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

(Help!) Rotor Blade CFD

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 18, 2012, 02:00
Red face (Help!) Rotor Blade CFD
  #1
New Member
 
zhangjian
Join Date: Nov 2012
Posts: 17
Rep Power: 4
zjvskobe is on a distinguished road
I wrote a simple code to compute the rotor flowfield. I give the inlet B.C. a total pressure and a total temperature, the outlet BC a back pressure. But it does not converge. So i have several questions:
1、Is the boundary conditons ok? How to treat the reverse flow?
2、How to initialize before the calculation?
3、How about the numerical schemes? I use Roe flux average for space and LU-SGS for time.
zjvskobe is offline   Reply With Quote

Old   November 18, 2012, 05:42
Default
  #2
Member
 
vicarious's Avatar
 
Pedram Mojtabavi
Join Date: Apr 2011
Location: Iran
Posts: 66
Rep Power: 6
vicarious is on a distinguished road
Send a message via Yahoo to vicarious
Hi,
Are you simulating a whole cascade of rotor blades?
The boundary conditions are ok.
But how do you determine the back pressure?
Th whole flow is reversing at outlet or just some faces?
Inappropriate values for back pressure results in reversed flow.

For initializing the calculation use the Mach number. determine the inlet velocity and calculate the dynamic pressure and static pressure (Ps=P0-Pv). set the static pressure for an initial guess for the inlet boundary and use the outlet pressure for initializing the outlet boundary.
For better results you can also add Van-lees's Flux splitting scheme for flux vectors. To prevent the oscillatory behavior of the numerical results you can add the Van-Leer's limiter to the flux splitting algorithm.

Regards.
vicarious is offline   Reply With Quote

Old   November 20, 2012, 00:39
Default Is it axial/centrifugal turbomachinery rotor blade or helicopter rotor blade
  #3
Member
 
A. S.
Join Date: Apr 2009
Location: Raipur (INDIA)
Posts: 38
Rep Power: 8
apoorv is on a distinguished road
Hi

The problem you are attempting is turbomachinery or helicopter rotor. Also in case of turbomachinery is it a compressor rotor or turbine rotor

After that may be help you

Apoorv
apoorv is offline   Reply With Quote

Old   November 20, 2012, 04:39
Default
  #4
Member
 
Shenren Xu
Join Date: Jan 2011
Location: London, U.K.
Posts: 63
Rep Power: 6
Shenren_CN is on a distinguished road
Compressor or turbine , how does it make a difference in this case?
Quote:
Originally Posted by apoorv View Post
Hi

The problem you are attempting is turbomachinery or helicopter rotor. Also in case of turbomachinery is it a compressor rotor or turbine rotor

After that may be help you

Apoorv
Shenren_CN is offline   Reply With Quote

Old   November 20, 2012, 05:46
Default It makes difference in stablity
  #5
Member
 
A. S.
Join Date: Apr 2009
Location: Raipur (INDIA)
Posts: 38
Rep Power: 8
apoorv is on a distinguished road
Hi,

If compressor it will work against pressure, turbine it has favourable pressure gradient. My tactics to handle both of them is different.

Regards

Apurva
apoorv is offline   Reply With Quote

Old   November 21, 2012, 01:10
Default
  #6
New Member
 
zhangjian
Join Date: Nov 2012
Posts: 17
Rep Power: 4
zjvskobe is on a distinguished road
Thank u first! My case is very simple, it has only one blade. It is from the FLUENT tutorial "mixing plane" case. I cut the mesh by half, so I got its rotor mesh. I think the outlet is too close to the rotor, so the backflow occurs. I tried some methods from FLUENT to prevent the reverse flow, for example, make the backflow normal to the boundary and set the back pressure as the total pressure at the outlet. The solution is better, but not as well as the result from FLUENT. So are there some other tips?
zjvskobe is offline   Reply With Quote

Old   November 21, 2012, 01:12
Default
  #7
New Member
 
zhangjian
Join Date: Nov 2012
Posts: 17
Rep Power: 4
zjvskobe is on a distinguished road
I think it's a compressor rotor.

