How can I calculate contact forces (contact reactions) in Traditional ANSYS?

WB ds.dat includes a POST1 procedure that can give the summed force at a contact (or target) surface. You need to know the REAL and TYPE attributes of the contact/target elements (REAL=5 and TYPE=5 in this example; use the appropriate numbers for your model):

esel,s,real,,5 ! select elements in contact pair
esel,r,type,,5 ! select element type corresponding to the desired side of the interface (contact or target)
nsle ! select all nodes attached to these elements
esln ! select all elements (including the underlying solid elements) attached to these nodes
esel,u,ename,,169,178 ! unselect the target/contact elements - this leaves just the underlying solids
fsum ! summed contact forces
allsel ! select everything again

To obtain the forces at individual nodes on the contact surface, simply replace the FSUM command with an NFORCE command.

Show Form
No comments yet. Be the first to add a comment!