# Laminar Circular pipe flow problem

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Display Modes
 September 12, 2011, 12:38 Laminar Circular pipe flow problem #1 New Member   Gavin Lee Join Date: Jul 2011 Location: Canada Posts: 4 Rep Power: 7 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

 September 12, 2011, 15:17 #2 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,285 Blog Entries: 6 Rep Power: 43 can you give details about mesh independence study, yplus values, turbulence model and boundary conditions?

 September 12, 2011, 15:29 #3 New Member   Gavin Lee Join Date: Jul 2011 Location: Canada Posts: 4 Rep Power: 7 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.

September 12, 2011, 19:28
#4
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,638
Rep Power: 98
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.

 September 13, 2011, 13:50 #5 New Member   Gavin Lee Join Date: Jul 2011 Location: Canada Posts: 4 Rep Power: 7 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.

 September 13, 2011, 15:51 #6 Super Moderator   Sijal Join Date: Mar 2009 Location: Islamabad Posts: 4,285 Blog Entries: 6 Rep Power: 43 Glenn is right about the yplus, as it is meaningless to laminar flows

 September 15, 2011, 10:57 #7 New Member   Gavin Lee Join Date: Jul 2011 Location: Canada Posts: 4 Rep Power: 7 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Quarkz Main CFD Forum 6 October 7, 2015 12:24 alireza.glz OpenFOAM 2 July 26, 2011 08:56 alquimista OpenFOAM Running, Solving & CFD 1 April 24, 2010 10:50 pertupd ANSYS 0 August 12, 2009 08:36 kjetil OpenFOAM Running, Solving & CFD 3 July 21, 2009 09:15

All times are GMT -4. The time now is 18:34.

 Contact Us - CFD Online - Top