Simulation of F1 Diffuser!


Hi Readers!

I’m facing some problems with my project.
Currently have multiple diffuser designs and I have been advised to
-Simulate using Omega SST Steady and then Transient
–Myquestion regarding this is, when using transient mode, my convergence of pressure diverges…What do I do?
–How can I effectively/accurate using Parametric CFD meshing to improve meshing quality of my diffuser.
–Do I need any particular settings for transient in simulation control settings?

-Simulate using LES
–How do I go about using this LES model?

More info on the design I am using:

THANK YOU in advance!


Hi @hmattoo, is this for, Incomp-LES-Ericmode?



Hi Darren
Sorry for missing out on this notification!

The simualtions you could look into are Incomp-LES-EricMODE + Incompressible-LES.
I am not able to understand why can’t I use any transient mode when I simulate? I always end up with an error. What am I doing wrong when I use transient?

Could I also understand-is Omega-SST Transient accurate enough considering I am not looking for the most accurate data?

(It would be great to use LES models, as I can show/report better results)


Hi @hmattoo, not sure if I got the right project/run but looking at the link I posted your courant numbers are too high:

here is a good post about courant number:

But you might want to consider just using auto timestep.

Hope this helps,


Hi Darren

I did try wrapping my head around CFL numbers…However, I cannot understand the formula.
C=velocity*(Time step/interval length) ; I want to firstly know are these all in the simulation control settings? Next interval length is the start and end time or is it something else?


Hi @1318980

I did try LES model (Model Diff Smaller, simulation: Incompressible-LES) and it did work however my Pressure did not converge rather diverged. Also if you could please have a look at the post process picture, the stream tracer is far away from the object.


Hi @hmattoo, yes that run was much better. I wouldn’t say it diverged but certainly didn’t converge, for this, you need to scrutinise the log more than the convergence plot here is a few snippets:

Time = 0.286886368375
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 6.74117971501e-06, Final residual = 6.74117971501e-06, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1.75298190874e-05, Final residual = 7.93333693667e-08, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 6.26020051249e-06, Final residual = 6.26020051249e-06, No Iterations 0
GAMG: Solving for p, Initial residual = 0.389706167708, Final residual = 0.000352334314097, No Iterations 5
time step continuity errors : sum local = 4.20726605867e-11, global = -2.16534466255e-14, cumulative = 2.08006533724e-09
PIMPLE: iteration 2
DILUPBiCG: Solving for Ux, Initial residual = 3.37594193009e-06, Final residual = 3.37594193009e-06, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 9.94923733837e-06, Final residual = 9.94923733837e-06, No Iterations 0
DILUPBiCG: Solving for Uz, Initial residual = 4.12905237522e-06, Final residual = 4.12905237522e-06, No Iterations 0
DICPCG: Solving for p, Initial residual = 0.158912061823, Final residual = 0.00152583737678, No Iterations 9
time step continuity errors : sum local = 1.91809715287e-10, global = 8.38393525006e-13, cumulative = 2.08090373077e-09
PIMPLE: not converged within 2 iterations
ExecutionTime = 4293.83 s ClockTime = 4765 s
Courant Number mean: 0.00985675328817 max: 0.199950292921
deltaT = 6.07334373398e-05

I’ve bold italicised the bits that are important, the pressure didn’t fall below the termination criteria in 2 iterations. I have found that with 2 correctors I rarely get convergence, I set it to 20 and let it end early if it converges, I find this usually happens in less than 5 outer iterations. This setting is dictated in the ‘Numerics’ section under the number of outer correctors.

As for the Courant number, unless you know the cell sizes its very hard to calculate, your choice to go with auto time stepping is good.

Kind regards,


Hi @1318980

Really appreciate this! I am still learning how to use simscale to its peak.
I cannot seem to find the auto time stepping?


No problem @hmattoo, I think you found it on your last simulation and run, If I remember correctly it is only available for PIMPLE not PISO solver for transient. you will find it under Simulation Control:

Where you define the maximal courant number, if it is a fairly stable simulation, i.e. no sudden peaks in velocity then you can set this high, close to 1 but if not then best leave it at 0.5.

Kind regards,


Hi @1318980
Thank you once again.

I’d like to add on in many of my post proceses, when I select stream tracer - the streamlines aren’t around the solid part rather somewhere in space. Why is this?


Hi @hmattoo, I did look at the post processing image and it looked ok, what do you mean in space? have you got an image you want it to look like? basically a few visual aids here would help :slight_smile:

Kind regards,


Hi @1318980

Here is the file


Oh ok, the stream line is point source so just adjust the point to be over the geometry (I would imagine somewhere around the origin 0,0,0)



Hi @1318980

I cannot thank you enough for all your support!
But I still have questions coming along as I progress.

In my simulation if I see negative static pressure, how do I see it? ie. is it simply pressure in the opposite direction of the positive axis?

Thank you!


Hi @hmattoo, yes basically in Incompressible flows we presume no density change and therefor there is no pressure change due to gravity effects allowing us to the calculation at any pressure with equal results. Most of the time we use pressure 0 as this allows us to quickly differentiate between low and high-pressure whether it is negative or positive, to apply that pressure to say 1atm you simply add it on.

Kind regards,


Hi @1318980

So its fair to say that negative just signifies pressure in the opposite direction?


Just think of it as gauge pressure, relative to the defined pressure (usually 0).



Hi @1318980

Thank you!
I also would like to ask for any material on how to use the hex-dominant parametric meshing CFD mode.
I am in need to control each surface meshing quality and currently have a Vortex project with 3 geometries that require indivivual meshing qualities.

I also have a project coming up with a full car sketch which would have multiple quality meshing required.

Would be great to know how to go about doing this?

Thank you!


Hi @hmattoo,

I found this one a while ago:

Another good resource now is actually the SimScale documentation, they were revamped since my post for hex dominant meshing with images of the mesh as a result of changing the settings.

The best way to get use to it is practice a little, I find it a lot better than automatic at the moment. You will be most interested in mesh layers and refinements on individual surfaces for your projects so that would be a good place to start. As well a volume refinements. And of course if you need more help when you do the project just start a forum post :slight_smile:

Kind regards,