## General Mechanical

#### Bending test simulation-help

• naga
Subscriber

I am trying to simulate four point bending test of glass specimen without symmetry but keep on getting the same error even after altering the conditions suggested in previous posts.

I would be greateful if someone could help me to find the problem.

• peteroznewman
Subscriber
It helps if you say what version of ANSYS are you using.nThere is a lot wrong with your loads and boundary conditions as shown below.nYou can see you have the force pointed in the wrong direction.nThe Displacement on the edge of the plank prevents displacement in Z which is wrong because as the plank bends, the nodes must be free to move in Z. Imagine a large displacement of the pushers in -Y. The ends of the plank will slide on the supports to such an extent that they could reach the support. This displacement boundary condition prevents this. nYou say you don't want to use symmetry, but X=0 is a symmetry boundary condition.nAll the contacts are Frictionless, so the plank is free to slide along Z as much as it wants to. Change at least one contact to frictional and enter a non-zero coefficient of friction to prevent this.nEach pusher body has 6 DOF but only 2 constraints (the line contact), so each one is missing 4 DOF to be constrained properly.nI recommend you delete the forces and instead create a translational joint to ground scoped to the two flat faces of the pushers. Edit the coordinate system under the Joint so that the X axis points in the -Y direction. Edit the Joint to have a behavior = Rigid. Add a Joint Load, type = Displacement to move the pushers down.nUnder Analysis Settings, turn on Large DeflectionnUnder Connections folder, insert a Contact Tool and check that all four contacts are Closed.n