Hi
I simulated the forming process of a metal plate (considering plasticity and large displacements) by incrementally imposing a displacement field on the plate. This simulation works well. Now, how do I simulate the plate’s natural (elastic) recovery (spring-back) by removing the imposed displacement boundary condition?
Thank you.
Thank you.
Jack.
BCs can be removed with *BOUNDARY, OP=NEW and no redefinition in the subsequent step.
Thanks for your answer.
I used *BOUNDARY, OP=NEW before the next *STEP block and ran the analysis. However, no convergence was achieved. I believe that removing the displacement boundary conditions instantaneously is causing convergence problems.
Is there a way to remove the boundary conditions gradually?
By the way, under the *BOUNDARY, OP=NEW command, should I list only the boundary conditions to be retained, or should I also include those to be removed?
Thanks,
Jack
The idea is to use *BOUNDARY, OP=NEW in the step where you want to release BCs and redefine only the necessary ones.
That’s also how Abaqus deactivates BCs:
And they are removed by replacing them with equivalent forces and ramping them down to zero during the whole step (or immediately in dynamic analyses due to a different default amplitude).
Thanks!
Now is working!
Replacing the removed BCs with equivalent forces sounds good. But, I not know how to replace them with the reaction forces in those BCs). Instead I using a second step considering dynamic response. However, how to reproduce a quase-static response?. Increasing the damping coefficient?
Thank you so much again!
(however
Jack
What I described is done automatically by the solver when you deactivate a BC with *BOUNDARY, OP=NEW.
Dynamic implicit ? Unfortunately, CalculiX (unlike Abaqus) doesn’t have predefined quasi-static application mode but you could try decreasing the alpha parameter:
The parameter ALPHA takes an argument between -1/3 and 0. It controls the dissipation of the high frequency response: lower numbers lead to increased numerical damping ([65]). The default value is -0.05.
So −0.333 is maximum damping.
What I described is done automatically by the solver when you deactivate a BC with ‘*BOUNDARY, OP=NEW’.
Ok!. This is part of the *.inp file. This way of do that is ok? (thanks again):
…
** BC displacement
*BOUNDARY,AMPLITUDE=Damp
33,1,1, 0.000000
33,2,2, 0.000100
33,3,3, 0.000200
65,1,1, -0.000304
65,2,2, 0.000401
65,3,3, 0.000500
97,1,1, -0.000604
…
**
*BOUNDARY
NFRO, 1,3
NEND, 1,3
**
** amplitude curve displacements
*AMPLITUDE,NAME=Damp
0.0000, 0.0000,
1.0000, 1.0000,
2.0000, 0.0000,
**
** step block
*STEP, NLGEOM,INC=1000,
*STATIC,
1.0000e-04,1.000e+00,1.0000e-06,1.0000e-01
**
*END STEP
**
** second step block
*STEP,INC=10000
*STATIC
1.0000e-04,1.000e+00,1.0000e-02
**
*BOUNDARY,OP=NEW,AMPLITUDE=Damp
**
*BOUNDARY
NFRO, 1,3
NEND, 1,3
**
…
No need for *AMPLITUDE, just *BOUNDARY, OP=NEW and respecification of the BC(s) that you want to keep in the second step.
But how to reduce to zero (slowly) the reactions in the removed BCs ?
This happens automatically with no need for explicit amplitude definition. At least that’s what Abaqus does. CalculiX User’s Manual is less informative but it should be the same.
If a boundary condition is removed in a stress/displacement analysis in Abaqus/Standard, it will be replaced by a concentrated force equal to the reaction force calculated at the restrained degree of freedom at the end of the previous step. If the step is a general nonlinear analysis step, this concentrated force will then be removed according to the AMPLITUDE parameter on the *STEP option. Therefore, if the default amplitudes are used, the concentrated force will be reduced linearly to zero over the period of the step in a static analysis and immediately in a dynamic analysis.
