
[Sponsors] 
Strange Velocity in impeller of MRFSimpleFOAM 

LinkBack  Thread Tools  Search this Thread  Display Modes 
April 10, 2008, 02:44 
Hi every one
i am trying to

#1 
Senior Member

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 

April 10, 2008, 03:10 
and here is the residual
http

#2 
Senior Member

and here is the residual


April 10, 2008, 04:00 
Take a look at k and epsilon r

#3 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 
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 

April 10, 2008, 04:56 
Hi Dragos
i will try it today

#4 
Senior Member

Hi Dragos
i will try it today and here is the p k and epsilon thanks wayne 

April 10, 2008, 05:04 
Well Wayne,
It seems that k a

#5 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 
Well Wayne,
It seems that k and epsilon are ok, you have to see which starts to diverge first: pressure equation or momentum? Dragos 

April 10, 2008, 05:40 
Hi Dragos
it looks like there

#6 
Senior Member

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 

April 10, 2008, 05:49 
Hmm, to me it looks that press

#7 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 
Hmm, to me it looks that pressure starts to diverge first. So you can try to converge better the pressure equation.


April 10, 2008, 06:46 
Hi Dragos
how to? would you

#8 
Senior Member

Hi Dragos
how to? would you mind to tell me more ? wayne 

April 10, 2008, 06:56 
Hi Wayne,
Is your outflow b

#9 
Member

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 

April 10, 2008, 07:05 
I use this seting for the pres

#10 
Senior Member
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 20 
I use this seting for the pressure equation (fvSolution):
p PCG}; tolerance 1e6; relTol 0.05; maxIter 100;</blockquote> }; </blockquote> 

April 10, 2008, 07:25 
To Eric:
i use the fixedValue

#11 
Senior Member

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 

April 10, 2008, 07:27 
To Dragos
thanks!
i will

#12 
Senior Member

To Dragos
thanks! i will try! Wayne 

April 10, 2008, 08:27 
Wayne,
Your outflow boundar

#13 
Member

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 

April 10, 2008, 22:50 
Hi:
i try to run the case in

#14 
Senior Member

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 

April 10, 2008, 22:51 
and is the velocity in 0.5 spa

#15 
Senior Member

and is the velocity in 0.5 spanwise


April 10, 2008, 22:53 
and the velocity in 0.5spanwis

#16 
Senior Member

and the velocity in 0.5spanwise in CFX


April 11, 2008, 01:45 
Hi Wayne,
Surely looks a bi

#17 
Member

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 

April 11, 2008, 02:12 
Hi Eric
would you mind to se

#18 
Senior Member

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 

April 11, 2008, 02:41 
Sure,
Send your email adr

#19 
Member


April 11, 2008, 03:01 
Hi
My email adress is wayne

#20 
Senior Member

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 

Thread Tools  Search this Thread 
Display Modes  


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 04:56 
MRFSimpleFoam  xdanielx  OpenFOAM Running, Solving & CFD  0  December 17, 2008 01:28 
Strange Velocity  JoeSa  CFX  1  September 28, 2006 09:13 
Strange oscillating velocity  zonexo  Main CFD Forum  2  April 6, 2006 11:38 