CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Nonphysical flow field while using coodles solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 24, 2007, 18:18
Default Hello, I am using coodles s
  #1
Member
 
Ankur Gupta
Join Date: Mar 2009
Posts: 38
Rep Power: 8
ankgupta8um is on a distinguished road
Hello,

I am using coodles solver in OpenFOAM 1.4.1 to simulate flow through a cylinder. The computational domain is very simple and consists of an annular pipe attached to a cylinder. This is an expansion problem where the flow through the annular pipe expands into the cylinder (annular jet expanding into a cylindrical pipe). The boundary conditions I am using are:
- fixed value velocity inlet at the annular cross-section; zero gradient for pressure.
- no-slip walls for annlar pipe and cylindrical pipe; zero gradient for pressure.
- waveTrnasmissive pressure BC at the downstream end of the cylinder; inletOutlet BC for velocity.

I am not able to get a reasonable flow field in the computational domain. It seems to me that the unphysical pressure waves in the domain are destroying the numerical solution. Initially, I used the default solver settings as given in the pitzdaily tutorial. Then I tried using recommended convective discretization schemes (eg, fliteredLinear) for LES but that didn't help. I also tried using upwind scheme with the hope that the increased dissipation will dissipate out the spurious pressure waves, but that also didn't help.
I tried different initializations at the start of the run (starting from the RANS solution, starting from a quiscent medium) but all led to unphysical flow field.

I think that the unphysical pressure waves are destroying the solution. The reason being: I ran a case where instead of using walls for the cylindrical surface, I used pressure transmissive boundaries (i.e., no confinement; annular jet expanding into an eclosure with pressure transmissive boundaries at the cylindrical periphery and at the downstream end). For this case, I could get a physical flow field. That suggests that the numerical disturbances in the form of spurious pressure waves exit the computational domain from the peripheral boundary of the cylinder when pressure Transmissibe BC is used there. When wall is used it reflects back and destroys the solution.

I have been trying to resolve this issue in coodles with the use of walls close to the jet for quite some time now but haven't had any success. I am stuck with this issue and need to resolve it in order to make some progress.

I would really appreciate it if someone can throw some light on what the potential causes for this problem are and how to resolve it. People having similar experiences with coodles are kindly requested to share them with the forum. Any information on getting coodles solver to work is also welcome !!

Thanks!
Regards,
Ankur
ankgupta8um is offline   Reply With Quote

Old   November 25, 2007, 13:55
Default What time discretization are y
  #2
Senior Member
 
Srinath Madhavan (a.k.a pUl|)
Join Date: Mar 2009
Location: Edmonton, AB, Canada
Posts: 698
Rep Power: 12
msrinath80 is on a distinguished road
What time discretization are you using?
msrinath80 is offline   Reply With Quote

Old   November 25, 2007, 17:20
Default Hello Srinath, I am using b
  #3
Member
 
Ankur Gupta
Join Date: Mar 2009
Posts: 38
Rep Power: 8
ankgupta8um is on a distinguished road
Hello Srinath,

I am using backward scheme for time discretization.

Regards,
Ankur
ankgupta8um is offline   Reply With Quote

Old   January 22, 2008, 01:55
Default Hello, I am using coodles s
  #4
Member
 
Ankur Gupta
Join Date: Mar 2009
Posts: 38
Rep Power: 8
ankgupta8um is on a distinguished road
Hello,

I am using coodles solver with adaptive time stepping to solve for a low mach number variable density flow through a cylinder with an annular inlet. I was encountering the non-physical pressure field in my computational domain. I ran some test cases and observed the following behavior:
1. The pressure field looks reasonable when I use a large time step (say, corresponding to a maximum courant number of 2). If I reduce the allowed maximum courant number to say 0.75, I see the nonphysical pressure field in my domain.
2. If I increase the number of correctors in the PISO algorithm from a default value of 2 to 5, I could get the physical pressure field.

I am not able to understand the cause of this behavior. I would highly appreciate if some body can throw some light here.

Thanks!!
Regards,
Ankur
ankgupta8um is offline   Reply With Quote

Old   January 22, 2008, 16:26
Default Hi Ankur, Try using Crank-Nic
  #5
Member
 
lillberg's Avatar
 
Eric Lillberg
Join Date: Mar 2009
Location: Stockholm
Posts: 80
Rep Power: 8
lillberg is on a distinguished road
Send a message via Skype™ to lillberg
Hi Ankur,
Try using Crank-Nicholson time stepping with some Euler for stability, e.g.

ddtSchemes
{
default CrankNicholson 0.9;
}

And try keeping your maximum Co < 0.5.

Good luck!

//Eric
lillberg is offline   Reply With Quote

Old   January 26, 2008, 17:54
Default Hi Eric and others, I tried
  #6
Member
 
Ankur Gupta
Join Date: Mar 2009
Posts: 38
Rep Power: 8
ankgupta8um is on a distinguished road
Hi Eric and others,

I tried running my case with CrankNicholson 0.9 with maximum Co < 0.5, but it didn't help. That again is resulting in the nonphysical pressure field and thus nonphysical velocity fields.
So far, from all the test runs I have made, I could get the physical pressure and velocity fields only with a higher number of correctors (~5) in the PISO algorithm.
Any comment on how to get reasonable pressure field with lesser number of correctors (~2) in the PISO algorithm is greatly appreciated. The use of a higher number of correctors tremendously increases the computational time.

Thanks!!
Regards,
Ankur
ankgupta8um 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
Coodles anja OpenFOAM Pre-Processing 33 January 14, 2010 10:05
Nonphysical volume fractions at multiphase inlet sylvester OpenFOAM Running, Solving & CFD 4 July 1, 2009 10:52
Coodles vs sonicTurbFoam hsieh OpenFOAM Running, Solving & CFD 10 February 3, 2009 07:17
Re: supersonic free jet nonphysical solution?? Patti Phoenics 0 October 23, 2008 21:12
User Solver in FoamX with a new field variable vvqf OpenFOAM Pre-Processing 2 October 28, 2005 20:24


All times are GMT -4. The time now is 07:16.