# difference between coupling and constrain equations in ansys

by anoopsrikanth
Tags: ansys, constrain, coupling, difference, equations
 P: 11 What is the difference between coupling and constrain equations in ansys
 Sci Advisor P: 1,497 IIRC one is on a nodal basis, while the other is on an element basis.
 P: 11 Thanks Can u explain be with a example or in detail and wt does iirc means
P: 1,497

## difference between coupling and constrain equations in ansys

IIRC == If I Remember Correctly

As far as an example, I typically preferred to do coupling on a nodal basis, via CP, CPINT, or CPCYC commands.

CP is used when typically when you're manually joining together two groups of nodes that may not necessarily be coincident.

CPINT is used when you have two adjacent surfaces that you'd like to connect. Often times I would use these instead of contact regions. Contact regions make the problem nonlinear and increase solution time drastically. Aside from that, they are picky and can often ruin a solution if not defined well.

So, as an example, let's say that you're doing a 2D axisymmetric analysis of two tubes, one which fits inside the other. You could take the nodes at the interface and couple them via CPINT only in the UX direction (radial). This would allow the parts to slip both tangentially (if doing 3D) and axially.

CPCYC is cyclic coupling. I've typically used it when doing a 3D sector analysis. The other option is the CYCLIC command which like coupling commands, increases solution drastically. If you were doing a slice of a part, you would select the outer slice nodes, issue the CPCYC command in all directions (ensuring you were in the correct coordinate system).

All of the CP commands assume that you either have matched nodes, or at least close. There is typically a tolerance on the commands, but aside from that they assume matched nodes. In fact, if you increase the tolerance too much, you'll get nodes being coupled to more than 1 node on the adjacent side, and the solution will bomb.

CE commands are very similar except they operate on an elemental basis, meaning they doing require matched nodes. Because of this, however, I find that they don't quite work as well.
 P: 11 thanks for the info. i am doing a chassie static analysis how can i best transfer the mass of a structure sitting on the chassie. i know that creat a mass element and it can transfer the load but connect it throug CP or RBEs confused pls help me
 Sci Advisor P: 1,497 I would use CPs. I know of RBEs, know that they have their uses, but haven't found myself using them very often. Create a mass and CP it to the applicable position(s) on the chassie...do you mean chassis?
 P: 11 I am doing a G load analysis,Can any suggest the correct value to GRAVITY Model Units in MM, Density in Tonne/mm3, Youngs Modulus in MPa I am confused weather to take 9810 or 9.810 Please Suggest
 Sci Advisor P: 1,497 What are the units of acceleration? What unit are you using for length? What about time? You're using metric, it should be pretty straightforward. Be lucky you doing have to worry about gc.
 P: 11 If Length in mm g is mm/s2 is the value of g will be 9810 mm/s2 or 9.810 mm/s2 confused little bit please help me out.
 P: 93 Try solving the following equation using [kg] and [m/sē] to get [N]: F = m.a Now try again combining [kg] or [tonne] and [m/sē] or [mm/sē]. Which mass and acceleration units can be combined to give the same numerical result as [kg] and [m/sē] ? Which combination returns consistent units ?