CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

FLuent simulation of taylor couette flow of concentric cylinder geometry.

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

Like Tree30Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   October 26, 2012, 08:44
Default FLuent simulation of taylor couette flow of concentric cylinder geometry.
  #1
New Member
 
rshbhb
Join Date: Oct 2012
Posts: 26
Rep Power: 4
rshbhb is on a distinguished road
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).
Attached Images
File Type: jpg Mesh Grid.JPG (34.5 KB, 123 views)

Last edited by rshbhb; October 26, 2012 at 09:12.
rshbhb is offline   Reply With Quote

Old   October 26, 2012, 08:56
Default
  #2
New Member
 
rshbhb
Join Date: Oct 2012
Posts: 26
Rep Power: 4
rshbhb is on a distinguished road
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 is offline   Reply With Quote

Old   October 26, 2012, 09:24
Default
  #3
New Member
 
rshbhb
Join Date: Oct 2012
Posts: 26
Rep Power: 4
rshbhb is on a distinguished road
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.
Attached Images
File Type: jpg At 1500rad,s. Vel vectoe magnitude.JPG (67.0 KB, 130 views)
File Type: jpg fig.2.JPG (19.5 KB, 139 views)
rshbhb is offline   Reply With Quote

Old   October 26, 2012, 10:00
Default
  #4
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Quote:
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.

Quote:
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.

Quote:
I had used SIMPLE MODEL (Pressure Velocity coupling). Is it correct?
Since you obtain a converged solution simple is ok.

Quote:
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 and rshbhb like this.
ghost82 is offline   Reply With Quote

Old   October 26, 2012, 10:13
Default
  #5
New Member
 
rshbhb
Join Date: Oct 2012
Posts: 26
Rep Power: 4
rshbhb is on a distinguished road
Quote:
Originally Posted by rshbhb View Post
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.
Thank you Daniele for your insights.

I'll do the simulations again and let you know the results.

-Rishabh.
rshbhb is offline   Reply With Quote

Old   October 26, 2012, 15:30
Default
  #6
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Just for fun I tried a laminar regime with Re=1000; you can see Taylor vortices.
Instead of wall for bases I set periodic condition (in gambit you have to link the faces before meshing and apply a periodic boundary for all the bases).

Daniele
Attached Images
File Type: jpg taylor.jpg (38.9 KB, 149 views)
Far, rshbhb and sk333bits like this.
ghost82 is offline   Reply With Quote

Old   October 26, 2012, 16:40
Default
  #7
New Member
 
rshbhb
Join Date: Oct 2012
Posts: 26
Rep Power: 4
rshbhb is on a distinguished road
Dear Daniele Sir/Ma'am,

I tried the simulation again with the new parameters as you described but still i m getting the same results as shown in the figure below (even with glycerine as the liquid).

Its good to know that you got taylor vortices. I want to ask you,

1.what did you use as fluid?
2.Which faces do I have to link ? (do you mean bottom faces together & upper tw faces together?)
3. I have simulated with k-w and k-e models, should I use laminar model to get taylor vortex?
4.Should the periodic conditions be given as described in the FLUENT tutaorial guide "Non newtonian flow..."?
5.how do you get this image? (I only know to get contours and vectors) Do you use any iso-suraface ?
6. How many number of nodes did you have in your mesh ?
7. Let me know If I am able to convey my doubts properly to you ?


-Rishabh.

Last edited by rshbhb; October 26, 2012 at 17:03.
rshbhb is offline   Reply With Quote

Old   October 27, 2012, 04:12
Default
  #8
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Quote:
Originally Posted by rshbhb View Post
Dear Daniele Sir/Ma'am,

I tried the simulation again with the new parameters as you described but still i m getting the same results as shown in the figure below (even with glycerine as the liquid).

Its good to know that you got taylor vortices. I want to ask you,

1.what did you use as fluid?
2.Which faces do I have to link ? (do you mean bottom faces together & upper tw faces together?)
3. I have simulated with k-w and k-e models, should I use laminar model to get taylor vortex?
4.Should the periodic conditions be given as described in the FLUENT tutaorial guide "Non newtonian flow..."?
5.how do you get this image? (I only know to get contours and vectors) Do you use any iso-suraface ?
6. How many number of nodes did you have in your mesh ?
7. Let me know If I am able to convey my doubts properly to you ?


