[shanleyk]

Hello -

I have considerable experience with CFD, but I’m brand new to OpenFOAM. I was able to work my way through the lid driven cavity flow and dam breaking tutorials without really any issues. However, now I am branching off on my own and having some difficulty.


I am trying to start out easy. I am simulating 2D flow between parallel plates. The flow is steady and Re is very low ~0.001 (creeping/Stokes flow). After some research I decided to use simpleFoam. It runs well and convergence looks good. Qualitatively the results look good when I view in paraFoam. However, the pressure drop does not obey the cubic law. The pressure drop across the domain should vary with the cube of the height. It does not. In fact it seems to vary linearly.


I have some more complicated fracture flows to look at, so I want to make sure I am doing this correctly.


Is simpleFoam not the best solver for this application?
Have I set it up incorrectly?
I am using OF 2.2.



I have uploaded a tarball case setup. Included in there is also the log from a run so you can see residuals. You will have to run blockMesh to generate the mesh.



Thank you for any assistance.


Kevin

[wyldckat]

Greetings Kevin and welcome to the forum!

I've kept a reminder to check this thread when I had the time and today I finally managed to look into this.

So, the issues I can figure out are as follows (I'm referring to a pipe, since it's somewhat similar and easier to write than "parallel plates" ):

• The pressure drop along the pipe's length is meant to be constant, so there was no problem there.
• The "fvSolution" was configured to have a very tight "tolerance" values in the "solvers" block. I lighten from 1e-17 to 1e-6 and it would run a lot faster
• The "divSchemes" in "fvSchemes" are mostly using "upwind". Switching to "linear" should improve the resulting solution.
• The mesh resolution along the pipe length and diameter is out of proportion. This wouldn't be much of a problem if you were only trying to assess how the flow goes along the pipe. But from what I can see, perhaps you also need more resolution along the diameter, since you're looking for a cubic relation between distance to the walls and pressure variation.

I changed the mesh resolution from "10 1 10000" to "100 1 1000". The results seem mostly the same, but at least the flow speed profile looks more refined.


Problem is that I can't figure out where exactly you're looking for a cubic profile for the pressure. The results I get with these improvements indicates that:

• the pressure is constant at each cross-section of the pipe, i.e. for a fixed X position I get a constant pressure along the diameter;
• the pressure drop is constant, which is in accordance with the analytical solution;
• the flow speed (velocity) profile in the same cross-section does have a parabolic shape which doesn't seem to be quadratic.

Can you provide more details on the simulation you're trying to do and the analytical reference data you're looking at? Because perhaps there was something lost in the translation to the OpenFOAM case, such as whether the two planes should be at the same pressure or perhaps some sort of friction should be present at the walls?

Best regards,
Bruno

[shanleyk]

Wyldckat,
Thank you very much. I had forgotten that I had posted this.
We got our case running. I don't remember all of the details, but mesh was an issue and a few other things.
The cubic law relationship I was looking for is that (aperture height)^3 should be related to pressure drop along the channel. We were able to show this with simpleFoam. We've moved on to more complex geometries and getting nice results.
Thanks!

[bagherij]

Dear
i use u file for creeping flow around cylnder between to plate.
i want to calculate the magnitude of shear rate tensor(|tau|) which
defined by
tau = -nu()*(fvc::grad(U)+(fvc::grad(U)).T());
|tau|=sqrt(1/2tr(tau^2)

where "nu()" is the dynamic viscosity of the system

where should i add to code ,and how can i get |tau| and compare it with some parameter.
Thanks