CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Strange Velocity in impeller of MRFSimpleFOAM (http://www.cfd-online.com/Forums/openfoam-solving/58483-strange-velocity-impeller-mrfsimplefoam.html)

waynezw0618 April 10, 2008 03:44

Hi every one i am trying to
 
Hi every one
i am trying to simulate the centrifugal impeller with MRFSimpleFoam. after about 5000 steps there are strange velocity in only one passage,the velcity is much larger(above 1e +6 m/s).
here is the image of vector plot
http://www.cfd-online.com/OpenFOAM_D...ges/1/7277.jpg

waynezw0618 April 10, 2008 04:10

and here is the residual http
 
and here is the residual
http://www.cfd-online.com/OpenFOAM_D...ges/1/7280.jpg

dmoroian April 10, 2008 05:00

Take a look at k and epsilon r
 
Take a look at k and epsilon residuals and see which starts to diverge first (U, k or epsilon). Then decrease de order of discretization (take upwind for example) for that particular equation.
To be on the safe side use upwind for all of them.

Dragos

waynezw0618 April 10, 2008 05:56

Hi Dragos i will try it today
 
Hi Dragos
i will try it today
and here is the p k and epsilon
http://www.cfd-online.com/OpenFOAM_D...ges/1/7282.jpg

thanks
wayne

dmoroian April 10, 2008 06:04

Well Wayne, It seems that k a
 
Well Wayne,
It seems that k and epsilon are ok, you have to see which starts to diverge first: pressure equation or momentum?

Dragos

waynezw0618 April 10, 2008 06:40

Hi Dragos it looks like there
 
Hi Dragos
it looks like there are the same
http://www.cfd-online.com/OpenFOAM_D...ges/1/7284.jpg


and it quit similar to the iteration procedure in cfx(i will post later,for i am not working on that computer),but there is no such strange velocity.

thanks

wayne

dmoroian April 10, 2008 06:49

Hmm, to me it looks that press
 
Hmm, to me it looks that pressure starts to diverge first. So you can try to converge better the pressure equation.

waynezw0618 April 10, 2008 07:46

Hi Dragos how to? would you
 
Hi Dragos

how to? would you mind to tell me more ?

wayne

lillberg April 10, 2008 07:56

Hi Wayne, Is your outflow b
 
Hi Wayne,

Is your outflow boundary the one in the picture or does it only show a part of the whole model. If it is your outflow boundary, what boundary conditions have chosen for it?

Also, post an image of your mesh or the output from the checkMesh utility.

Regards

//Eric

dmoroian April 10, 2008 08:05

I use this seting for the pres
 
I use this seting for the pressure equation (fvSolution):
p PCG
{
<blockquote>preconditioner GAMG
{
<blockquote>tolerance 1e-6;
relTol 0.05;

smoother DICGaussSeidel;
nPreSweeps 0;
nPostSweeps 2;
nBottomSweeps 2;

cacheAgglomeration false;
nCellsInCoarsestLevel 10;
agglomerator faceAreaPair;
mergeLevels 1;
};

tolerance 1e-6;
relTol 0.05;
maxIter 100;</blockquote>
};
</blockquote>


waynezw0618 April 10, 2008 08:25

To Eric: i use the fixedValue
 
To Eric:
i use the fixedValue in p for my output condition. the calcualtion region is a impeller without the voulte,so you can see them on the first image!

Wayne

waynezw0618 April 10, 2008 08:27

To Dragos thanks! i will
 
To Dragos

thanks!

i will try!

Wayne

lillberg April 10, 2008 09:27

Wayne, Your outflow boundar
 
Wayne,

Your outflow boundary is way to close to the region where things happen to allow for fixed pressure BC. Use totalPressure BC instead together with appropriate BC's for U pressureInletOutletVelocity, k inletOutlet and epsilon inletOutlet.

Regards

/eric

waynezw0618 April 10, 2008 23:50

Hi: i try to run the case in
 
Hi:
i try to run the case in the parallel again without change anything in fvSolution.i still get a divergence. but the different is i donot get strange velocity like before,and the velocity is also looks quiet strange.it looks like that there is no velocity inlet just angular velocity everywhere including the velocity inlet.

here is the residual
http://www.cfd-online.com/OpenFOAM_D...ges/1/7302.jpg

waynezw0618 April 10, 2008 23:51

and is the velocity in 0.5 spa
 
and is the velocity in 0.5 spanwise
http://www.cfd-online.com/OpenFOAM_D...ges/1/7304.jpg

waynezw0618 April 10, 2008 23:53

and the velocity in 0.5spanwis
 
and the velocity in 0.5spanwise in CFX
http://www.cfd-online.com/OpenFOAM_D...ges/1/7306.jpg

lillberg April 11, 2008 02:45

Hi Wayne, Surely looks a bi
 
Hi Wayne,

Surely looks a bit strange! Could just be a fault in the setup!? What about your makeMesh config, are the faceZones set up properly in the parallel case?

I've run dozens of impellers like yours using the MRF and also comparing with sliding mesh simulations (in general < 5% difference in total flowrate) and also tabulated values (generally < 15% difference on coarse meshes).

Two things about your simulations tells me you'll end up in trouble sooner or later and therefor should be fixed. Firstly, change the location and/or type of your outflow BC. Secondly, if things don't work in serial runs don't bother doing them in parallel. If your case is too big use a coarser mesh to start with.

Also, try the pressure solver settings Dragos showed above. Additionally, run the case with upwind defferencing only for all variables and add "Interpolate(U) upwind phi;" to your interpolation settings in fvSchemes.

Good luck,

/Eric

waynezw0618 April 11, 2008 03:12

Hi Eric would you mind to se
 
Hi Eric
would you mind to send one of your setting(such as makemesh/fvSolution/fcScheme/MRFZones/dynamicMeshDict/Boudary/0 dictionary )or me ?

thanks!

wayne

lillberg April 11, 2008 03:41

Sure, Send your e-mail adr
 
Sure,

Send your e-mail adress to eric.lillberg@afconsult.com

/E

waynezw0618 April 11, 2008 04:01

Hi My email adress is wayne
 
Hi

My email adress is waynezw0618@163.com i have sent a email to you.if it was too large for you to send me.please send the setting files(such as makemesh/fvSolution/fcScheme/MRFZones/dynamicMeshDict/Boudary/0 dictionary or other)to me!

thanks!

wayne


All times are GMT -4. The time now is 06:28.