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

How to define cells which belongs to ratating patch in MRFSImpleFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 20, 2008, 03:05
Default Hi Bharat, On short change 8
  #21
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Hi Bharat,
On short change 8 with 1.
I think the error comes from the number of rotating reference frames that you specify: 8.
I suspect that your intention was to specify the number of rotating patches (I see that you have 8).

Dragos
dmoroian is offline   Reply With Quote

Old   May 20, 2008, 03:14
Default hi I tried by replacing 8 wi
  #22
New Member
 
bharat varshney
Join Date: Mar 2009
Location: iit-delhi, new delhi, india
Posts: 12
Rep Power: 8
bharat is on a distinguished road
hi
I tried by replacing 8 with 1, but still I am getting the same error
do I need to define all patches individually ?

Regards
bharat
bharat is offline   Reply With Quote

Old   May 20, 2008, 03:50
Default Could you send me your case? I
  #23
Senior Member
 
dmoroian's Avatar
 
Dragos
Join Date: Mar 2009
Posts: 647
Rep Power: 11
dmoroian is on a distinguished road
Could you send me your case? I'll try to have a look at it.

Dragos
dmoroian is offline   Reply With Quote

Old   May 20, 2008, 09:49
Default hi Finally, after lots of hi
  #24
New Member
 
bharat varshney
Join Date: Mar 2009
Location: iit-delhi, new delhi, india
Posts: 12
Rep Power: 8
bharat is on a distinguished road
hi
Finally, after lots of hit and trial I removed that error. It was just the problem of spacing in some brackets also the number is 1 not 8. Tomorrow, I will run the final simulation and will update you with the results. Hope I will not find any other hurdle ahead.

Thanx a lot Dragos and Jaswinder.

Below is the corrected MRFZone file:

1
(
VB
{
patches (BB INT-BO-SIDE-1 INT-BT-SIDE-1 PER-B-SIDE-1 PER-B-SIDE-2 SB-E SB-I VB-DEFAULT);
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] 19.625;
}
)


Regards
Bharat
bharat is offline   Reply With Quote

Old   October 6, 2008, 02:04
Default Hi People, I am struggling a
  #25
Member
 
Mahendra
Join Date: Mar 2009
Location: Pune, Maharashtra, India
Posts: 65
Rep Power: 8
mahendra is on a distinguished road
Hi People,
I am struggling a lot for the MRFSimpleFoam case. I completed the tutorial for the same, but my blower case is giving me some errors while creating the MRF zones. Below is the error....
Please let me know what can be done to fix the error.

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Reading mesh for time = 0
Create mesh

Reading cellSetDict

Backing up wall into wall_old
Set:wall Size:0 Action:new
Adding all cells of cellZone wall ...
--> FOAM Warning :
From function zoneToCell::combine(topoSet&, const bool)
in file sets/cellSources/zoneToCell/zoneToCell.C at line 75
Cannot find zone named wall
Valid zones are
0
(
)

Writing wall (size 0) to "constant/polyMesh/sets/wall"
mahendra is offline   Reply With Quote

Old   August 10, 2013, 14:03
Default
  #26
Member
 
reza1980's Avatar
 
reza
Join Date: Jan 2013
Location: Goteborg-Sweden
Posts: 79
Rep Power: 4
reza1980 is on a distinguished road
Hi ,
Would you please tell me this implemenation is needed as we use mergeMeshes.



Quote:
Originally Posted by jaswi View Post
Hi Bharat

Sorry for the delay. Below given is the description of makeMesh upto my understanding. it might have mistake and I hope forum experts will correct me if its wrong.

Provided you have the correct cellZone corresponding to your rotating domain, your makeMesh shall look like this:

(Note:replace mixerVessel2D with your case name everywhere.)
---------------------------------------------
cellSet .. mixerVessel2D
cp system/faceSetDict_rotorFaces system/faceSetDict
faceSet .. mixerVessel2D
cp system/faceSetDict_noBoundaryFaces system/faceSetDict
faceSet .. mixerVessel2D
setsToZones .. mixerVessel2D -noFlipMap

---------------
Now lets take a quick look what all these commands do. Its all very logical and easy....

