Abaqus Contact Analysis

[Rocco_d1]

I have build a contact simulation (surface to surface, hard contact) in Abaqus in which a concave part is pushed against a convex part by a simple displacement along the U1 Axis. The main goal is to get the contact force. The result is quite fine, but I've got two problems.

1. It seems like the History Output for 'Contact Normal Force' (when selecting your contact surface as the set of interest) is adding up every single force of each node so the result is a force magnitude very much higher than you see in the field output. Is there a way to get a an average force applied on the surface?
2. I dont quite understand the difference between Reaction Force and Contact Force. In my result, the Contact Force is 'correctly' applied and displayed (by concerning the contact area), but the concave part which is the part displaced does not have any Reaction Force at its contact surface, just somewhere in the center of the budy. This is strange because the force is built up in the contact area but I dont get a Reaction force there.

Can someone help me with those issues?

 

[FEA way]

If you really need an average contact force instead of a total contact force (sum), you can save contact forces as history output and use Operate on XY Data to perform the averaging operation on them.

Reaction forces are non-zero only for nodes (and DOFs) with boundary conditions applied.

 

[Rocco_d1]

Thanks for your reply. In order to displace the part I've coupled a rigid body's RP (same diameter, RP placed in the center) to the outer surface of the part and I am displacing this RP. Isn't that a boundary condition with DOF in the U1 direction?

 

[FEA way]

In such a case, there will be a reaction force at the reference point of a rigid body constraint.

 

[Rocco_d1]

Many thanks for your advice. I've got a final question regarding the contact forces. Maybe I have an incorrect understanding of the way Abaqus is calculating the forces. In the field output (where the part is displayed with the colored forces acting on the nodes) I've got much lower forces than in the History Output for CFN. Is the CFN the correct totally applied force on the surface and the forces displayed in the field output are just something like an incremental force for calculation? Because in my undestanding, if I apply a uniform force of for example 200N to a surface and the force is evenly distributed to the surface nodes, the force applied to one node should also be around 200N.

 

[FEA way]

Forces are uniformly distributed on a surface, meaning that each node has only a fraction of the total force acting on the surface. Take a cube, fix its bottom and load the top with a known force (via rigid body constraint because concentrated force applied to a whole face would result in each node being loaded with the specified force magnitude). You will see that you have to sum the nodal reaction forces to get the same force as the applied one.