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

Ansys fluent grid independence test

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

Like Tree6Likes
  • 3 Post By scipy
  • 1 Post By scipy
  • 1 Post By scipy
  • 1 Post By LuckyTran

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 28, 2016, 07:26
Unhappy Ansys fluent grid independence test
  #1
New Member
 
MANI VINAYAK
Join Date: Mar 2016
Posts: 5
Rep Power: 7
Jesh is on a distinguished road
Hii.. i am new to CFD. I am doing spanwise lift analysis for my wing design.i have no idea how to do grid independence test for my model.please help me with it.
Jesh is offline   Reply With Quote

Old   April 28, 2016, 10:27
Default
  #2
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
Just start with a coarse grid (let's say 50 points spanwise) and refine the mesh in all directions (both normal to the wing and spanwise/chordwise) until results stop differing between the solutions (or at least differ <2%). Then you can call your solution grid independent.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   April 28, 2016, 10:38
Default
  #3
New Member
 
MANI VINAYAK
Join Date: Mar 2016
Posts: 5
Rep Power: 7
Jesh is on a distinguished road
okay...but what u mean by solution? the Cl values which i want to get from cfd post?
Jesh is offline   Reply With Quote

Old   April 28, 2016, 10:48
Default
  #4
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
Yes. Any observable value or whatever you're aiming to present. You can also set up a Cl, Cd, Cm or other monitor in FLUENT (no need to wait until it's all over to get to CFD-Post). So, let's say you're trying to match the results of an experiment and those are Cd=0.15 and Cl=0.5 or whatever.

Your first (coarse/rough) grid gives you Cd=0.19 and Cl=0.33, then you refine your grid and run the simulation again, this time Cd=0.17 and Cl=0.42. Next refinement step Cd=0.157 maybe and Cl=0.485.. and last refinement you get to 0.152 and 0.496.

The percentile change between the last two Cd results is ~3% and for Cl it's ~2,3%. You might as well call this grid independent or do another refinement and run again. It's just important to show that you are asymptotically approaching a single value (this can be an experimental value or an analytical solution) - at least until things like round off errors and discretisation errors come into play.
Jesh, Paku and ENG.AHMAD like this.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   April 28, 2016, 10:54
Default
  #5
New Member
 
MANI VINAYAK
Join Date: Mar 2016
Posts: 5
Rep Power: 7
Jesh is on a distinguished road
oh okay..thank you so much..that was very helpful sir
Jesh is offline   Reply With Quote

Old   February 3, 2020, 17:24
Default
  #6
New Member
 
AHMAD ABOULKHAIL
Join Date: Nov 2018
Location: Turkey
Posts: 9
Rep Power: 4
ENG.AHMAD is on a distinguished road
Quote:
Originally Posted by scipy View Post
Yes. Any observable value or whatever you're aiming to present. You can also set up a Cl, Cd, Cm or other monitor in FLUENT (no need to wait until it's all over to get to CFD-Post). So, let's say you're trying to match the results of an experiment and those are Cd=0.15 and Cl=0.5 or whatever.

Your first (coarse/rough) grid gives you Cd=0.19 and Cl=0.33, then you refine your grid and run the simulation again, this time Cd=0.17 and Cl=0.42. Next refinement step Cd=0.157 maybe and Cl=0.485.. and last refinement you get to 0.152 and 0.496.

The percentile change between the last two Cd results is ~3% and for Cl it's ~2,3%. You might as well call this grid independent or do another refinement and run again. It's just important to show that you are asymptotically approaching a single value (this can be an experimental value or an analytical solution) - at least until things like round off errors and discretisation errors come into play.
When the number of grid elements increased from 28 million to 29 million, the Nusselt number and the pressure drop were changed by 2.61% and 0.39%, respectively, can my grid be now considered independent?!
ENG.AHMAD is offline   Reply With Quote

Old   February 3, 2020, 17:39
Default
  #7
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
This depends on the grids you used previously and where exactly you squeezed the 1 million elements.