1)cellSet .. mixerVessel2D

creates a cell set according to the definition given in the cellSetDict (this file lives in <case>/system). now the cellSetDict given for the mixerVessel2D has the following in it:

-----------------------------------
// Name of set to operate on
name rotor;

// One of clear/new/invert/add/delete|subset/list
action new;

// Actions to apply to cellSet. These are all the topoSetSource's ending
// in ..ToCell (see the meshTools library).

topoSetSources
(
// Cells in cell zone
zoneToCell
{
name rotor; // name of cellZone
}

);
-------------------------
It says that create a cellSet (action new called
rotor (name rotor from a topological source. The source can be set by calling topoSetSources(). The argument which is passed to the topoSetSources() is the cellZone called rotor (name rotor hence the code

zoneToCell
{
name rotor; // name of cellZone
}

At the successfull execution of this step one will get a cellSet called rotor in the directory /polyMesh/sets

2)faceSet .. mixerVessel2D

This creates a face set according to the definition given in the faceSetDict (this file lives in <case>/system). One can clearly observe the analogy with the cellSet command and cellSetDict.

Now the faceSet creation for the rotor is a two step process.

2.1) create a face set corresponding to the cellSet rotor (created in step 1). Thus the faceSetDict for this step should look like this:

+++++++++++++++++++++++++++++++++++++
// Name of set to operate on
name rotor;

// One of clear/new/invert/add/delete|subset/list
action new;

// Actions to apply to pointSet. These are all the topoSetSource's ending
// in ..ToFace (see the meshTools library).
topoSetSources
(
// Select based on cellSet
cellToFace
{
set rotor;
option all; // All faces of cells
}
);
++++++++++++++++++++++++++++++++++++++++++++++++++
One can see that its structure is similar to cellSetDict i.e. create a face set from a topological source which in this case is a cellSet named rotor. The "option all" implies that the created faceSet has all the faces of the cells in cellSet rotor

2.2) remove the faces corresponding to the boundary faces from the faceSet created in the step 2.1). and the faceSetDict for this step should look like this:
+++++++++++++++++
// Name of set to operate on
name rotor;

// One of clear/new/invert/add/delete|subset/list
action delete;

// Actions to apply to pointSet. These are all the topoSetSource's ending
// in ..ToFace (see the meshTools library).
topoSetSources
(
// Select boundary faces
boundaryToFace
{
}
);
++++++++++++++++++++++++
Now this faceSetDict says that delete the faces corresponding to the boundary, from the existing faceSet rotor and the topological source for this operation is the faceSet created in the previous step.

3)setsToZones .. mixerVessel2D -noFlipMap

the last command create the faceZone from the faceSet created in the step 2.2. what does the switch -noFlipMap does is not clear to me yet but no using it throws up error so use it.


Now if you still wonder what does this statement does :-) :
cp system/faceSetDict_noBoundaryFaces system/faceSetDict

then it should be clear by now.

I encourage you to try the easy step from the console. If at the end you still wonder whether you have the correct faceSet then you can use the following to visualize the set in paraFoam

foamToVTK root case -faceSet rotor

This will create a folder VTK and in there it saves your cellset rotor in VTK format which you can see with paraFOAM

I hope that you will now be able to execute the script and if required modify it to suit your needs.

Regards
Jaswi

P.S: For a detailed list of options for the topoSetSources() look in the sample cellSet, face set, pointSet dictionaries given in the

mesh/manipulation/cellSet
mesh/manipulation/faceSet
mesh/manipulation/poinTSet
reza1980 is offline   Reply With Quote

Old   August 18, 2013, 18:35
Default
  #27
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,178
Blog Entries: 34
Rep Power: 83
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Reza,

Quote:
Originally Posted by reza1980 View Post
Would you please tell me this implemenation is needed as we use mergeMeshes.
A bit more information here would help.

Best regards,
Bruno
wyldckat 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
MRFSimpleFoam command to run shyam OpenFOAM Running, Solving & CFD 2 February 5, 2009 06:38
MRFSimpleFoam xdanielx OpenFOAM Running, Solving & CFD 0 December 17, 2008 02:28
How to define a patch group number in pre-process? jacky CFX 4 December 19, 2002 05:31
How to define a patch group number in pre-process? jacky CFX 0 December 19, 2002 03:46
Define a zone to patch Maurizio Barbato FLUENT 1 October 13, 2000 00:10


All times are GMT -4. The time now is 00:29.