# hydrodynamic forces using fluent

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

 November 27, 2010, 03:05 hydrodynamic forces using fluent #1 New Member   Nimmy Thankom Philip Join Date: Aug 2010 Posts: 6 Rep Power: 8 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

 November 28, 2010, 17:17 #2 New Member   Kevin Erhart Join Date: Nov 2010 Location: Orlando, FL Posts: 10 Rep Power: 7 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

 November 29, 2010, 03:19 #3 New Member   Nimmy Thankom Philip Join Date: Aug 2010 Posts: 6 Rep Power: 8 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

 December 3, 2010, 14:03 #4 New Member   Kevin Erhart Join Date: Nov 2010 Location: Orlando, FL Posts: 10 Rep Power: 7 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

 December 7, 2010, 01:41 #5 New Member   Nimmy Thankom Philip Join Date: Aug 2010 Posts: 6 Rep Power: 8 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

 February 6, 2012, 00:30 UDF for pressure variation #6 Member   Nirav Join Date: Jul 2011 Posts: 42 Rep Power: 7 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.

 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 ivanbuz FLUENT 11 March 10, 2010 16:13 changkiang FLUENT 2 March 5, 2006 02:18 Syed Haider FLUENT 1 February 20, 2006 05:49 Tim Pugh FLUENT 0 July 27, 2004 03:05 P Smith Main CFD Forum 2 October 26, 1999 15:00

All times are GMT -4. The time now is 21:03.