[rshbhb]

Hello,

I have a concentric cylinder geometry as shown i the figure, such that,

Inner wall is Rotating
Outer wall is stationary
Upper wall is stationary
lower wall is stationary
Fluid (liquid) is confined in the annular region (volume).

Do I have to use a dynamic mesh or moving mesh OR I can mesh the geometry normally and rotate the inner walls in FLUENT ? (I have used the 2nd option).
------------------------------------------------------
REGARDING SIMULATION (I have referred to "Non-Newtonian Transitional Flow in an Eccentric Annulus")

STEP BY STEP ANALYSIS OF MY PROBLEM

1. Models: As I am simulating the taylor couette flow of an incompressible fluid, my problem will go from laminar to turbulent flow pattern. In this case what kind of model should I use :Viscous-> k-epsilon or K-omega ? (I had used standard k-epsilon with standard wall functions).

[rshbhb]

2. Boundary Conditions: For interior rotating wall. I gave MOVING WALL -> Absolute -> Speed (rad/s) -> Rotational axis origin (0,0,0) -> roation axis direction (0,0,1) -> No slip

For Fluid (liquids): Rotation axis direction (0,0,1) & Motion type -> Stationary (IS IT CORRECT or should I use MRF or Moving Mesh???)

I HAVE NOT USED periodic conditions.

[rshbhb]

3. Solve -> Control -> Solution -> I had used SIMPLE MODEL (Pressure Velocity coupling). Is it correct?

Equations used FLOW & TURBULENCE

4. Solve ->Initialize -> in the compute from list i ha used inner wall. is it correct or should i just keep it empty and press INITIALIZE button??

5.After Iterating it. Solution did converge and I got a velocity magnitude vector profile like the one shown in figure below (fig.1) but at an angular vel. of 1500 rad/s i expected to get tayloe vortex as shown in fig.2 .

I THINK I HAVE GONE WRONG SOME WHERE please help me out with this.


Kind Regards,
Rishabh.

[ghost82]

In this case what kind of model should I use :Viscous-> k-epsilon or K-omega ?

It depends on the turbulence; how do you define if your regime is laminar or turbulent?

If you have a turbulent regime just try different turbulence model to find which is approaching the "real" solution.
You can use k-epsilon for fully turbulent flow, k-omega for transitional laminar to turbulent flow. Use laminar if you have a laminar regime.
Consider that you must verify your y+ values depending on the model you use.

IS IT CORRECT or should I use MRF or Moving Mesh???

I think it is correct, since in the tutorial "Non-Newtonian Transitional Flow in an Eccentric Annulus" only the inner cylinder is rotating without mrf nor sliding mesh.

I had used SIMPLE MODEL (Pressure Velocity coupling). Is it correct?

Since you obtain a converged solution simple is ok.

in the compute from list i ha used inner wall. is it correct or should i just keep it empty and press INITIALIZE button??

I imagine that you perform a stationary simulation, so it doesn't matter with what values you initialize the solution. The important thing is that starting from the initialization values you can reach a converged solution.

Try to change your model (turbulence, transition) depending on the rotational speed and set in your parameters second order upwind schemes.
You set the bases as walls; are you sure the second picture is taken by applying the same boundary conditions?Are you sure the domain is not periodic in the second picture?

Daniele

[Far]

IS IT CORRECT or should I use MRF or Moving Mesh???

I think it is correct, since in the tutorial "Non-Newtonian Transitional Flow in an Eccentric Annulus" only the inner cylinder is rotating without mrf nor sliding mesh.

I think both will have the same results (MRF and moving wall). What do you think when to use the MRF and moving wall only.

[ghost82]

Originally Posted by Far

I think both will have the same results (MRF and moving wall). What do you think when to use the MRF and moving wall only.

This is a good question and I don't have an answer.
I found this:
http://www.cfd-online.com/Forums/flu...ting-wall.html

This can explain why we use mrf or sliding mesh for a rushton turbine, which is not a surface of revolution and we can use moving wall in this case (?).

I also think that mrf will give the same results.

[Far]

I am unable to access the links. Would you like to send the papers (also tutorial you were referring earlier in this post) on my email id turboenginner@gmail.com.

Thank-you for your very informative post.

[ghost82]

Originally Posted by Far

I am unable to access the links. Would you like to send the papers (also tutorial you were referring earlier in this post) on my email id turboenginner@gmail.com.

Thank-you for your very informative post.

Sent!

Added also a mediafire link.

Daniele

[Far]

Thankyou very much, got em.

