pimpleFoam Simulation aroud a cylinder does not converges
Hi all,
I'm trying to learn how to use pimpleFoam. In order to do this I'm trying to simulate the flow around a cylinder, I'm doing this at high Reynolds (7.10^6) because I will have to make simulations at this Reynolds. I read this about pimpleFoam : http://www.cfd-online.com/Forums/blo...hm-part-i.html http://www.cfd-online.com/Forums/blo...m-part-ii.html At all of the timesteps, the simulation did not converged after 50 pimple iterations (nOuterCorrectors = 50). It seems to be an easy simulation (flow around a cylinder). Can you tell me what is wrong in my simulation .. Thanks for answers !! An extract of the log.pimpleFoam file (first part of the file and a part of the last timestep): Code:
/*---------------------------------------------------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ Code:
/*--------------------------------*- C++ -*----------------------------------*\ |
Hi,
You can probably use higher relaxation factors in your inner iterations: Code:
relaxationFactors There may however be something wrong with your boundary conditions or mesh as well. |
Thanks for the answer !!
As you thought with higher relaxation factors it does not converge. Does anyone have an idea about something that could be bad with my mesh or other ?? |
Hi,
As usual, please post: 1. checkMesh output 2. Your initial and boundary conditions (or just an archive of 0 folder) 3. And finally geometry of your problem (or a screenshot of the mesh), as several times on this forum people thought they are simulating flow around cylinder and yet they were not. |
4 Attachment(s)
Thanks for answer :
Here are the information you ask me. There is :
If you need more information tell me !! The log.checkMesh file : Code:
/*---------------------------------------------------------------------------*\ |
Change the boundary condition for pressure on your inlet to zeroGradient. I generally do not use the freestream boundary types, but I guess they could be used. I do believe there is also a freestreampressure boundary condition, that one may also work.
Regards, Tom |
Hi,
Agree with tomf about BC for pressure. You impose inlet velocity and no pressure gradient along the channel. It is a little bit strange, no? Mesh seems to be OK (hope inlet is really inlet and outlet is really outlet), though usually people make it denser not only around cylinder but also near the center of the channel. |
Thanks for answers :
I'm confused about pressure boundary conditions: If I want to simulate my the cylinder in a total free flow (not in a channel), should I use zeroGradient for all of the boundaries (even for inlet and oulet) ?? |
Well your setup inevitably results in a channel-like flow. If you want (almost) freestream conditions I would suggest this setup:
Increase the height of your domain and prescribe your freestream conditions on the top and bottom boundaries as if they were inlets: fixedValue for velocity and turbulence, zeroGradient for pressure. For the outlet set a fixedValue pressure (0) and zeroGradient for all other variables. Otherwise look at the setup for the case: $FOAM_TUTORIALS/incompressible/simpleFoam/airFoil2D That one uses a setup with freestream boundary conditions. Regards, Tom |
Ok thanks for the details about boundary conditions.
I'e seen the airfoilD tutorial but it is a 2D simulation, I would like to do this in 3D but I don't know what boundary condition to use for the frontAndBack patches. I will try the first solution you gave me. |
Quote:
For 3D I would use slip on the frontAndBack patches for velocity, calculated for nut and zeroGradient for all others. If you have a finite length of your cylinder and want to include end effects you could make these freestream as well, but I think you should decide that for yourself after thinking about what it is exactly that you want to simulate. |
1 Attachment(s)
One more thanks for answer
Quote:
Quote:
I'm still trying to set freestream boundary conditions when I'm using those parameters I've got an error about field p. I join the 0 folder. Here is an extract of the log.pimpleFoam with the error message : Code:
[16] |
This means you need something like this in your system/fvSolution (the bold font part) but than in the PIMPLE subDict. Instead of pRefCell you can also use pRefPoint (search the forum for explanations). I took this from the airfoil2D tutorial.
Code:
SIMPLE |
All times are GMT -4. The time now is 02:35. |