Radial inflow through rotating cavity
This is my first post here, I hope someone can give me help in my problem:
I am modelling a rotating cavity in CFX, similar to this, with a superimposed radial inflow. My geometry differs in the following manner;
The left-hand disk extends all the way down to a central shaft.
The inlet is the same as in the schematic. Air enters the central slot at the periphery of the cavity, flows inward radially turns right and is expelled through a annular hole in the center of the right-hand disk (outer radius 36 mm, inner radius 12 mm). This flow is imposed using blowers.
I am having issues posing reasonable boundaries and would like some guidance.
What I know:
1. Total Pressure at inlet
2. Swirl at inlet is 1 (inlet flow tangential velocity is the same as periphery of disks)
3. The mass flow through the cavity is around 9 g/s
4. Angular velocity of disks
5. Geometry of disks
The main issue I'm having is posing a good outlet boundary, as the flow is highly tangential and I get backflow very easily.
What I am using so far is an L-shaped domain in the rotating reference frame. A Total Pressure inlet with the direction set to normal to boundary. At the outlet (extended roughly 7 times the distance of last obstacle) I have a "Radial Equilibrium" average static pressure outlet.
The problem with this is that I have to vary the pressure until I get the desired mass flow, as the pressure here is unknown to me. Needless to say, this is painful:)
Is my outlet boundary even reasonable (I am not sure I understand the radial equilibrium outlet correctly)?
Any guidance or comments would be very much appreciated!
If you know the mass flow then use a mass flow boundary condition. No point using a pressure boundary when you do not know the pressure.
Thank you for your reply!
Could I then please ask you which mass flow boundary you think would be the most suited for my case? I have tried using a mass flow outlet, and this gives the correct mass flow (of course). But is there a mass flow boundary that would give me the correct pressure distribution at outlet too?
I am fairly new to CFX and have therefore not yet had time to learn what all the options do, as I'm under some time pressure (this is school work). From what I understood of the manual, the "shift pressure" option would do this, but this option leads the solver to build walls, thus disqualifying the solution.
I have tried the constant flux boundary, as my outlet flow is highly tangential, but I fear this is unphysical.
If there is only one inlet and one outlet you cannot specify mass flow at the inlet and outlet. This is over specifying the simulation. In this case, if you specify the mass flow at the outlet then you have to have the same mass flow at the inlet to conserve mass - so you define the pressure at the inlet intead.
You comment the flow is highly tangential at the outlet - this is not a good idea. I would consider extending your outlet to a location where the flow is simpler and the flow can cross the outlet approximately at right angles to the boundary.
Thank you for the reply Glenn!
I understand that mass both in and out is a bad idea and have not done that, I appologise for the bad description. What I meant was that I have tried using a mass flow outlet and a total pressure inlet, as you write.
What I would like to do is impose a radial pressure profile at the outlet as well as mass. Because of this highly swirling flow, I know that the pressure will vary with radius. So I would like to specify the mass flow rate out, and enforce a pressure distribution radially. But I am unsure if this is possible? As I stated before, I have tried using the following outlet BC:
Mass flow rate
Massflow Update > Shift Pressure
This, seemingly, allwos me to impose a pressure profile using a CEL expression? Am I correct in this assumption? I have read the manual but I'm unsure that I understand it correctly, why I wanted to ask on the forum:)
Regarding the outlet BC having swirling flow I agree, ideally I would like to place it further away from the bend. But I am trying to model an experiment and am thus trying to keep to the real geometry as much as possible.
I should also add for clarity, the annular outlet pipe also rotates with the same angular velocity as the cavity (it is an extension of the disks). Thus, the swirl doesn't dissipate with axial position.
As for the boundaries - You cannot specify pressure and flow rate at a boundary. Rather you should specify flow rate at the other boundary and pressure at this one.
I will expect that you will get "backflow" caused by the swirl close to the outlet. If the flow will exit the rotating domain in reaility you have the option to use the opening boundary condicton or to model the geometrie after the rotating domain. This is the "first basic step" to be able to get a reasonable simulation!
Second step is to play with boundaries! If you use incompressible fluid it does not matter waht will be the absolute pressure value at the inlet or outlet. It is only important that the pressure difference is correct because this drives the flow. so you could use the mass flow boundary condicton, finish the calculcation and shift the pressuere field to the value you want in cfd-post. Or you need to set the correct pressure difference and get the mass flow. Hope these ideas help.
|All times are GMT -4. The time now is 06:25.|