For example... a grid that goes from 28 mil to 29 mil is baaasically the same. Unless you fit all 1 million elements directly into an area that was under-defined (let's say the boundary layer). I'd say that grid is already detailed enough but I don't know the details of your problem. To show grid independence for a problem that you now know requires around 30 million elements, you should start much lower/coarser.

Grid 1 = 500 000 elements
Grid 2 = 2 mil elements
Grid 3 = 5-8 mil
Grid 4 = 12-15 mil
Grid 5 = 25-30 mil

Then you can show that the change from Grid 4 to Grid 5 was negligible OR if it wasn't for some reason, you should change your approach. Use higher quality elements for the domain (such as hex instead of tetra), add elements in the normal direction of the wall (boundary layer), place elements in areas where flow features require it or something else entirely. Maybe you can do a Grid 6 of 35 mil to show that the change is then irrelevant and then call Grid 5 your grid-independent solution.

It all depends on the problem you're trying to solve, your resources, meshing methods, solvers used and a shitload of other stuff.

o/
ENG.AHMAD likes this.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   February 4, 2020, 02:54
Default
  #8
New Member
 
AHMAD ABOULKHAIL
Join Date: Nov 2018
Location: Turkey
Posts: 9
Rep Power: 4
ENG.AHMAD is on a distinguished road
Quote:
Originally Posted by scipy View Post
This depends on the grids you used previously and where exactly you squeezed the 1 million elements.

For example... a grid that goes from 28 mil to 29 mil is baaasically the same. Unless you fit all 1 million elements directly into an area that was under-defined (let's say the boundary layer). I'd say that grid is already detailed enough but I don't know the details of your problem. To show grid independence for a problem that you now know requires around 30 million elements, you should start much lower/coarser.

Grid 1 = 500 000 elements
Grid 2 = 2 mil elements
Grid 3 = 5-8 mil
Grid 4 = 12-15 mil
Grid 5 = 25-30 mil

Then you can show that the change from Grid 4 to Grid 5 was negligible OR if it wasn't for some reason, you should change your approach. Use higher quality elements for the domain (such as hex instead of tetra), add elements in the normal direction of the wall (boundary layer), place elements in areas where flow features require it or something else entirely. Maybe you can do a Grid 6 of 35 mil to show that the change is then irrelevant and then call Grid 5 your grid-independent solution.

It all depends on the problem you're trying to solve, your resources, meshing methods, solvers used and a shitload of other stuff.

o/
Thank you very much for your prompt response. I followed the method of changing the value of y + in order to change the size of the grid. Is this method correct, or should the size of the maximum element size or the number of layers in the inflation of the boundary layer be changed? please follow any methods that should be used for scaling the grid size.
Many thanks in advance
ENG.AHMAD is offline   Reply With Quote

Old   February 4, 2020, 04:45
Default
  #9
Senior Member
 
scipy's Avatar
 
Alex Pasic
Join Date: Aug 2011
Location: Croatia
Posts: 199
Rep Power: 12
scipy is on a distinguished road
Send a message via Skype™ to scipy
It's not possible for me to know that since I don't know anything about your problem. Also, there's a LOT of difference in grids that need to have a y+<1, y+<5 or wall-function grids where y+ can be anywhere from 30-300. If you're in the log-law region then refining the grid for y+ won't really bring you that much, but if it's a direct wall resolving grid then all the solutions where y+ is out of the specified range are basically garbage.

y+ in an of itself might not be enough. Imagine you had the first element close enough to the wall for the y+ to be OK but then you just transition right away into tetrahedral elements. That grid would be garbage since it wouldn't resolve the whole boundary layer. You should read the meshing recommendations that come with your solver or at least ones for your specific turbulence model and wall resolving approach (wall functions or direct). Usually these will say "at least 10 prism elements in the normal direction with a growth no more than 20% in this direction". For wall resolving grids, even that is too low and you usually have to have as many layers as needed so that the last prismatic elements are "tall" enough so that the volumetric transition ratio into the first tetra or poly elements is not more than 30% - the volume of the last prism has to be just 20-30% less than the volume of the first attaching tetra/poly element.

