SimScale CAE Forum

Transient CFD


#21

You’re right @Novak_Ondrej, mea culpa - already trying with the transient one :slight_smile:

And I should have mentioned that I just adapted the BC’s and not the step size. Do you have reference values for this calculation? Would be interesting to know.

Cheers,

Jousef


#22

Good.
Well according to AVL and XFLR5 the aircraft should be getting about Fz=23,2 N and in steady state i m getting about 23N . This trend is consistent with my steady state simulations ( using old coarse mesh).
This tells me my simulations in steady state were done corretctly.
So now only transient one …


#23

Hi @Novak_Ondrej,

as in your case my transient simulation failed and it might take a bit until I find the mistake and the right settings to make it work. Maybe @Get_Barried and @vgon_alves can give some additional input on that topic. Keeping you up-to-date.

Jousef


#24

Hi everyone,

Running my own runs on this project. Had to remesh as the domain was much too big and costly to run. There might be some fine tuning needed for the geometry and mesh. The issue with Transient simulations is that the mesh is much more sensitive to mesh quality than steady-state, hence why both of you are running into errors or results that don’t converge/are inaccurate. So while you @Novak_Ondrej may be able to get results out for steady-state, it doesn’t mean the mesh/geometry is of sufficient quality to be able to run for transient.

Let you know the needed fixes after the runs.

Cheers.

Regards,
Barry


#25

Hi guys!

Just looked up some stuff about PIMPLE. With this algorithm we search a steady-state solution with under-relaxation in one time step. We move forward in time as we find a solution. We use the outer correction loops, to ensure that explicit parts of the equations converged. @Get_Barried, had a look at your setup and the simulation will probably take a huge amount of core hours. About the methodology: @Novak_Ondrej, are you looking for transient phenomena anyway or is it a simulation to see if the transient solution converges to the one from steady-state?

Cheers,

Jousef


#26

My goal is to find, if there are some flow structures that are not steady and transient CFD is going to be neccesary or if flow is mainly steady-state and i dont have use transient simulations.


#27

Hey Jousef,

Agreed. The timestep needed is much too small and takes too long. We will need to optimize aggressively to obtain something workable.

Any suggestions atm? I might go for further mesh optimization.

Cheers.

Regards,
Barry

EDIT: Tuning this run will take awhile so get back to you when a concrete solution is found.


#28

Hi @Novak_Ondrej,

So I aggressively optimized the mesh by significantly decreasing the bounding box and reducing the levels of refinement throughout the mesh which dropped the total number of nodes to around 200,000 instead of 3 million. The domain is also much shorter which reduces the end time needed in a sense. I made a small error by not setting the results control and saved timesteps properly, but below is the timestep of around 0.1s for what seems like an oscillatory converged run.

While pressure is having issues converging, that is to be expected with such a corase mesh. Overall, the sim seems very stable (the second run is on going now, same mesh). The Co is set to 1 and if you have a really well optimized mesh, you can aim for a Co of 0.7 and that may help the pressure to converge. We’ll probably deal with that later after I finish another run.

Flow separation can be seen for sure as seen in the more clearer screenshot below. So things are looking not bad. The layers for the mesh are holding up though despite the coarseness of the mesh so that is one less headache.

Update again once I have more information.

Cheers.

Regards,
Barry


#29

Hello

that is great ! i m happy to see you made progress.
Thanks a lot a keep me updated


#30

Hi @Novak_Ondrej,

Yep the simulation runs fine. My mesh and setup is a good starting point. You can find the project here. Do copy it over to your side as I won’t keep user projects on my end for long and will delete them after awhile. Here is a quick gif of the run.

ezgif-1-e2c2edf66857

The end time is 0.4s with a Co of 1. Only 8 timesteps were saved hence the low frame rate. Flow separation indeed does occur and you can observe the convergence plots and all the relevant data in the project link.

From this point on, you should first check the CL/CD or some variable to see how much error the corase mesh produces and from there continually refine the mesh by keeping the geometrical values of the bounding box the same so as to keep computational costs down to a minimum. You should only touch the domain only if you have continually refined the needed areas significantly and the results don’t deviate significantly anymore, which would then indicate that the domain is the source of error.

You will also need a longer end time instead of my 0.4s. Maybe even double as from the point probes, the flow is still developing.

Do note to keep an eye on your node count as you mesh. This 200,000 node mesh already takes about 9 hours to simulate and 300 core hours so you can imagine what a longer timestep, change of relaxation factors and a finer mesh will do to the time needed for the simulation to complete.

Good luck and keep us posted on your progress.

Cheers.

Regards,
Barry


#31

Hello

thanks a lot, this great ! To all above, thank you and i consider this case solved.

All the best in 2019 !