CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Laminar Circular pipe flow problem (http://www.cfd-online.com/Forums/cfx/92366-laminar-circular-pipe-flow-problem.html)

GLee September 12, 2011 12:38

Laminar Circular pipe flow problem
 
I'm running some simulations on laminar pipe flow at Reynolds number of 200 and 500 with a pipe radius of 0.01m. When I ran the simulations with 1m long pipe length, the residuals converged. When extending the pipe to 2m (scaled in the x direction using ICEM) the residuals show a transient behaviour.

I will check if there is something wrong with the grid but I was wondering if anyone has experienced this phenomena.

Thanks

Far September 12, 2011 15:17

can you give details about mesh independence study, yplus values, turbulence model and boundary conditions?

GLee September 12, 2011 15:29

Currently I am looking at the laminar case so no turbulence at the moment (although I haven't observed this problem when running in the turbulent regime).

The mesh is made using ICEM and the cross sectional area is meshed with an O-grid. The grids I have currently extended have a wall spacing of 0.00015 and 0.0001 (m), I can check yplus values later if that will be helpful. The first three grids used have 395K, 785k and 1.07mil nodes and have all run fine when the length is at 1m but behave quite differently when stretched to 2m.

The current boundary conditions are run at steady state, isothermal (25C), laminar with a specified inlet velocity (0.1546m/s or 0.3865m/s). The outlet is taken as an average static pressure over the whole outlet to atmospheric and the walls have a no slip boundary condition.

I swapped out the mesh files in pre for the longer grid and the odd behaviour is observed. Additional information on the simulation can be supplied if required.

ghorrocks September 12, 2011 19:28

Quote:

I can check yplus values later if that will be helpful.
y+ is meaningless for laminar flows. You check you have adequate wall resolution by doing a mesh sensitivity study.

It appears your simulation is very mesh quality sensitive. Try running double precision. Also, rather than stretching your mesh glue two domains together. This will double the number of elements but keep the quality the same.

GLee September 13, 2011 13:50

Thanks for the suggestions. I ran a simulation with the same grid spacing axially and the residuals converged but the RMS pressure and momentum residuals were higher. I have not tried running double precision but may explore that option if I have the time.

I have done mesh refinement but I did not expect the axial spacing to be so sensitive.

One curious problem during the simulation with the extended length (same axial spacing as the original mesh) was that the notice "A wall has been placed at portion(s) of an OUTLET boundary condition..." with a maximum of 8.4% of the faces and 6.2% of the area. I understand that this should not be a concern if the area is small but I recall this being an indication of back flow at the outlet, which makes little sense to me for laminar pipe flow.

Edit: Upon inspection, the velocity contours parallel to the inlet plane are no longer symmetrical and I will examine if something is wrong with the mesh or setup.

Far September 13, 2011 15:51

Glenn is right about the yplus, as it is meaningless to laminar flows

GLee September 15, 2011 10:57

With the new grid created in ICEM with the same quality, the simulation converged normally. From what it seems, there may have been some error when creating the mesh file with scaling in the axial direction (x) although it is hard to pinpoint why at the moment.

Thanks for the input


All times are GMT -4. The time now is 10:13.