# Massflow or average velocity boundary condition

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

 November 18, 2011, 10:55 Massflow or average velocity boundary condition #1 New Member   Jan Willem Krijger Join Date: May 2010 Posts: 6 Rep Power: 9 Hello I'm trying to simulate a pipeflow with 2 inflow boundary conditions and 1 outflow boundary condition using simpleFoam. I tried using a fixedValue boundary condition for the velocity at the outflow. But the simulation didn't converged and I got disturbances at the outflow. Which is expected because the flow is not uniform when it approaches the outflow boundary. I would like to define the velocity with zeroGradient at the inflow and the massflow or average velocity at the outflow. And the pressure with fixedValue at the inflow and zeroGradient at the outflow. How can I set the massflow or the average velocity at the outflow boundary? Any suggestions are appreciated!!

November 18, 2011, 15:33
#2
Assistant Moderator

Bernhard Gschaider
Join Date: Mar 2009
Posts: 4,016
Rep Power: 43
Quote:
 Originally Posted by Sideshore Hello I'm trying to simulate a pipeflow with 2 inflow boundary conditions and 1 outflow boundary condition using simpleFoam. I tried using a fixedValue boundary condition for the velocity at the outflow. But the simulation didn't converged and I got disturbances at the outflow. Which is expected because the flow is not uniform when it approaches the outflow boundary. I would like to define the velocity with zeroGradient at the inflow and the massflow or average velocity at the outflow. And the pressure with fixedValue at the inflow and zeroGradient at the outflow. How can I set the massflow or the average velocity at the outflow boundary? Any suggestions are appreciated!!
So you want a boundary condition that keeps the velocity at the outlet the same but only rescales it to satisfy the prescribed mass flow. I'm not aware of such a BC (which doesn't mean that there is none).

If I had to do such a thing I'd use groovyBC (basically using an expression for the value like "U*mfTarget/mfCurrent" - the two mfs being specified/calculated). Note that probably to get this stable you'll have to make it a bit more complicated: at least some kind of underrelaxation to avoid trouble during the startup-phase and you'll have to decide whether you allow backflow (because that would be accelerated by the scaling too). And of course there is the general problem of specifying the massflow at the outlet ....

 November 18, 2011, 20:20 #3 Senior Member   Wouter van der Meer Join Date: May 2009 Location: Elahuizen, Netherlands Posts: 186 Rep Power: 10 hello, If you have two inlets and one outlet. I think the best thing to do is set the two inlet velocities (fixed value). Calculate the velocities from the ratio of flows through the inlet and the area of the inlets by hand and let simpleFoam calculate the outlet flow, what being an incompressible steady state should result in the asked for massflow. hope this helps Wouter

November 21, 2011, 05:05
#4
New Member

Jan Willem Krijger
Join Date: May 2010
Posts: 6
Rep Power: 9

Ansys CFX does have a massflow boundary condition, could be a very nice addition to OPENFOAM!

Quote:
 If I had to do such a thing I'd use groovyBC (basically using an expression for the value like "U*mfTarget/mfCurrent" - the two mfs being specified/calculated).
GroovyBC sounds interesting! But as you said it might be a struggle to get a stable solution. I'm going to look into groovyBC thanks!

Quote:
 If you have two inlets and one outlet. I think the best thing to do is set the two inlet velocities (fixed value). Calculate the velocities from the ratio of flows through the inlet and the area of the inlets by hand and let simpleFoam calculate the outlet flow, what being an incompressible steady state should result in the asked for massflow.
Prescribing the inflow velocity at both inlets does not give an accurate result. Because when you prescribe the inflow velocity normally you also prescribe the fixed pressure at the outlet. Therefore you end up with a pressure difference between both inlets. Which is not the case I would like to simulate.

Of course you could iterate between inlet velocities to end up with a similar pressure at both inlets.

 November 21, 2011, 13:50 #5 Senior Member   Wouter van der Meer Join Date: May 2009 Location: Elahuizen, Netherlands Posts: 186 Rep Power: 10 hello Jan Willem, Maybe you can use my suggestion as a stable start for the simulation with groovyBC Best Wouter

 August 10, 2016, 05:16 #6 Senior Member     Anton Kidess Join Date: May 2009 Location: Germany Posts: 1,261 Rep Power: 23 I think the fixedMean boundary condition works nicely for such a case. __________________ *On twitter @akidTwit *Spend as much time formulating your questions as you expect people to spend on their answer.

 September 27, 2016, 15:09 Conservation of momentum #7 New Member   Rizvi Join Date: Sep 2016 Posts: 3 Rep Power: 3 Hello i am trying to solve the same problem in Ansys fluent , how do i check if momentum is conserved?

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Saturn CFX 45 February 8, 2016 05:42 akhenathon FLUENT 6 April 24, 2012 18:32 fumiya OpenFOAM 4 June 17, 2011 02:58 bearcharge Main CFD Forum 0 May 14, 2010 11:32 Tudor Miron CFX 15 April 2, 2004 06:18

All times are GMT -4. The time now is 20:03.