CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

Advice needed - laplacian pressure drop in gas-liquid flow

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   August 18, 2017, 08:03
Default Advice needed - laplacian pressure drop in gas-liquid flow
  #1
New Member
 
Join Date: Nov 2016
Posts: 5
Rep Power: 9
Simsey is on a distinguished road
Hello everybody,

I am trying to model the laplacian pressure drop in a vertical y-junction mini-channel with gas-liquid flow. Basically I try to verify that I am able to simulate the correct laplacian pressure before moving to a more complex model.

The numbers (pressure [Pa]) which my model generates are far behind the pressure I would expect. If the pressure drop dp is calculated by dp=pressure(inside)-pressure(outside) I observe ~80 Pa instead of 292 Pa (for a 1mm channel diameter; surface tension = 0.073 N/m; contact angle=0°). So there must be something fundamentally wrong in my setup.

The theoretical dp of 292 Pa is calculated by: 2*0.073/0.0005*cos(0)

I tried it with different mesh qualities (~400k tet mesh right now), a hex mesh and a more tightly convergence (1e-5) but my best result is ~135 Pa for dp.

If anyone could give me an advice how to match the theoretical pressure drop or dig in the correct direction I would be very thankful.

Thanks in advance

Simsey
Attached Images
File Type: jpg solver_manager1.jpg (158.4 KB, 6 views)
File Type: jpg solver_manager2.jpg (167.9 KB, 6 views)
File Type: jpg 2794_full.jpg (52.5 KB, 5 views)

Last edited by Simsey; August 23, 2017 at 07:40.
Simsey is offline   Reply With Quote

Old   August 20, 2017, 11:24
Default
  #2
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 731
Rep Power: 25
siw will become famous soon enough
What is going on with the surface mesh on the cicruclar face in the last picture? There is not clearly shown evenly sized surface triangles from the volume tetrahedrons, is there a section plane there?
siw is offline   Reply With Quote

Old   August 20, 2017, 15:02
Default
  #3
New Member
 
Join Date: Nov 2016
Posts: 5
Rep Power: 9
Simsey is on a distinguished road
Hey,
yes there is a section plane to show the mesh quality as I am unsure if my "uncertainty" is connected to the mesh or my setup.

Normally the mesh looks like the attached images.. The 1st image shows the full mesh, the 2nd image shows the mesh with removed inlets. I'm constantly trying different things to improve my results, therefore it looks a bit different now.
Attached Images
File Type: jpg mesh.jpg (87.2 KB, 6 views)
File Type: jpg mesh with removed inlets.jpg (82.9 KB, 9 views)
Simsey is offline   Reply With Quote

Old   August 20, 2017, 19:37
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,665
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I recommend you try to model a drop in free space with surface tension as a basic model to develop a method which can predict laplacian pressures accurately. In my experience, if you want accurate laplacian pressures you must use hex meshes (tets will not be accurate enough) and you must have a maximum aspect ratio less than about 1.2. This is an extremely high quality mesh, and far more restrictive than the mesh requirement for other CFD models.

Secondly: If the contact line is moving on a wall boundary then you will come across the moving contact line problem (http://www.sciencedirect.com/science...95034915303160). You will find that the motion of a moving contact line on a wall boundary and the laplacian pressures it generates do not converge with mesh refinement. This is due to a fundamental paradox in the Navier-Stokes equations. This means no Navier Stokes solver is going to give you good results for this type of flow
ghorrocks is offline   Reply With Quote

Reply

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Pressure drop in pipe flow with Large Eddy Simulation xerox FLUENT 1 October 16, 2019 09:55
Sudden pressure drop - Multiphase Flow koscfd OpenFOAM Running, Solving & CFD 3 August 25, 2016 09:22
Guessing the static pressure needed to produce flow rate jpo FLUENT 0 June 22, 2009 13:53
Advice on multi-phase flow modelling Martin Main CFD Forum 3 October 14, 2008 06:16
Total pressure in real gas (compressible flow) Bart Prast Main CFD Forum 3 November 14, 2000 11:44


All times are GMT -4. The time now is 07:54.