|
[Sponsors] |
The initial transient part of the solution takes too long to fade |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
January 23, 2023, 11:17 |
The initial transient part of the solution takes too long to fade
|
#1 |
Member
Ashkan Kashani
Join Date: Apr 2016
Posts: 46
Rep Power: 10 |
Hi all,
I'm doing a series of 2D transient simulations of separated and reattached flow past a sharp-edged rectangular body. According to previous recommendations on this forum, I opted to set an adaptive timestep based on a target minimum/maximum number of coefficient loops to ensure a proper temporal resolution, which leads to very small timesteps in my simulation. Despite initializing the simulation using a relevant solution previously obtained, the initial transient part of the solution appears to take a very long simulation time to fade, considering the small timesteps imposed by the adaptive timestepping. This is unfortunately beyond the computational resources available to me. I'm wondering what could be done to reach the stationary solution faster since I'm not interested in the initial transient part. Is it reasonable to manually choose a much bigger timestep? I appreciate any comments. |
|
January 23, 2023, 16:46 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
Yes, you can use a bigger time step. Returning to a smaller time step to fully resolve the flow will then result in a new transient which you will have to wait for it to fade out, but as long as you carefully choose the bigger time step it should be manageable.
Another alternative is you could use 1st order time differencing for a while. That will have extra dissipation and mean you will not have to change the time step as much.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|
January 28, 2023, 14:08 |
|
#3 |
Member
Ashkan Kashani
Join Date: Apr 2016
Posts: 46
Rep Power: 10 |
Thank you for your comment. I would also appreciate any comments on the following.
1- Among the options for adaptive timestep setting in CFX, homing on 3 to 5 loops has been mostly recommended on this forum. I'm wondering about the physical explanation behind such a setting and also wondering why it's said that setting the timestep based on max/rms courant number is not as useful. 2- Regarding my simulation objective (time-averaged flow past a sharp-edge rectangular body), i think the timestep based on 3 to 5 loops leads to a very conservative time marching, probably picking on very slowly-evolving structures that delay statistically converged flow and are also insignificant in the time-averaged field. Could this be true? 3- According to the literature and my personal understanding, the best practice is to choose a timestep based on the range of Strouhal numbers known from previous works. This is done by sweeping each cycle of vortex shedding (corresponding to the dominant frequency) through a number of timesteps, let's say n. What is an appropriate value for n. Well, i couldn't find any consensus on this matter in the literature. I understand that this should be really determined through a sensitivity analysis. But since i can't afford the computational costs, i'm hoping there's a reasonable empirical choice to go with. |
|
January 28, 2023, 18:52 |
|
#4 | ||||
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,830
Rep Power: 144 |
Some astute questions there.
Quote:
Through experience (both mine and that of ANSYS) it has been found that almost always when you are using 3-5 coeff loops per iteration you also have an accurately time resolved simulation. If you actually want to prove your time accuracy you should do a sensitivity check, but for most purposes if you have 3-5 coeff loops per iteration that is good enough and means you can be confident you are adequately time resolved with having the hassle of doing the sensitivity check. Quote:
Quote:
But do not fall into the mistake of thinking that a simulation which is not fully time resolved and therefore blurrs out some of the smaller transient features is the same as the time averaged result. This is not correct! A not fully time resolved simulation has an uncontrolled error of some size in it, and the time averaged result is the time average of a fully accurate time resolved simulation. They are not equivalent. Quote:
But repeating my previous point, do not assume that a transient simulation which does not properly resolve the time scales is equivalent to the time-averaged flow.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum. |
|||||
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
[solidMechanics] Support thread for "Solid Mechanics Solvers added to OpenFOAM Extend" | bigphil | OpenFOAM CC Toolkits for Fluid-Structure Interaction | 686 | December 22, 2022 09:10 |
Maximum number of iterations exceeded chtmultiregionsimpleFoam | Moncef | OpenFOAM Running, Solving & CFD | 28 | July 13, 2020 14:26 |
pressure in incompressible solvers e.g. simpleFoam | chrizzl | OpenFOAM Running, Solving & CFD | 13 | March 28, 2017 05:49 |
Cannot run the code properly: very large time step continuity error | crst15 | OpenFOAM Running, Solving & CFD | 9 | December 14, 2014 18:17 |
[snappyHexMesh] crash sHM | H25E | OpenFOAM Meshing & Mesh Conversion | 11 | November 10, 2014 11:27 |