Learning Forum

[Philippe DIERCKX]

I entered an elastic support in my Ansys model (steel structure on concrete where the concrete is modelled as the elastic support). This works just fine. I now want to check the resultant pressures on the elastic support (the same as pressure you can derive form the contact tool in case of contact). I can't seem to find a standard result item that generates this output. Anyone experience in this ?

Kind Regards

[Erik Kostson]

Hello
The element used for elastic support is SURF154 (see help manual for more info), and it has a result for foundation pressure. So we want to use that, do as follows:
Insert a user defined result.
In Scoping method choose Result File Item
Choose either Element Name IDs if (you do not have a pressure load), or Element Type IDs (if you have surface pressure loads – because that creates surf154)
Under Solver Comp. IDs choose depending on the above option 154 or find the Element type ID for the elastic support (can be done in the solve.out or the worksheet results summary).

Finally in expression write SMISC21

This gives the pressures (see help manual under surf154 in the element reference for more info.)
All the best
Erik