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

 waynezw0618 April 10, 2008 02:44

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 03:10

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 04:00

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 04:56

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 05:04

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 05:40

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 05:49

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 06:46

Hi Dragos how to? would you

Hi Dragos

how to? would you mind to tell me more ?

wayne

 lillberg April 10, 2008 06:56

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 07:05

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 07:25

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 07:27

To Dragos thanks! i will

To Dragos

thanks!

i will try!

Wayne

 lillberg April 10, 2008 08:27

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 22:50

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 22:51

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 22:53

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 01:45

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 02:12

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 02:41

Sure,

/E

 waynezw0618 April 11, 2008 03:01

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 10:09.