SimScale CAE Forum

Help with CFD problem/ wavy force plots

Hi I am trying to compare forces for different ride hight and angles on a 3 wheeled racing bike.
The problem I am having is the force plots for lift (Y) are inconsistent and wavy so no good for comparative purposes.
I have tried parametric and automatic wind tunnel meshes with no improvement. I have also tried soften the edges on the cad model and re mesh but no luck. my attempts can be found here

I would be grateful if someone have a look and point me in the right direction.

Thanks in advance

1 Like


Thanks for posting your question and welcome to SimScale.

I see what you mean: @sjoshi or @Ali_Arafat, any tips to improve this?

Hi @c3po,

I’ve copied your project. My (wrong) guess was that the missing Initial condition was the problem:


I ran the simulation (

The result is identical to yours so it was not the problem.

I checked other settings and one thing hit my eyes:

your k and omega values are strange for me. I mean I’m not an expert - I found this in the topic: . I usually go with the default parameters which are different in the degree of magnitude with yours:

Default k: 0.00375 m2/s2
Your k: 1.5 m2/s2

Default omega: 3.375 1/s
Your omega: 44.72 1/s

Maybe they are well-defined and correct but currently I don’t find anything else that could lead for such unstable result. So my suggestion is to double-check these parameters and let me know about your thoughts.


Hi János
Thanks for your help. I have tried what you suggested changing omega and K to default but the results are the same. unstable :frowning:
I got my omega and K values from the f1 aerodynamics workshop in SimScale where there is a table for different speeds and associated K and omega values. I have used these values before with no problems I cant find out now why the simulations are so unstable. I have tried STEP and STL file format. parametric and automatic wind tunnel meshes with no improvement I have also tried copying the FSAE-Workshop-S3 simulation and using the Numeric values from that but still unstable.
I cannot understand what the problem could be. any more suggestions?


1 Like

Hi Tony,

I see.
Based on what you wrote I suspect of two things:

  • Problems with model (I know you’ve tried several formats but maybe there are some invalid surfaces)

  • Under “Numerics” there are several options like changing the solver type, and a lot of other parameters.It is more like a black box for me but changing here and there maybe could solve this issue. But I suggest to ask the support team for more professional answer. :smiley:

Some info here:

In case you need an estimation of forces I’d do the following:

  • Extract the force plot to Excel
  • Define a time range where the convergence was stable
  • Select the force values of that time domain
  • Calculate the avarage value

I know it is not the nicest method but good for a rough estimation and a quick check for drag/lift coefficient validation.

I’m quite busy today but I’ll keep na eye on the topic and will have a look on it when able.

Keep me updated about the progress!



@c3po, this means that your simulation has not sufficiently converged. We could simply run the simulation for longer, however, I don’t think this will get the convergence you require, instead, I would add some dampening in the numerics section (relaxation factor set lower). This removes instability at the cost of time to converge. Monitoring the force plot is a great way to tell if your simulation is converged, depending on the problem convergence could be obtained in the residual range anywhere between 1e-3 and 1e-8 (in your case some residuals only just reached 1e-3) so it really is advised to check force plots to ensure convergence is reached. I would expect with the increased dampening that these plots would eventually even out. I would set residual termination low and just kill the simulation when this happens that way we won’t have to re-run if convergence is not reached at 1e-5 (default value).

Hope this helps,
Anything else just drops a message.

Kind regards,


Hi Tony, hi Darren,

I set up a quick simulation with coarse automatic mesh and reduced boundary box to speed things up for some experimenting.

The first was just a simple reference run with the default parameters.
By the second I changed the solver types to Smooth solver.
Unfortunately I typed 20m/s instead of 50 at the runs so I’m running a third one with Smooth solver as well.

First run force plot (run time: 15"):

Second run force plot (run time: 34"):

In both cases the drag force is around 131N which gives a drag coeff of about cD=0.54.

My conclusion is that using Smooth solver doesn’t really improve result quality neither convergence although the initial phase is much smoother. The big hump near the end in both cases is quite strange for me. Do you have any idea what happened there?

I’m wondering about what Darren said. How do you define the magnitude of relaxation factor? Is it something that can be calculated, or some kind of experience?

Best regards,

1 Like

Hi all,

I think these force instabilities could actually be stemming from the mesh. As you can see in Simulation 0.8 +0 WT 3, the size of the mesh is changing a lot in the wake region behind the car:

By increasing the size of the Cartesian box region (A1…0.8_ _0.0_PMesh adj - modified mesh) and making the mesh in the wake region more uniform, the force plots flatten out:

It could also be that since I’m using a coarser mesh, the convergence is faster; thus as @1318980 said above you may just need to use more time steps to get a converged solution regarding the force plots.

Hope this helps!

Project link:



Hi Everyone Thank you all for your input/help I am now getting much better results. My meshes were on reflection much to fine and taking forever to converge and like Anna pointed out the Cartesian box region behind the car was also to small.
The results I got between the fine and coarse meshes when they worked were very similar. I think for this simple model a coarser mesh is fine.

Thanks again