ABAQUS Explicit - define rotary inertia for a rigid body reference node

[pirs]

Hi everyone,

I have got the following problem I require some assistance with: suppose you got a rigid body (for instance,a rigid plate), which is globally restrained using boundary conditions on the reference node - every displacement and rotation is restrained, except for the vertical displacement of said rigid plate.

Now, I want to release one of the rotations, which requires the definition of a rotary inertia. My idea is that I need to define a ROTARYI element, which contains my rigid plate reference node.

*RIGID BODY, REF NODE=SupportPlate.40, ELSET=SupportPlate.SupportPlateElements

*ROTARY INERTIA, ELSET=??
I11, I22, I33, I12, I13, I23

My question is, how do I define the ELSET, which includes the REF NODE, as defined in the *RIGID BODY line?

Thanks in advance for any input on this.

 

[pirs]

Regarding my previous question, I realize that my question was not too clear. So, let me try again...

I have defined a rotary inertia element set (1 ROTARYI element, 1 node) with *ROTARY INERTIA. Now I want to associate this element with a rigid plate reference node, which is a well defined node set in my model. Does anyone know how to do this? It is worth mentioning I am writing an input file..

 

[akabarten]

Hi,

You need to define your inertia element at reference node of rigid body.

**
** rigid body definition
*RIGID BODY, REF NODE=1000, ELSET=myRigidBody-ELSET
**
** create rotary inertia element at rigid body reference node
*ELEMENT, TYPE=ROTARYI, ELSET=myInertia-ELSET
  1, 1000
**
** define rotary inertia
*ROTARY INERTIA, ELSET=myInertia-ELSET
 i11, i22, i33, i12, i13, i23
**

Regards,
Bartosz