I have an interesting FSI problem. I have an interesting FSI problem. I have a rotating shaft with blades on the end. The blades are non-symmetric so the shaft "whirls". I am trying to perform a FSI analysis on this model. The problem is once the structural model rotates, the FSI crashes.

I have been able to model in CFX by itself the effect of rotation by using a rotating domain where the shaft/blades in a rotating reference frame and the wall is "counter-rotating". I have also used a stationary domain an imposed a rotating boundary condition on the shaft/blades.

So, I am wondering how to get this type of problem to work when I add a rotating structural model and perform an FSI analysis. Is there some way to get the CFX mesh to rotate with the structural model during the transient run? Is there a way to perform a coordinate transformation on the structural model after rotation and input those coordinates into CFX every time step? Any suggestions?

Dr. Golf,

Firstly, what you describe at the end of your second paragraph I have also used a stationary domain an imposed a rotating boundary condition on the shaft/blades. will not give you the right result. Although you can specify a wall velocity normal to a wall, the solver can only apply a velocity that is tangential and ends up projecting your velocity components. The only way to model this is to either run it in a rotating frame of reference, as you have done, or specify the mesh motion to be rotating, which would require a transient simulation.

What is not clear here is what you are doing in your structural model. You can model rotation in ANSYS by specifying an angular velocity for the part. This behaves much like the rotating frame of reference in CFX; the effect of the rotation is accomplished through coriolis terms but the coordinates of the model do not change. If you have modeled it this way, there should be no problem.

-CycLone

Thanks CycLone, The trouble is that this is a transient problem. So, I'm specifying a rotation as a function of time. So, the structural model rotates. I'm not modeling the effect of rotation but actually the rotation itself.

I wish there was a way to rotate the CFX mesh along with the structural model.

You can do this by specifying the mesh motion as a rotation, but it isn't necessary. You can still have a transient rotation using rotating frames, just make the rotation rate a function of time.

CycLone, Yes, I've done that several times and it crashes on the first time step.

The issue is the Ansys structural model rotates and the nodal coordinates change. When the change is large due to a rigid body rotation, you get "A negative ELEMENT volume has been detected". Thus, the CFX mesh doesn't rotate with the ansys structural model.

Have you actually tried a model similar to what I am describing?

Yes, I have done this kind of simulation and I understand your issue. What I am asking is whether you need the structural model to rotate. If you specify a rotational velocity ANSYS won't actually move the nodes other than their defromation (unless you do not properly constrain the model). If this is not what you are doing, then please explain what you have set up.

CycLone, I'm giving the model a RemoteDisplacement as a function of time to impose a angular velocity on the model since I do need the structural model to rotate.

Do you need it to rotate to interact with another stationary component? If not, I would use the angular velocity instead.

OK, assuming you must rotate the model using a remote displacement you will need to ensure the rest of the CFX moving mesh boundary conditions behave properly. The FSI interfaces will receive a rotation rate through the interface. At inlets, outlets and openings you will need to specify the mesh motion as "undefined"; this will allow their motion to be solved implicitely. You could do the same for all the boundary conditions, but you might find that your walls deform slightly.

At the outer wall, the shroud, specify the mesh motion to be an angular rotation using the same function of time as the structural model but specify the wall velocity to be relative to the reference frame, as opposed to the mesh motion. This will keep it moving with the domain, but effectively apply a "counter-rotating" condition. Since CFX currently only allows you to specify the cartesian components of displacement, you'll need to do some trig. A possible alternative would be to use FSI here as well and create a very stiff dummy part in ANSYS with the same remote displacement as the blades.

Since you are in fact rotating the domain, don't specify the domain as rotating. The effect of rotation will arise from the mesh motion terms.

-CycLone

CycLone, Thanks for your response.

I understand now about using FSI with an angular velocity on the structural model. I can do this on some of my models.

On the remote displacement, I'm not sure about a couple of things. Let me see if I understand you. I have 4 domains: inlet, outlet, shaft/blades, outerwall. On the overall domains -- domain motion = stationary/ The inlet and outlet: mesh motion = unspecified. On the shaft / blades: don't specify a wall velocity and the mesh motion comes from the structural model. On the outerwall: check wall velocity relative to boundary frame and mesh motion specified displacement and create some user functions or CEL routines to specify the displacement at each time step with respect to the angular velocity of the structural model. So, am I understanding you correctly?

One thing that concerns me is that I understand how this with move the mesh on the shaft/blades and outerwall boundary. But, with the mesh comprising the volume between the shaft/blades and outerwall rotate as well?

Thanks again for your response.

Hi Dr. Golf,

That's essentially correct, although my advice is only for the rotating domain. If you have inlet and outlet domains that are not rotating, just leave them stationary and put a grid interface between them and the rotating domain. Note that in the case of a normal rotating domain (i.e. specified domain rotation rather than moving the mesh) CFX will clock the interface so simulate the rotation relative to the stationary domains if you specify the transient rotor-stator interface.

As for your last question regarding the mesh in between the moving parts... CFX solves mesh motion by applying the specified X, Y and Z displacements as boundary conditions to a diffusion equation. The motion is then diffused through the domain. If all the boundaries move together, the result is solid body motion. In your case the blades will move slightly differently because of the deformation of the solid body, which is just a slight +/- motion relative the net solid body motion.

-CycLone