switch rigid body on and off between steps

[liq001]

Hello everyone,

I am wondering is there any possibility that I can switch rigid body on and off between steps? or can I use import analysis to import the rigid body as deformable?

Best
Lee

 

[FEA way]

Rigid body constraint can’t be deactivated during an analysis but you are right that the import technique can help with this.

 

[SWComposites]

import the rigid body as deformable? huh? this makes no sense. what exactly are you trying to model?

 

[liq001]

I have a simulation that need 100 hours to finish. Thus I would like to use rigid body at some of the steps while switch to deformable body to capture the deformation. @SWComposites

 

[liq001]

Thanks, FEAway. do you know any examples can do this? Thanks again

 

[TimAero]

I had a similar issue once, and was able to throw all the nodes of the 'rigid body' in a set and apply a BC=0 to all which can be easily turned on/of between steps. This will only work if your rigid body is not needed to move during analysis. I was able to rearrange the BCs such that everything moved around my rigid body. I do not know if this is an option for you.

 

[FEA way]

Setting zero displacement BCs may work but it's risky due to potential overconstraint issues with contact and other constraints. Another trick, used before rigid bodies were introduced, is to apply a very high Young's modulus. It can be changed in time as well.

But in this case, I would just recommend using the import procedure. It's quite simple in Abaqus/CAE. Just import the parts from the odb file from the previous analysis and apply the initial state field to those that should keep the material (stress-strain) state. Other parts can be added/redefined as desired.

 

[liq001]

@TimeAero, thanks so much for your comments. Could you please share a sample input file? In my model, all the rigid body parts are moving around.

 

[liq001]

@FEAway, I tried to import the rigid body in the second analysis. However the imported parts still keep as rigid, could you please guide me on how to apply the initial state field? I will need velocity field from last step as well.

 

[TimAero]

@liq001 please find attached. Created in Abaqus/CAE 2020. Please be aware of computational convergence when releasing and overconstraints in general using this method.

 

[liq001]

@TimAero Thanks so much for sharing.

 

[liq001]

@FEAway, I tried to import the rigid body in the second analysis. However the imported parts still keep as rigid, could you please guide me on how to apply the initial state field? I will need velocity field from last step as well.

 

[liq001]

@FEAway, any idea of this? I tried to import the rigid body in the second analysis. However the imported parts still keep as rigid, could you please guide me on how to apply the initial state field? I will need velocity field from last step as well.

 

[FEA way]

It should work, I tested this on a simple model with 2 cubes on top of each other - one deformable and one rigid (due to rigid body constraint, not rigid elements). In the second model, both cubes are imported with their deformed configuration using File --> Import --> Part and selecting odb from the previous simulation. Also, an initial state field is applied to the one that was previously deformed and material is applied to the one that was previously rigid. They both act as deformable parts now.

 

[liq001]

@FEAway, Thanks for your input, could you please share your simple model? The input files for the 1st and 2nd analysis will be very useful. Thanks again,

 

[FEA way]

I attached the input files.

 

[liq001]

Thanks so much @FEAway