## General Mechanical

Topics relate to Mechanical Enterprise, Motion, Additive Print and more

#### Inputting displacement to get reaction force results work but not the other way

• Hakim Dina Anjum
Subscriber

I want to find the minimum pull force to pull out a glass shelf from the grip of its clamp. I have used displacement boundary conditions that inserts and retains the glass shelf into and from the clamp, and extracted reaction forces of 230N.

Now on another analysis, I want to give this 230N force as boundary condition on the glass to pull it out of the clamp. But in this analysis the solution does not converge. Errors suggest to check the model constraints and contacts. Can I have some understanding as to why this happens? I have provided the same contacts and constraints in both analyses, the only difference is that in the first one I had given a displacement to extract reaction force results, and on the second one I want to input a force to extract deformation results.

• Dave Looman
Ansys Employee

It's recommended to apply displacement loading for such an analysis and the force produced is completely valid.  When you specify displacement you are telling the program the solution at each time point so it's naturally easier, but with a force when the connection slips you have no stiffness to carry the load and the program can't solve that case.

• mjmiddle
Ansys Employee

I believe Dave is getting at rigid body motion when he says "when the connection slips." A displacement constraint is a load which directly defines the degree of freedom values on the nodes involved. So while rigid body motion is not allowed in a static structural analysis, and causes nonconvergence, it is allowed if that RBM is fully applied on the DOF by a displacement load. By the look of your model, it does not seem like it is a model with RBM, but any failure or slippage at the contact would allow RBM. So contact slippage can allow convergence when the load is applied as a displacement but not as a force.