[Rockytime]

Hi All,

CFX solve pop out this error before it starts to run.

The angle between the specified velocity and the element surface is|
| 43.727 degrees at this face. This is considered an error because |
| it implies that the mesh is moving. The following are possible |
| reasons for the error message.

In the CFX setup, I set my fluid wall to counter rotating wall. It works in cylindrical enclosure but it fail to work in a rectangular enclosure. Anyone can tell me how should I setup? in order to make the rectangular enclosure stay stationary?

Fluid Wall

[ghorrocks]

The counter rotating wall condition applies a tangential velocity to the selected wall such that it opposes the domain rotation and results in a stationary wall in the absolute frame.

But, as the error message says this requires the velocity to be tangential and that means axisymmetric about the rotation axis. Your rectangular box is not axisymmetric, so you cannot model the walls of your rectangular box with counter rotating walls. This approach will work with cylindrical walls as they are axisymmetric.

[Rockytime]

Hi Glen,

Thanks

So did you have anyway to let my rectangular duct stay in stationary frame while I setting the domain as rotating motion?

[ghorrocks]

The rotor goes in a rotating frame of reference and the stationary rectangular duct goes in a stationary frame of reference. So there will be 2 domains, and they are connected by a GGI with some form of frame change model.

[Rockytime]

So for the frame change of model, can I just select general connection with frozen rotor?

[ghorrocks]

If frozen rotor is an applicable frame change model for you then yes. From what I can see of your model I suspect it is appropriate.

[Rockytime]

Another question, I have 1 enclosure and 1 import turbine geometry. Do I need to use boolean to subtract them into 1 body? No right?

[ghorrocks]

Probably - but I do not know what your enclosure is. I can guess what your turbine is.

This question is best asked on the geometry and meshing forum. But before you do, make sure you do the tutorial examples on turbomachinery for the meshing software and CFX so you understand the basics. You can download these from the ANSYS customer website.

[Rockytime]

Ok. Thanks for your advice.

I Have set my turbine in rotary domain with a rotational velocity and setup the wall boundary as well. I'm just wondering do I need to turn on mesh deformation and specific mesh motion at my wall turbine boundary? Is it ok if i specify my mesh motion with surface of revolution? Sorry for asking too much question. I try to understand mesh motion through the cfx tutorial but I still not quite sure how it function.

[ghorrocks]

If the device only rotates then you do not need mesh motion. It can be done as rotating frame of reference.

You only need mesh motion if it does some other motion (eg translates and rotates) or it deforms.

[Rockytime]

Ok. I run my simulation in transient analysis, but it seem the result is not in my expectation. Will it be different if i run my result in steady state analysis?

The reason I run my result in transient is I can vary my inlet velocity with CEL function. So I can see how much my torque increase when the flow increase in one graph.

[ghorrocks]

So I can see how much my torque increase when the flow increase in one graph.

A common misconception. Do not do this - how do you know the transient effects have faded out? Also this approach is much slower than doing a series of steady state simulations.

As for your first sentence: I have no idea what results you got, what results you expect and how you have set your model up. I cannot answer that question with more information.

[Rockytime]

Ok. My simulation consists 2 domain. 1 is the Rectangular Duct ( Fluid Body) and another 1 is rotor.

I setup both domain as fluid domain with air @ 25 degree. The Rectangular Duct domain motion is set as stationary domain and the rotor is set as rotating domain and specific with a rotating speed (-4500 rpm). The fluid model is set as Shear Stress Transport (SST) with the advanced turbulence model curvature correction and production limiter.

Rectangular Duct Domain, contain 3 boundary, Inlet, Outlet and Wall Boundary. The face that located at +y axis is inlet, -y axis is outlet, the remaining faces is set as Wall boundary with stationary domain. No slip wall is applied on the wall boundary.

Rotor Domain, I named all the selection ( Shaft, blade, hub) and create them together as Wall boundary with (frame type= Rotating). No slip is applied on the wall boundary.

The result I expect is the turbine should be stall at some point when the flow increase jsut like the what picture below shown.

Now the problem im facing is I keep getting the same torque value even with I set different value of flow for inlet flow velocity.





Bellow is the Cel Code for your better understanding.

[turbo]

Your geometry setup is wrong. CFD is only for a negative volume from CAD where fluid is filling. If sticking to your original intent, you should have a single domain. But such an approach is wrong, too, in the square duct enclosure case.

[Rockytime]

Originally Posted by turbo

Your geometry setup is wrong. CFD is only for a negative volume from CAD where fluid is filling. If sticking to your original intent, you should have a single domain. But such an approach is wrong, too, in the square duct enclosure case.

Hi turbo, I cant get what you mean. Can you further explain what wrong with my geomtery?

[turbo]

1) Make a negative volume solid.
2) Make two solids : one is a cylindrical solid immediately surrounding the rotor, the other is the rest volume with the square duct boundary.
3) One is for rotating frame, the other for stationary.
4) Stage interface.

[Rockytime]

Originally Posted by turbo

1) Make a negative volume solid.
2) Make two solids : one is a cylindrical solid immediately surrounding the rotor, the other is the rest volume with the square duct boundary.
3) One is for rotating frame, the other for stationary.
4) Stage interface.

Hi turbo, do you have any example what is negative volume solid?

Is it like the step below?

1)Create---> Rectangular Enclosure
2) Create --> Boolean ---> Operation: subtract, target body: select recetangular enclosure, tool body: select Rotor. Preserve tool bodies? Yes
3) Create ---> Cylindrical Enclosure around rotor.

Am i right?

[turbo]

Yes, the negative volume is what CAD people say using Boolean.

[Rockytime]

HI turbo and Glen,

I had done the negative volume (booelan) in the geometry.

)Create---> Rectangular Enclosure--> target bodies rotor
3) Create ---> Cylindrical Enclosure ---> target bodies rotor.
2) Create --> Boolean ---> Operation: subtract, target body: select cylindrical enclosure , tool body: select Rotor. Preserve tool bodies? No.

And after that I have create 2 domain.

1st Domain - Rectangular Enclosure

Stationary Domain

- Boundary

1)Inlet (Constant Velocity) ,

2)Outlet (Average Static Pressure, Relative Pressure = 0 Pa,

3)Fluid Wall - Location 4 surface around the Rectangular Enclosure, No Slip Wall Condition.

Rotating Domain

- Boundary

1) Wall Boundary - " Whole Rotor " - Frame type Rotating - No Slip Wall

2) Wall Boundary - Rotating Wall - Frame Type Rotating - Wall Velocity -Counter Rotating Wall - No Slip Wall

Interface

Frozon Rotor

I run the simulation as steady state and the torque value I got from the blade does not increase even though I keep increasing the flow. I expect it
will increase like the graph i show above.

Did I do anything wrong on my setup part? I attach my CCL inside the word file if you need any further information.



StreamLine


Rotor rotating


Counter Rotating Wall -

[Rockytime]

Hi Guys, I know it is quite long. But I really hope u guys can help me. thank you. Apologize in advance if I did any basic mistake.