CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Strange Velocity in impeller of MRFSimpleFOAM

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 10, 2008, 02:44
Default Hi every one i am trying to
  #1
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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

waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 03:10
Default and here is the residual http
  #2
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
and here is the residual

waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 04:00
Default Take a look at k and epsilon r
  #3
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
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
dmoroian is offline   Reply With Quote

Old   April 10, 2008, 04:56
Default Hi Dragos i will try it today
  #4
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi Dragos
i will try it today
and here is the p k and epsilon


thanks
wayne
waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 05:04
Default Well Wayne, It seems that k a
  #5
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Well Wayne,
It seems that k and epsilon are ok, you have to see which starts to diverge first: pressure equation or momentum?

Dragos
dmoroian is offline   Reply With Quote

Old   April 10, 2008, 05:40
Default Hi Dragos it looks like there
  #6
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi Dragos
it looks like there are the same



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
waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 05:49
Default Hmm, to me it looks that press
  #7
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Hmm, to me it looks that pressure starts to diverge first. So you can try to converge better the pressure equation.
dmoroian is offline   Reply With Quote

Old   April 10, 2008, 06:46
Default Hi Dragos how to? would you
  #8
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi Dragos

how to? would you mind to tell me more ?

wayne
waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 06:56
Default Hi Wayne, Is your outflow b
  #9
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
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
lillberg is offline   Reply With Quote

Old   April 10, 2008, 07:05
Default I use this seting for the pres
  #10
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
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>

dmoroian is offline   Reply With Quote

Old   April 10, 2008, 07:25
Default To Eric: i use the fixedValue
  #11
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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 is offline   Reply With Quote

Old   April 10, 2008, 07:27
Default To Dragos thanks! i will
  #12
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
To Dragos

thanks!

i will try!

Wayne
waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 08:27
Default Wayne, Your outflow boundar
  #13
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
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
lillberg is offline   Reply With Quote

Old   April 10, 2008, 22:50
Default Hi: i try to run the case in
  #14
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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

waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 22:51
Default and is the velocity in 0.5 spa
  #15
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
and is the velocity in 0.5 spanwise

waynezw0618 is offline   Reply With Quote

Old   April 10, 2008, 22:53
Default and the velocity in 0.5spanwis
  #16
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
and the velocity in 0.5spanwise in CFX

waynezw0618 is offline   Reply With Quote

Old   April 11, 2008, 01:45
Default Hi Wayne, Surely looks a bi
  #17
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
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
lillberg is offline   Reply With Quote

Old   April 11, 2008, 02:12
Default Hi Eric would you mind to se
  #18
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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
waynezw0618 is offline   Reply With Quote

Old   April 11, 2008, 02:41
Default Sure, Send your e-mail adr
  #19
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Sure,

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

/E
lillberg is offline   Reply With Quote

Old   April 11, 2008, 03:01
Default Hi My email adress is wayne
  #20
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 9
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
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
waynezw0618 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
Equations in the MRFsimpleFOAM waynezw0618 OpenFOAM Running, Solving & CFD 5 May 7, 2015 04:43
Convergence with MRFSimpleFoam grugg OpenFOAM Running, Solving & CFD 7 March 28, 2014 05:56
MRFSimpleFoam xdanielx OpenFOAM Running, Solving & CFD 0 December 17, 2008 02:28
Strange Velocity JoeSa CFX 1 September 28, 2006 09:13
Strange oscillating velocity zonexo Main CFD Forum 2 April 6, 2006 11:38


All times are GMT -4. The time now is 13:54.