Quote:
Originally Posted by apoorv View Post
Hi

The problem you are attempting is turbomachinery or helicopter rotor. Also in case of turbomachinery is it a compressor rotor or turbine rotor

After that may be help you

Apoorv
zjvskobe is offline   Reply With Quote

Old   November 21, 2012, 01:52
Default
  #8
Member
 
A. S.
Join Date: Apr 2009
Location: Raipur (INDIA)
Posts: 38
Rep Power: 8
apoorv is on a distinguished road
Hi

Have domain down stream the rotor atleast 50% of chord in case of isolated rotor.

In case of compressor rotor, I will prefer to ramp up the back-pressure from a reasonable low value to target value (final pressure) in 200-300 iteration for stability. Also don't start with zero initial velocity. You can give velocity in axial flow direction say 100 m/s and start.

Hope this is helpful.

Apoorv
apoorv is offline   Reply With Quote

Old   November 21, 2012, 02:04
Default
  #9
Member
 
vicarious's Avatar
 
Pedram Mojtabavi
Join Date: Apr 2011
Location: Iran
Posts: 66
Rep Power: 6
vicarious is on a distinguished road
Send a message via Yahoo to vicarious
Quote:
Originally Posted by zjvskobe View Post
Thank u first! My case is very simple, it has only one blade. It is from the FLUENT tutorial "mixing plane" case. I cut the mesh by half, so I got its rotor mesh. I think the outlet is too close to the rotor, so the backflow occurs. I tried some methods from FLUENT to prevent the reverse flow, for example, make the backflow normal to the boundary and set the back pressure as the total pressure at the outlet. The solution is better, but not as well as the result from FLUENT. So are there some other tips?
So you are simulating a cascade consisting of one rotor blade in wind tunnel? Since the mixing plane approach is a steady procedure, you may need to run an unsteady simulation for just one blade because there may be high fluctuations or large separations. The mesh, as you mentioned, has to get extended up far enough from upstream and downstream the blade (almost 2 or 3 times of the chord). If the flow is turbulent, the same standard k-epsilon is OK for the problem. You may also need to relax the momentum and turbulence quantities as well (for a personal code "limiters" is necessary for preventing the oscillation of the numerical results).
vicarious is offline   Reply With Quote

Old   November 22, 2012, 07:36
Default
  #10
New Member
 
zhangjian
Join Date: Nov 2012
Posts: 17
Rep Power: 4
zjvskobe is on a distinguished road
Thanks a lot! That's helpful. The distance is just 50% or less of the chord, so that's the problem. But i'm wandering how commercial softwares deal with the backflow. For example, the fluent user's guide just tell us how to set the condition, but didn't tells us their implementation details.....
Quote:
Originally Posted by apoorv View Post
Hi

Have domain down stream the rotor atleast 50% of chord in case of isolated rotor.

In case of compressor rotor, I will prefer to ramp up the back-pressure from a reasonable low value to target value (final pressure) in 200-300 iteration for stability. Also don't start with zero initial velocity. You can give velocity in axial flow direction say 100 m/s and start.

Hope this is helpful.

