don't understand why.
The model dimensions are shown below:
The material is set tot he default steel values.
The boundary conditions on the solid model (50 kN nodally distributed. All 6 DOF = 0 on bottom face):
The boundary conditions on the shell model are the same. The PSHELL thickness is set to 20 mm:
The stress results are very different:
What's going on?
Answers
-
the default for OptiStruct is to output stress values at the centroid of your element.
For a solid mesh, you would need a finer mesh to better capture the surface stress, as it is given by the shell model.
You can create a membrane shell over your solid mesh, or use setting such as 'ISOP=INT0' in your PSOLID, and request STRESS(GAUSS) to have a better approximation on surface stresses.
Or also you can request GPSTRESS output as it will calculate stresses at the nodes.
But in general, your solid mesh is too coarse thickness-wise to capture this bending effect.
1 -
Also the load is not applied to the same location. For the shell load is at midplane, for solid it seems applied to the top surface. These comparisons are tricky. You need to pay attention to location of load and BC as well as result evaluation. Also fixing all DOFs on the bottom is not correct for the solid model. The shell can contract freely in local z, while the solids are prevented by your BCs.
In addition, contouring element stress is not showing the calculated result. Do not average element stress.
0 -
Uwe Schramm said:
Also the load is not applied to the same location. For the shell load is at midplane, for solid it seems applied to the top surface. These comparisons are tricky. You need to pay attention to location of load and BC as well as result evaluation. Also fixing all DOFs on the bottom is not correct for the solid model. The shell can contract freely in local z, while the solids are prevented by your BCs.
In addition, contouring element stress is not showing the calculated result. Do not average element stress.
What do you mean by "The shell can contract freely in local z"? The solid elements are restricted in x, y, and z displacement, and their location/thickness restricts rotation of the bottom face.
The shell edge is restricted in displacement and rotation.Also, should I be comparing unaveraged results for both cases?
0 -
Hi AM,
I recreated your models in a way I think the modeling is correct. The results are much closer now, in the same order. Why don't they match better? I would say the (thin) shell is not a good representation of the solid geometry. Further more around the T-junction both models are very different. The shell model is not able to resolve the complex stress state there.
A closer match will be obtained if the assumption of "thin" is closely matched. Say thickness goes to 2mm.
I don't think mesh refinement will get a whole lot better match. There is a singularity in the solid model under the T.
Another modeling issue that I did not fix is that the forces on the rim need to be reduced to have a true even force distribution like a pressure. The rim forces need to be half the forces on the inside, the corner forces 1/4. This is because each element brings four forces and these add up at the nodes. This is a very common oversight.
As said earlier, these comparisons are tricky. The shell element makes some assumptions, simplifications and making a solid model that really follows is not easy. Loads, BCs and location of stress evaluation are important, also the assumption that the shell is thin needs to be considered. Complex stress states like T-connections cannot be resolved by a shell model.
Hope this helps,
Uwe
0 -
Uwe Schramm said:
Hi AM,
I recreated your models in a way I think the modeling is correct. The results are much closer now, in the same order. Why don't they match better? I would say the (thin) shell is not a good representation of the solid geometry. Further more around the T-junction both models are very different. The shell model is not able to resolve the complex stress state there.
A closer match will be obtained if the assumption of "thin" is closely matched. Say thickness goes to 2mm.
I don't think mesh refinement will get a whole lot better match. There is a singularity in the solid model under the T.
Another modeling issue that I did not fix is that the forces on the rim need to be reduced to have a true even force distribution like a pressure. The rim forces need to be half the forces on the inside, the corner forces 1/4. This is because each element brings four forces and these add up at the nodes. This is a very common oversight.
As said earlier, these comparisons are tricky. The shell element makes some assumptions, simplifications and making a solid model that really follows is not easy. Loads, BCs and location of stress evaluation are important, also the assumption that the shell is thin needs to be considered. Complex stress states like T-connections cannot be resolved by a shell model.
Hope this helps,
Uwe
Thank you for this. I have not had a chance to study your attached files yet. But I will.
The T-joint in my original post is a simplification of a much more complicated model that I'm trying to resolve. The real device has a plate that is being pulled and pushed at an angle by a vibrating motor. The plate is supported by ribs that are currently fillet welded, as in the image below.
The assembly is quite large, and consists of plates and slim beams, so I've modeled it with shell elements.
I'm investigating the stresses on the welds and the effect of switching to a complete joint penetration butt weld, which would be similar to the similar to the simplified T-joint in the first post.This is what my model with a butt joint between the plate and the ribs looks like:
The rib nodes and plate nodes are equivalenced.
Obviously, I want to make sure that I am not overestimating the stresses at the joint. But more importantly, that I'm not underestimating them.
Thanks.
0
Altair Employee