Ansys Learning Forum › Forums › Discuss Simulation › General Mechanical › How to retrieve pressure on a elastic support › Reply To: How to retrieve pressure on a elastic support
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