CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   Main CFD Forum (https://www.cfd-online.com/Forums/main/)

 zjvskobe November 18, 2012 02:00

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.

 vicarious November 18, 2012 05:42

Hi,
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.

 apoorv November 20, 2012 00:39

Hi

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

Apoorv

 Shenren_CN November 20, 2012 04:39

Compressor or turbine , how does it make a difference in this case?
Quote:
 Originally Posted by apoorv (Post 393104) 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 November 20, 2012 05:46

It makes difference in stablity

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

 zjvskobe November 21, 2012 01:10

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 November 21, 2012 01:12

I think it's a compressor rotor.

Quote:
 Originally Posted by apoorv (Post 393104) 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 November 21, 2012 01:52

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.

Apoorv

 vicarious November 21, 2012 02:04

Quote:
 Originally Posted by zjvskobe (Post 393327) 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).

 zjvskobe November 22, 2012 07:36

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 (Post 393331) 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 November 22, 2012 07:57

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 (Post 393333) 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 November 22, 2012 08:55

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 November 22, 2012 10:18

Thanks a lot!!!:):)

Quote:
 Originally Posted by vicarious (Post 393644) 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

 All times are GMT -4. The time now is 16:31.