[plmauk]

Hi,
cellSets and faceSets are a community of cells or faces. These supply certain geometrical (but not only)conditions, for example a box or a surfase inside the mesh.
You need sets, to create face- or cellZones (even MRFzone "rotor" from MRFsimpleFoam tutorial). The zones were created using setToZone-utility.

[plmauk]

by the way, important is, that the names of the zones in faceZones-list and in MRFzones-dictionary are the same. You shouldn't repeat the name of boundary "rotor", you can call they "stator", "John" or "Diana" - what ever you want...

[waynezw0618]

Hi
thanks! but what is the "rotor" in facesetdict and cellsetdict?there are two "rotor" in both of the two file?could you tell me more?

[plmauk]

Hi,
I tell you much more about this case and its zones on monday, when I'll be on my workplace - I don't have any linux-PC at the moment.
OK?

[waynezw0618]

thanksa lot�

[plmauk]

Hi,
As promised, I tell you about Mixer2D case.
In the constant-dictionary is a "file MRF-zones". It should declare, which part of the mesh will rotate. The name of the MRF-zone is "rotor", so we need to create a cellZone, that consists of the cells, that will rotate. To create this cellZone, we need first create cellSet.

In the mixer Vessel2D-dictionary is an Utility named makeMesh. Open it and look carefully at all the steps, that were done:

1-2 blockMesh .. mixerVessel2D - mesh is generated.
3. cellSet .. mixerVessel2D - sellSet is created using sellSet-dictionary.
Now we have cells, that should rotate, but the cellSet contains also faces, wich belong to bondary. These have to be deleted.
4-5 cp system/faceSetDict_rotorFaces system/faceSetDict faceSet .. mixerVessel2D - faceSet of boundary-faces is created using faceSetDict_rotorFaces.
6-7 cp system/faceSetDict_noBoundaryFaces system/faceSetDict faceSet .. mixerVessel2D
- boundary-Faces were deleted using faceSetDict_noBoundaryFaces.
8.setsToZones .. mixerVessel2D -noFlipMap - the cellZone is created. The name of the Zone should be the same, that the name of MRFZone.
That's the end.
Now, you can start first the makeMesh-utility and then run your MRF-case.

[waynezw0618]

Hi
Q1: in 3 to 8 ,your aim is to creat a "Zone" for "MRFZones",which should rotate.So is

that mean if the whole zone of the mesh is rotating,there is no need to delete these

faces,the only thing is to make the name of zone in the file MRFZone the same as in the

cellZone file? take impeller of pump for example, the boundary of hub and shroud is also

rotating,so do i still need to do the step 3 to 8 to remove the hub and shroud or not?(i

guess there is no need to delete the boundary for they do have rotating speed, or just

deleting the none rotating boundary)

Q2:you say the cellSets contains faces,i don`t understand the faces mean,are they

surface of zone makeup of lots of cell or the faces of a cell? so if it is surface of the

zone,after deleting the boundary .the remainder are cells of rotating zone and interface

between rotor and stator,is that right?

Q3:when we do cellSet and faceSet there is two "rotor", one in cellZones("A"),the

other in boundary("B"),when we do cellSet there is the 3rd--in "set"("C"). so i

guess in the cellSetDict:

// Name of set to operate on
name rotor; ® this one is "C",which will be created after cellSet

// 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 ®this one is "A" ,which is the

utility cellSet will convert from cellZone to cellset
}

);

And in thefaceSetDict_rotor:
// Name of set to operate on
name rotor; ®this one is "C",which has been created before


// 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; ®what is the rotor refer to?"B"? the boundary one?
option all; // All faces of cells
}
);

[waynezw0618]

by the way
Q4: according to Q2,if we delete the boundary from cellSet ,how can i add the angular velocity to the boundary (i.e. blade,rotor,hub and shroud)
Q5: in the dynamicMeshDict
mixerFvMeshCoeffs
{
coordinateSystem
{
type cylindrical;
origin (0 0 0);
axis (0 0 1);
direction (1 0 0); what is this direction
}

rpm 10; what is this angular speed?

slider
{
inside insideSlider;
outside outsideSlider;
}
}

wayne

thanks!

[plmauk]

Only cells belonging to MRF-Zone should rotate. And you specify this zone when you create cellSet and then cellZone from this cellSet.
By the way, did you run makeMesh utility befor you run the case?
You are desperate to do that, on the other way the solver can't find MRF-Zones.

[waynezw0618]

i can run that case ,but i want to do my case-- a centrifugal pump impeller,so could you please give me help about the question above?

[plmauk]

yuo don't need the dynamicMeshDict, and you can delete it. You don't solve any moving meshes using MRFSimpleFoam. The required dictionary is the MRFZonesDictionary.

