Mesh Independent Study
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)? :confused::confused::confused: This is my very first post and any advice would be highly appreciated guys :) 
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. 
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 .. 
I think what FM Denaro was trying to say is that the RANSequations 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. 
Quote:
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... 
@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.:o
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? 
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. 
Quote:
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. http://www.youtube.com/watch?v=TXMPE5mtXcw 
@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 Kmodel in fluent. 
Quote:

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. 
1 Attachment(s)
@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. 
Quote:
standard Kepsilon 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. 
Since we know now that you are using Fluent...:rolleyes:
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:
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. 
I am sorry @flotus1 i should have mentioned that before :o. 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?

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. 
Ok i get it. Thanks a lot guys @flotus1 @FMDenaro @Totalsim. You guys are awesome :) thanks a lot for all the advise

All times are GMT 4. The time now is 19:02. 