# Mesh Independent Study

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

 March 25, 2013, 12:20 Mesh Independent Study #1 New Member   isuru Join Date: Mar 2013 Posts: 8 Rep Power: 5 I am doing a mesh independent study on a 'flow over the car' simulation. I have simulated the study using 1 million, 2 million and 4 million mesh elements but there is a considerable difference in the final drag value. (The difference of drag for 2 million and 4 million mesh models are 1.8% and this is similar between 1 million and 2 million mesh elements). So what does this mean? Am i doing something wrong? Can this be due to the mesh quality (Aspect ratio, Skewness)? This is my very first post and any advice would be highly appreciated guys

 March 25, 2013, 15:29 #2 Member     Jon Join Date: Mar 2013 Posts: 47 Rep Power: 5 Hi Isuru, You can keep going up with mesh count forever and continuously get different answers. We have run cars with up to 250M cells and have still not got a 'mesh independent' solution, according to the text books. The main problem with cars is that they are inherently unstable. For us we start to see diminishing returns past 60M. Good luck. vangelis and rgd like this. __________________ TotalSim CFD Engineer www.totalsimulation.co.uk

 March 26, 2013, 04:53 #3 Senior Member   Filippo Maria Denaro Join Date: Jul 2010 Posts: 2,500 Rep Power: 31 what about the solution you expect to converge? Grid independence means that your local truncation error was small, but if you use some turbulence modelling (RANS) then you must have care in what grid independence is ..

 March 26, 2013, 07:07 #4 New Member   isuru Join Date: Mar 2013 Posts: 8 Rep Power: 5 @Totalsim Well at the moment the maximum number of mesh elements I can have is 8 million. I don't have enough computational resources to create a mesh with more than 8 million elements. So what is the general number of mesh elements you use for your simulations? @FMDenaro What do you mean by 'the solution you expect to converge'? And i am using K- model to solve this problem.

 March 26, 2013, 07:17 #5 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,266 Rep Power: 22 I think what FM Denaro was trying to say is that the RANS-equations themselves are only an approximation. So there is no need to reduce the truncation error to 0.01% with an abundance of computational resources while the error introduced by the RANS approximation is much higher.

March 26, 2013, 07:24
#6
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,500
Rep Power: 31
Quote:
 Originally Posted by flotus1 I think what FM Denaro was trying to say is that the RANS-equations themselves are only an approximation. So there is no need to reduce the truncation error to 0.01% with an abundance of computational resources while the error introduced by the RANS approximation is much higher.
yes, this is the clue ... the RANS modelling contribution overcomes the magnitude of the local truncation error, therefore rather than a "grid independence", you should expect a "model parameters independence". But I am not sure if that has actually some sense for RANS where the solution towards you would converge is statistical.

However, using your code, did you get a grid independent solution for an academic case such as the channel or backward facing step? I would first check that before working on the car...

 March 26, 2013, 08:07 #7 New Member   isuru Join Date: Mar 2013 Posts: 8 Rep Power: 5 @flotus1 @FMDenaro I am checking for mesh Independence by comparing the number of elements against the drag value I get by solving the problem using Ansys Fluent. I am sorry guys if i am not providing the exact answers to your questions. I am new to this field and still getting to know all the technical terms. Now when I solve the problem for a like 200 iterations it converges (Msg appears saying solution converged). But how can I find the local truncation error value? Can this be done using fluent?

 March 26, 2013, 08:20 #8 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,266 Rep Power: 22 With only 200 Iterations, it is highly probable that the solution is not converged. At least not to a point where it makes sense to compare results on different meshes. You should definitely monitor the drag force vs. iterations and judge convergence based on this figure. rgd, Totalsim and engineer.iman like this.

March 26, 2013, 08:20
#9
Member

Jon
Join Date: Mar 2013
Posts: 47
Rep Power: 5
Quote:
 Originally Posted by isuru @Totalsim Well at the moment the maximum number of mesh elements I can have is 8 million. I don't have enough computational resources to create a mesh with more than 8 million elements. So what is the general number of mesh elements you use for your simulations?
We use typically between 55 and 65M cells depending upon the level of complexity in the model, but each model is different. As the other guys are saying, your choice of turbulence model and solution settings are paramount.

We run a combination of RANS and DES to try and address this. The DES helps us pickup the transient flow phenomena that RANS cannot, but it comes at a computational penalty.

One of our DES simulations, if you're interested.
__________________
TotalSim CFD Engineer
www.totalsimulation.co.uk

 March 26, 2013, 08:39 #10 New Member   isuru Join Date: Mar 2013 Posts: 8 Rep Power: 5 @flotus1 When I use the 4 million mesh profile the fluent says that 'the solution is converged' at around 180 iterations. But is there a link between the amount of iterations required and the performance of the computer? @totalsim the model i am working on is very basic and got no details like mirrors, air vents etc. Thanks for the simulation mate it is mint. I am using K-model in fluent.

