CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   FLUENT (http://www.cfd-online.com/Forums/fluent/)
-   -   hydrodynamic forces using fluent (http://www.cfd-online.com/Forums/fluent/82470-hydrodynamic-forces-using-fluent.html)

nims November 27, 2010 03:05

hydrodynamic forces using fluent
 
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

kerhart November 28, 2010 17:17

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

nims November 29, 2010 03:19

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

kerhart December 3, 2010 14:03

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

nims December 7, 2010 01:41

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

niravtm007 February 6, 2012 00:30

UDF for pressure variation
 
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


All times are GMT -4. The time now is 07:33.