CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Main CFD Forum (http://www.cfd-online.com/Forums/main/)
-   -   About theory:how to get the pressure equation when solving u-p simultaneously? (http://www.cfd-online.com/Forums/main/99224-about-theory-how-get-pressure-equation-when-solving-u-p-simultaneously.html)

lzw2003 March 28, 2012 22:33

About theory:how to get the pressure equation when solving u-p simultaneously?
 
Hi,

Now i want to solve u,v,w,p simultaneously using coupled solver. But there is no equation for pressure. So i think the important is to get a pressure euqation.A method i know is to use mass conservation equation and equation of state to get a pressure equation.
I think this method is not suitable for my situation.

So,
Need the mass conservation equation special handle?Or
is there any other way to get the pressure equation ?

lzw2003 March 28, 2012 22:38

Or how to solve u,v,w,p simultaneously compared to segregated solver?

arjun March 29, 2012 06:14

I am afraid not many people can help you on it here.

Anyway to answer your question, there are two main class of treating this whole thing, but both of them will converge to similar approaches in the end.

First approach is not to construct pressure equation but rather create a saddle system.

| Au G | | u | = src_u
| D 0 | | p | = src_p

And solve this. Solving this could be done with the help of GMRES or BiCGStab. To run Kyrlov method you will need preconditioner and this preconditioner could be constructed in many ways.

Search for Preconditioner for saddle system or for Stokes problem.

Have a look at Ales Janka's work too. He has some ppts that Summarizes it very well.


Second approach is to create a velocity and pressure correction matrix based on finite volume approach. Here velocity correction could be written in terms of pressure correction gradients (SIMPLE Method). And this system will come out to be of form:


| Au G | | u' | = src_u
| D Ap | | p' | = src_p

Again you can apply same methods as above to solve this system or you could construct coupled AMG on it. Look at Ales Janka's work.


If you read this whole business in deep you will find that ultimately after some re-arragements you are solving the same thing in both approaches.

PS: If you are using AMG, traditional Gauss-Seidel does not work well as smoother. Braess Sarazin is good smoother but is costly. (Try it first because it is surefire method, if you get it working experiment with other things).


I hope this helps.

lzw2003 March 29, 2012 21:36

2 Attachment(s)
Hi, arjun:
thank you for this. I think i should study the first approach,maybe it will be helpful.

And i also want to know that is it identity when i transfer the mass conservation equation base on density (Eq.9.1)to that base on pressure(Eq. 2.13). Will the mass conserve if i used FVM to handle (2.13)?



http://www.cfd-online.com/Forums/att...1&d=1333071141
http://www.cfd-online.com/Forums/att...1&d=1333071118

lzw2003 March 29, 2012 22:57

Hi,arjun
Now I reading some papers, there is a method for coupled solver, using the Rhie-Chow interpolation
(momentum interpolation method, MIM),
proposed by Rhie-Chow
(Paper name: Numerical study of the turbulent flow past an airfloil with trailing edge separation) .
it is a method for coupled solver in co_located grid. I think this is suitable for me.
I dont know if you are familar in this field. But I want to know is there any other method for the coupled solver in co-located grid?

Thanks!

FMDenaro March 31, 2012 15:29

but is your goal to fulfill div V=0 ? Uzawa method was an old unsplit procedure...

arjun April 2, 2012 00:17

Quote:

Originally Posted by lzw2003 (Post 352241)
Hi, arjun:
thank you for this. I think i should study the first approach,maybe it will be helpful.

And i also want to know that is it identity when i transfer the mass conservation equation base on density (Eq.9.1)to that base on pressure(Eq. 2.13). Will the mass conserve if i used FVM to handle (2.13)?



http://www.cfd-online.com/Forums/att...1&d=1333071141
http://www.cfd-online.com/Forums/att...1&d=1333071118


I have not implemented coupled solver for compressible case so I can not say much. But my understanding is that density based solvers are already coupled in nature. (the way they are implemented).
And for pressure based coupled I am sure with using Rhie Chow momentum interpolation and other terms coupled solver could be created. (Fluent it seems has one). I have no time to dwell onto it so did not do it.


Quote:

Originally Posted by lzw2003 (Post 352245)
Hi,arjun
Now I reading some papers, there is a method for coupled solver, using the Rhie-Chow interpolation
(momentum interpolation method, MIM),
proposed by Rhie-Chow
(Paper name: Numerical study of the turbulent flow past an airfloil with trailing edge separation) .
it is a method for coupled solver in co_located grid. I think this is suitable for me.
I dont know if you are familar in this field. But I want to know is there any other method for the coupled solver in co-located grid?

Thanks!

I implemented coupled solver based on this approach and it is not difficult to do.

This is my break of time for implementing coupled version in iNavier.
3 days to create coupled multigrid for coupled system of equation.
1 day to convert segregated algorithm into coupled one.
2 hours to create 2 D version of coupled solver.

So my advise first concentrate of matrix solver for this system. Once you have it working things are very easy after that.


Edited to add: Look for work done by M. Darwish also on coupled solver. His papers give very good explanation on implementing it.

lzw2003 April 8, 2012 21:14

Yes, my goal is to fulfill the div V=0.

arjun April 8, 2012 22:13

Quote:

Originally Posted by lzw2003 (Post 353729)
Yes, my goal is to fulfill the div V=0.


All the methods are trying to do exactly this. Uzawa's method is slow and can not compete with AMG based methods.


All times are GMT -4. The time now is 12:05.