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

Boundary condition for bifurcated flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 22, 2010, 19:38
Default Boundary condition for bifurcated flow
  #1
Senior Member
 
Jie
Join Date: Jan 2010
Location: Australia
Posts: 119
Rep Power: 7
jiejie is on a distinguished road
Dear all

Does any one have experience on simulation of bifurcated flow - flow with one inlet and two outlets. I am trying to run a simulation of bifurcated blood flow and just wonder what will be the appropriate boundary condition to use. I have the information for inlet pressure & velocity, tow outlet pressures.

What I implemented so far is to specified the pressure boundary condition only and let the OpenFOAM to evaluate the flux normal to the patch with pressureInletVelocity.

Inlet: U with pressureInletVelocity (value uniform (0 0 0)),
p with fixed value of P1 Pa/kg/m^3

outlet1: U with inletOutlet (uniform (0 0 0 ))
p with fixed value of P2 Pa/kg/m^3

outlet2: U with inletOutlet (uniform (0 0 0 ))
p with fixed value of P3 Pa/kg/m^3

wall: U with fixed value (uniform (0 0 0))
p with zeroGradient

However, the simulation seems to be highly unstable. Is there anyone know a better way to setup the appropriate boundary condition for this type of flow?

Thank you very much.

Last edited by jiejie; September 23, 2010 at 19:18.
jiejie is offline   Reply With Quote

Old   September 23, 2010, 07:05
Default Change outlet biundary conditions
  #2
Senior Member
 
Antonio Martins
Join Date: Mar 2009
Location: Porto, Porto, Portugal
Posts: 112
Rep Power: 8
titio is on a distinguished road
Send a message via MSN to titio Send a message via Skype™ to titio
Hi,

I am runing a case with two inlets and two outlets, akin to a cross-slot. At the inlet, I impose the average velocity, and at the outlet I impose zero gradient, ensuring that the flow has enough length to fully developed. For pressure at the outlets I used uniform fixed value equals to zero. Works great...

Titio
titio is offline   Reply With Quote

Old   September 23, 2010, 10:49
Default
  #3
New Member
 
Robert Langner
Join Date: Dec 2009
Location: Freiburg, Germany
Posts: 27
Rep Power: 7
Robat is on a distinguished road
Hi JieJie,

I think a small example illustrates the source of your problem:
Imagine an incompressible fluid in a pipe(constant diameter).
If you set U_inlet = 100 m/s and U_outlet = 1 m/s, the calculation will crash whatever you do!
In your case the pressure on all patches is fixed. But are these values physically correct? If your bifurcation is asymmetric the pressure values at the outlets surely differ from each other.

You may did this pressure assumption with regard to the natural original, but:
The walls of a blood artery are elastic, so their shape depends to the lokal pressure. Is your model capable to represent this characteristic?
Otherwise you can't assume an equal outlet pressure. (But it would be a good verification, if your numerical results fit to that fact.)
And I hope you not need to be overprecise or the blood neoplasm overthrow your mass conservation.

To increase the stabillity (I think it's staedy state?):
1. set a higher number of outer correction cycles for SImPLE
2. use setFieldsDict to guess a near by solution for the fields inside your model. It's easier for the solver to find convergence.
3. You may try a test and change pd_inlet and U_outlet to zeroGradient and see how stable it runs. From numerical point of view defined velocity at inlet and pressure at outlet is the most stable combination.

But I would'nt trust the results as long as the pressure on both outlets is fixed.

sorry for the big text
bests,
Robert
Robat is offline   Reply With Quote

Old   September 23, 2010, 11:16
Default velocities will never work
  #4
Senior Member
 
Antonio Martins
Join Date: Mar 2009
Location: Porto, Porto, Portugal
Posts: 112
Rep Power: 8
titio is on a distinguished road
Send a message via MSN to titio Send a message via Skype™ to titio
Dear All,

Because of the overall mass balance, if inlet and outlet velocities are different, it means the channel dimensions are different. If they are the same, the simulation naturally blews...
That is why pressure boundary conditions at the exit are natural. If you want to imposed velocities, you have to used derivatives, otherwise it will be impossible...

Titio
titio is offline   Reply With Quote

Old   September 23, 2010, 18:59
Default
  #5
Senior Member
 
Jie
Join Date: Jan 2010
Location: Australia
Posts: 119
Rep Power: 7
jiejie is on a distinguished road
Quote:
Originally Posted by titio View Post
Hi,

I am runing a case with two inlets and two outlets, akin to a cross-slot. At the inlet, I impose the average velocity, and at the outlet I impose zero gradient, ensuring that the flow has enough length to fully developed. For pressure at the outlets I used uniform fixed value equals to zero. Works great...

Titio
Hi Titio

what is your pressure condition at the out let?

I tired some similar as well. I set velocity at inlet with averaged velocity and at outlet I set zero velocity gradient. For pressure, I set zero pressure graident at inlet and fixed pressure value of uniform 0 at the outlet. However, I found the flow hardly moves in the blood vessel.

Thanks

jie

Last edited by jiejie; September 23, 2010 at 19:15.
jiejie is offline   Reply With Quote

Old   September 23, 2010, 19:05
Default
  #6
Senior Member
 
Jie
Join Date: Jan 2010
Location: Australia
Posts: 119
Rep Power: 7
jiejie is on a distinguished road
Quote:
Originally Posted by Robat View Post
Hi JieJie,

But I would'nt trust the results as long as the pressure on both outlets is fixed.

sorry for the big text
bests,
Robert
Hi Robert

Thanks for the reply. The pressure on the two outlets are different, but the difference is very small.

Also the cross-sectional area for inlet and two outlets are different, A_inlet > A_outlet1 > A_outlet2.