[plmauk]

After you succesfully converted the mesh using fluent3DMeshToFoam, you need first need specify a part of the mesh, that should rotate. This happens with help of a sellSetDict. this one is not the same dictionary, that is located at the system directory. You have to create it youself. For example, as a rotating box. Possible sellSetDict. were:


name Mixer;

action new;

topoSetSources
(
boxToCell
{
box (-25 -7.5 -35) (25 7.5 35);
}
);

this one is from my own case.
After you made the cellSet, you have to create a cellZone from this cellSet:

setsToZones root case -cellSet nameOfcellSet -no flipmap.

When it'done, you can delete this cellsetDict. or replace it with this one:

// Name of set to operate on
name rotor; ® this one is "C",which will be created after cellSet

// 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 ®this one is "A" ,which is the

utility cellSet will convert from cellZone to cellset
}

You need also the faceZone, that represent the surface area of your impeller (or even of the part of the mesh, that should rotate). The faceZone for it is for Example:

arguments "/home/cfduser/kesselMRF";

name mixer;//name of the zone

action new;

topoSetSources
(
patchToFace
{
name Ruehrer;//name of boundary
}

);

Now you have to build once again a zone - not a cellZone, but a faceZone. And once again using setsToZones-command.

Now you can add two faseSetDict. from MixerVessel2D case into your system-directory. Be carefull, look after names in each Dict.
Then you should edit the makeMesh utility. Steps, that you don't need are beeng deleted.
I hope, my advices help.

[waynezw0618]

Hi
thanks lot! i have got lot from you,but still questions!
Q1:do i still need to add the two faseSetDict from MixerVessel2D case into my system-directory? i think faceSetDict_rotor is to make surfaces from cellSet and faceSetDict_noboundary is deleted the boundary from sufaces which have been maked by faceSetDict_rotor .by using setsTonZones-commond after these two steps, the aim is to add some special rotate faceZones for case.so if i have had the all faceZones defined such as rotating boundary,there is no need to do these steps.is that rigt?

Q2:there is boudary correction in the MRFZones.c,but if i have rotating boundary,such as hub shround, do i still need to patch or give the angular velocity to the rotating boundary in 0-directory??

thanks�
wayne

[plmauk]

toQ1 : my opinion is: you need these two faceSetDict. To check that, simply try to run the case without makeMesh (and makeMesh-utility is designed for making steps defined in these faceSetDict.)
to Q2 -I don't know. I've never seen the MRFZones.c,because I had no need in that. I simply created my own case, and this case worked. That's all.
Greetings,
Paul.

[waynezw0618]

thanks!
i mean if i need to run the makemesh for my case. i have seen the makemesh file fot mixvessel2D case.
thank!

wayne

[samiam1000]

Dear All,

I know that it is an old conversation. I hope that someone is still following it.

Anyway, I am trying to solve this kind of problem.

I am running OpenFOAM 2.1. I have a msh mesh (built with Workbanch) and I have converted it with fluent3DMeshToFoam.

I want to simulate an opening door. And I want that a zone of my domain remains fixed. I have 2 different zones, called fixed and moving.
How can I make the fixed zone stay fixed?

Thanks,
Samuele

[WernerW]

Hi All,

I'm using fluent3DMeshToFoam to export a mesh to OpenFoam and the process seems to work fine but it simply doesn't save any folder with the mesh in the directory constant/region0. I'm working with a cluster and submiting this command through a submission file whose only comannd is:

fluent3DMeshToFoam nrel.msh

and the mesh: nrel.msh is located in the case folder besides 0.org, system and constant.

Does anyone know what could be the reason and the fix for it ?

Here is the output of the converter. I replaced many lines reporting the conversion of the several faceGroups and patches for "..." and the host and Case name for "###".

Build : 2.4.0-dcea1e13ff76
Exec : fluent3DMeshToFoam nrel.msh
Date : Nov 30 2015
Time : 12:00:52
Host : ######
PID : 28590
Case : ######
nProcs : 1
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Dimension of grid: 3
Number of points: 5818249
PointGroup: 1 start: 0 end: 5818248. Reading points...done.
Number of faces: 17176189
FaceGroup: 4 start: 0 end: 5433. Reading mixed faces...done.
...
FaceGroup: 24 start: 278804 end: 17176188. Reading mixed faces...done.
Number of cells: 5678929
CellGroup: 2 start: 0 end: 3776481 type: 1
CellGroup: 3 start: 3776482 end: 5678928 type: 1
Zone: 2 name: sliding_mesh type: fluid. Reading zone data...done.
...
Zone: 24 name: default-interior type: interior. Reading zone data...done.

FINISHED LEXING

Creating patch 0 for zone: 4 name: top_walls type: wall
...
Creating patch 18 for zone: 22 name: inlet type: velocity-inlet
Creating cellZone 0 name: sliding_mesh type: fluid
Creating cellZone 1 name: farfield type: fluid
Creating faceZone 0 name: default-interior type: interior
faceZone from Fluent indices: 278804 to: 17176188 type: interior
patch 0 from Fluent indices: 0 to: 5433 type: wall
...
patch 18 from Fluent indices: 267456 to: 278803 type: velocity-inlet

Writing mesh to "/scratch/carter/w/wwahanik/WT/NREL/str/constant/region0"

End