-Rishabh.
Hi,
first of all you need to evaluate the fuid dynamic regime; you need to evaluate the Reynolds number to know if your regime is laminar, transitional or turbulent.
In the free article "Direct numerical simulation of turbulent Taylor–Couette flow" you can read that the authors obtain a laminar regime for Re=1000 and a turbulent regime for Re=3000, Re=5000 and Re=8000.
When you evaluate the Reynolds number take in mind that U0 is expressed in m/s and it's omega*Rinternal (omega in rad/s and Rinternal in m).
Once you know what regime you have you can start your simulations.
I imposed the periodic boundary because I read in this article "Consider the incompressible flow between two infinitely long concentric cylinders".

1. I simulated Re=1000 with water as fluid, so my regime is laminar.
2. Yes, you have to link bottom and upper faces in gambit, so when you will mesh the bottom faces, the upper ones will be automatically meshed; also you have to set one periodic boundary contidion for all these 4 faces.
Read here:
Hard-linking faces in Gambit (periodics)
If you will not link the faces, or if you will not set one periodic boundary gambit will not let you export the mesh.
3. It depends on your regime as written above.
4. All you have to do, once you have imported the mesh into fluent, is to set translational periodic condition in the boundary condition panel (you can choose between rotational and translational).
I imposed a 0 pressure gradient.
5. the image is a plot contour of velocity magnitude; then from display->scene I checked overlays and plot the vector graph.
For the vector graph I choosed from vector options "in plane", black color, and a scale factor of 3.
6. I'm on a mac now so I don't remember exact value but for the laminar regime I choosed a mean of 2-3 mm between the nodes; take in mind that the distance between nodes is a function of the turbulence model you will use, check the fluent guide for y+ values.
7.

All the bests,

Daniele

P.S.
I'm a Sir

P.S.2
Can you upload your image in the post above? I can't see it
Attached Images
File Type: jpg taylor2.jpg (24.9 KB, 94 views)
Far and rshbhb like this.

Last edited by ghost82; October 27, 2012 at 04:35.
ghost82 is offline   Reply With Quote

Old   October 27, 2012, 04:49
Default
  #9
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Also,
if you need to refine your grid and you have not a "powerful pc" you can simulate only a slice (for example 60 degrees; the angle must be a divisor of 360 degrees) of the 2 concentric cylinders (see the attached image I found on google, just for reference).
In this case you will have to set an additional rotational periodic boundary on the 2 vertical faces; as for the horizontal faces the 2 vertical faces have to be linked before meshing them.
Attached Images
File Type: jpg velo_streamline_full.jpg (38.4 KB, 101 views)
Far and rshbhb like this.
ghost82 is offline   Reply With Quote

Old   October 27, 2012, 13:00
Default
  #10
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
At Re = 8000, flow is still considered as taylor couette flow?


http://www.compassis.com/downloads/M...tte%20Flow.pdf
Far is offline   Reply With Quote

Old   October 27, 2012, 17:45
Default
  #11
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
I want to try this flow. Could you please tell me the following:

1. speed in rad/s
2. density and viscosity
3. length of cylinder
4. inner and outer dia
5. How you define the Reynolds number
6. Flow is laminar or turbulent and what are basis to consider flow laminar or turbulent.

I have tried with arbitary values and this is what I get.



ghost82 likes this.

Last edited by Far; October 27, 2012 at 18:26.
Far is offline   Reply With Quote

Old   October 28, 2012, 02:23
Default
  #12
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
Originally Posted by ghost82 View Post
Also,
if you need to refine your grid and you have not a "powerful pc" you can simulate only a slice (for example 60 degrees; the angle must be a divisor of 360 degrees) of the 2 concentric cylinders (see the attached image I found on google, just for reference).
In this case you will have to set an additional rotational periodic boundary on the 2 vertical faces; as for the horizontal faces the 2 vertical faces have to be linked before meshing them.
It is possible to define the double periodicity in ICEM? Any idea?

Edit : Not possible in ICEM, should be defined in Fluent using command define>boundary-conditions>modify-zone>make-periodic

Some quick results from the sector cut simulation are given below with same parameters but refined mesh in the axial direction, radial and tangential direction due to only 45 deg geometry. u1 = 20 rad/sec (arbitrary value)







After more iterations:



ghost82 and rbgamblin like this.

