CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Rotating Domain

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   December 27, 2012, 08:29
Default Rotating Domain
  #1
New Member
 
Michal
Join Date: Sep 2012
Posts: 12
Rep Power: 4
Szczepan is on a distinguished road
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
Szczepan is offline   Reply With Quote

Old   December 28, 2012, 05:31
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,662
Rep Power: 84
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   December 28, 2012, 17:39
Default
  #3
New Member
 
Join Date: Jun 2010
Posts: 21
Rep Power: 7
altano is on a distinguished road
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.
altano is offline   Reply With Quote

Old   December 31, 2012, 09:50
Default
  #4
New Member
 
Michal
Join Date: Sep 2012
Posts: 12
Rep Power: 4
Szczepan is on a distinguished road
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?


Last edited by Szczepan; December 31, 2012 at 10:12.
Szczepan is offline   Reply With Quote

Old   December 31, 2012, 10:46
Default
  #5
New Member
 
Join Date: Jun 2010
Posts: 21
Rep Power: 7
altano is on a distinguished road
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.
altano is offline   Reply With Quote

Old   January 12, 2013, 13:31
Default
  #6
New Member
 
Michal
Join Date: Sep 2012
Posts: 12
Rep Power: 4
Szczepan is on a distinguished road
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?

Last edited by Szczepan; January 12, 2013 at 13:46.
Szczepan is offline   Reply With Quote

Old   January 12, 2013, 14:55
Default
  #7
New Member
 
Join Date: Jun 2010
Posts: 21
Rep Power: 7
altano is on a distinguished road
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..
altano is offline   Reply With Quote

Old   January 19, 2013, 10:02
Default
  #8
New Member
 
Michal
Join Date: Sep 2012
Posts: 12
Rep Power: 4
Szczepan is on a distinguished road
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?
Szczepan is offline   Reply With Quote

Old   January 19, 2013, 10:27
Default
  #9
New Member
 
Join Date: Jun 2010
Posts: 21
Rep Power: 7
altano is on a distinguished road
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
altano is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Can CFX do CHT simulations with a solid domain rotating in a stationary fluid domain? acro CFX 8 July 8, 2013 08:11
How mesh a rotating domain? car_gon CFX 4 July 24, 2012 21:02
Is this correct? (Rotating domain) paulo CFX 10 June 17, 2010 13:19
rotating domain Jackie CFX 2 July 18, 2003 03:06
A rotating solid domain in CFX551? rotlin CFX 2 January 7, 2003 06:59


All times are GMT -4. The time now is 13:42.