Hello, Since Abaqus uses a 3 x 3 x 3 - Gauß quadrature one of the 27 integration points is actually located at the centroid of the element. Therefore, it is not reasonable to obtain a higher stress value at the centroid as compared to at the corresponding integration point. Accordingly, Abaqus does not interpolate the stress at the centroid from the stresses at the integration points. One other option would be to extrapolate the stresses from the 27 integration points to the 20 nodes. The stresses at the nodes can than be significantly higher at the nodes (if the mesh is not fine enough). These nodal values can then be used to coumpute the stress at the centroid (either by interpolation using the shape functions ore by simple averaging). Another option could be to compute the nodal stress values as before and than average them for adjacent elements. If one node belongs to 3 finite elements the stress value differs for each of those elements (this jump is also a measure of the result quality). We then first average the stress values from adjacent elements and then compute the stress value at the centroid. From my experience it is almost impossible to find the information in the manual. So the best you could do is to test the different methods and see when the results coincide. This is the answer by Mr Duczek.

Hi Prithwish,

I think there is some confusion regarding the "Center" of the element. In a shell you have multiple section points throughout the thickness, and by default you get the values from the top and bottom, but you can request midpoint as well, if I remember correctly.

Now the S4R element itself has a centroid, but the stress values there are still output throughout the thickness, so at a section point. If I understand correctly, what you are looking for is to get outputs at the centroid of the element (what you have already requested), but plot the mid section point value. You should be able to set this up easily in the output requests/during post processing.

Hope this helps,

Best regards,

David

Hi.

For shell element, there are several integration points though the thickness (the quantity is up to you in Property-Section-Thickness integration points, default is 5). To output the stress of the middle point (or central), i.e. the 3rd point, (e.g. if u set 9, it should be 5th). Anyway, just go to "Edit Field Output Request", in the bottom "Output at shell, beam, and layered section points- specify: 1,2,3,4,5 ",then u can get all the stress of those 5 points (default is 1 and 5, "SP1" is the point on the inner surface or bottommost, and "SP5" is on the outermost or topmost, if u only want the middle, just type 3 )

Someone may need the integral average stress instead of that on the inner/outer surface. The way to obtain is: output the stresses of each points, and average them by timing the weighted coefficients (Simpon/Gauss coefficients, remember to check your set in "Property-Section")

By the way, if u need the visualization of the middle-point stress (or topmost /bottommost), the way is: Result- Section points