[Daniel L]

Dear FLOW 3D users,

I need to calculate the pressure drop in a pipe-fitting (90° bend), but my simulation produces a large pressure drop:
In the pipe before and after the bend the pressure drop is ~50% above the theoretical calculated pressure drop (turbulent flow), and the pressure drop in the bend is way too large (+80% ).

here are the settings I used for the simulation:
Rectangular blocks, with ~20-35 cells/D (because of the 90° bend I can't use the cylindrical blocks)
Pressure solver: GMRES (I also tried imp=1)
Turbulent model: RNG (I also tried the k-epsilon model)
frcof = -1 (no relevant differences by changing this value)
Momentum advection: second order monotonicity preserving

Thanks you for your help,
Daniel

[JBurnham]

Daniel - It's most likely that you're seeing mesh-dependency for the near-wall turbulence treatment (log-law-of-the-wall). Search at www.flow3d.com for 'turbulence' to find technical notes on the turbulence models. TN-86 ("On the Implementation of 2-Equation Turbulence Models..." describes the mesh-dependency. For large-scale simulations, the error introduced near the wall is negligible, but for pipe flow where frictional drag losses are important, the error can be significant (as you've seen).

You can solve the problem either by running a series of mesh-dependency simulations and looking for the 'not-too-big, not-too-small' range of cell sizes where the losses level off (see Fig. 6 in TN-86 for an example), or alternatively, you can manually estimate a good cell size as a function of a suitable dimensionless normal distance y+, which, again, is described in the Technical Note.

[Daniel L]

Hi Jeff, thanks for you reply.
I followed the the instructions on TN-86 and I get much better results for the pressure drop in the pipe.