
[Sponsors] 
Incompressible Flow: Retrieving Pressure from Velocity Field 

LinkBack  Thread Tools  Search this Thread  Display Modes 
July 5, 2013, 18:57 
Incompressible Flow: Retrieving Pressure from Velocity Field

#1 
Senior Member
Robert
Join Date: Sep 2010
Posts: 158
Rep Power: 15 
Hello all,
I have been trying to retrieve the pressure field from a divergencefree velocity field in 2D incompressible flow. I am using the following formula for the pressure Poisson equation: (underscore denotes partial differentiation) Laplacian(p) = ( u*u_x + v*u_y )_x + ( u*v_x + v*v_y )_y (I arrived here from http://cfd.ce.gatech.edu/docs/CEE7751_7.pdf, labeled as Equation 3, and applying continuity: u_x = v_y) I apply a Poisson solver (http://arc.aiaa.org/doi/abs/10.2514/6.20123068), which I know works properly because I have used it for computing wall distances for a turbulence model (http://www.researchgate.net/publicat...tial_Equations). I however get a totally wrong solution for pressure on a 2D liddriven cavity case (The velocity field is very similar to that I get in OpenFOAM). Any comments or suggestions on this problem of recovering the pressure field from a divergencefree velocity field? Thanks a ton. 

July 6, 2013, 04:33 

#2  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,777
Rep Power: 71 
Quote:
first, for incompressible flow there is no meaning in the "thermodinamic pressure". What you compute is only a scalar field such that its gradient ensures the correct divergencefree velocity. second, what do you compare in the liddriven solution? you have some file with the pressure computed by some code? Remember that you have a solution apart a constant value. what kind of BC are you prescribing in the Poisson equation? 

July 6, 2013, 06:39 

#3 
Senior Member
Robert
Join Date: Sep 2010
Posts: 158
Rep Power: 15 
I obtain the velocity field by the "exact fractional step method" (http://www.ecs.umass.edu/mie/tcfd/Pa...ot_cfd2007.pdf). Then, I try to obtain the pressure as a postprocessing step.
I am enforcing a pressure value of 0 at one point in the corner, then using Neumann (zerogradient) boundary conditions everywhere for pressure, since walls enclose the whole space. Thanks for the help. 

July 6, 2013, 06:51 

#4  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,777
Rep Power: 71 
Quote:
2) the fixed zero value is a constant fixed arbitrarily, any other value give you the same solution for the Poisson equation. 3) be careful in the BCs, they are Neumann conditions but actually not homogeneous. Finally, you have to solve DGp= q, in discrete form this can be very different from solving the Laplacian operator 

July 6, 2013, 07:03 

#5 
Senior Member
Robert
Join Date: Sep 2010
Posts: 158
Rep Power: 15 
1) Yes as mentioned in my first post I am comparing with OpenFOAM (icoFoam).
2) I do realize that the problem is solvable up to an arbitrary constant. 3) As mentioned in the first post I use the solver referenced above; I have used fixed and zerogradient boundary conditions successfully with the solver on wall distance computations. I think your third and fourth points are addressed in the reference. 

July 6, 2013, 07:28 

#6 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,777
Rep Power: 71 
how do ensure that also OF fixed the zero value for the pressure? It would be useful if you post the figures of the two pressure field, just 34 isolevel curves are sufficient.
Furthermore, consider also that in the classical fractional step (as the method described by Kim and Moin on an old JCP paper), when implicit integration in time is used for the diffusive term the computed "pressure" results affected by a viscous term, too. 

July 6, 2013, 08:05 

#7 
Senior Member
Robert
Join Date: Sep 2010
Posts: 158
Rep Power: 15 
Is there anything wrong with what I would think is the most general approach starting from the incompressible NavierStokes, manipulating it to the Poisson pressure form, and discretizing this?


July 6, 2013, 08:15 

#8 
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,777
Rep Power: 71 
no, but what you get in term of the scalar solution can be very different from code to code.


July 6, 2013, 09:36 

#9 
Senior Member
Jonas T. Holdeman, Jr.
Join Date: Mar 2009
Location: Knoxville, Tennessee
Posts: 128
Rep Power: 18 
There is another approach that I use. By the Helmholtz theorem, the incompressible NSE is decomposable into a pressurefree solenoidal governing equation for the velocity and an irrotational equation for the pressure as a functional of the velocity, grad p = irrotational part of (u dot grad u). The variational form of this is (grad q, grad p) = (grad q, u dot grad u), where q lies in the same space as p. Note that you would get this by integrating the variational form of the pressure Poisson equation by parts, but here there is no Neuman bc involved here since you don't integrate by parts.
For the discrete FE form, I like to use a continuous cubic Hermite pressure element since the pressuregradient degreesoffreedom might also be useful, but this is not necessary. The (vector) test function grad q is orthogonal to the solenoidal velocity space (by the Helmholz theorem) and projects out the irrotational pressure terms. Of course the velocity functions I use are the curl of a modified Hermite element and so are necessarily divergencefree. I have not tried this projection method using velocity elements that are only weakly divergencefree, bu it should work OK. 

July 6, 2013, 11:24 

#10  
Senior Member
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 6,777
Rep Power: 71 
Quote:
you are correct, this approach is substantially that one described in the book of Peric and Ferziger and drives to see that the "pressure" function is only a Lagrangian multiplier. 

Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Which pressure OpenFOAM use for incompressible flow? P/rho or (P101325)/rho ?  panda60  OpenFOAM  16  August 14, 2018 04:57 
Boundary Conditions : Total Pressure or Velocity  Gearb0x  OpenFOAM Running, Solving & CFD  2  February 28, 2011 21:18 
flow simulation across a small fan  jane luo  Main CFD Forum  15  April 12, 2004 17:49 
mass flow inlet  Denis Tschumperle  FLUENT  7  August 9, 2000 02:19 
Hydrostatic pressure in 2phase flow modeling (CFX4.2)  HB &DS  CFX  0  January 9, 2000 13:19 