error message slave DOF

[alexos1975]

Hello!

I got an ANSYS error message, which consequence is still unclear to me:

Specified constraint not allowd on slave DOF in coupled set. Coupled set No.1 First node=2 Slave node= xxxx DOF=volt
Move constraints to first node or remove coupling and constrain all.

Does anyone can give me a hint, where to find some more information concerning this error message? Or can anyone explain me the backgrounds of this error?

Thanks

Alex

 

[cbrn]

Hi,
that means that, on the "slave" node, there is a conflict between a directly-applied boundary condition (voltage in your case, it seems...) and another one coming to that node from a constraint-equation or a DOF coupling. Let me take an example from the structural field:
suppose you have a cyclic sector of an axisymmetric structure; suppose that all the nodes belonging to an anular surface orthogonal to the sector's "edge" faces must be fully-restrained (this is not physical - it's just an example); now, suppose you select this area ASEL,s,... and all the nodes belonging to it NSLA,s,1 and then you constrain them by setting UX, UY and UZ to 0. What will happen then? When ANSYS will generate the cyclic constraint equations, it will set each traslational DOF of each node on the "upper edge" of the sector to be equal to the corresponding nodes on the "lower edge" of the sector. BUT it will find that these nodes on the "upper edge", whose displacements must depend upon (= are slave of...) the corresponding ones on the "lower edge", already have an imposed displacement. Thus, a contradiction will arise and the message will appear. Then, the program won't generate the constraint equation for the contradictory nodes.
The correct way to proceed is to unselect the nodes on which the constraint equations will be applied (only the dependent ones, of course, not the "pilot" ones) before applying the desired imposed boundary condition(s).

Regards