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

modeling potential flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 14, 2012, 19:52
Default modeling potential flow
  #1
New Member
 
ab
Join Date: Jun 2010
Posts: 5
Rep Power: 6
imaloke is on a distinguished road
Hi,

I wonder if anyone can suggest that, whether it is possible to model a flow domain defined by potential flow theory i.e. irrotational flow using FLUENT. If so, how?

Thnx.
imaloke is offline   Reply With Quote

Old   January 15, 2012, 14:18
Default
  #2
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 448
Rep Power: 10
LuckyTran is on a distinguished road
Yes. Use the inviscid model for your viscous model.

Potential flow and inviscid flows are the same, depending on what background you have in fluids they are called one or the other or both.
LuckyTran is offline   Reply With Quote

Old   January 15, 2012, 14:59
Default
  #3
New Member
 
ab
Join Date: Jun 2010
Posts: 5
Rep Power: 6
imaloke is on a distinguished road
Are you sure? To my knowledge, potential flow can be viscous and inviscid depending upon the viscosity condition implemented in the flow. So, the point I would like to mention that, in FLUENT, all option to define a flow is kind of realistic approach. However, potential flow is sort of simplistic approach with sum assumption that makes it irrotational, which I don't know if at all feasible in practice and so, if FLUENT can model it, that is my question? If possible in FLUENT, what to select under DEFINE>MODELS>SOLVER and under DEFINE>MODELS>VISCOUS?

Thnx.
imaloke is offline   Reply With Quote

Old   January 15, 2012, 17:12
Default
  #4
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 448
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by imaloke View Post
Are you sure? To my knowledge, potential flow can be viscous and inviscid depending upon the viscosity condition implemented in the flow. So, the point I would like to mention that, in FLUENT, all option to define a flow is kind of realistic approach. However, potential flow is sort of simplistic approach with sum assumption that makes it irrotational, which I don't know if at all feasible in practice and so, if FLUENT can model it, that is my question? If possible in FLUENT, what to select under DEFINE>MODELS>SOLVER and under DEFINE>MODELS>VISCOUS?

Thnx.
Okay I stand corrected. There are viscous potential flows, though they need very peculiar properties as you say.

Fluent allows you to model inviscid flows, the inviscid potential flows, by selecting the inviscid flow model under viscous models. You can use either solver, but the pressure-based solver is cheaper, simpler, and should suffice.
LuckyTran is offline   Reply With Quote

Old   January 15, 2012, 17:35
Default
  #5
New Member
 
ab
Join Date: Jun 2010
Posts: 5
Rep Power: 6
imaloke is on a distinguished road
Ok. Thnx Lucky.
imaloke is offline   Reply With Quote

Old   January 16, 2012, 02:46
Default
  #6
Member
 
Phoevos
Join Date: Mar 2009
Posts: 84
Rep Power: 7
fivos is on a distinguished road
I would be hesitant using fluent inviscid solver to solve a potential flow. The reason for that is that fluent solves the N-S equations, which when viscosity is omitted reduce to the Euler equations.

Now, Euler equations can be solved using potential flow theory, assuming the flow is irrotational and steady state. Generally it is valid to assume so, since if there is no viscosity, there is no reason for the fluid elements to start rotating, right?

However, since fluent does not solve the potential flow model, but the Euler equations, the inherent numerical viscosity of the used schemes (even if you use the highest order schemes possible, which will limit numerical viscosity), will produce viscosity and vorticity effects, which will give a totally different answer from the expected, when solving pure potential flow (Δφ=0, solve for φ and then spatial derivatives of φ give u,v,w).

A simple experiment to check this would be to solve flow over a cylinder with the fluent inviscid model (steady state). You will see that pressure will not be fully recovered after the cylinder (D' alamberts paradox : http://en.wikipedia.org/wiki/D%27Alembert%27s_paradox), as it would be expected from a pure potential flow solver. On the other hand you will get small vortices after the cylinder and eventually you will get drag (again contrary to what you would expect from potential flow).

To sum up, using inviscid fluent for potential flow is, according to my opinion, inaccurate (inaccurate here means that you won't get the expected, from potential theory, results - the results you'll get will be closer to reality, than the potential theory, though). You should use another software for that (for example Comsol has the ability to solve Laplace equation, which is used for potential flow). However, using inviscid fluent solver, can still give you an initial flow field for more complex physics.

Any comments are welcome.
fivos is offline   Reply With Quote

Old   January 16, 2012, 11:02
Default
  #7
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 448
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by fivos View Post
I would be hesitant using fluent inviscid solver to solve a potential flow. The reason for that is that fluent solves the N-S equations, which when viscosity is omitted reduce to the Euler equations.

Now, Euler equations can be solved using potential flow theory, assuming the flow is irrotational and steady state. Generally it is valid to assume so, since if there is no viscosity, there is no reason for the fluid elements to start rotating, right?

