## General Mechanical

#### Electrical contact simulation problems

• Oriol
Subscriber

Hi you all!

I am working on a simulation in which my idea is to see the displacement of an electrical contact when you apply a force on it.

• Ashish Khemka
Ansys Employee

Please use a revolute joint instead of using frictionless support and cylindrical support. Also, force imbalance of 1N will give rigid body error. Instead, apply displacement and then find the force reaction at the displacement b.c. to see what force will cause the applied displacement.

Regards Ashish Khemka
• Oriol
Subscriber

Even though, I got very high values of the force reaction for a 5,5N simulating a spring load...
I was wondering how can I apply the force reaction using this other approach:
I cannot find any option from the force reaction probe to work on the highlighted yellow area.

• Ashish Khemka
Ansys Employee

If you have a contact defined at the highlighted yellow region then you can extract the force reaction at the contact location. Nodal forces must be turned on before extracting the force reaction.

Regards Ashish Khemka
• peteroznewman
Subscriber
The high force you measure moving the surface D in the Z direction is because that BC keeps the surface flat, but in reality, that surface rotates as it moves to open the contact.
Instead of using a Displacement on the surface D, use a Remote Displacement, Behavior = Deformable and enter the Z displacement leaving all others Free. Now the surface can rotate as it deforms. You will find the Reaction force from the Remote Displacement is lower.
Once you have a Remote Displacement (or plain Displacement) as a BC replacing a Force, you no longer need the other side of the contact. Suppress that part, the solution will be faster.
You should also try creating elements half the size, or smaller to get 2 elements through the thickness. This may lower the force further.