Original Question

I am familiarising myself with OpenFOAM and want to run a simple pipe flow case.

Schematic of the test case

I would like to be able to compare my computational pipe-flow results to a well established case (like the lid-driven cavity flow or Ahmed's body): given certain $L,\,D,\,v_{1},\,p_{2}$ (atmosphere) and $\mu,\,\rho$ of the fluid, what ${\bf U}$ and ${\bf p}$ fields would I expect to get. There seems to be little (1, 2) information online; especially with a clear definition of inputs and the expected output.


I have set up a case in OpenFOAM using:

  • $D=0.0008 \, m$
  • $L=0.02 \, m$
  • $v=0.1 \, m/s$
  • $p_{2}=0 Pa$
  • $\mu=0.001 \, N \, s/m^2$ (in OpenFOAM one enters the kinematic viscosity $\nu=0.000001 \, m^{2}/s$)

The solver gives me a solution of $p_{1}=0.1 \, Pa$.

The $Re=\frac{\rho v D}{\mu}=80$ (the flow is laminar), so (as mentioned by @Bill) I can use the Hagen-Poiseuille equation $dp=\frac{128 \mu L v A}{\pi D^4}$. It gives me a predicted $p_{1}=100 \, Pa$ -- 1000 times higher than the simulation result. The value seems to be correct, but there is a problem with the magnitude, but I can't spot where the mixup is occurring. As far as I know OpenFOAM is operating in SI.

Below is the screenshot of the pressure distribution in the pipe. enter image description here

  • 2
    $\begingroup$ For Reynolds numbers below transition, this problem has an analytical solution for certain inflow and outflow boundary conditions. What Re are you planning to study, and what are the inflow and outflow conditions that interest you? $\endgroup$
    – Bill Barth
    Feb 13, 2014 at 17:26
  • $\begingroup$ Any $Re$ would do -- I want to check that the solver works, that I am setting the case correctly. Although the real life equivalent of this I would be interested in would likely be laminar due to small $D$. Analytic or experimental, I am just looking for something to use as a benchmark. $\endgroup$ Feb 14, 2014 at 12:21
  • $\begingroup$ Well, you should be able to setup a case that gives you Poiseuille flow pretty easily. $\endgroup$
    – Bill Barth
    Feb 14, 2014 at 12:54
  • $\begingroup$ Yes, OpenFOAM operates in SI. Is your solution steady state? Did it converge (and is the velocity profile parabolic)? Is the development length of the flow much shorter than your pipe? $\endgroup$
    – akid
    Apr 23, 2014 at 13:51
  • $\begingroup$ That factor 1000 is about the density of water, are you sure haven't forgotten $\rho$ somewhere? $\endgroup$
    – chris
    Nov 7, 2014 at 7:24

1 Answer 1


As it was discussed in the comments, the fluid density is most likely the culprit. If you are using an incompressible solver, such as icoFoam, simpleFoam or pimpleFoam, then no density is used. If you take a look at the source code of the said solvers, you will find no reference to any density. Also, in the case set-up, the pressure field will have the dimension of pressure divided by density.

OpenFOAM operates on a need-to-know basis, it reads the information it needs from the case files, all other content of the case files in ignored. So, even if you specify a density in the transportProperties, an incompressible solver will always solve the equations of fluid motion, which are divided by density.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.