Your refinements should be in all these directions AND account for areas with large pressure gradients or other values of interest. If you have shockwaves in your problem, then your mesh has too be refined along the lines of huge pressure changes in order to be able to resolve that area at all. Just an example..
ENG.AHMAD likes this.
__________________
If you're in need of some free quality CFD video tutorials - check out SiriusCFD @ YouTube
scipy is offline   Reply With Quote

Old   February 4, 2020, 08:47
Default
  #10
New Member
 
AHMAD ABOULKHAIL
Join Date: Nov 2018
Location: Turkey
Posts: 9
Rep Power: 4
ENG.AHMAD is on a distinguished road
Quote:
Originally Posted by scipy View Post
It's not possible for me to know that since I don't know anything about your problem. Also, there's a LOT of difference in grids that need to have a y+<1, y+<5 or wall-function grids where y+ can be anywhere from 30-300. If you're in the log-law region then refining the grid for y+ won't really bring you that much, but if it's a direct wall resolving grid then all the solutions where y+ is out of the specified range are basically garbage.

y+ in an of itself might not be enough. Imagine you had the first element close enough to the wall for the y+ to be OK but then you just transition right away into tetrahedral elements. That grid would be garbage since it wouldn't resolve the whole boundary layer. You should read the meshing recommendations that come with your solver or at least ones for your specific turbulence model and wall resolving approach (wall functions or direct). Usually these will say "at least 10 prism elements in the normal direction with a growth no more than 20% in this direction". For wall resolving grids, even that is too low and you usually have to have as many layers as needed so that the last prismatic elements are "tall" enough so that the volumetric transition ratio into the first tetra or poly elements is not more than 30% - the volume of the last prism has to be just 20-30% less than the volume of the first attaching tetra/poly element.

Your refinements should be in all these directions AND account for areas with large pressure gradients or other values of interest. If you have shockwaves in your problem, then your mesh has too be refined along the lines of huge pressure changes in order to be able to resolve that area at all. Just an example..
Thanks a lot for the explanation you provided
ENG.AHMAD is offline   Reply With Quote

Old   February 4, 2020, 09:02
Default
  #11
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 4,142
Rep Power: 50
LuckyTran has a spectacular aura aboutLuckyTran has a spectacular aura about
Grid independence is a misleading term. You'll never get 0% change.


Grid sensitivity is a better mindset to have. You need to quantify the sensitivity of the "sought-after-parameter" on the grid by testing various grids. You'll find some finite % change. You decide whether that % change is acceptable or not using whatever criteria is relevant.
ENG.AHMAD likes this.
LuckyTran is offline   Reply With Quote

Old   February 4, 2020, 09:54
Default Very true
  #12
Senior Member
 
vinerm's Avatar
 
Vinerm
Join Date: Jun 2009
Location: Nederland
Posts: 2,946
Blog Entries: 1
Rep Power: 32
vinerm will become famous soon enough
Yes, that's true; grid independence is a misnomer. Grid Sensitivity is more appropriate and is subjective. Similarly, this is also true that most users think of refining the mesh whenever they have to study the grid sensitivity. While this is incorrect. Coarsening of the mesh is equally effective and is used by professionals most of the time. If lift or drag variation is within 1 to 2% for two meshes, then both are equally good; of course, coarser is meant to be used. Lift and drag are only examples; you should monitor the field that is most specific to your case.
__________________
Regards,
Vinerm

PM to be used if and only if you do not want something to be shared publicly. PM is considered to be of the least priority.
vinerm is offline   Reply With Quote

Reply

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
Fluent in Ansys Workbench : Change Working Directory sral FLUENT 4 March 29, 2019 10:29
How to open Icem mesh in Ansys Fluent? emmkell FLUENT 27 February 6, 2018 03:34
grid independence test issue djordje8 STAR-CCM+ 0 September 8, 2014 10:21
grid independence test in ansys14 fot fluent abinashlipun FLUENT 1 January 17, 2013 10:48
[GAMBIT] 3.5 years overtake by Ansys: Where are the enhancements in grid generation Volker P. ANSYS Meshing & Geometry 22 January 17, 2012 17:27


All times are GMT -4. The time now is 06:54.