CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Cfd simulation on a smooth cylinder (drag coefficient)

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

Like Tree1Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 12, 2016, 21:03
Default Cfd simulation on a smooth cylinder (drag coefficient)
  #1
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Hi to everyone!
Now I will explain my problem:

-Software: STARCM+
-Goal: find the right value of drag coefficient on my cilinder
-Details: u=45.9 m/s, D=1 m, Re=2.9*10^6
- 2D Domain: 10D over the cylinder, 10D belowe the cylinder, 10D at the left of the cylinder, 20D to the right od the cylinder
-Boundary conditions: top and bottom planes are symmetry planes, the right plane is pressure outlet, the left plane is velocity inlet

I can't find the right value of the drag coefficient on my cylinder!! I am getting crazy since the beginning of Semptember!
I have tried both (steady) k-epsilon and k-omega model, but nothing, I have always oscillations (small or large) on the drag coefficients, around 0.4 (that is the right value if I would have a Reynolds of 1*10^6), but I need a value around 0.7 , 0.8 ... Can anyone help me, please?!
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 02:52
Default
  #2
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
Oscillations in a steady-state solution can be a sign that the flow has an unsteadiness that can not be captured correctly by the steady-state approach. In this case this is definitely true.
Consequently, at least an unsteady RANS approach would be necessary to get a converged solution. But even then you will not get the correct value for the drag coefficient without tweaking the turbulence model. The correct approach here is a LES.
flotus1 is offline   Reply With Quote

Old   October 13, 2016, 03:43
Default
  #3
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Thank you for your answer!
After having seen a lot of scientific articles, I know for sure that the only good available methods are the U-RANS and the LES.. And I need to make a comparison between these two method for my master thesis.. I know that by the Strohual number I am able to decide the suitable time-step for my unsteady simulations, so right now I am performing my first unsteady simulation.. do you know how much I have to wai until I get my statistically steady result?
Do you have any suggestion to make some improvements on my simulation?
I have already a very fine mesh: 20 prism layers, 1E-6 first prism layer to the wall, 0.01 m total thickness prism layer, a wally+ between 0.01 and 0.22, a mesh refinement around the cylinder and on its wake.
Maybe something on the initial condition? I don't know, I am desperate..
Thank you very much for your patience!
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 05:20
Default
  #4
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
Let me throw in a few thoughts:
  • Your Y+ values are rather low. Increase the height of the first layer until the maximum y+ value is around 1. The boundary layer will still be resolved accurately but you will have less trouble with high aspect ratio cells away from the wall. And keeping a low volume jump in the transition between prism layers and the rest of the mesh. Keep in mind that a wall-resolving RANS formulation is necessary with y+ values of 1 and below.
  • Don't get me wrong but I heard the phrase "I have already a very fine mesh" numerous times on this site. If you did not estimate the suitable cell sizes in each region of the flow carefully and performed a sensitivity analysis on the cell size this statement is disputable. Feel free to show some images of the mesh you use.
  • The amount of time necessary to reach the steady state is typically in the order of 100 vortex shedding cycles.But do not rely entirely on an initial guess here, simply check your results when they become statistically stationary.

Last edited by flotus1; October 13, 2016 at 09:12.
flotus1 is offline   Reply With Quote

Old   October 13, 2016, 10:31
Default
  #5
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
Are you using the force coefficient report to get cd?
fluid23 is offline   Reply With Quote

Old   October 13, 2016, 11:14
Default
  #6
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 53
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Check these videos. May be useful to you... I will discuss more in detail after you watch these videos...


https://www.youtube.com/watch?v=anTkWfMyEPM

https://www.youtube.com/watch?v=TFQ_0HaBXXM
Far is offline   Reply With Quote

Old   October 13, 2016, 12:13
Default
  #7
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
Let me throw in a few thoughts:
  • Your Y+ values are rather low. Increase the height of the first layer until the maximum y+ value is around 1. The boundary layer will still be resolved accurately but you will have less trouble with high aspect ratio cells away from the wall. And keeping a low volume jump in the transition between prism layers and the rest of the mesh. Keep in mind that a wall-resolving RANS formulation is necessary with y+ values of 1 and below.
  • Don't get me wrong but I heard the phrase "I have already a very fine mesh" numerous times on this site. If you did not estimate the suitable cell sizes in each region of the flow carefully and performed a sensitivity analysis on the cell size this statement is disputable. Feel free to show some images of the mesh you use.
  • The amount of time necessary to reach the steady state is typically in the order of 100 vortex shedding cycles.But do not rely entirely on an initial guess here, simply check your results when they become statistically stationary.
Ok, thank you for your advices!
Here I atached some pictures of my general mesh, then the detail about the cylinder and the result about the drag coefficient (it is about 0.38.. and I would need a greater value!)
I have used k-epsilon method, with implicit unsteady of 2nd order in time, and a time-step of 0.001 s.
I think that I have kept a low volume jump in the transition regionbetween the layers and the general mesh, as you can see..
I wait for your answer, thank you very much again!
Attached Images
File Type: png Screenshot 2016-10-13 09.56.58.png (101.4 KB, 54 views)
File Type: png Screenshot 2016-10-13 09.59.40.png (21.5 KB, 37 views)
File Type: png Screenshot 2016-10-13 10.06.04.png (82.3 KB, 36 views)
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 12:15
Default
  #8
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by Far View Post
Check these videos. May be useful to you... I will discuss more in detail after you watch these videos...


