Rotating Domain
 

Hello,

i am looking for some advices about the "rotating domain". I would like to integrate a rotating fan into a simulation, where i have to connect "rotating domain" with "stationairy domain". Rotating domain is a radial fan.
The question ist about the size of the rotating domain: How much bigger should be the rotating domain as the mechanical geometry of the fan only?

Thank You,
Michal Szczepaniak

It does not matter. The GGI can be close or far, either way works fine. A little bit away is marginally optimal as it means the interface is not very close to the blade and this should help convergence slightly.

Dear Szczepan,

Is there any casing (for example; a spiral housing) around impeller?
if there is , CFX suggest that; rotating and stationary interface should be on halfway between blade end and nearest stationary wall.

Dear Altano,

thank you for you advise.
Yes, this is a closed impeller of a radial fan. (see example in the attached file)
One more question:
Blade was designed in BladeGen and meshed in TurboGrid. Have you any advice to design the housing? I have this in CAD-Software, but then I have in CFX an assembly (blade + housing).
Is there any possibility to to this as one part?

http://www.mcnallyinstitute.com/images/14-02-02.gif

Dear Szczepan,

If you mean, design parameters of volute, this is very long subject to write here. I suppose you asking a practical tool for drawing and meshing, just like Bladegen-Turbogrid pair.

I'm sorry, with your available tools, quick answer is no.

I've completed hundreds of centrifugal fan simulation, if I choose bladegen and turbogrid to CAD and meshing my routine would be like below;

-Create a rotational domain for Turbo-grid in Bladegen,
-In Bladegen, export your domain for other CAD tool as IGES
-Create your full stationary domain in traditional CAD software( solidworks, inventor, proE etc..), (neglect impeller volume)
- import your IGES part (rotating domain) in to CAD software, then subtract from your full stationary domain.
-now you got your real stationary domain.
- Create a Mesh in ANSYS Mesher for your stationary domain, create a named selection for interfaces and other boundaries.
- Create your impeller mesh in Turbogrid.
- import both meshes into CFX-pre, you are going see, interfaces will be perfectly matched. (geometricaly)

- Don't forget to create full rotor, as you know you got a mesh for just one blade passage. (for this, you can use, turbomachinery mode, or in general mode "mesh translation" in CFXpre.

Dear altano,

thank you for you advises. I followed their. I've made a test simulation with the radial fan. I attached below a image:

http://postimage.org/image/hw75yzbob/

Red colour is a rotating domain and blue is a stationary domain.

I have gived interfaces as follows:

- Rotating is an area of blades + ~50mm inside + ~50mm outside (outside diameter of fan is 400mm)
- Interface between rotating domain and stationary domain is FROZEN ROTOR
- Interfaces between blades passages are ROTATIONAL PERIODICY
- Interfaces betweend 2 stationary domains is GENERAL CONECTION

Is this setup OK?

One more question, what say pratcice about this: I would like to simulate a new design of fan, which wasn't tested. So I have any information about the physical boundary conditions (Pressure by inlet and outlet). Which boundary contitions should i give in this case?

Dear Szczepan,

The image looks OK. But I'm not sure about "- Interfaces between blades passages are ROTATIONAL PERIODICY" because it seems you have defined full rotor as I suggested before, if you use "turbo" mode and in component definition tab, choosen "available volumes" option as "entire passage" you don't need to define interface between passage.

If you use general mode I think interface between passage are should not be periodic because you don't use single passage.

As for the boundary condition; Total pressure@volute_inlet and static pressure@volute_outlet couple is the most realistic option.

Define TotalPressure@Volute_inlet= 0 [units], staticpressure@outlet=0[units].
It is give you free blowing capacity. Then increase your outlet pressure step by step with different runs and get your Pressure vs Flow performance curve..

Dear altano,

thank you for you advises.

1) I've deleted interfaces between blade passages. I've multiplied blade passages in CFX -> Mesh -> Transform mesh -> Rotation.
2) I've given boundary conditions, as you wrote (Total pressure @ inlet 0 Pa, Static pressure @ outlet 0 Pa).
Below there is a link to boundary conditions (wall type) and the solution

http://postimage.org/image/st9849xqf/

3) Is the pressure drop @ outlet area OK (See the picture above)? I've expected, that the pressure at outlet area still increases?!
4) At every wall i've defined no slip wall (no slip wall rotating at rotating interface). Is this acceptable?

Dear Szczepan,

Your boundary conditions is set for simulating a free blow radial fan.
The pressure drop @ outlet area is quite normal. , To blow out of volute the pressure in volute should be higher than the pressure @outlet section, otherwise air would move in to volute from outside ;).

In case of CFD all these images looks ok. But I have to say that your volute design is not good at all. There is too much recirculation in your volute because the cut water tongue is located too far from impeller