CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   need help for simulation of axial fan (https://www.cfd-online.com/Forums/cfx/79338-need-help-simulation-axial-fan.html)

 rahulv August 20, 2010 06:31

need help for simulation of axial fan

Hi

i am confuse what should be the inlet and outlet boudary condition for
axial fan.the atmospheric air is axially going in the fan.
and the inlet and outlet velocity can be determined by rotation of rotor...
i could not predict the boundary condition for such problem.

 Turbomachine August 20, 2010 14:02

boundary conditions

It really depends on the purpose of the simulation. If you want to determine the characteristic curve for instance, you would want to set the inlet static pressure to a known upstream condition, or ambient pressure at infinity, and vary the outlet static back- pressure. Alternatively, if your fan is required to deliver a certain amount of mass flow then you should set this as boundary condition.

My best advice is to check some tutorials. There is one for axial fans.

 Arevik August 23, 2010 06:58

In similar cases I used massflow boundary condition at the inlet and static pressure at the outlet. I got stable simulations with these boundary conditions. but as "Turbomachinery" said before, it depends on what exactly you want to know. For example, if you know the velocity profile from another simulation or from experiments, you can set this as inlet-bc.

 rahulv August 30, 2010 04:14

ok let us assume..I am designing a completely new fan and i have unavailability of experiment results.
In this case i am doing study of a fan which is open to atmosphere.
i am assuming the outlet and inlet both are open to atmosphere , so i have taken the static pressure zero as outlet boundary condition, because the fan inlet is also open to atmosphere i am taking total pressure = 0 in fan inlet bc.

i want to to know the mass flow rate given by the fan on a given rmp..

but i am not getting appropriate results please let me know if i am making some mistake.

 Arevik August 30, 2010 04:41

Are you sure that the boundary condition is set far enough from the fan? because directly before the fan, pressure is lower, after the fan higher than atmosphere. Otherwise you wouldn't have a pressure difference over the fan, and that's nonsense.
you should also consider, that the fan is usually a part of a whole machine, with inlet casing etc. usually the pressure and velocity profiles in front of the fan are not uniform over the 360°. this might have a strong impact on efficiency!

 rahulv August 30, 2010 05:57

indeed i refer the boundary condition given in a thread for similar situation
http://www.cfd-online.com/Forums/flu...onditions.html by Razvan.
Actually i don't want to give mass flow rate boundary condition because it is a forced boundary condition.i was expecting to do simulation for 0 static pressure at outlet.

 Arevik August 30, 2010 07:04

I completely agree with what Razvan says. But as he says, you need to model some space before and after the fan:
"let's say we have an axial fan in a tube, and both ends of this tube are directly connected to the atmosphere."
If you put you atmospheric pressure condition directly in front and after the fan, it can't work, as the fan can't produce a pressure gradient. That's why I asked you "Are you sure that the boundary condition is set far enough from the fan?"

 rahulv August 30, 2010 07:52

i agree with you that i should perform the same simulation in a tube and i will be going to perform simulation in a tube as Razvan and you suggest. i'll discuss the results tomorrow, but here i am not just talking about the pressure only.. i am applying static pressure and total pressure boudnary condition, which are quite logical bc for such case.

 rahulv August 30, 2010 23:30

I didn't even work out this way

 Arevik August 31, 2010 04:33

Did the simulation run and the results were strange, or didn't it run at all?

 rahulv August 31, 2010 06:32

simulation runs but the results are not appropriate...
when i look the result details i found that there is no effect of blade rotation in the domain.
i have performed some test to simulation of simple problems with rotating solid part , but even in tests i couldnt see the effect of rotating part on fluid motion.may be i am doing some mistake for appling rotating boundary condition.

 Arevik August 31, 2010 06:36

If you like, you can send me the *.out-file, so I can check the boundary conditions. (baraka.so(at)hotmail.com)

 rahulv September 1, 2010 07:19

i got the solution...
with the same boundary condition.
i kept the blade stationary and i rototate the fluid over the blate at given rpm.

 Saima September 3, 2010 05:24

Rahul, i am doing the 2D rotor blade and having problem in solution.

I made my mesh in ICE CFD like a cascade vertical (inlet and outlet). Then i try to solve in CFX. CFX converted this 2D into 3D.

I have calculated my boundary condition through velocity triangles. I know experimental data but with blade rotatng point of view. Now, i solved it in CFX but i have not found option for moving mesh. (As i cant take rotating option because it is not complete blade just a section of blade)

Could u pls let me know how did u setup and wat are your boundary conditions plus your software?

 rahulv September 3, 2010 06:54

hi saima
i have performed 3d simulation of a mixed flow impeller in cfx..
I think there is no need of rotating mesh in ur problem..
you can perform the simulation with section of blade only.
you keep the blades stationary and give rotation to the fluid .
this way cfx will just add a tengential velocity component at the each fluid control volume.
"just imagine you are sitting on the blade. For you blade is stationary and the whole world is revolving around you."

in my case i want to know the mass flow rate on a given rmp and at zero static pressure..
so
i gave
outlet bc = static pressure =0
inlet bc = total pressure = 0

or you can contact me on rah00002004[at]gmail.com

 chaudhry_hashim August 2, 2014 08:57

Finding fan curve

Hi I am quite new to CFD i am trying to find out the fan curve. My fan diameter is 71mm and what did uptill now I made inlet duct 15 times of fan dia with pressure inlet (0.0 Pa), outlet duct 30 times of fan dia with pressure outlet (0.0 Pa) and I am giving fixed rpm to the rotating region in between. I am measuring pressure in inlet and outlet duct at a position 10 times of fan dia. but Still I didnt find the relevant pressure difference across the fan and also the solution is not converges. If i want to give the value of dynamic pressure at the inlet then how can i calculate this value as i know the flowrate.

I would be very grateful if you people help me out

 singer1812 August 4, 2014 11:23