[Far]

Previous results were with u1 = 20 rad/sec and this one with 5 rad/sec. Other parameters areRefer to this article http://www.compassis.com/downloads/M...tte%20Flow.pdf)

Density = 1 Kg/m3

Kinematic viscosity = 0.1 m2/sec

d1 (inner cyclinder dia) = 2 m

d2 (outer cylinder dia) = 4 m

Length of cylinder = 2 m



So what is the Reynolds number for u1= 5 rad/sec, 20 rad/sec ?
http://research.ncl.ac.uk/quantum-fl...willis-phd.pdf

http://www.cats.rwth-aachen.de:8080/...ette181207.pdf

http://www.cats.rwth-aachen.de:8080/...ette181207.pdf

[ghost82]

Originally Posted by Far

So what is the Reynolds number for u1= 5 rad/sec, 20 rad/sec ?

In my opinion, the Reynolds number, which is dimensionless is:

Re=(U0*d*density)/mu

U0 cannot be expressed in rad/s, otherwise the Re is not dimensionless, so it must be in m/s, so I think U0 is the peripheral speed of the rotating cylinder.
U0=omega*radius, where omega is the angular velocity in rad/s

d is the characteristic length, in my case=(outer radius - inner radius) and it is expressed in m

density is the density of the fluid (kg/m3)

mu is the dynamic viscosity of the fluid, expressed in Pa*s or, in other words, kg/(s*m)

With the dimensional analysis:

Re=(m/s)*(m)*(kg/m3)*(s*m/kg)

Re is dimensionless.
This is how I calculate the Re

Referring to your data and your cited article I think Re, to be dimensionless is calculated as:
Re=(density*(angular velocity)*radius*radius)/mu

where (angular velocity)*radius is the peripheral velocity; the only difference is the characteristic length

density in kg/m3
angular velocity in rad/s
radius in m (of the rotating cylinder)
mu in Pa*s

So for u1=5 rad/s, Re (your article)=50
for u2=20 rad/s, Re (your article)=200

PS: I think in page 4 of your cited article there's an error: Re is calculated with radius=1 m, but it is not rotating!

PS2: density=1 kg/m3: what type of fluid is it?is it a gas?Is the Taylor-Couette flow valid for gases??

[Far]

Originally Posted by ghost82

PS2: density=1 kg/m3: what type of fluid is it?is it a gas?does the Taylor-Couette flow is valid for gase??

I think in the end what matters is the Reynolds number! It does not matter as I believe and it is the essence of non dimensional quantities.

[rshbhb]

Originally Posted by Far

I think in the end what matters is the Reynolds number! It does not matter as I believe and it is the essence of non dimensional quantities.

Dear Sirs,

I want to ask you which fluent version are you using?

I am using GAMBIT for geometry and FLuent Solver (Fluent 6.3.26). I want to know that will i get such good images with the versoin of Fluent that I have?

Sir I'll upload the geometry (in GAMBIT) in 15 mins or so could you please verify if it'll be ok for correct simulation. MY Laptop is not very fast (only 3GB RAM).

[Far]

Originally Posted by rshbhb

Dear Sirs,

I want to ask you which fluent version are you using?

I am using GAMBIT for geometry and FLuent Solver (Fluent 6.3.26). I want to know that will i get such good images with the versoin of Fluent that I have?

Sir I'll upload the geometry (in GAMBIT) in 15 mins or so could you please verify if it'll be ok for correct simulation. MY Laptop is not very fast (only 3GB RAM).

I am using Ansys Fluent 14.

Yes you can get the same images in Fluent, there is no change in these features. They have just improved flow schemes and included other turbulnece model and wall treatments.

I have also 4GB laptop. But I will be more than happy to look at your mesh. Meanwhile you can compare your mesh with mine or Daniele's. Daniele's opinion will be more valuable in this regard.

[rshbhb]

Originally Posted by Far

I am using Ansys Fluent 14.

Yes you can get the same images in Fluent, there is no change in these features. They have just improved flow schemes and included other turbulnece model and wall treatments.

I have also 4GB laptop. But I will be more than happy to look at your mesh. Meanwhile you can compare your mesh with mine or Daniele's. Daniele's opinion will be more valuable in this regard.

Dear Sir,

For faster communication i have sent you chat request on your gmail id.
Please accept it.

[rshbhb]

Sir,

How do I hard link the faces before meshing in GAMBIT?

I am just getting the option of linking the face meshes.

[ghost82]

Originally Posted by rshbhb

Sir,

How do I hard link the faces before meshing in GAMBIT?

I am just getting the option of linking the face meshes.

Yes, you have to link the faces. See button in the attached image.

[behzad.ramtin]

finally any one could model this?
pls email me

behzadfakour@gmail.com

[Far]

someone indicated that link for dropbox files is not working : Post # 25. Here is new link:

https://dl.dropboxusercontent.com/u/...ute_taylor.rar

[R4RAHUL]

if you want to know your flow near the surface wall of your domain then you can use " k-episilon" and if you want to know far away from the surface wall then use "k-omega