Hello all,
how can I link two components rigidly?
How can I simulate the kinematic coupling of Abaqus that It Is used to link the portions of two components?
*MPC, EQUATION or TIE CONSTRAINTS?
Thank you
Rigidly ? Then you should use rigid body constraints. Their ref nodes can be connected with equation constraints or springs: Simplified spring model for coupling two bodies
But kinematic and distributing coupling constraints are also available in CalculiX, just with some limitations.
Tie constraints serve a different purpose. They permanently bond the selected touching surfaces like contact with no relative motion.
1 Like
The same keywords as in Abaqus… try to use element surfaces instead of nodes, if possible.
*COUPLING, ...
*KINEMATIC, ...
There are some small differences in syntax though. Explained under point 9 here: A Guide to Modifying Abaqus Input Files for Use in CalculiX
1 Like
I should specify in kinematic all dof 123456?
In the card kinematic I read that I can specify only 123
How can I do to create a kinematic couplic 123456?
That’s how it works in CalculiX, rotational DOFs are not explicitly available and just constrained internally:
Since CalculiX does not have internal rotational degrees of freedom, the translational degrees of freedom of an extra node (rotational node) are used for that purpose, cf. *RIGID BODY. Therefore, in the case of kinematic coupling the following equations are set up:
• 3 equations connecting the rotational degrees of freedom of the reference node to the translational degrees of freedom of an extra rotational node.
• per node belonging to the surface at stake, for each degree of freedom specified by the user (maximum 3) a rigid body equation.
You can try connecting their reference nodes via *EQUATION constraint.
1 Like