[jamalf64]

I've done everything that friends said, but my problem does not converge whether with one phase or multiphase.
any suggestion?

[-mAx-]

hot spots still here?

[jamalf64]

Originally Posted by -mAx-

hot spots still here?

Yes, they are available

[-mAx-]

then is your interface problem not solved

[jamalf64]

Originally Posted by -mAx-

then is your interface problem not solved

So what do I do?

[-mAx-]

check if interfaces are well defined (gambit and fluent)
Else try mrf as ghost82 mentioned

[ghost82]

Originally Posted by -mAx-

hot spots still here?

I saw Jamal's dbs file of the tank and setutp the cas file in fluent; in my opinion the cas and dbs are ok..
In my opinion, big discontinuities should disapperar if you will obtain a converged solution..
Fluent's guide tell about slight discontinuities across interfaces:

"Data displayed on these surfaces will be "one-sided''. That is, nodes on the interface zones will "see'' only the cells on one side of the grid interface, and slight discontinuities may appear when you plot contour lines across the interface."

In my opinion, Jamal should modify the mesh, to not create interfaces (if he want to solve the problem with mrf), to have more possibilities to make to converge the problem.
As stated, multiphase problems + interfaces + quite high rotational velocity are not simple to solve..
Do you agree guys?

Daniele

[jamalf64]

Originally Posted by -mAx-

check if interfaces are well defined (gambit and fluent)
Else try mrf as ghost82 mentioned

Thank you so much

[ghost82]

I tried to solve the monophase problem (only water), with mrf, deleting interfaces: mesh inside the rotor is tetra (size function applied from impeller faces to rotor volume, from 0,25 cm to 0,4 cm, ratio 1,3, same dimensions as the original grid), outside is hexa.
I'm attaching the scaled residual plot: as you can see, with fluent default parameters, continuity doesn't drop below 1e-03, and other residuals oscillate a bit; at about the 2750th iteration I changed momentum under relaxation factor to 0,1, but as you can see residuals keep oscillating a bit..
Velocity monitors at the 2 planes below and above the impeller are not 100% stable, but I think solution is not too far to full convergence.

See the other 2 images: do you think is it reasonable solution?the generated flow is similar to the Taylor-Couette flow.

I think you have to refine more the mesh..but I'm not so expert to tell you how big a cell should be..
I think the monophasic simulation can be the first step to test your case; once you will reach the full convergence you can try to switch to the multiphase simulation..

Daniele

[-mAx-]

Originally Posted by ghost82

I think the monophasic simulation can be the first step to test your case; once you will reach the full convergence you can try to switch to the multiphase simulation..

Yes always starting with simple case, then increase complexity

[jamalf64]

Originally Posted by ghost82

I tried to solve the monophase problem (only water), with mrf, deleting interfaces: mesh inside the rotor is tetra (size function applied from impeller faces to rotor volume, from 0,25 cm to 0,4 cm, ratio 1,3, same dimensions as the original grid), outside is hexa.
I'm attaching the scaled residual plot: as you can see, with fluent default parameters, continuity doesn't drop below 1e-03, and other residuals oscillate a bit; at about the 2750th iteration I changed momentum under relaxation factor to 0,1, but as you can see residuals keep oscillating a bit..
Velocity monitors at the 2 planes below and above the impeller are not 100% stable, but I think solution is not too far to full convergence.

See the other 2 images: do you think is it reasonable solution?the generated flow is similar to the Taylor-Couette flow.

I think you have to refine more the mesh..but I'm not so expert to tell you how big a cell should be..
I think the monophasic simulation can be the first step to test your case; once you will reach the full convergence you can try to switch to the multiphase simulation..

Daniele

Dear Daniele,
I dont know approximate answer. Perhaps your answer is correct.

[ghost82]

Am I wrong or your domain is periodic?
If you have not enough computational resources you can model only a 90 degree domain..I will try.

Daniele

[jamalf64]

Originally Posted by ghost82

Am I wrong or your domain is periodic?
If you have not enough computational resources you can model only a 90 degree domain..I will try.

