[mgdenno]

Hi Jon,

Thanks for the input. I did as you suggested and set cAlpha = 0 and started the run. It takes a while to run, but I will post back when I know something.

I started the simulation back at 18 seconds where it was still running stable. does this seem reasonable? Or should I start it back at t=0?

Thanks again,

MD

[JonW]

Originally Posted by mgdenno

Hi Jon,

Thanks for the input. I did as you suggested and set cAlpha = 0 and started the run. It takes a while to run, but I will post back when I know something.

I started the simulation back at 18 seconds where it was still running stable. does this seem reasonable? Or should I start it back at t=0?

Thanks again,

MD

I would start from fresh, just in case. Start at t = 0 since we are trying to debug.

[JonW]

p.s. how long takes each simulation (up to break) and what computer do you have?
Jon

[mgdenno]

It is taking about an hour per second of simulation to run. I am running it on a virtual machine running kubuntu that has 4 2.3 Ghz CPU and 8 GB ram allocated to it. I am not sure of the specifics other than that, such as interconnect speed since they are vCPU...it is something I want to look into to see if it can be increased, etc.

[mgdenno]

Hi JonW,

I did as you suggested and started a new simulation run (t=0) and set cAlpha = 0. Unfortunately the simulation still blows-up (it is still running but deltaT is getting very small...it is only a matter of time now). However, a came across your post regarding cAlpha (here), and I think I am having the same problem with waves. It seems as though it is not what is causing it to blow-up, but it is still a problem. I was hoping the waves would go away if I could get it to run, but based on what you have experienced, I am now thinking maybe they are separate issues.

Did you ever solve your issue?

I think I will work play around with the fvSchemes and my mesh and try to get it to run without pulling away from the walls (picture in previous post).

Thanks,

MD

[JonW]

Originally Posted by mgdenno

Hi JonW,

I did as you suggested and started a new simulation run (t=0) and set cAlpha = 0. Unfortunately the simulation still blows-up (it is still running but deltaT is getting very small...it is only a matter of time now). However, a came across your post regarding cAlpha (here), and I think I am having the same problem with waves. It seems as though it is not what is causing it to blow-up, but it is still a problem. I was hoping the waves would go away if I could get it to run, but based on what you have experienced, I am now thinking maybe they are separate issues.

Did you ever solve your issue?

I think I will work play around with the fvSchemes and my mesh and try to get it to run without pulling away from the walls (picture in previous post).

Thanks,

MD

Ok, if cAlpha = 0, did not work then I am clueless.

Yes, the waves are a problem in interFoam, and also when I import STL surface with snappy (into a good basic mesh with no problems), then I can see small wave generations surrounding the STL. Also, even I have completed the simulation, the reconstructPar have died on me (which it did not when I excluded the STL). NOTE, everything was OK when I put cAlpha = 0 (but the simulation becomes fubar, as there is no interface compression). So something is not right with interFoam in terms of interface compression of the alpha equation

I have gone thoroughly into alphaEqn.C and alphaEqnSubCycle.C (if misspelled, then dont remember the name exactly), and I see no problems there (i.e. everything is correct, as far as I can see). So the question is if the problems is in MULES.H and MULES.C and how it treats the compression part of the alpha equation. I don't know

The only thing I can suggest is to remesh. Begin with something simple and then gradually increase the complexity of the mesh. I know this is time consuming, but I dont think there is a way around this.

P.s. If you are manly interested in steady state interFoam, then maybe this is for you
http://www.openfoam.com/version2.0.0/steady-vof.php

cheers
Jon

[MOHAMMAD67]

Dear Matthew
Hi
I simulate a stepped spillway without any interruption but the result is very strange. when the flow face the outlet it doesn't pass the outlet and turn back like facing on the wall.
I don't know how to correct it I searched alot especially I read this thread carefully but I couldn't understand what to do.
could you please help me?
Here are the main files.

[mgdenno]

Mohammad,

The download link is not working for me, I think it is blocked for me.

Based on what I am seeing in your picture though, I have the following thoughts:

1. Is it possible that what you are seeing is just a hydraulic jump?
2. If the outlet is really acting like a wall then I would guess that there is a problem with your velocity boundary condition. It should probably be either inletOutlet or zeroGradient.

Can you post your case to this forum? If it is too large maybe try removing all files except for the blockMeshDict from the constant/polyMesh directory and only include the original files from 0/ directory (the ones from before you ran setFields).

MD

[MOHAMMAD67]

Dear Matthew

Really thanks for your reply. I really need to my gods help through you to solve my problem . It's taken along time that i couldn't get a good result.
Files are attached. Could you please give me your email.
also I corrected the file and you can download.
BTW I'm using Salome 6.3 for meshing and geometry building. Also I use funkysetfields instead of setfield dictionary to patchthe second phase.

