CFD Online Logo CFD Online URL
Home > Forums > Software User Forums > ANSYS > FLUENT

mass flow rate not conserved in turbomachine, interface defined wrong?

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

LinkBack Thread Tools Search this Thread Display Modes
Old   February 9, 2010, 15:06
Default mass flow rate not conserved in turbomachine, interface defined wrong?
New Member
Join Date: Dec 2009
Posts: 11
Rep Power: 16
wildli is on a distinguished road
Dear all,
I am simulating two counter rotating axial wheel in one cylinder chamber using ANSYS FLUENT 12 and encountering a problem with mass flow rate not conserved.

Basically this is the flow description in this chamber:
flow runs into chamber inlet --> 1st axial wheel --> short volume before second wheel --> 2ed counter rotating axial wheel--> outlet

Boundary condition:
Pressure inlet with total temperature and gauge total pressure defined
Pressure outlet with gauge pressure and back flow temperature define
Moving reference frame to two wheels and stationery condition for other fluid field

Model: Pressure-based, steady-state, ideal gas setting, simple scheme,
mixing plane model for each interface between rotating area and stationery area

Result: Mass flow rate at inlet and outlet not conserved, and there is about 20% difference when they are stable.
Severe reverse happens at each interface

Possible reason: Interface between 1st wheel and short volume is set up as default in mixing plane model (radial mixing plane geometry + area averaging method), I doubt mass averaging method would be the right one for my setting, but reverse flow never dies out at interface and switching into averaging method diverges the result immediately.

Question: would FLUENT not be able to solve my problem? or because of my blade design, this is not a steady state problem so that reverse flow happens which can not allow me continuing the calculation?

If anyone here has similar experience, please help me.
wildli is offline   Reply With Quote

Old   March 24, 2010, 19:23
New Member
Carlos Ventura
Join Date: Feb 2010
Posts: 3
Rep Power: 16
cventura is on a distinguished road
Hi Wild,

Well, my case is a little bit different from yours: I am trying to run a few steady-state simulations regarding a radial-inflow turbine, considering both the stator and rotor using Fluent-ANSYS 12. I am also using a mixing plane (axial mixing plane geometry + area averaging method) to model the stator-rotor interaction.
However, I have been experiencing similar problems and tested many different options to run the cases.
Initialisation is a key factor and therefore I am running my cases in a step-by-step mode increasing its complexity during calculation. I changed the inlet boundary condition for both the rotor and stator from "pressure inlet" to "mass-flow inlet" and used a stationary rotor to start with. By changing the boundary conditions this way Fluent will force mass conservation across the mixing plane (see manual). In a preliminary stage I did not use the mixing plane, so I set fixed reasonable values for both the stator outlet and rotor inlet.
I have also lowered the under-relaxation coefficients to reasonably low values and let the residuals decay a few orders of magnitude between each simulation step.
I am not sure if this can help you since I might not be able to answer your question directly.
These cases were also tested with CFX and the simulations without any problem, so I am not sure if this would be a better option for this type of cases.
cventura is offline   Reply With Quote

Old   July 8, 2015, 11:38
New Member
Join Date: Jun 2015
Posts: 6
Rep Power: 10
johntynanrrp is on a distinguished road
Wildi / Carlos,

Did you find any solutions. I am running a simple model in Star CCM+. I have an inlet plenum going into a fan fluid section and on to an outlet plenum. Moving reference frame on fan fluid is driving the fluid flow. Boundary conditions: Inlet 0 Total Pressure, Outlet 0 Static Pressure, No mass flow specified on boundaries.

When I add a mixing plane at the interface between the fan fluid and the outlet plenum I am seeing a difference in the inlet and outlet mass flow.

For example the mass flow at the inlet is 9.18Kg/s in comparison to 12.57Kg/s at the outlet.

johntynanrrp is offline   Reply With Quote

Old   September 15, 2022, 12:19
New Member
Join Date: May 2017
Posts: 1
Rep Power: 0
arjun1992 is on a distinguished road

Not sure who is still reading this, but for anyone struggling with a similar issue to Wildli.

I had a very similar issue in fluent with mixing planes using pressure-inlet to pressure-outlet boundary coupling for a compressible rotor-stator 3D simulation. I had a rough 20% increase in outgoing massflow compared to incoming. This was mainly because I used mass-flow-inlet for incoming air to my domain.

Using mass-flow-inlet (as I have now learned) for a compressible simulation is not a great idea as using this condition means the density becomes a floating number driven my massflow. Thereby the increased outgoing massflow. Switching to velocity-inlet for incoming air helped resolve the mass flow imbalance for my compressible simulation.
arjun1992 is offline   Reply With Quote


Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On

Similar Threads
Thread Thread Starter Forum Replies Last Post
mass flow rate (CFX post) sanchezz CFX 2 January 14, 2010 06:54
Mass Flow Rate student87 CFX 4 January 2, 2010 04:45
mass flow rate on the Iso-clip surface & interior Sunil Gupta FLUENT 0 April 22, 2008 09:29
User defined function of mass flow rate Eric FLUENT 1 April 22, 2005 18:15
static pressure from mass flow rate SAM FLUENT 5 October 22, 2004 09:37

All times are GMT -4. The time now is 04:19.