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

hydrodynamic forces using fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 27, 2010, 03:05
Default hydrodynamic forces using fluent
  #1
New Member
 
Nimmy Thankom Philip
Join Date: Aug 2010
Posts: 6
Rep Power: 7
nims is on a distinguished road
Hallo all,

I have simulated the vertical oscillation of a cylinder in a tank.I got the drag and lift forces. Drag is negligible, but there is considerable amount of lift force. But it includes the hydrostatic pressure also. since my depth of immersion is varying with respect to time the hydrostatic pressure is also varying. Because of this hydrostatic pressure i am getting non zero values of forces...Can anybody suggest me a way of eliminating the hydrostatic pressure so that the force i get from fluid is only the hydrodynamic forces..i have given the effect of gravity also while simulating.

Regards,
Nimmy
nims is offline   Reply With Quote

Old   November 28, 2010, 17:17
Default
  #2
New Member
 
Kevin Erhart
Join Date: Nov 2010
Location: Orlando, FL
Posts: 10
Rep Power: 6
kerhart is on a distinguished road
Nimmy,

This should be completely controlled by the gravity term that you have set in Fluent. If you turn off gravity, then the pressure within a fluid will not vary with depth. That should be all you need to do. If you need gravity for your simulation to function properly, but want to neglect pressure variation with depth, you will likely need to use a UDF to accomplish this (and I suspect it will not be simple).

If you need more help, feel free to describe your simulation in a little more detail and I will offer whatever additional advise I can.

Kevin Erhart, PhD
Research Vice President
Central Technological Corporation
www.centecorp.com
kerhart is offline   Reply With Quote

Old   November 29, 2010, 03:19
Default
  #3
New Member
 
Nimmy Thankom Philip
Join Date: Aug 2010
Posts: 6
Rep Power: 7
nims is on a distinguished road
Thanks Kevin

I tried with gravity off also.But fluent is giving error. I will provide more details of simulation. I am using DEFINE_CG_MOTION udf for giving motion to the cylinder with hexahedral meshes in a cylindrical domain. The following are the solver options

Model Settings
----------------------------------------------------------------
Space 3D
Time Unsteady, 1st-Order Implicit
Viscous Standard k-epsilon turbulence model
Wall Treatment Standard Wall Functions

FLUENT
Version: 3d, dp, pbns, dynamesh, vof, ske, unsteady (3d, double precision, pressure-based, dynamic mesh, VOF, standard k-epsilon, unsteady)
Release: 6.3.26
Title:

Boundary Conditions
-------------------

Zones

name id type
---------------------------------------
fluid 2 fluid
cylinder 3 wall
bottom_wall 4 wall
side_wall 5 wall
pressure_outlet 6 pressure-outlet
default-interior 8 interior
Discretization Scheme

Variable Scheme
------------------------------------------------
Pressure PRESTO!
Momentum Second Order Upwind
Volume Fraction Geo-Reconstruct
Turbulent Kinetic Energy Second Order Upwind
Turbulent Dissipation Rate Second Order Upwind
If i turn off gravity will it model the free surface correctly?
Do the operating pressure and reference pressure location affect the values?
also i am doubtful about the value to be given for the gauge pressure in the pressure outlet BC.
The domain is 1 m deep with 0.6m depth water and rest air. First i am initializing with air and later patching with water.
Hope these much details will help u understand my problem.
Actually i need to compare the values with some thearetical values.
Hope ur inputs will help me solve the problem.
Thanking you
Nimmy
nims is offline   Reply With Quote

Old   December 3, 2010, 14:03
Default
  #4
New Member
 
Kevin Erhart
Join Date: Nov 2010
Location: Orlando, FL
Posts: 10
Rep Power: 6
kerhart is on a distinguished road
Nimmy,

Let me try to help with a couple of your questions where I have some experience.

" If i turn off gravity will it model the free surface correctly?" - I am not sure, but I know that the lighter fluid will not rise if gravity is turned off. So if bubbles are forming within the liquid, than you will NEED to have gravity on the properly solve.

