Constraining a 2D Rigid Body

[sd90]

Hi

I am trying to simulate a cylinder pressing on a plate, modelled as rigid which is fixed to ground in 2D in Workbench. How can I constrain the rigid plate so that it does not move? Obviously fixed support does not work and Ansys isn't allowing the use of joints in 2D. Any ideas?

 

[Erik Panos Kostson]

One way could be to use hard springs instead, see image below.

 

[sd90]

Hi, thanks for the reply. Would it be possible to simmulate the plate as a rigid body by setting its stiffness to a very high number? I.e. if the cylinder is 1Gpa, have the plate as 1000 GPa? Would that be sufficient?

 

[karachun]

This is bad idea, you can get ill-conditioned stiffness matrix and big errors.
Link
You can constrain all nodes of rigid plate, which will make this body absolute rigid without additional stiffness.

 

[sd90]

How do I constrain all nodes in the rigid plate?

 

[Erik Panos Kostson]

You can constrain the nodes of the rigid body, by first defining them as a named selection (select nodes on the rigid body plate), and then using a FEA nodal displacement BC where you fix these nodes. See image below (highlighted shows the FEA node. displ. BC).

This is better than the springs.

 

[L_K]

Is there a particular advantage of setting nodal displacement to zero instead of setting
the stiffness behavior of the body to "rigid"? Does it also lead to possible ill-conditioned
matrix (similar to changing E's value)?

 

[karachun]

If you increase E by 1000 than all be ok. However, if you multiply it by 1e15 then you can get problems.
There are rule of thumb: difference in stiffness of three orders lead to inaccuracy of one order/digit. With single precision, you have 8 digits for results.