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.