Attach Spring to a rigid element

There are tow ways to get rigid behavior.

Increasing young modulus which will negatively affect the time step

or, while creating the RBODY, you can get the rigid behavior by selecting the all nodes from the upper one of the cuboids. In this way, the upper one of the cuboids will be rigid. Then you can define the INIVEL by selecting main node of RBODY you created.

There are tow ways to get rigid behavior.

 

Increasing young modulus which will negatively affect the time step

 

or, while creating the RBODY, you can get the rigid behavior by selecting the all nodes from the upper one of the cuboids. In this way, the upper one of the cuboids will be rigid. Then you can define the INIVEL by selecting main node of RBODY you created.

Thank you, that helped!

Follow up question: My time step is still limited by the models I'm simulating as rigid.

Is there a way to tell radioss to disregard parts in the timestep calculation?

Thank you, that helped!

Follow up question: My time step is still limited by the models I'm simulating as rigid.

Is there a way to tell radioss to disregard parts in the timestep calculation?

I'm not sure what your aim is with the modelling you have, in your HM you have used /RBE3 which suggests you are trying to distribute the loading to the solid mesh? But you want the Solid mesh to be Rigid? so there is no need to do that?

Any entity that is fully in an /RBODY will be disregarded for timestep, but in your HM, you have only the top and bottom surfaces selected? And you are using /RBE3 (which do not have the effect of removing the elements from the timestep calculation)

Are you interested in the Stresses and Strains in the solid elements at all? If your only interest is the spring, then you can lose the /RBE3 and just make the solid entities fully rigid with /RBODY?

I'm not sure what your aim is with the modelling you have, in your HM you have used /RBE3 which suggests you are trying to distribute the loading to the solid mesh? But you want the Solid mesh to be Rigid? so there is no need to do that?

Any entity that is fully in an /RBODY will be disregarded for timestep, but in your HM, you have only the top and bottom surfaces selected? And you are using /RBE3 (which do not have the effect of removing the elements from the timestep calculation)

Are you interested in the Stresses and Strains in the solid elements at all? If your only interest is the spring, then you can lose the /RBE3 and just make the solid entities fully rigid with /RBODY?

Thanks for your in-depth response!

I built the model in a way that I could reverse the rigid behaviour of the parts.

The model you were looking at was outdated, the new working model is attached.

However I also tried your recommendation this morning and when I make the solid entity fully rigid by checking the Rbody option, I end up with the error 402 ** ERROR IN ELEMENT PART DEFINITION. Do you have any suggestion why this is the case?

Edit: I checked the output file of my main model. There the limiting factor (column Element) for the time step seems to be the main node of one of my rigids. How can that be?

Thanks for your in-depth response!

I built the model in a way that I could reverse the rigid behaviour of the parts.

The model you were looking at was outdated, the new working model is attached.

However I also tried your recommendation this morning and when I make the solid entity fully rigid by checking the Rbody option, I end up with the error 402 ** ERROR IN ELEMENT PART DEFINITION. Do you have any suggestion why this is the case?

 

Edit: I checked the output file of my main model. There the limiting factor (column Element) for the time step seems to be the main node of one of my rigids. How can that be?

Odd, I get no error on running it... in fact it seems to do what you wanted? Timestep is over 100 times larger than the stable timestep of the deformable model? (7.8e-2 vs 4.5e-4)

If you intend the cubes to be steel, and your units are kg/mm/ms, your steel density is 10x too low (should be 7.8e-6, not 7.8e-7) it runs even quicker if you correct it (timestep is then 1.7e-1)

Rigid Bodies still have a timestep calculation as follows calculated from the stiffness and mass of connected entities, (below from help), it is many times larger than deformable

Odd, I get no error on running it... in fact it seems to do what you wanted? Timestep is over 100 times larger than the stable timestep of the deformable model? (7.8e-2 vs 4.5e-4)

If you intend the cubes to be steel, and your units are kg/mm/ms, your steel density is 10x too low (should be 7.8e-6, not 7.8e-7) it runs even quicker if you correct it (timestep is then 1.7e-1)

Rigid Bodies still have a timestep calculation as follows calculated from the stiffness and mass of connected entities, (below from help), it is many times larger than deformable

Thank you for pointing that out! The steel density was a typo in my simplified model but the main model had a lot of different flaws.

After reading throgh radiOSS help again I noticed the reason for the low time step was a spring I modelled to be insanely stiff after reaching the end stop - in hindsight not very smart.

So the problem after all wasn't the RBody but a spring connected to it.

Thanks for all the help!