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

Incompressible Flow: Retrieving Pressure from Velocity Field

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 5, 2013, 18:57
Default Incompressible Flow: Retrieving Pressure from Velocity Field
  #1
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 143
Rep Power: 5
lordvon is on a distinguished road
Hello all,
I have been trying to retrieve the pressure field from a divergence-free 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/10.2514/6.2012-3068), 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 lid-driven 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 divergence-free velocity field?

Thanks a ton.
lordvon is offline   Reply With Quote

Old   July 6, 2013, 04:33
Default
  #2
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,099
Rep Power: 16
FMDenaro will become famous soon enough
Quote:
Originally Posted by lordvon View Post
Hello all,
I have been trying to retrieve the pressure field from a divergence-free 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/10.2514/6.2012-3068), 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 lid-driven 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 divergence-free velocity field?

Thanks a ton.

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 divergence-free velocity.

second, what do you compare in the lid-driven 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?
FMDenaro is offline   Reply With Quote

Old   July 6, 2013, 06:39
Default
  #3
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 143
Rep Power: 5
lordvon is on a distinguished road
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 post-processing step.

I am enforcing a pressure value of 0 at one point in the corner, then using Neumann (zero-gradient) boundary conditions everywhere for pressure, since walls enclose the whole space.

Thanks for the help.
lordvon is offline   Reply With Quote

Old   July 6, 2013, 06:51
Default
  #4
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,099
Rep Power: 16
FMDenaro will become famous soon enough
Quote:
Originally Posted by lordvon View Post
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 post-processing step.

I am enforcing a pressure value of 0 at one point in the corner, then using Neumann (zero-gradient) boundary conditions everywhere for pressure, since walls enclose the whole space.

Thanks for the help.
1) do you compare your pressure field to some other solution?
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
FMDenaro is offline   Reply With Quote

Old   July 6, 2013, 07:03
Default
  #5
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 143
Rep Power: 5
lordvon is on a distinguished road
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 zero-gradient boundary conditions successfully with the solver on wall distance computations. I think your third and fourth points are addressed in the reference.
lordvon is offline   Reply With Quote

Old   July 6, 2013, 07:28
Default
  #6
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,099
Rep Power: 16
FMDenaro will become famous soon enough
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 3-4 iso-level 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.
FMDenaro is offline   Reply With Quote

Old   July 6, 2013, 08:05
Default
  #7
Senior Member
 
Robert
Join Date: Sep 2010
Posts: 143
Rep Power: 5
lordvon is on a distinguished road
Is there anything wrong with what I would think is the most general approach starting from the incompressible Navier-Stokes, manipulating it to the Poisson pressure form, and discretizing this?
lordvon is offline   Reply With Quote

Old   July 6, 2013, 08:15
Default
  #8
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,099
Rep Power: 16
FMDenaro will become famous soon enough
Quote:
Originally Posted by lordvon View Post
Is there anything wrong with what I would think is the most general approach starting from the incompressible Navier-Stokes, manipulating it to the Poisson pressure form, and discretizing this?
no, but what you get in term of the scalar solution can be very different from code to code.
FMDenaro is offline   Reply With Quote

Old   July 6, 2013, 09:36
Default
  #9
Member
 
Jonas T. Holdeman, Jr.
Join Date: Mar 2009
Location: Knoxville, Tennessee
Posts: 68
Rep Power: 7
Jonas Holdeman is on a distinguished road
There is another approach that I use. By the Helmholtz theorem, the incompressible NSE is decomposable into a pressure-free 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 pressure-gradient degrees-of-freedom 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 divergence-free. I have not tried this projection method using velocity elements that are only weakly divergence-free, bu it should work OK.
Jonas Holdeman is offline   Reply With Quote

Old   July 6, 2013, 11:24
Default
  #10
Senior Member
 
Filippo Maria Denaro
Join Date: Jul 2010
Posts: 1,099
Rep Power: 16
FMDenaro will become famous soon enough
Quote:
Originally Posted by Jonas Holdeman View Post
There is another approach that I use. By the Helmholtz theorem, the incompressible NSE is decomposable into a pressure-free 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 pressure-gradient degrees-of-freedom 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 divergence-free. I have not tried this projection method using velocity elements that are only weakly divergence-free, bu it should work OK.

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.
FMDenaro 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
Which pressure OpenFOAM use for incompressible flow? P/rho or (P-101325)/rho ? panda60 OpenFOAM 7 October 12, 2013 10:26
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 2-phase flow modeling (CFX4.2) HB &DS CFX 0 January 9, 2000 13:19


All times are GMT -4. The time now is 08:27.