March 26, 2013, 08:45
#11
Senior Member

Filippo Maria Denaro
Join Date: Jul 2010
Posts: 2,500
Rep Power: 31
Quote:
 Originally Posted by isuru @flotus1 When I use the 4 million mesh profile the fluent says that 'the solution is converged' at around 180 iterations. But is there a link between the amount of iterations required and the performance of the computer? @totalsim the model i am working on is very basic and got no details like mirrors, air vents etc. Thanks for the simulation mate it is mint. I am using K-model in fluent.
the fact that fluent says "the solution is convergent" is only an indication that the residual is smaller than the tolerance fixed in the code. Therefore, what about the tolerance you set, did you change from the default values? If it is not properly made small, the "convergence" is only a false indication ..

 March 26, 2013, 09:07 #12 Member   Thiagu Join Date: Oct 2012 Location: India Posts: 59 Rep Power: 5 You are not providing any clear information about the case setup for complex problem like this. In CFD it is very common to blame turbulence model , without much investigating case setup/mesh/fluid properties/covergence critria/sover control & so... always provide reasonable details such as # mesh cut section # Key solver parametes & BCs # residual plots & monitor plots or error informations.

March 26, 2013, 09:08
#13
New Member

isuru
Join Date: Mar 2013
Posts: 8
Rep Power: 5
@FMDenaro In fluent how can i check/edit the tolerance? And what factors would determine a sensible value for tolerance?
I have attached a screenshot of the convergence study for 1M element mesh profile.
Attached Images
 Untitled.jpg (92.8 KB, 73 views)

March 26, 2013, 09:14
#14
New Member

isuru
Join Date: Mar 2013
Posts: 8
Rep Power: 5
Quote:
 Originally Posted by jthiakz You are not providing any clear information about the case setup for complex problem like this. In CFD it is very common to blame turbulence model , without much investigating case setup/mesh/fluid properties/covergence critria/sover control & so... always provide reasonable details such as # mesh cut section # Key solver parametes & BCs # residual plots & monitor plots or error informations.
Well I am using
standard K-epsilon model
Inlet,outlet walls, road and car boundary conditions. Inlet velocity is 20m/s and all the walls and road are moving walls moves in the downward flow direction.
I am using standard fluent values and only changing velocity.

March 26, 2013, 09:41
#15
Senior Member

Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,266
Rep Power: 22
Since we know now that you are using Fluent...
go to the "Monitors" tab and edit the Residuals.
Untick the "check convergence" boxes for every equation.
Now your simulation will run the specified amount of iterations.

Here you can also add the "drag" and "lift" monitors. Make sure to specify the correct reference values.

Quote:
 all the walls and road are moving walls
It it more appropriate to have only the floor as moving wall. The side and top walls should be symmetry boundary conditions.
This doesnt make much difference if these walls are sufficiently far away from the region of interest. But still, one thing less to worry about.

 March 26, 2013, 11:10 #16 New Member   isuru Join Date: Mar 2013 Posts: 8 Rep Power: 5 I am sorry @flotus1 i should have mentioned that before . Now when i untick the "check convergence" boxes fluent does not stop the convergence study right. But what would be a residual value i should be looking for? Can it be 0.001?

 March 26, 2013, 12:19 #17 Senior Member     Alex Join Date: Jun 2012 Location: Germany Posts: 1,266 Rep Power: 22 Judging convergence solely on the global residuals for the equations solved is dangerous. Since it is the drag coefficient you are interested in, you should monitor this value. At some point, it will (hopefully) level out. This tells you that the solution is converged, at least with respect to the drag coefficient. Of course you should still keep an eye on the global residuals. For example if they do not drop at all, this indicates that something might be wrong with the setup. rgd likes this.

 March 26, 2013, 12:35 #18 New Member   isuru Join Date: Mar 2013 Posts: 8 Rep Power: 5 Ok i get it. Thanks a lot guys @flotus1 @FMDenaro @Totalsim. You guys are awesome thanks a lot for all the advise

 Tags ansys 13, cfd, mesh, mesh dependency, mesh quality

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post thezack CD-adapco 6 August 26, 2016 10:12 Anorky ANSYS Meshing & Geometry 4 November 12, 2014 01:27 chelvistero OpenFOAM 11 January 15, 2010 20:43 hung FLUENT 7 April 18, 2005 09:38 Danard Main CFD Forum 1 December 5, 2002 08:32

All times are GMT -4. The time now is 12:36.