# Why we normally provide velocity at inlet and pressure at outlet for pipe flow?

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

 April 30, 2012, 08:18 Why we normally provide velocity at inlet and pressure at outlet for pipe flow? #1 New Member   PARESH GUJARATI Join Date: Jan 2012 Posts: 4 Rep Power: 6 Hello, Why we normally provide velocity at inlet and pressure at outlet for pipe flow? In FLUENT, We need to provide boundary condition like velocity inlet and pressure outlet. When we provide velocity inlet value, where this velocity value will be used to calculate flow field? What is the use of pressure outlet information at outlet condition? which equations will use these values at inlet and outlet? Sorry for asking simple question but I am having doubt so. Please answer it. rgd likes this.

 April 30, 2012, 11:24 #2 New Member   Join Date: Mar 2012 Posts: 8 Rep Power: 6 The choice of variables at inlet/outlet boundary conditions is in fact not unique. However, you have to ensure that information which enters the domain at the boundary is given by a proper choice of variables at the boundary. For example for the 1D compressible Euler equations, you have 3 characteristic waves in the fluid - a sound wave traveling to the left (at speed u-c), a sound wave traveling to the right (at speed u+c) and an entropy wave (convection at speed u). At the boundaries you have to distinguish four different cases: - sub-sonic inlet: 2 characteristics enter the domain (u, u+c), 1 characteristic leaves the domain (u-c) - sub-sonic outlet: 1 characteristic enters the domain (u-c), 2 characteristics leave the domain (u, u+c) - super-sonic inlet: all 3 characteristics enter the domain (u, u+c, u-c) - super-sonic outlet: all 3 characteristics leave the domain (u, u+c, u-c), no further boundary information is necessary For a boundary condition to be well-posed you have to provide the information that fully determines the characteristic waves which _enter_ the domain. This information is needed to solve the fluid field, i.e. to determine the fluxes through the boundary interfaces. The other characteristic waves leaving the domain can be determined from the values within the domain. For example, for a sub-sonic inlet, the sound and entropy waves entering the domain are fully determined if _one_ of the following pairs of variables are given at the boundary: (density,energy) or (density,velocity) or (pressure, mass flux) For a sub-sonic outlet, the sound wave entering the domain can be determined by _one_ of the following variables at the outlet: pressure,velocity,mass flux,temperature,enthalpy The best choice of variables depends on your problem. Good references for further reading are the book by Hirsch "Numerical computation of internal and external flow. Volume 2" or the paper by Jean-Michel Ghidaglia "The normal flux method at the boundary for multidimensional finite volume approximations in CFD" (European Journal of Mechanics - B/Fluids, Vol. 24/1, 2005)

 April 30, 2012, 11:57 #3 Senior Member   Jonas T. Holdeman, Jr. Join Date: Mar 2009 Location: Knoxville, Tennessee Posts: 108 Rep Power: 10 That is a good question. There may be mathematical, computational, and physical reasons. From notions of causality, one might expect that some sort of entrance boundary conditions might be necessary to "prepare" the flow for the region of interest. And this might be necessary for the algorithm one is using. Incompressible flow is a little strange. For an incompressible fluid in a rigid container, any perturbation of the flow at one point is instantly felt everywhere in the fluid. The state of flow is everywhere consistent. In such a case, inlet and outlet boundary conditions may not be necessary. This is the case if strictly divergence-free finite elements are used in the FEM. There one can use "do nothing" boundary conditions, where inlet and outlet B.C. are not specified. Considering Poiseulle (so-called pressure-driven) flow in a straight channel for example, one can simulate developed flow with just a few elements along the channel and no in- or out- BCs. One can match the known velocity profile (parabolic in 2D) at the center of the channel as accurately as the cross-channel resolution will allow, while the error at the entrance and exit will be at most a few percent. The Navier-Stokes equation is a composite equation, being the sum of a pressureless velocity-governing equation and an equation for the pressure as a functional of the velocity. This result follows from the Helmholtz decomposition theorem. In this view, no pressure BC is needed (other than specifying the pressure at one point) because the velocity doesn't depend on the pressure. Now if one does not use strictly divergence-free functions in a primative variable formulation, then one must use some sort of projection to remove the non-solenoidal component of the approximation. Unfortunately the pressure is often confused with this projected term (they both satisfy the same equation but different BC). The confusion is that when people talk about BC on the "pressure", they are really talking about the projection.

 August 3, 2012, 05:53 velocity inlet in fluent #4 Senior Member   kunar Join Date: Nov 2011 Posts: 117 Rep Power: 6 Dear friends, In fluent, For analysis of 2D naca0012 airfoil velocity inlet we give vcostheta in x component & vsintheta in y component, v is inlet velocity. 1)here i start analysis of 3D wing, for that i take naca 0012 airfoil & extrude 100mm, in gambit and analysis in fluent i have doubt how to set velocity inlet, here i consider my velocity is 50m/s, then what is xyz component,please let me know. 2)if you consider 3D wing, (vtantheta for z component) is correct or wrong, please let me know. 2) how to find angle of attack for 3D wing? please let me know

 Tags pressure outlet, velocity inlet

 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 Mohsin FLUENT 6 January 15, 2015 18:15 nikhil FLUENT 5 December 11, 2013 13:30 Antech Main CFD Forum 0 April 25, 2006 02:15 Abhi Main CFD Forum 12 July 8, 2002 09:11 chong chee nan FLUENT 0 December 29, 2001 06:13

All times are GMT -4. The time now is 05:51.