Hi everyone, any insight is appreciated. I am simulating with a D/1000 [first boundary layer height] mesh the flow past a square cylinder (inside a Circular domain). For Coarser mesh, I had no issues with the simulation but with D/1000, I get a Floating Point Error!
For a very low time step size (Courant Number around 0.5) the error vanishes but the simulation is super slow and even slightly increases the time step size results in a Floating Point Error!
Has anyone got any idea on it?
Hi
I think you need to check your aspect ratio and skewness. In this way, Be careful that the size of your mesh around the solid is finer than the domain. For example, you can use sizing order and reduces your size mesh around your solid. Besides, Check the jointing of the nodes is ok.
Hi
Solving your problem numerically requires a very large array for storing data in terms of space and time. I offer you some solutions hoping to find them useful:
· use another more powerful laptop.
· test with a little coarser mesh D / 900 then D / 800..etc until the Floating Point Error disappears.
· gradually increase the time step
· reduce the relaxation factor to a low number and especially for the energy equation if you use it.
good luck
You may need to check the mesh metrics particularly mesh skewness and non-orthogonality.
To everyone who devoted their time to give their insights on this topic. Thank you.
Here is what I have come to understand regarding this problem.
Regarding Mesh:
A colleague of mine and I are using the same mesh for the simulation and she has no problem with the mesh. I have also checked the mesh quality in Fluent and I believe it is highly unlikely that mesh is the problem.
Solution: I could do away with the Floating Point error with the following.
1. Hand calculating, for my simulation I needed 1e-4 sec as time-step size. Using Piso with this timestep gave me Floating Point Error (FPE hereafter).
If I was using Piso I had to reduce the time-step to even lower values and it was computationally expensive.
So I went with SIMPLEC with lower timestep values. FPE disappears with 1e-5 timestep and it's faster than Piso but I just finished the simulation and the accuracy isn't very good.
If you all have a similar experience with FPE, it would be nice to hear from you all.
For steady-state simulations in Fluent in any version beyond 2019. Rx the built-in pure (elliptic equation) steady-state solvers are no longer recommended.
Use instead:
* Coupled solver
* pseudo-transient solution approach
* HOTR = on
* Auto-timestep works usually fine, but you might want to play around with it manually to even more speed-up the simulation or to enhance solver stability by manually reducing the pseudo-timescale.
This behaves much more stable than the outdated steady-state approaches with SIMPLEC and PISO and so on. It is essentially the adapted algorithm, which ANSYS CFX had already used forever.
Regards,
Dr. Th. Frank.
Dr. Thomas Frank, thank you for the insight.
I have read prior literature and they have got proper results using PISO and SIMPLE so I would like to continue with the same. But I will remember your suggestion and thank you for recommending it.
Manoj
Manoj Pradhan : Potentially it is possible, if the solution process converges properly, to obtain correct solutions with the old and outdated elliptic solver algorithms too. But it is a waste of time and computational resources. You have experienced the difficulties with these solvers by yourself already.
Regards,
Dr. Th. Frank.
Dr. Thomas Frank, I think I understand the significance of your suggestion. I would like to go with a pseudo-transient solution approach and use PBCS.
The manual states that the pseudo-transient solution approach is meant for Steady-State cases but my simulation (Flow Past a Cylinder) is a Transient Problem I suppose. Is it recommended to use the pseudo-transient solution approach in my case?
If your problem is transient by nature, than a full transient solution scheme of course needs to be used. Have you written here somewhere, that you are solving a transient problem? Should I have overlooked something?
Nevertheless you can apply the PBCS solver with 2nd order backward Euler transient scheme as well.
Regards,
Dr. Th. Frank.
- Badges
- Science topic