Daniele

I dont know that you're wrong or not, but because my geomtry is whole, I dont think that domain is periodic

[ghost82]

Originally Posted by jamalf64

I dont know that you're wrong or not, but because my geomtry is whole, I dont think that domain is periodic

Jamal your domain is periodic; you can cut a 90 degrees and if you imagine to paste each cut to make the full 360 degrees you will obtain your full domain; look at the picture.
To make the domain periodic, in gambit, cut your volumes with 2 vertical planes (centered XZ, y=0 and centered YZ, x=0) and retain only a 90 degrees slice; then mesh-link each pair of the new vertical faces (refer to some other tutorial to make periodic faces in gambit, or search this forum).
Make each pair of the new vertical faces as periodic boundaries, then in fluent set rotational periodic for the periodic boundaries.

I refined the grid of this new domain, but I haven't enough time to make it full hexa, so I make it tetra with size functions; problems are the same as in the other case, residuals continue to oscillate a bit.
However I think that periodic simulation is a good approximation of the full domain (see at the new pictures and compare them with others).

Daniele

[behruz]

Hi all
I want to solve a rushton turbine in stirred tank in fluent. I do this according to a fluent tutorial .A part of this tutorial describe MRF method. And it named a space that is.named rotational zone. Can any one explaine me what have to do for use MRF method?
and what is rotational zone?
thank

[ghost82]

Originally Posted by behruz

Hi all
I want to solve a rushton turbine in stirred tank in fluent. I do this according to a fluent tutorial .A part of this tutorial describe MRF method. And it named a space that is.named rotational zone. Can any one explaine me what have to do for use MRF method?
and what is rotational zone?
thank

Hi Behrooz,
as you can read in the tutorial, if you use mrf, you have to divide your domain (fluid), into 2 zones: a cilindrical rotating zone, which surrounds the impeller, and a static zone, which is the remaining.
A common question in this type of approach is: "how big the rotating zone should be?": Fluent user guide tells that "the rotating zone must include the rotating element, so every size is good; you should try different size of the rotating zone and see if/how results change.
Mrf approach is good in respect to sliding mesh, because it require less computational efforts, but on the other hand you have less accurate results and you shouldn't use this approach if the tank has baffles, because of the flow interactions.
Once you have your mesh, with the 2-fluid zones, you should setup fluent as:

- rotating zone (fluid): rotating, choose a point on rotating axis, and the rotation vector
- static zone (fluid): stationary
- impeller walls and part of the shaft wall (inside the rotating zone): rotating, relative velocity, in respect to adjacent cells equal to 0 rpm (this means that impeller rotates with the same velocity of the rotating zone)
- tank wall and bottom wall (adjacent to the static zone): rotating with 0 rpm absolute velocity
- remaining shaft wall: rotating with an absolute velocity of xxx rpm (same as rotating fluid zone)

Hope that helps a bit,

Daniele

[behruz]

thank mr DANIELE for compelete and clear discribtion
i have one other problem : when i choose file .msh in fluent , show a extra wall that i did not select az a boundry condition!!! does this boundry make an error in my results?!
and one other problem : fluent show a warning that number of grid does
not mach...do u know what is this error?!!
thanks

[ghost82]

Originally Posted by behruz

thank mr DANIELE for compelete and clear discribtion
i have one other problem : when i choose file .msh in fluent , show a extra wall that i did not select az a boundry condition!!! does this boundry make an error in my results?!
and one other problem : fluent show a warning that number of grid does
not mach...do u know what is this error?!!
thanks

Pictures are welcome
Make sure you don't have a "double face".
What's the software you used to make the mesh?any warning/error when exporting the mesh?
Sometimes happened also to me (nodes don't match): with no errors in geometry a remesh usually solve the problem.

Daniele

[behruz]

i mesh it with GAMBIT
there is this error in gambit: "a physics entity labeled wall already exists and thus the input label cannot be used. a default (unspecified)boundry entity was created for 4 entities including the folowing: face 78,72,73,70

[-mAx-]

If you read the message returned, you may understand that you tried to create a BC with a name which is already used. Gambit created then another boundary without any type