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

Fan @ low flow rates (10m^3/hr) -> Entire upstream domain starts rotating

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

Like Tree1Likes
  • 1 Post By Wolfram

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 29, 2019, 04:50
Default Fan @ low flow rates (10m^3/hr) -> Entire upstream domain starts rotating
  #1
New Member
 
Wolfram Schneider
Join Date: Jan 2018
Location: Germany
Posts: 20
Rep Power: 4
Wolfram is on a distinguished road
Dear all,

I am facing a physical not valid flow pattern - i think. When simulating a fan with really low flow rates (10m^3/hr), the entire upstream inlet domain in front of the impeller starts rotating. The flow enters inlet straight (in dependeny of the inlet BC) and the more iterations, the stronger the swirl becomes upstream. So it has to be induced by the impeller.
In front of the impeller you can find a small grid. The simulation is running with k-epsilon, frozen rotor and the following BC:
https://www.bilder-upload.eu/bild-2d...51403.jpg.html

Here you can see the swirling inlet:
https://www.bilder-upload.eu/bild-e0...51444.jpg.html

Switching to first order in advection scheme reduced the swirl remarkable, but is still persistent.

Due to the swirl directly in front of the impeller, the head is much to low in comparison to the performance curve. High volume flow rates show a good match regarding head with performance where the pre swirl does not occur.

I made an attempt with a porous media as inlet domain. To prevent any swirl, i set the permeability close to zero for theta direction. Surprisingly the head hits the performance curve really close for the entire operation range. But for sure i cannot rate other inlet geometries with this porous media. Here you can see the reduced swirl:
https://www.bilder-upload.eu/bild-72...53980.jpg.html


--> So is this pre-swirl for low volume flow rates a numerical phenomenon?


Kind regards

Wolfram
Ahmed Fakhrey likes this.
Wolfram is offline   Reply With Quote

Old   January 29, 2019, 15:27
Default
  #2
Senior Member
 
Join Date: Jun 2009
Posts: 1,270
Rep Power: 24
Opaque will become famous soon enough
Questions for thought:

1 - Are you using the Alternate Rotation Model? Otherwise, there will be numerical errors for axial flows in the stationary frame.

2 - Have you evaluated alternatives model to the Frozen Rotor approximation? Recall this is a major approximation.

3 - Using Upwind to obtain better results is a sign that something is wrong elsewhere. Upwind should only be used to obtain converged solutions to start cases which more accurate schemes when those cases do not converge from poor initial guesses. I will not trust an Upwind converged solution where there are velocity gradients.

4 - Have you contacted ANSYS CFX turbomachinery specialists for assistance?
Opaque is offline   Reply With Quote

Old   January 29, 2019, 19:43
Default
  #3
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,192
Rep Power: 18
Gert-Jan is on a distinguished road
- I would have made my inlet geometry significant larger.
- I think this can happen in real life, depending how the inlet close to the fan looks like. You mention a kind of grid. Can you show the exact geometry?
- is this the same geometry that was used in the test by the fan supplier? Or did he use an anti-rotation device?
Gert-Jan is offline   Reply With Quote

Old   January 30, 2019, 05:58
Default
  #4
New Member
 
Wolfram Schneider
Join Date: Jan 2018
Location: Germany
Posts: 20
Rep Power: 4
Wolfram is on a distinguished road
Quote:
Originally Posted by Opaque View Post
Questions for thought:

1 - Are you using the Alternate Rotation Model? Otherwise, there will be numerical errors for axial flows in the stationary frame.

2 - Have you evaluated alternatives model to the Frozen Rotor approximation? Recall this is a major approximation.

3 - Using Upwind to obtain better results is a sign that something is wrong elsewhere. Upwind should only be used to obtain converged solutions to start cases which more accurate schemes when those cases do not converge from poor initial guesses. I will not trust an Upwind converged solution where there are velocity gradients.

4 - Have you contacted ANSYS CFX turbomachinery specialists for assistance?
1 - Alternate rotation model is applied

2 - Tried Mixing Stage as well, without huge change. The fan consists of one blade row (impeller only). The upstream grid is nearly axially symmetrical.

3 - Using upwind was just an attempt. In Autodesk CFD there is an option called "adv5_no_dtime_flag" for the advection scheme and the issue of rotating inlet was solved.

4 - I have not contacted the turbomachinery specialists for assistance. Is there a special site for this? I have found the general contact regarding their products and so on
Wolfram is offline   Reply With Quote

Old   January 30, 2019, 06:10
Default
  #5
New Member
 
Wolfram Schneider
Join Date: Jan 2018
Location: Germany
Posts: 20
Rep Power: 4
Wolfram is on a distinguished road
Quote:
Originally Posted by Gert-Jan View Post
- I would have made my inlet geometry significant larger.
- I think this can happen in real life, depending how the inlet close to the fan looks like. You mention a kind of grid. Can you show the exact geometry?
- is this the same geometry that was used in the test by the fan supplier? Or did he use an anti-rotation device?

I have enlarged the inlet geometry and designed it is a cube. The swirl within the huge inlet decreased and is negligible. But the swirl in the duct upstream the impeller has not changed.

The grid consists of simple struts reaching from one side to the other as you can see in the picture posted above: https://www.bilder-upload.eu/bild-2d...51403.jpg.html
The main purpose of the grid is to shelter the user to stick finger inside the fan.

The simulated geometry and the geometry tested in our test bench is equal.
Wolfram is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
transient simulation of a rotating rectangle icesniffer CFX 1 August 8, 2009 08:25
How to model flow of centrifugal fan? Peter Main CFD Forum 0 April 2, 2008 07:07
Multicomponent fluid Andrea CFX 2 October 11, 2004 06:12
flow simulation across a small fan jane luo Main CFD Forum 15 April 12, 2004 18:49
axial flow in counter rotating ducted fan Vishu FLUENT 4 January 13, 2004 18:52


All times are GMT -4. The time now is 13:59.