[dunapkt]

Hi all, I am currently working on a CFX tutorial about flow in an axial turbine stage provided by ANSYS. However, after the simulation, I noticed discontinuous contours between the stator and rotor domains. I have attached two pictures showing velocity and velocity in stn frame at 0.5 span. Does anyone know why this is happening?

[ghorrocks]

The velocity is a FAQ: https://www.cfd-online.com/Wiki/Ansy...f_reference.3F

The Velocity in Stn Frame will be discontinuous due to some combination of:
* Your choice of frame change model. Some frame change models are discontinuous. Make sure you undestand the frame change model you are using.
* Coarse mesh
* Poor convergence

[dunapkt]

Thanks for the reply ghorrocks. However, the velocity contour is just an example, and the same issues have occurred with other parameters such as pressure, temperature, and so on. The convergence criteria were set to 1E-4, and I believe the mesh is fine enough. Should I change the convergence criteria to E-5 or E-6?

[ghorrocks]

OK, let's go through them:

What frame change model are you using? Please attach your output file.

You say the mesh is fine enough - how do you know this? How did you tell?

Convergence - yes, you should try tighter convergence and see what effect this has.

[Opaque]

Originally Posted by dunapkt

Thanks for the reply ghorrocks. However, the velocity contour is just an example, and the same issues have occurred with other parameters such as pressure, temperature, and so on. The convergence criteria were set to 1E-4, and I believe the mesh is fine enough. Should I change the convergence criteria to E-5 or E-6?

Just to emphasize Glenn's comment on the mesh. There is no such thing as "I believe" in engineering. Either is fine or it is not. it must be an unbiased statement based on standardized metrics.

In the case of the mesh, you MUST verify your solution is insensitive to mesh refinement, if so you can then positively and definitely state "My mesh is fine enough to produce an accurate solution for the selected model".

Of course, to compare solutions on different meshes you must be certain the solution is converged. That is, the solution fields do not change if the residual is converged/reduced further.

[dunapkt]

Sorry for the late reply.

First, I used the stage(mixing-plane) with steady-state analysis.

Second, my initial mesh consisted of 1M cells for stator domain & 2M for the rotor domain, resulting in a total of 3 million cells. I attempted to improve mesh quality by increasing the total number of cells from 3M to 30M step by step, and in each cases, y+ was set to less than 1 at all walls and less than 0.5 at the blade surface. Of course, results are slightly different from case to case, but not by much (less than a 1% difference). This is why I believe mesh is fine. However, I still have the same discontinuous problem. Could it be a problem with the boundary conditions?

[ghorrocks]

First, I used the stage(mixing-plane) with steady-state analysis.

That is why you are getting discontinuous variables then. See the CFX Reference Guide, section 11.4.2 for details on the mixing plane model, especially note: "The model is not suitable for applications with tight coupling of components and/or significant wake interaction effects..."

If you want the variables to be continuous across the frame change then use a frame change model which supports it, such as frozen rotor or transient rotor-stator.

Yes, I agree your final comment suggests your mesh is not the problem. Thanks for explaining that.

[dunapkt]

Ohh.. I see. Thanks for your help! I hope you to have a good day.