[olivierG]

hello,

Your BC are not correct, and i think also that your geometry either. (You should extend the outlet zone in your geometry, if this is the cas in reality)

For your BC:
* alpha seems ok, but inlet = 0.5 is a bit strange however, even if you use setFields. You may try zerogradient instead, or use groovyBC to set the level of your flow.
* U: ok
* p_rgh: all wall and inlet should be " buoyantPressure", not zeroGradient.
- outlet should not be a totalPressure like your upperwall (not consistent), but try zeroGradient here. But if your upperwall is a wall, then -> buoyantPressure, and outlet: totalPressure.
* k,epsilon: try zeroGradient for the upperwall (if this is a free atmosphere. In case this is a wall, then ok)
* nut: wall = nut wall function ok, all other (inlet/outlet/top: calculated).

hope this help,

regards,
olivier

[MOHAMMAD67]

Hi Oliver
Thanks for your comments. I'll implement changes and report the results.
Regard

[MOHAMMAD67]

Dear Oliver
I did all things except extending the domain. Unfortunately it didn't work and after 1.3 seconds it blows out. I don't know how deal with. I reduced the delta T to 0.00001 and turn the adjustable time step off. It is running now. I will inform you from the result.
Maybe I should make the mesh finer. Whats your opinion. Does it help me to get result.
Kind Regard

[mgdenno]

Mohammad,

I agree with what Oliver has said. Let us know how it goes.

Oliver,

You mentioned using groovyBC to control the water level at the inlet. I posted a question about this sometime ago and never got an answer on how to accomplish it. I normally specify and inlet patch and set alpha=1. Do you have a simple working example of how to do this? I have never used groovyBC but if it can be used to do this I may have to give-it-a-go.

MD

[mgdenno]

Mohammad,

Have you run checkMesh on your mesh? That should give some idea if you have mesh problem. Do you have a picture showing your mesh (maybe a slice through your domain)?

MD

[olivierG]

hello,
mgdenno:
Take a look at the openfoamwiki about groovyBC, you will see some exemple (like the groovyWaveTank). And if you look in the svn repo, you will see some test case.
In short, you can set a z level like (pos().z<1 ? 0 : 1) In this case, you set alpha=0 if z<1, and 1 if z>= 1.

Mohammad:
You may try LTSInterFoam for your case, if your solution are steady state. It will be much faster. And yes, mesh is allways important, and with interFoam even more because interfacecompression is done over ~ 2 cel.

regards,
olivier

[mgdenno]

Thanks Oliver. I think I will dive into goovyBC this weekend.

[MOHAMMAD67]

Dear friends
Hi
I make the mesh finner but It didn't work . Unfortunately all the simulation has been blown out between 0.9 to 1.3 seconds.

Mattew
Could you please tell me how did you choose initial condition for k and epsilon? Is it possible to upload the 0 folder of your simulation? Did you change that folder uploaded in the first post of this thread?
secondly How did you mesh your model. I used netgen3d hypothesis with max. size of element 0.04.
I'm really confused about that!! Unfortunately I don't have access to HPC and wrong simulation really waste my time but I'm grateful because it helped me to learn a lot of new things about openfoam.

[mgdenno]

Mohammad,

Did you run checkMesh on your mesh? This program will check your mesh for problems. I would do this next.

I have used GMesh, snappyHexMesh and blockMesh to generate my meshes. The ones in the pictures at the beginning of this post were made with snappyHexMesh and an STL file. You should probably take an incremental approach if you are just starting out. Maybe, start with a simple 2D geometry from blockMesh, which will also run much faster so you can try more things in a shorter time. Gradually make your geometry more complex.

Regarding k and epsilon, I think if you are having trouble, and suspect that your turbulence may be the problem, you should try to run a laminar simulation first, then you won't have to worry about your turbulence properties.

MD

[The King]

I has probolems with my pressure outlet as well, but it is a little different 2D case. When I used:

out
{
type totalPressure;
p0 uniform 0;
U U;
phi phi;
rho rho;
psi none;
gamma 1;
value uniform 0;
}

it started to work fine. However, I has to change my fvsolutions file with a reference point and value:

PISO
{
momentumPredictor no;
nCorrectors 3;
nNonOrthogonalCorrectors 0;
nAlphaCorr 1;
nAlphaSubCycles 4;
cAlpha 2;
pRefPoint (0.0 0.018 0.0);
pRefValue 1e5;

}

Good luck!

[ardjouna]

Hi Mathiew,

I Start with OpenFoam and have the same case labyrinth spillway and hope some help I start with dam break tutorial but have some troubles (when running rasInterFoam error message say this application not valable )

Thank you for your reply and best regards