However, since fluent does not solve the potential flow model, but the Euler equations, the inherent numerical viscosity of the used schemes (even if you use the highest order schemes possible, which will limit numerical viscosity), will produce viscosity and vorticity effects, which will give a totally different answer from the expected, when solving pure potential flow (Δφ=0, solve for φ and then spatial derivatives of φ give u,v,w).

A simple experiment to check this would be to solve flow over a cylinder with the fluent inviscid model (steady state). You will see that pressure will not be fully recovered after the cylinder (D' alamberts paradox : http://en.wikipedia.org/wiki/D%27Alembert%27s_paradox), as it would be expected from a pure potential flow solver. On the other hand you will get small vortices after the cylinder and eventually you will get drag (again contrary to what you would expect from potential flow).

To sum up, using inviscid fluent for potential flow is, according to my opinion, inaccurate (inaccurate here means that you won't get the expected, from potential theory, results - the results you'll get will be closer to reality, than the potential theory, though). You should use another software for that (for example Comsol has the ability to solve Laplace equation, which is used for potential flow). However, using inviscid fluent solver, can still give you an initial flow field for more complex physics.

Any comments are welcome.
Fluent uses the Euler equations (and not Navier-Stokes, directly) when using the inviscid model. So none of these are worries.
LuckyTran is offline   Reply With Quote

Old   January 16, 2012, 11:13
Default
  #8
Member
 
Phoevos
Join Date: Mar 2009
Posts: 84
Rep Power: 7
fivos is on a distinguished road
Ehm, sorry but solving the Euler equations does not mean that there is no numerical dissipation. Numerical dissipation (or numerical viscosity) comes from the truncation of the Taylor expansion at the derivative approximations and it is inherent in any numerical scheme.

Increased resolution and higher order schemes will limit numerical dissipation, but it will always be there. According to my experince, trying to solve inviscid flow (Euler equations) with Fluent will not result to the same results as a potential flow solver and, from my experience again, results will differ substantially.

I don't know if anyone else has any experience with the inviscid flow solver, but if you perform the small numerical experiment I described above you'll see what I mean when I say that fluent is not appropriate for simulating potential flow. See also this post:

Potential incompressible flow around an aerofoil
(It is somewhat old, but I don't think that fluent's numerics on inviscid solver changed much)
or this one:
potential flow vs. Euler flow

Again any comments welcome.
fivos is offline   Reply With Quote

Old   January 16, 2012, 11:25
Default
  #9
Senior Member
 
Lucky Tran
Join Date: Apr 2011
Location: Orlando, FL USA
Posts: 448
Rep Power: 10
LuckyTran is on a distinguished road
Quote:
Originally Posted by fivos View Post
Ehm, sorry but solving the Euler equations does not mean that there is no numerical dissipation. Numerical dissipation (or numerical viscosity) comes from the truncation of the Taylor expansion at the derivative approximations and it is inherent in any numerical scheme.

Increased resolution and higher order schemes will limit numerical dissipation, but it will always be there. According to my experince, trying to solve inviscid flow (Euler equations) with Fluent will not result to the same results as a potential flow solver and, from my experience again, results will differ substantially.

I don't know if anyone else has any experience with the inviscid flow solver, but if you perform the small numerical experiment I described above you'll see what I mean when I say that fluent is not appropriate for simulating potential flow. See also this post:

Potential incompressible flow around an aerofoil

It is somewhat old, but I don't think that fluent's numerics on inviscid solver changed much.

Again any comments welcome.
Numerical dissipation is present in any finite discretization scheme. It can always be dealt with.
LuckyTran is offline   Reply With Quote

Old   January 16, 2012, 11:36
Default
  #10
Member
 
Phoevos
Join Date: Mar 2009
Posts: 84
Rep Power: 7
fivos is on a distinguished road
Quote:
Originally Posted by LuckyTran View Post
It can always be dealt with.
Well I have to disagree (depending on what you mean dealt with). Numerical dissipation's influence can be minimised/lessened/reduced but cannot be absolutely removed. That is what you are doing when you are testing for grid dependence, testing when numeircal dissipation is very small so you can assume that your solution is unaffected, within a tolerance, by it. It will always be there, though.
fivos 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
A role of combustion modeling in flow solver? Yoon Main CFD Forum 0 November 26, 2006 12:00
transform navier-stokes eq. to euler-eq. pxyz Main CFD Forum 37 July 7, 2006 08:42
potential energy& static enthalpy in buoyant flow Atit CFX 0 May 3, 2006 10:05
mold flow modeling Pei Hsieh Main CFD Forum 0 May 4, 2005 10:08
CFD Modeling of Two-phase Flow in Small Dia.Tubes Eric Poindexter Main CFD Forum 2 September 22, 2000 09:21


All times are GMT -4. The time now is 13:35.