CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

Very high or negative pressures

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 23, 2009, 16:42
Default Very high or negative pressures
  #1
jpo
Member
 
Join Date: Apr 2009
Posts: 93
Rep Power: 9
jpo is on a distinguished road
Dear All,

I am modeling a pipe with dynamic mesh. One end is a piston, the other end is an outlet/outflow.

Case setup: k-epsilon incompressible: air density = 2.33 kg/m^3 = constant.
Operating pressure = 265kPa at piston; also tried 0 Pa.
I tried the open pipe end as outlet as well as outflow.

The first step of the motion ends always with wrong static pressures. Next to piston they are very high (>1E+6). If the open end is an outflow, then the pressure there becomes negative.

Please help me correct the errors in this case.
jpo is offline   Reply With Quote

Old   July 24, 2009, 01:33
Default
  #2
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,125
Rep Power: 32
-mAx- will become famous soon enough
*switch to pressure-outlet
*check your units (scale)
*what kind of method are you using for moving mesh (layering/remeshing/...)
display the grid while plotting the pressure, and check if the high pressures aren't linked with bad cells
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 24, 2009, 11:26
Default
  #3
jpo
Member
 
Join Date: Apr 2009
Posts: 93
Rep Power: 9
jpo is on a distinguished road
Hello mAx,

thank you for your time.

* switched to pressure outlet, still calculated static/absolute pressure at piston is > 1E+7
* my pressure unit is Pa
* I am using layering, it is a hex mesh on a rectangular pipe
* equiangle/equivolume skew is < 0.2
jpo is offline   Reply With Quote

Old   July 24, 2009, 12:19
Default
  #4
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,125
Rep Power: 32
-mAx- will become famous soon enough
*check the scale: grid/scale
*how fast is your piston moving?
*do you see any discontinuity in the fluid domain (display pressure)?
*does the fluid flows out?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 24, 2009, 13:49
Default
  #5
jpo
Member
 
Join Date: Apr 2009
Posts: 93
Rep Power: 9
jpo is on a distinguished road
* grid/scale: all scales = 1, unit = [meter]
* piston moves with 32 m/s
* no discontinuity: pressure is 265kPa at outlet and grows smoothly to 5E+7 at piston
* mass flux at outlet converged to -8.5kg/s
Pipe/duct has rectangular cross section, 0.3m x 0.1m, length ~20m
jpo is offline   Reply With Quote

Old   July 24, 2009, 14:00
Default
  #6
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,125
Rep Power: 32
-mAx- will become famous soon enough
post a picture with pressure and grid.
did you check the mesh motion?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 24, 2009, 14:14
Default
  #7
jpo
Member
 
Join Date: Apr 2009
Posts: 93
Rep Power: 9
jpo is on a distinguished road
Yes, the mesh motion is fine.

If the time step is dt=1E-4, mass flux at outlet is -8.5kg/s, pressure at piston is 5E+7Pa

If the time step is dt=1E-6, mass flux at outlet is -600kg/s, pressure at piston is 3E+11Pa

This is totally bogus. Something seems to be conceptually wrong.
jpo is offline   Reply With Quote

Old   July 24, 2009, 14:21
Default
  #8
Super Moderator
 
-mAx-'s Avatar
 
Maxime Perelli
Join Date: Mar 2009
Location: Switzerland
Posts: 3,125
Rep Power: 32
-mAx- will become famous soon enough
disable the MDM, switch to steady solver.
Change your moving piston to massflow inlet and give the 8.5kg/s.
Iterates and check the pressure distribution.
are you working 2d or 3d?
__________________
In memory of my friend Hervé: CFD engineer & freerider
-mAx- is offline   Reply With Quote

Old   July 29, 2009, 19:43
Default
  #9
jpo
Member
 
Join Date: Apr 2009
Posts: 93
Rep Power: 9
jpo is on a distinguished road
Apologies for the delayed reply.
Solution:

start the simulation with ideal-gas on, run for sufficient number of time steps. Switch to incompressible.

It works now.

Many thanks, mAx for the useful analysis; it has helped me tackle the problem from many aspects.

Cheers,
-jpo
jpo is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
BlockMesh FOAM warning gaottino OpenFOAM Native Meshers: blockMesh 7 July 19, 2010 14:11
Negative pressures in the flow domain mahut FLUENT 2 September 27, 2007 05:07
Axisymmetrical mesh Rasmus Gjesing (Gjesing) OpenFOAM Native Meshers: blockMesh 10 April 2, 2007 14:00
dynamic mesh, negative absolute pressures Jason FLUENT 0 March 15, 2005 10:36
Multicomponent fluid Andrea CFX 2 October 11, 2004 05:12


All times are GMT -4. The time now is 19:57.