Wrong direction of flow!!!
I was simulating the flow of Vane tidal turbine. After running in CFX-Solver, I analysed the result in CFX-Post, the direction of flow made me surprised and confused. I mean the direction of flow tends to run from the outlet to the inlet. Physically, the flow must direct from inlet to the outlet.
I divided the inlet and outlet into 2 parts for each (Part no.1 for water, and part no.2 for Air). In term of outlet boundary condition, I setup part no.1 (Water) as "outlet"; meanwhile, part no.2 (Air) is setup as "opening".
If I change part no.2 into "outlet", it will immediately appear the error "Overflow". But if I keep setting up part no.2 as "opening", that'll run well. however, the direction of flow is still wrong in this case.
Are there anyone able to give me some explainations and useful advices for this??? If u really care about my problems, I can send several images of my model and my set-up parameters to u.
You obvious have something very wrong in your setup. Please post an image and your CCL on the forum.
This is a link of my document, including one powerpoint file and some pictures of my calculation domain in CFX-Pre.
Please check carefully the informations of my calculation. I'm so confused about this. I over and over re-designed and changed many parameters, but it was still wrong. :((
For this model you should use the alternate rotation model. This is because the fluid is still really travelling in the stationary frame and not rotating in the rotating frame. This will improve convergence a small amount. Look in the documentation for more details on this.
Remove the specified pitch angles, make that "none". You are modelling the whoel rotor so you do not need pitch correction.
This model would be MUCH simpler if the inlet is purely water. You appear to have half water and half air. Is that what you really want to model? Wouldn't the water fill the whole inlet runner, at least at the inlet?
Unless you know what you are doing and have done a sensitivity analysis do not define the time step size yourself. Use adaptive time stepping, homing in on 3-5 coeff loops per time step. The most common mistake by newbies in transient simulation is by setting a time step size that is far too big.
Remove the minimum coeff loops in the convergence tolerance, and make the maximum 10.
Obviously this is a transient simulation. There is no way this was ever going to work steady state.
Oh yes - and your mesh quality at the bottom of the rotor where the blades almost touch the bottom is likely to be horrible. It might be worth your while to distort the geometry slightly in this region to improve mesh quality.
Many thanks for your advice, Mr.Ghorrocks
I'm reading about "alternate rotation model" to understand clearly before I set up. the link above is my "*.def" file that I setup before to simulate.
As u know, the inlet must include water and air because that's my professor's project. And I'm an assistant for him. I have a mission of modeling it.
I'm new user of Ansys CFX. Then I have a little experience. And I have to learn about this so much!
Again, many thanks to your comments.
|All times are GMT -4. The time now is 03:53.|