[joegi.geo]

Hi,

I wonder if somebody else is experiencing this, I am having an strange stair-step behavior on the pressure when using rhopimplefoam and I don’t manage to pinpoint the reason of this.

The case consists of a simple straight pipe (Poiseuille case, so we have an analytical solution). I am computing the solution using icoFoam, pimpleFoam, and rhoPimpleFoam for the same mesh, physical properties, and same boundary conditions. The peak velocity is about 2.8 m/s, so I expect rhoPimpleFoam to yield to the same results as those of the incompressible solvers. While the velocity is pretty much the same, the pressure along the pipe axis of rhoPimpleFoam shows a stair-step (wiggles) behavior, whereas the pressure reported by the incompressible solvers has a smooth behavior (as expected and desired). At this point, I wonder if you have seen this behavior.

I have used many different numerical schemes and I always see the same behavior. Using finer meshes did not yield to better results.

By the way, I see the same behavior using the Heat transfer and buoyancy-driven flows solvers.


To reproduce the results:

Download the case file and go to rp5:

blockMesh -dict system/blockMeshDict

rhoPimpleFoam

sample -latestTime


Then go to pimple:

blockMesh

pimpleFoam

sample -latestTime


Then compare the solutions for both cases (pressure).


In figure 1 it is plot a comparison between icofoam and rhopimplefoam. In figure 4 it is plot a compariosn between fluent a openfoam. The numerical setup, mesh, bc and ic are identical in fluent.

[tomf]

Hi this is probably related to the setting for the writePrecision in your controlDict. If you change this to 12 instead of 6 you will loose the wiggles I assume.

Or you could use binary instead of ascii.

Regards,
Tom

[joegi.geo]

Hi Tom,

Thank you for point that out.

This is the second time that this bites me with totally different solvers.

FYI, SnappyHexMesh is also sensitive to this issue.

Now I wonder why do they give the double precision version, and do not save the solution using all the significant digits (as default option).

Have a good one,

jg

[tomf]

Hi

If you are referring to the tutorials as "default option" I would say that I never consider the tutorials as anything else than example cases showing the general working of a solver and the information that is needed. You should check any option they use and see if it fits your purpose and you would get a "best practice" for that solver, after all many tutorials use upwind for many terms in fvSchemes, which should not be used in production runs!

Kind regards,
Tom