pimpleDyMfoam simulation keeps blowing up
1 Attachment(s)
Hi all;
I'm running a pimpleDyMFoam simulation and it keeps blowing up. Even reducing the time step down to 1e-5 does not solve the problem. Code:
Courant Number mean: 5.46684e+95 max: 8.98336e+97 Any help would be greatly appreciated. |
Hi
I would suggest doing the following until it stops blowing up. Change to upwind on U. And relax the components by 0.5. If it stops blowing up you can then try to switch to higher order schemes and decrease the relaxation. |
Thank you Linnemann.
Relax the components by 0.5 means that I need this in my fvSolutions: Code:
relaxationFactors About the rest, what do you mean with change to upwind on U and switch to hig order schemes? Thank you again for your help! |
yes
relaxationFactors { "(p|U|k|epsilon).*" 0.5; } in fvSolutions and div(phi,U) Gauss upwind;// in fvSchemes you are using linearUpwind which is a higher order scheme and thus inherently more unstable. |
Thank you linnemann, unfortunately had no luck with your tips…
First of all I increased the time step from 1e-5 to 1e-4 and my simulation blew up at time 0.0266. So I changed this line I had in my fvSolution: Code:
"(U|k|epsilon).*" 1; Code:
"(p|U|k|omega).*" 1; So I changed the line to this: Code:
"(p|U|k|omega).*" 0.5; So I changed these lines in my fvSchemes: Code:
divSchemes Code:
divSchemes At this time I moved back to a time step of 1e-5 to reduce the Courant Number but the simulation blew up at 0.026… What do you think? Thank again. |
2 Attachment(s)
Try with transientSimpleDyMFoam
with this fvSolution file. |
Thank you. Do I need to compile it?
|
Yes you have to
|
Thank you!
I'll see what I can do! |
By the way, what's the difference between this and the one that comes with openFoam?
|
Actually, my geometry is quite a simple one: just a 2D cube… How comes it cannot be solved? I mean, what can you solve with the original pimpleDyMFoam then?
|
Hi
If it is that simple I suggest you upload it so we can have a look at your setup. If its too big to fit here use Dropbox with a public link or a similar file sharing method. |
1 Attachment(s)
Thank you linnemann.
Here's my case. Regards |
Quote:
|
Greetings to all!
In case Linnemann doesn't see the question about the differences between the two solvers, here's what I know:
Best regards, Bruno |
just a thought... you know your running an incompressible solver and your using a reference pressure of 1atm
Code:
pRefPoint (0.1 0.1 -0.005); |
Hi lovecraft
Had a look at your case and it looks like you haven't (not to be rude) understood the setup involving rotating stuff. If you follow the tutorial /tutorials/incompressible/pimpleDyMFoam/mixerVesselAMI2D I think you will get a better understanding of the whole setup involving rotating parts. Back to your case. I had to split it up into two meshes and then merge them back together and attach them using AMI's. You cant have a moving mesh where you only have one mesh and a zone. If you want to do it this way you should use the steady MRF approach. Also a lot of your BC's where wrong for such a case. Here is a nice little animation of it running. http://dl.dropbox.com/u/15968063/output.avi and also a link to the case that works. http://dl.dropbox.com/u/15968063/cubo.tar.gz And to follow up on the difference transientSimpleDyMFoam has some hard-coded stuff that makes it more stable, but it should be able to tweak pimpleDyMFoam to have a similar stability. |
Thank you a lot linnemann, that's really great! I'll have a look at the setup tomorrow. Could you also explain me what commands you ran?
Thanks again! |
I did some digging around and also looking at the case you uploaded I think I understood this:
1. You need to create an interface between the rotating and the stationary meshes. In my case it was a cylinder. This is the AMI (Arbitrary - btw, why "arbitrary??" - Mesh Interface); 2. You need to mesh the two regions separately, making sure you have the same cell dimensions on the AMI; 3. Merge the two meshes using mergeMesh on the running case and then run it. I'll dig deeply on the propeller tutorial tomorrow. What I did wrong (and I'm sorry for having posted here and on another discussion my wrong conclusions about that…) was that I only set the rotating region as a zone. This is what I usually do for the MRF and, at this point, I hope that at least is correct… Looking forward to try an run it as I'm getting really excited about that! Anyway thanks anybody for you help and sorry for my mistakes… |
@linnemann @lore
http://dl.dropbox.com/u/70019943/roCube.tar.gz Hello linnemann, appreciate your effort on pimpleDyFoam above. plz find my case folder with implementation of rotating cube. * I have only done the meshing of rotor stator inside rocube/Mesh folder. * the next step would be to merge rotor-Mesh and stator-Mesh!!! How to go about it? Note: Still the case is not fully modeled, so most of the BC files are missing. |
All times are GMT -4. The time now is 06:53. |