Apoorv
zjvskobe is offline   Reply With Quote

Old   November 22, 2012, 07:57
Default
  #11
New Member
 
zhangjian
Join Date: Nov 2012
Posts: 17
Rep Power: 4
zjvskobe is on a distinguished road
Yes, you are right! And my final goal is to simulate multistage compressor. But now the work just begin. I'am not quite familiar with it. So I want to start with a simple rotor. I read some paper, some use absolute variables in the govering equation relative system for convenience(e.g the message change between rotor and stator is easy). But the Inviscid flux term is different(add some terms), and the source term is no longer zero. Questions come, I don't know how to Implement the Space discretization. Because the Roe average matrix is different now, or for Van Leer spiliting the eigenvalues are changed?. And what about the turbulence model in the rotational system? Due to these problems, my code may have some mistakes......
Quote:
Originally Posted by vicarious View Post
So you are simulating a cascade consisting of one rotor blade in wind tunnel? Since the mixing plane approach is a steady procedure, you may need to run an unsteady simulation for just one blade because there may be high fluctuations or large separations. The mesh, as you mentioned, has to get extended up far enough from upstream and downstream the blade (almost 2 or 3 times of the chord). If the flow is turbulent, the same standard k-epsilon is OK for the problem. You may also need to relax the momentum and turbulence quantities as well (for a personal code "limiters" is necessary for preventing the oscillation of the numerical results).
zjvskobe is offline   Reply With Quote

Old   November 22, 2012, 08:55
Default
  #12
Member
 
vicarious's Avatar
 
Pedram Mojtabavi
Join Date: Apr 2011
Location: Iran
Posts: 66
Rep Power: 6
vicarious is on a distinguished road
Send a message via Yahoo to vicarious
The idea of Roe consist of determining the solution by solving a modified equation, where the flux vector E is quasilinearized by introducing a matrix A and adopting :
E=AQ
where Q is the unkown vector. the description of governing equation is though and I do not recall them very well, but I can suggest you to look at "computational fluid dynamics for engineers" by "Hoffman". you can find the method conditions and the matrix form of Van-Leer's flux splitting vectors for two dimensional studies.
You can also consider the Baldwin-Lomax turbulent model. Since the flow in through a turbine or compressor is very complex, the calculation of shear layer thickness in a CFD code is difficult. Hence, using the BL model is more easier since it is a zero-equation model. Further explanation about this model could be found at this article:

Granville,P. S., "Baldwin-Lomax factors for turbulent boundary layers in pressure gradients", AIAA Journal.
http://www.cfd-online.com/Wiki/Baldwin-Lomax_model
vicarious is offline   Reply With Quote

Old   November 22, 2012, 10:18
Default
  #13
New Member
 
zhangjian
Join Date: Nov 2012
Posts: 17
Rep Power: 4
zjvskobe is on a distinguished road
Thanks a lot!!!

Quote:
Originally Posted by vicarious View Post
The idea of Roe consist of determining the solution by solving a modified equation, where the flux vector E is quasilinearized by introducing a matrix A and adopting :
E=AQ
where Q is the unkown vector. the description of governing equation is though and I do not recall them very well, but I can suggest you to look at "computational fluid dynamics for engineers" by "Hoffman". you can find the method conditions and the matrix form of Van-Leer's flux splitting vectors for two dimensional studies.
You can also consider the Baldwin-Lomax turbulent model. Since the flow in through a turbine or compressor is very complex, the calculation of shear layer thickness in a CFD code is difficult. Hence, using the BL model is more easier since it is a zero-equation model. Further explanation about this model could be found at this article:

Granville,P. S., "Baldwin-Lomax factors for turbulent boundary layers in pressure gradients", AIAA Journal.
http://www.cfd-online.com/Wiki/Baldwin-Lomax_model
zjvskobe 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
STAR-Works : Mainstream CAD with CFD CD adapco Group Marketing CD-adapco 0 February 13, 2002 13:23
Where do we go from here? CFD in 2001 John C. Chien Main CFD Forum 36 January 24, 2001 22:10
ASME CFD Symposium, Atlanta, July 2001 Chris R. Kleijn Main CFD Forum 0 August 21, 2000 04:49
Since Last June John C. Chien Main CFD Forum 3 July 12, 1999 09:38
Which is better to develop in-house CFD code or to buy a available CFD package. Tareq Al-shaalan Main CFD Forum 10 June 12, 1999 23:27


All times are GMT -4. The time now is 03:23.