https://www.youtube.com/watch?v=anTkWfMyEPM

https://www.youtube.com/watch?v=TFQ_0HaBXXM
Thank you very much for the kindness!
As soon as I can, I will see these videos!
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 12:19
Default
  #9
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by MBdonCFD View Post
Are you using the force coefficient report to get cd?
Yes, why?
Here I atached some pictures of my general mesh, then the detail about the cylinder and the result about the drag coefficient (it is about 0.38.. and I would need a greater value!)
I have used k-epsilon method, with implicit unsteady of 2nd order in time, and a time-step of 0.001 s.
I think that I have kept a low volume jump in the transition regionbetween the layers and the general mesh, as you can see..
After having seen a lot of scientific articles, I know for sure that the only good available methods are the U-RANS and the LES.. And I need to make a comparison between these two method for my master thesis.. I know that by the Strohual number I am able to decide the suitable time-step for my unsteady simulations, so right now I am performing my first unsteady simulation.. do you know how much I have to wai until I get my statistically steady result?
Do you have any suggestion to make some improvements on my simulation?
I have already a very fine mesh: 20 prism layers, 1E-6 first prism layer to the wall, 0.01 m total thickness prism layer, a wally+ between 0.01 and 0.22, a mesh refinement around the cylinder and on its wake.
Maybe something on the initial condition? I don't know, I am desperate..
Thank you very much for your patience!
Attached Images
File Type: png Screenshot 2016-10-13 10.06.04.png (82.3 KB, 9 views)
File Type: png Screenshot 2016-10-13 09.59.40.png (21.5 KB, 6 views)
File Type: png Screenshot 2016-10-13 09.56.58.png (101.4 KB, 8 views)
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 12:30
Default
  #10
Senior Member
 
Matt
Join Date: Aug 2014
Posts: 947
Rep Power: 17
fluid23 is on a distinguished road
I have run into issues with this before. There is a bug, or as CD-Adapco would call it a philosophical difference that they won't resolve, related to how the issue of unit depth is handled. The coefficient report is a 3D tool. For 2D analysis it assumes you have a depth of 1 m regardless of unit system so the reference area you input needs to reflect this to get the 'correct' coefficient back out of it.

Now that being said, it sounds like you are already in SI units so this may not be the issue you are experiencing. However, given that this bug exists I always shy away from using the coefficient reports and extract force data directly to calculate my own coefficients. It is easier to track down why a coefficient is wrong if you can look and/or control all of the inputs directly.

Try calculating Cd yourself from the drag force and see what you get. There is a good chance you will get a different and possibly better answer.
fluid23 is offline   Reply With Quote

Old   October 13, 2016, 12:40
Default
  #11
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Yes, I know what you are talking about and I have tried few days ago to calculate the drag coefficient like you said, but I've obtained the same result..
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 15:20
Default
  #12
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 53
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Originally Posted by Simone94 View Post
Ok, thank you for your advices!
Here I atached some pictures of my general mesh, then the detail about the cylinder and the result about the drag coefficient (it is about 0.38.. and I would need a greater value!)
I have used k-epsilon method, with implicit unsteady of 2nd order in time, and a time-step of 0.001 s.
I think that I have kept a low volume jump in the transition regionbetween the layers and the general mesh, as you can see..
I wait for your answer, thank you very much again!

what reference values you are using for the Cd?

how did you decide this time step? in how many time steps you are resolving one vortex shedding frequency??

keep Yplus at 0.5-0.8...
Far is offline   Reply With Quote

Old   October 13, 2016, 16:21
Default
  #13
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by Far View Post
what reference values you are using for the Cd?

how did you decide this time step? in how many time steps you are resolving one vortex shedding frequency??

keep Yplus at 0.5-0.8...
I am using as reference values: 101325 Pa, 1,18415 kg/m^3, reference area: 1 m^2 (my diameter is 1 m, so in 2D simulation they coincide), free-stream velocity 45.9 m/s ...
Since the Strohual number should be around 0.25, re-expressing the formula I obtain the inverse of the frequency, that is the period one vortex, and that will be the maximum time-step! However, I resolve in 20, 30 times one vortex shedding..
I will stop the simulation when the solution become statistically steady..
Honestly, I have the y+ quite low (<0.2)..
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 17:05
Default
  #14
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 53
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
that is the period one vortex, and that will be the maximum time-step!
that can be quit dangerous


Quote:
I will stop the simulation when the solution become statistically steady..
I guess that is the time when you start to observe key parameters and take the time mean of values such as Cd...
Far is offline   Reply With Quote

Old   October 13, 2016, 17:23
Unhappy
  #15
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by Far View Post
that can be quit dangerous

I guess that is the time when you start to observe key parameters and take the time mean of values such as Cd...
I didn'the understand both of your statements.. explain yourself better, please
Simone94 is offline   Reply With Quote

Old   October 13, 2016, 18:42
Default
  #16
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 53
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
Quote:
Originally Posted by Simone94 View Post
I didn'the understand both of your statements.. explain yourself better, please
Quote:
that is the period one vortex, and that will be the maximum time-step!
put in this way : you should divide your time for one vortex shedding frequency into 20, 40 or 80 intervals and see which one gives you results which does not change with decreasing time step size.

