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

MRFZonesC questions what is the mesh_V and why only Coriolis force no centrifugal force

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 7, 2008, 03:27
Default Hi i am sorry for the last i
  #41
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi
i am sorry for the last image is vector of U on shroud wall,which is also the rotating zone like hub,and you can the angular velocity clearly here,and the same as HUB.
does that mean i have imposed the angular velocity to the boundary in a right way?

wayne
waynezw0618 is offline   Reply With Quote

Old   April 7, 2008, 03:54
Default Hi Wayne, Maybe I did not und
  #42
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12
dmoroian is on a distinguished road
Hi Wayne,
Maybe I did not understand the MRFSimpleFoam solver very well, but I think you should set up the case in a different way.
First of all, in MRFZones I think you should specify the rotating zones not surfaces. In other words, IMPELLER should be the name of the zone containing all the cells that are in the rotating domain.
Second, in the patches dictionary you can put all the rotating boundaries (blades, hub, ...).
And that's it.

For instance, this is how I would setup an MRFZones file:

1
(
<blockquote>rotating
{
<blockquote>patches (rotor hub);
origin origin [0 1 0 0 0 0 0] (0 0 0);
axis axis [0 0 0 0 0 0 0] (0 0 -1);
omega omega [0 0 -1 0 0 0 0] 10.472;
}</blockquote>
)</blockquote>
I have considered a zone called rotating and two boundaries rotor and hub.

Dragos
dmoroian is offline   Reply With Quote

Old   April 7, 2008, 04:26
Default Hi so according to you,i s
  #43
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi
so according to you,i should delete boundary by a faceSet? and make the boundary by defining them in patch dictionary MRFZones?
wayne
waynezw0618 is offline   Reply With Quote

Old   April 7, 2008, 04:52
Default i have just try your way ,and
  #44
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
i have just try your way ,and both yours and mine are face the problem. there is a error in the first step

--> FOAM FATAL ERROR : fixedValue is the wrong k patchField type for wall-functions on patch INLET
should be zeroGradient
wayne
waynezw0618 is offline   Reply With Quote

Old   April 7, 2008, 05:06
Default and if i change the k and epsi
  #45
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
and if i change the k and epsilon patchField to the zeroGradient, the calculation will divgence after about 200 steps. when i check the flow inside, there is some strange velocity:


can you help me ?
waynezw0618 is offline   Reply With Quote

Old   April 7, 2008, 06:04
Default It is normal to set zeroGradie
  #46
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12
dmoroian is on a distinguished road
It is normal to set zeroGradient for k and epsilon at walls, since you are using standard k-epsilon turbulence modeling. Divergent solution means that you should start from a better initial solution. Start with potentialFoam. Then continue with simpleFoam, and then with MRFSimpleFoam but with very low angular velocity. After you have a solution, you can further increase the angular velocity until the value that you are looking for.

Dragos
dmoroian is offline   Reply With Quote

Old   April 7, 2008, 09:19
Default hi i will try.thanks! wo
  #47
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
hi

i will try.thanks!
would you mind to tell me more about the faceSet, i can not understand the both two faceSet in "mix2D".
for the last one i guess i will delete the boundary for the boundary will be patched,and the boundary condition is modified by the memberfuntion in the MRFZone.C.
what about the first one?why to creat all faces on the cellSet? and what is the "face",i have trid in my case that,if i creat faceZone with the set by "option all" , i will get n1 faces,if i creat facezone bying add whole surfaces of the Set.i will get n2 faces.and
n1>>n2.so what are the faces creat with the set by "option all"?why creat them?
waynezw0618 is offline   Reply With Quote

Old   April 8, 2008, 02:25
Default Hi Dragos: can you help me?
  #48
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi Dragos:
can you help me?
waynezw0618 is offline   Reply With Quote

Old   April 8, 2008, 02:52
Default Very interesting questions, an
  #49
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 648
Rep Power: 12
dmoroian is on a distinguished road
Very interesting questions, and I have to say 'I don't know the complete answers'. I checked what the makeMesh script does and here is what I understood:
  1. m4 <constant/polymesh/blockmeshdict.m4> constant/polyMesh/blockMeshDict - generate a blockMeshDict
  2. blockMesh .. mixerVessel2D - generate the mesh containing one zone of cells called 'rotor' (it seems there is a need for both cellZones and faceZones, so the face zone has to be generated too)
  3. cellSet .. mixerVessel2D - convert the zone 'rotor' to a set of cells
  4. cp system/faceSetDict_rotorFaces system/faceSetDict; faceSet .. mixerVessel2D - convert all the faces of the cells in the cell set into a set of faces
  5. cp system/faceSetDict_noBoundaryFaces system/faceSetDict; faceSet .. mixerVessel2D - remove all the boundary faces from the previous generated set of faces (why???)
  6. setsToZones .. mixerVessel2D -noFlipMap - convert the last generated set of faces into a face zone called 'rotor'

That's it! I hope somebody with a more in depth view will explain more.

I hope this is helpful,
Dragos
dmoroian is offline   Reply With Quote

Old   April 8, 2008, 04:23
Default Hi Dragos for 4,i think it
  #50
Senior Member
 
wayne.zhang
Join Date: Mar 2009
Location: Shanghai, Shanghai, P.R.China
Posts: 307
Rep Power: 10
waynezw0618 is on a distinguished road
Send a message via MSN to waynezw0618 Send a message via Skype™ to waynezw0618
Hi Dragos

for 4,i think it creat all faces of cells,here,faces including internal faces and boundary faces which is n1as i metioned last time.and the boundary faces is n2. so n1 >>n2.
and in the MRFZone.C there is boundary correction funtion.so if not 5 ,the solve will calculate it as internalface.
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
Centrifugal force/ Rotating Wall david FLUENT 4 January 2, 2014 07:30
centrifugal force sue FLUENT 0 November 25, 2008 04:01
cyclone separator- centrifugal force kumar FLUENT 2 May 29, 2008 03:33
Cyclone separator-centrifugal force aPpA FLUENT 0 July 6, 2005 14:22
Coriolis force Saturn FLUENT 5 September 30, 2004 15:56


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