Last edited by Far; October 28, 2012 at 03:01. Reason: given in post
Far is offline   Reply With Quote

Old   October 28, 2012, 03:29
Default
  #13
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Quote:
IS IT CORRECT or should I use MRF or Moving Mesh???
Quote:
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.
Far is offline   Reply With Quote

Old   October 28, 2012, 05:49
Default
  #14
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Quote:
Originally Posted by Far View Post
I want to try this flow. Could you please tell me the following:

1. speed in rad/s
2. density and viscosity
3. length of cylinder
4. inner and outer dia
5. How you define the Reynolds number
6. Flow is laminar or turbulent and what are basis to consider flow laminar or turbulent.
Hi Far!

these were my parameters:

1. 2.5 rad/s
2. Water: density: 1000 kg/m3, viscosity: 0,001003 Pa*s (default)
3. referring to this last simulation: 0.12 m
4. Inner radius: 0.02 m, outer radius: 0.04 m
5. Re=density*U0*d/viscosity, where:
U0 is omega*Inner radius, omega is the angular velocity in rad/s, d is outer radius minus (-) inner radius.
See here:
http://www.math.purdue.edu/~sdong/pd...ette-jfm07.pdf

or here:
http://www.mediafire.com/?4varocdijzhfm5g

6. The article above states that Re=1000 is laminar, Re=3000, 5000 and 8000 are turbulent; so I suppose that between Re=1000 and 3000 there's transition regime (?)
I don't know if when Re=8000 flow is still considered Taylor-Couette, from the article it seems is still considered Taylor-Couette; I only tried one simulation with basic scientific literature research.

In this last simulation I consider a slice (60 degrees) with a very fine grid (a mean of 0.5 mm with a total of 576000 hexa cells), with a double periodic boundary (rotational around z axis and translational in z direction).
I obtained a converged solution when residuals drop under 1*10^-7 (monitor some z iso surface to see if converged solution is reached!!)

However I have problems in post processing with the fluent built in; I receive this error when:

- plot contour
- Display-->Views-->Periodic repeats-->define

Error: CAR: invalid argument [1]: wrong type [not a pair]
Error Object: #f

I think this is related with the double periodic boundary (rotational and translational). No problems in post processing as you can see from the pictures below in CFD-POST and Tecplot.

Herein below some pictures:
Attached Images
File Type: png taylor60-1.png (15.3 KB, 59 views)
File Type: jpg taylor60-2.jpg (92.7 KB, 54 views)
File Type: jpg taylor60-3.jpg (32.8 KB, 73 views)
File Type: jpg taylor60-4.jpg (61.0 KB, 65 views)
File Type: jpg taylor60-monitor1.jpg (28.7 KB, 51 views)
Far and rshbhb like this.

Last edited by ghost82; October 28, 2012 at 06:42.
ghost82 is offline   Reply With Quote

Old   October 28, 2012, 05:50
Default
  #15
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Some other pictures:
Attached Images
File Type: jpg taylor60-monitor2.jpg (29.7 KB, 44 views)
File Type: jpg taylor60-monitor3.jpg (27.8 KB, 39 views)
File Type: jpg taylor60-residuals.jpg (26.4 KB, 38 views)
ghost82 is offline   Reply With Quote

Old   October 28, 2012, 05:53
Default
  #16
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Quote:
Originally Posted by Far View Post
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:
Fundamental Question about Rotating wall!

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.

Last edited by ghost82; October 28, 2012 at 07:07.
ghost82 is offline   Reply With Quote

Old   October 28, 2012, 06:15
Default
  #17
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to 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.
Far is offline   Reply With Quote

Old   October 28, 2012, 06:31
Default
  #18
Senior Member
 
ghost82's Avatar
 
Daniele
Join Date: Oct 2010
Location: Italy
Posts: 731
Rep Power: 13
ghost82 will become famous soon enough
Quote:
Originally Posted by Far View Post
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
ghost82 is offline   Reply With Quote

Old   October 28, 2012, 06:36
Default
  #19
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Thankyou very much, got em.
Far is offline   Reply With Quote

Old   October 28, 2012, 11:20
Default
  #20
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,899
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to 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 likes this.
Far 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
Simulation of cylinder aligned in the flow direction using k-e model Eliasjal FLUENT 2 June 13, 2012 09:00
Simulation of steam (CO2 and Water vapor mixture) flow through nozzle using Fluent. Jimmy FLUENT 0 March 2, 2011 13:30
Simulation Flow Around cylinder 3D Jwolf CFX 19 November 25, 2009 15:21
Compressible flow simulation using FLUENT arun Main CFD Forum 0 February 16, 2004 16:44
Simulation of the Flow past a circular cylinder using STAR-CD M. S. GUEROUACHE Main CFD Forum 0 October 1, 1998 11:51


All times are GMT -4. The time now is 13:07.