Quote:
I guess that is the time when you start to observe key parameters and take the time mean of values such as Cd...
You should run your solution up to point when the solution becomes periodic with time. This can be achieved after a long time, so patience. Once this is achieved next thing is to activate the monitors for the lift and drag. This is usually done for 5 cycles, but can be increased to increase accuracy.

Let say for each cycle, you have 20 time steps. so for 5 cycles it is 100 time steps and 100 values for Cd. Just sum all values of Cd and divide sum by 100. that is your time mean drag.

For Cl, practice is different. Normally people quote the root mean square value, because simple mean will give you zero Cl for symmetric bodies such as cylinder.
Far is offline   Reply With Quote

Old   October 13, 2016, 20:56
Default
  #17
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by Far View Post
put in this way : you should divide your time for one vortex shedding frequency into 20, 40 or 80 intervals and see which one gives you results which does not change with decreasing time step size.



You should run your solution up to point when the solution becomes periodic with time. This can be achieved after a long time, so patience. Once this is achieved next thing is to activate the monitors for the lift and drag. This is usually done for 5 cycles, but can be increased to increase accuracy.

Let say for each cycle, you have 20 time steps. so for 5 cycles it is 100 time steps and 100 values for Cd. Just sum all values of Cd and divide sum by 100. that is your time mean drag.

For Cl, practice is different. Normally people quote the root mean square value, because simple mean will give you zero Cl for symmetric bodies such as cylinder.
Ah ok! Thank you very much, I have understood what you said! The only problem is that the residuals are too high, for example in that simulation stated before.. And I don't know why..
However, I will try to apply your advices and I will let you know
Simone94 is offline   Reply With Quote

Old   October 14, 2016, 04:16
Default
  #18
Super Moderator
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 3,384
Rep Power: 46
flotus1 has a spectacular aura aboutflotus1 has a spectacular aura about
The residuals are too high? This means that the results we are discussing here are not converged? Run more iterations per time step.

You should also have a look at these resources:
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
http://www.cfd-online.com/Forums/flu...nvergence.html
flotus1 is offline   Reply With Quote

Old   October 14, 2016, 05:25
Default
  #19
Far
Super Moderator
 
Sijal
Join Date: Mar 2009
Location: Islamabad
Posts: 4,552
Blog Entries: 6
Rep Power: 53
Far has a spectacular aura aboutFar has a spectacular aura about
Send a message via Skype™ to Far
or alternatively reduce the time step by order of magnitude (means divide your current time step by 10, two orders means divide by 100 and so on...)

Example : current time step Delta T = 0.05

order of magnitude reduction = 0.05 / 10 = 0.005

Two orders of magnitude reduction = 0.05 / 100 = 0.0005
Far is offline   Reply With Quote

Old   October 14, 2016, 19:14
Default
  #20
New Member
 
Simone
Join Date: Oct 2016
Posts: 11
Rep Power: 9
Simone94 is on a distinguished road
Quote:
Originally Posted by flotus1 View Post
The residuals are too high? This means that the results we are discussing here are not converged? Run more iterations per time step.

You should also have a look at these resources:
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
http://www.cfd-online.com/Forums/flu...nvergence.html
Ok, thank you
Now I have almost finished my time-step independence study and the residuals are periodically converged, and the same for my drag coefficient.. what I'm worried about is the fact that, smaller the time-step is, smaller the drag coefficient.. I know that I have to do the space grid-indepence study yet, but it is not so comforting..
I would desire my drag coefficient to grow up towards the right value.. XD
Simone94 is offline   Reply With Quote

Reply

Tags
cfd, cylinder, drag coefficient

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Flow past a 2D cylinder - High Re (1E+05) - Cd too high Pervispasco OpenFOAM Running, Solving & CFD 4 March 14, 2022 03:19
Flow past a cylinder at Re 1e05 using LES, drag force coefficient is to low Scabbard Main CFD Forum 21 June 19, 2018 14:58
2D cylinder drag coefficient miku11 OpenFOAM Running, Solving & CFD 0 June 28, 2016 08:36
Pump's Torque in CFD simulation is higher than experience. ngoc_tran_bao CFX 6 June 7, 2016 00:00
Forces Acting on a Rotating Cylinder (Moving Mesh) dreamchaser CFX 5 April 25, 2015 07:01


All times are GMT -4. The time now is 20:56.