I might need to find more clinical data set for the case I am running.

jie

Last edited by jiejie; September 23, 2010 at 19:23.
jiejie is offline   Reply With Quote

Old   September 24, 2010, 05:39
Default
  #7
New Member
 
Robert Langner
Join Date: Dec 2009
Location: Freiburg, Germany
Posts: 27
Rep Power: 7
Robat is on a distinguished road
Hi JieJie,
to know the (measured) pressure values for the outlets is great.
But then you shall set the inlet pressure to zeroGradient (otherwise your measurement error would increase instabillity). The case is completely defined with outlet pressure and inlet velocity.
If you use an incompressible solver: They are very sensitive to the pressure field. You better set wallBuoyantPressure to the walls not zeroGradient and reduce the tolerance for pressure solution.

bests,
Robert
Robat is offline   Reply With Quote

Old   September 27, 2010, 20:46
Default
  #8
Senior Member
 
Jie
Join Date: Jan 2010
Location: Australia
Posts: 119
Rep Power: 7
jiejie is on a distinguished road
Quote:
Originally Posted by Robat View Post
Hi JieJie,
to know the (measured) pressure values for the outlets is great.
But then you shall set the inlet pressure to zeroGradient (otherwise your measurement error would increase instabillity). The case is completely defined with outlet pressure and inlet velocity.
If you use an incompressible solver: They are very sensitive to the pressure field. You better set wallBuoyantPressure to the walls not zeroGradient and reduce the tolerance for pressure solution.

bests,
Robert
Hi Robat

I tried constant velocity inlet and zero velocity gradient outlets with zero pressure gradient inlet and constant pressure outlets. However, I found that the flow hardly moves in the bifurcated vessel no matter how big the inlet velocity I use.

Cheers,

jiejie
jiejie is offline   Reply With Quote

Old   September 28, 2010, 17:29
Default Boundary conditions
  #9
Senior Member
 
Antonio Martins
Join Date: Mar 2009
Location: Porto, Porto, Portugal
Posts: 112
Rep Power: 8
titio is on a distinguished road
Send a message via MSN to titio Send a message via Skype™ to titio
Hi,

I believe the right conditions for your case are:

- Velocity: constant velocity inlet and zero gradient at the outlet. This means that the flow is fully developed at the outlet.
- pressure: zero gradient at the outlet and fixed value, say zero at the outlet. OpenFoam calculates the pressure relative to the exit pressure.

Questions such as variable tube diameter can be taken into account using this boundary conditions. For pipe flow the previous conditions work like a charm to me.

Regards,

António Martins
titio is offline   Reply With Quote

Old   September 28, 2010, 18:38
Default
  #10
Senior Member
 
Jie
Join Date: Jan 2010
Location: Australia
Posts: 119
Rep Power: 7
jiejie is on a distinguished road
Quote:
Originally Posted by titio View Post
Hi,

I believe the right conditions for your case are:


- pressure: zero gradient at the outlet and fixed value, say zero at the outlet. OpenFoam calculates the pressure relative to the exit pressure.
Hi titio

DO you use both zero gradient and fixed value of zero at the outlet???

or you suppose to say zero pressure gradient at inlet and fixed value of zero pressure at the outlet?

Thanks

jiejie
jiejie is offline   Reply With Quote

Old   September 28, 2010, 19:13
Default Correction
  #11
Senior Member
 
Antonio Martins
Join Date: Mar 2009
Location: Porto, Porto, Portugal
Posts: 112
Rep Power: 8
titio is on a distinguished road
Send a message via MSN to titio Send a message via Skype™ to titio
Hi,

I meant zero pressure gradient at inlet and fixed value of zero pressure at the outlet. Worked hard today. Going to sleep. Is midnight in my time zone.....

Titio
titio is offline   Reply With Quote

Old   September 28, 2010, 19:18
Default
  #12
Senior Member
 
Jie
Join Date: Jan 2010
Location: Australia
Posts: 119
Rep Power: 7
jiejie is on a distinguished road
Quote:
Originally Posted by titio View Post
Hi,

I meant zero pressure gradient at inlet and fixed value of zero pressure at the outlet. Worked hard today. Going to sleep. Is midnight in my time zone.....

Titio
Just start working here =)

The flow noting moving problem is solved. It was due to the orientation used in the previous mesh model.

Thanks for help everyone =)

Last edited by jiejie; October 7, 2010 at 07:16.
jiejie is offline   Reply With Quote

Old   March 3, 2011, 11:35
Default Gas Turbine combustor inlet conditions
  #13
Member
 
José Rodrigues
Join Date: Jun 2010
Location: IN+/IST Lisbon
Posts: 53
Rep Power: 7
jose_rodrig is on a distinguished road
Hi all,

Im trying to simulate a gas turbine combustor for which I know inlet conditions (massflow, pressure, temperature) and I want to evaluate efficiency of the combustor based on the outlet conditions.

I have experienced that OF blows up whenever I specify at the inlet (fixedValue BC) either:

a) temperature pressure and velocity (T p U - fixedValue)
b) pressure and massflow (p phi - fixedValue)
c) pressure and velocity (p U - fixedValue)

The other quantities are set to zeroGradient (note for velocity also used pressureInletValocity)

Any suggestions?
Thx
jose_rodrig 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
RPM in Wind Turbine Pankaj CFX 9 November 23, 2009 05:05
specify boundary condition type in particle tracking in order to trace flow filed payam_IUST FLUENT 1 October 15, 2009 17:16
mass flow in is not equal to mass flow out saii CFX 2 September 18, 2009 08:07
How can apply mass flow rate boundary condition? Sima Phoenics 1 December 1, 2007 19:55
Outlet boundary condition for pulsatile flow Timite FLUENT 0 January 22, 2003 04:56


All times are GMT -4. The time now is 01:59.