"Do the operating pressure and reference pressure location affect the values?" - These values should not affect the solution if used properly. The operating pressure is typically set to atmospheric pressure (which is the default in Fluent). All pressures are then specified relative to this pressure. The reference location tell Fluent where to set the pressure to the specified operating pressure. This location will affect the pressure values if you have gravity turned on. I would set the location to a meaningful point, such as at the open surface of your tank (or at an outlet if it exits to ambient conditions).

"also i am doubtful about the value to be given for the gauge pressure in the pressure outlet BC." - This value should be specified Relative to the operating pressure as mentioned above. So if the outlet is open to the surroundings the gauge pressure should be zero.

"The domain is 1 m deep with 0.6m depth water and rest air. First i am initializing with air and later patching with water." - This should be fine.

You stated you are using a VOF model, which fluid is set to the primary phase? The VOF model is usually NOT consistent meaning that you may get different results depending on which fluid is the primary versus which is the secondary. You may want to try switching the fluid roles to see if the solution is more stable this way (if you try this don't forget to change your volume fraction BCs and initializations as well). You may also want to try reading through the multi-phase section of the Fluent manual and depending on the details of your flow field, you may find that one of the other Multi-phase models may be more appropriate than VOF.

Good luck and I hope that helps you out some more.

Kevin Erhart, PhD
Central Technological Corporation
www.centecorp.com
kerhart is offline   Reply With Quote

Old   December 7, 2010, 01:41
Default
  #5
New Member
 
Nimmy Thankom Philip
Join Date: Aug 2010
Posts: 6
Rep Power: 7
nims is on a distinguished road
Thanks a lot Kevin for your ideas.
It did help me a lot.I simulated it without gravity.But noticed that the surface effects are not modeled correctly.As per ur advice i gave the reference position also correctly.Thanks a lot for ur help.And for ur information i am using air as the primary phase and water secondary.Expecting same in future.
Regards,
Nimmy
nims is offline   Reply With Quote

Old   February 6, 2012, 00:30
Default UDF for pressure variation
  #6
Member
 
Nirav
Join Date: Jul 2011
Posts: 42
Rep Power: 6
niravtm007 is on a distinguished road
Send a message via Skype™ to niravtm007
Hii friends
My problem is flow through river channel, I have taken a orbitary region so at exit of my geometry flow exits into river itself. so i need to know how to apply UDf at exit, as pressure must vary with P=row*g*h. my exit cross section is not uniform so what should i do please help. is it possible to apply custom field function ???? in fluent please help ASAP. my gravity is turned on still i cant see pressure variation in the geometry. how should i initialize the solution relative or absolute ? and at the exit pressure variation is not seen as flow exits in to water only what am i doing wrong ???
these are the conditions pplied by me
Model Settings
----------------------------------------------------------------
Space 3D
Time Unsteady, 1st-Order Implicit
Viscous Standard k-epsilon turbulence model
Wall Treatment Standard Wall Functions

FLUENT
Version: 3d, pbns, vof, unsteady (3d, pressure-based, VOF, standard k-epsilon, unsteady)
Release: 6.3.26

Boundary conditions
velocity inlet from one side and and at exit pressure outlet, even tough gravity is turned on i cant see pressure variations?

Pressure PRESTO!
Momentum Second Order Upwind
Volume Fraction CISCAM
Turbulent Kinetic Energy 1st Order Upwind
Turbulent Dissipation Rate 1st Order Upwind

Last edited by niravtm007; February 6, 2012 at 00:55.
niravtm007 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
problem of running parallel Fluent on linux cluster ivanbuz FLUENT 11 March 10, 2010 16:13
a variance of forces in FLUENT changkiang FLUENT 2 March 5, 2006 02:18
Integration of a Custom C++ Model into FLUENT Syed Haider FLUENT 1 February 20, 2006 05:49
Hydrodynamic forces Tim Pugh FLUENT 0 July 27, 2004 03:05
Fluent forces -lift/drag interpretation P Smith Main CFD Forum 2 October 26, 1999 15:00


All times are GMT -4. The time now is 03:20.