[yangzhuan]

Hi,
I just learn openFOAM for a short time. And a problem has been bothering me for a week. Why my setFields is not work. My setFields is that.
defaultFieldValues
(
volScalarFieldValue alpha.water 0
);
regions
(
boxToCell
{
box (0 0 0) (1.0 0.1 0.1);
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);

This case is a channel od dimensions 1.00m*0.10m*0.15m(length, width, height). No matter how to change the boxToCell, there is nothing to change. Only the inlet is water. But i want a half water and the rest is air. I have seen many posts here. But there is still no solution. I really nead help.
Thank you!

[Dipsomaniac]

Hi Alice

It will help to show the axes and extent of the domain, so that we know where the origin is relative to the domain. setFields works with respect to the origin, and your defined box may actually be outside of the domain of interest.

Regards,
Brian

[Blanche]

I think it is that. I also want to ask this question.

[yangzhuan]

Originally Posted by Dipsomaniac

Hi Alice

It will help to show the axes and extent of the domain, so that we know where the origin is relative to the domain. setFields works with respect to the origin, and your defined box may actually be outside of the domain of interest.

Regards,
Brian

Thanks a lot,
I marked several special points on the Figer. I don't know where is wrong. I hope you can give me some advice.
Thank you again.

[Dipsomaniac]

can you please run

checkMesh

and post the results?

[Tomatenbart]

What exactly do you want to be covered in water?

Have you changed your mesh after you firstly executed setFields?
Try deleting your alpha.water file in the 0 folder and get a new fresh one in there, so that in the alpha.water file is no water field set and you don't see any 1 and 0. And then execute setFields again.


Sent from my iPhone using CFD Online Forum mobile app

[yangzhuan]

Originally Posted by Dipsomaniac

can you please run

checkMesh

and post the results?

Ok, I run the "checkMesh". The result is that,

Create time
Create polyMesh for time = 0
Time = 0
Mesh stats
points: 126000
faces: 354288
internal faces: 331458
cells: 114291
faces per cell: 6
boundary patches: 4
point zones: 0
face zones: 0
cell zones: 0
Overall number of cells of each type:
hexahedra: 114291
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0
Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
Number of regions: 1 (OK).
Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
in 102 126 ok (non-closed singly connected)
out 459 504 ok (non-closed singly connected)
bimian 18036 18352 ok (non-closed singly connected)
atmosphere 4233 4500 ok (non-closed singly connected)
Checking geometry...
Overall domain bounding box (0 -3.55271e-15 -3.55271e-15) (1000 100 150)
Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
Mesh has 3 solution (non-empty) directions (1 1 1)
Boundary openness (-2.341e-17 8.36564e-18 -5.38205e-15) OK.
Max cell openness = 1.50386e-16 OK.
Max aspect ratio = 2.71493 OK.
Minimum face area = 8.70147. Maximum face area = 38.3754. Face area magnitudes OK.
Min volume = 51.1851. Max volume = 154.118. Total volume = 1.5e+07. Cell volumes OK.
Mesh non-orthogonality Max: 0 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 2.8308e-13 OK.
Coupled point location match (average 0) OK.
Mesh OK.
End

[Phicau]

There you go, your overall domain bounding box is (1000 100 150) and you are filling only (1.0 0.1 0.1).

You need to modify blockMeshDict, either changing the coordinates to metres or add "convertToMeters 0.001;" to it.

Best,

Pablo

[yangzhuan]

Originally Posted by Phicau

There you go, your overall domain bounding box is (1000 100 150) and you are filling only (1.0 0.1 0.1).

You need to modify blockMeshDict, either changing the coordinates to metres or add "convertToMeters 0.001;" to it.

Best,

Pablo

I use the ICEM to draw the mesh. There is no blockMeshDict. So what should I input in the terminal?

[Phicau]

Then run this utility:

transformPoints -scale '(0.001 0.001 0.001)'

[yangzhuan]

Originally Posted by Phicau

Then run this utility:

transformPoints -scale '(0.001 0.001 0.001)'

I have tried. it works. This problem has been bothering me for several days, and finally solved. Thank you for your help. Thank you!
Hope you have a nice day!