Contact pressure vs. Normal Stress

[rlkillian]

I'm modeling a column with a 2" thick base plate sitting on a concrete foundation. I compared the contact pressure on top of the foundation with the normal stress on the top of the foundation and while the pattern was similar the values were different. The maximum contact pressure is a bit over 10 ksi but the maximum normal stress is about 6 ksi. I've compared these before on other models and my memory is they were much closer. I don't really see why they wouldn't be the same. Any ideas? 

I've posted about contact pressure before and in general how splotchy the results are makes no sense but I guess that's the subject of another post.

[rlkillian]

Hello? Is this thing working? I know you're out there, I hear you breathing.

[John_Holtz]

Wow, you have good hearing. (Better than my wife. 😁)

I am not 100% positive how the contact pressure is calculated, but I suspect that it is more accurate than the elements stress.

• The contact pressure is most likely calculated from the contact force. There is one force per node, divided by the area of the surface around the node.
• The element normal stress is calculated from the displacement of the nodes (1 displacement per node), then the strain at the internal gauss points due to the displacement, then the stress at the gauss point, then projected/extrapolated to the corner nodes. Since there are multiple solid elements connected to the node, each element can have a different stress value at the same node. The value shown in Inventor is the average of all the elements. (With a tet mesh, there can be many internal elements connected to the nodes, more than the few elements you see on the surface.) All of these calculations lead to some inaccuracy.

John

[John_Holtz · Accepted solution]

I just learned that the contact pressure is calculated and report at the "centroid", so there is only 1 result per element face. Inventor smooths the results from centroid to centroid which makes it look like a "smoothed" plot, and the marker flags and "Nodes > Query Display" make it appear that the result is from the nodes. (It is not; that is an interpolated result from the face centroid.)

The stress result is calculated at each corner of the element, and the average of all elements connected to the node is displayed. Since the contact pressure and normal stress are from two different locations on the element, 

• the results should be similar where there is no change from element to element
• I would expect the results to be different where there is a large difference from element to element.

Hope this helps.

John