Plastic deformation visualization with *boundary/*cload

[Vision78]

When using forced displacement the displacement exists within *Boundary as do the fixed constraints, I'm having some issues deloading the displacement without fiddling the fixed constraints that in my understanding have to exist before the displacement.

It works when using CLOAD, OP=NEW as fandaL has described on the forums before, (thank you) as you can remove that as its under a different input but I'm just wondering if its possible to do it to BOUNDARY as well.

The goal is to see the plastic deformation of the part after the load/displacement is removed.

[NewJoker]

Yes, you can do the same with boundary conditions - remove them in the second step using OP=NEW. Boundary conditions that should be kept must be redefined in that step then.

[Vision78]

Thanks, I thought I had tried this yesterday but maybe I placed the line after the other boundaries or something, works like a charm now.

Displacement on the random steel used went from the set 5mm to 3,72 on a random test case, I'll verify better once I get on my project as it takes a while to run those simulations.

For anyone googling after (me in a week), simply put the BOUNDARY, OP=NEW first in there and then redefine the other constraints you did not want to delete.

*STEP, NLGEOM
*STATIC

*BOUNDARY, OP=NEW

***********************************************************
** Fixed Constraints
** ConstraintFixed
*BOUNDARY
ConstraintFixed,1
ConstraintFixed,2
ConstraintFixed,3

Also noticed some people on ANSYS and Abaqus forums fighting with this sometimes.

Edit: Now fighting with convergence issues I assume come from Calculix trying to do the whole step in 1 go, running different kinds of attempts to see what works

[Vision78]

This is really weird, when I remove the displacement, calulix will fail with the error, too many cutbacks or the solution diverging, but when the same amount of movement is done using a load that is removed in the same fashion, it manages to do the increments and post a result.

Displacement did function well with a simpler model though

[Vision78]

Issue solved.

After doing the displacement, I made a new step to run the displacement to 0 and then deleted the displacement to show plastic deformation.

For some reason it was not applying any kind of incrementation for the second step when removing the displacement straight out, causing convergence issues.

Second thing that worked was usking CLOAD instead to drive it as far as the displacement would have and deleting it, for some reason in that instance there was no convergence issues.

Step 1: displace

Step 2: drive displacement to 0 (do not do if plastic deformation is severe enough that going back to 0 would cause deformation that way, use smaller steps or smth)

Step 3: OP=NEW the displacement and re-specify the fixed constraints to keep the model constrained.