|
[Sponsors] |
November 19, 2015, 12:49 |
Centrifugal fan
|
#1 |
New Member
Joćo
Join Date: May 2014
Posts: 6
Rep Power: 12 |
Hi my frineds,
I am starting to simulate a CENTRIFUGAL FAN in ANSYS CFX 15 I want to calculate the efficiecy depending on the number of blades. I have made the rotor with SW14 and and saved in IGES format to import into ansys. I have many questions, first I simulate in ansys with the rotor (left image) or the inside with the flow (right image)? Second, When import(in step, iges, etc. format) the rotor is broken in half. Why? Its normal? 3. Do I need to create a volute If yes, Why? in SW? Ansys? I have made some experiencies, this is right? please nyone can help me answering the doubts? I'm completely lost. Regards j0hnny |
|
November 19, 2015, 16:16 |
|
#2 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,829
Rep Power: 144 |
Sounds like you should:
* Do the CFX tutorials which are provided with the software. Several of these are for rotating machinery. See the documentation under the help options. * Read the best practices guides in the CFX documentation. There is one for rotating machinery. |
|
November 20, 2015, 03:20 |
|
#3 |
Member
Thomas
Join Date: Dec 2014
Location: Poland
Posts: 49
Rep Power: 11 |
Hi
In the past I made some simulation of this type of rotating machines. First of all, if you try do do a comparison between experimental data and numerical simulations, you should build a CAD model similar to the test stand. This fan mostly work in the volute, because the efficiency of this machine is the highest then. The leakage offten occured in this situation, because generally we suck the air by the pipeline. Then you should take into account this phenomena. In the rotating machines, there is always efficiency peak. In this point the influence of blades number is less importance on efficiency. But when you lead fan to the stall, then this is significant, because the secondary loss and profile loss will be arise. Take into account inlet and outlet angles of the blade. The ralative velocity should be always tangential, when you look for improve efficiency. |
|
November 24, 2015, 15:29 |
|
#4 | |
New Member
Joćo
Join Date: May 2014
Posts: 6
Rep Power: 12 |
Hi, Thanks for the answers
I have read tutorials about turbomachinery and I have learned a lot I defined boundary conditions for the rotor, volute and pipe Interfaces between Pipe and rotor and between rotor and volute But this error appears when trying to run my simulation: Update failed for the Solution component in Fluid Flow (CFX). The solver failed with a non-zero exit code of : 2 Quote:
|
||
November 24, 2015, 18:31 |
|
#5 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,829
Rep Power: 144 |
||
November 25, 2015, 03:57 |
|
#6 |
Member
Thomas
Join Date: Dec 2014
Location: Poland
Posts: 49
Rep Power: 11 |
Your model in preprocessor looks good. I think, that you did some small mistakes somewhere. Could you paste a CFX Command Language for Run from CFX Solver? There are described in details your boundary conditions. I will look them closer and try to help you
|
|
November 25, 2015, 11:55 |
|
#7 | |
New Member
Joćo
Join Date: May 2014
Posts: 6
Rep Power: 12 |
I have checked the proprieties of material, mesh, etc and i didnt found the possivel mistakes
Tomson199, if you dont mind checking CFX Command Language, I will be very grateful Quote:
I just put the total pressure = 183pa |
||
November 25, 2015, 17:38 |
|
#8 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,829
Rep Power: 144 |
In the rotating domain you have "Alternate Rotation Model = true". You probably don't want that, turn it off. Also if you are having problems with convergence you don't want to use the auto time scale. You will need to use smaller time steps (as the FAQ says).
The problem is most likely to be your mesh quality (As the FAQ said - did you read it? Your question really has been asked a thousand times before). Please post an image showing a cross section through your mesh. |
|
November 26, 2015, 02:31 |
|
#9 |
Member
Thomas
Join Date: Dec 2014
Location: Poland
Posts: 49
Rep Power: 11 |
I see that you use reference pressure 0 atm. On the first attempt, switch your energy model to none, because compressibility effects is negligible and pressure increase is relatively small. It might be wrong with Isothermal model and it produce values close to zero. Put the reference pressure equal 1 atm. In the test stand I am in 99% sure, that you analyze this machine in ambient condition. I think that it is the most possible cause of your problem. Next things is your boundary condition. In the real test stand you have after outlet any pipe or air from this place run out to the atmosphere? If yes, try to use massflow on the inlet and static pressure on the outlet. Last thing is pitch on the interfaces. On the both sides of them, you have a full 360 deg revolution of area, so change this option to NONE. When I starded my adventure in CFD, in the first attempts I used very badly mesh and despite this my calculations were made.
Sorry for my english, I practise my language every day to improve my communication |
|
November 26, 2015, 05:59 |
|
#10 |
Super Moderator
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,829
Rep Power: 144 |
Hi Thomas:
The model is isothermal. It is not modelling compressible flow, it is an incompressible flow model. Your other points are correct, well spotted. |
|
November 26, 2015, 06:35 |
|
#11 |
Member
Thomas
Join Date: Dec 2014
Location: Poland
Posts: 49
Rep Power: 11 |
I admit, I tell wrong with this Isothermal model.
Thanks Glenn |
|
January 6, 2016, 09:04 |
|
#12 |
New Member
Joćo
Join Date: May 2014
Posts: 6
Rep Power: 12 |
Thanks you a lot and i'm sorry not to have answered earlier.
I've been writing the thesis, and only now i returned to the part of the simulation. Now works so well with your help But I have some doubts. Is it normal those streamlines recede backwards? As illustrated in the next image. I dont know why, but it seems the simulation is wrong. I have tried other ways, for example only the rotor, and already seem right. |
|
January 7, 2016, 02:44 |
|
#13 |
Member
Thomas
Join Date: Dec 2014
Location: Poland
Posts: 49
Rep Power: 11 |
I'm happy, that you did it It is normal, that some streamlines go back through leakage, because there is a difference of pressures. You can minimilize thaht by minimize the gap in the leakage seal.
|
|
October 1, 2019, 13:55 |
Centrifugal fan
|
#14 |
New Member
Join Date: Jun 2009
Posts: 21
Rep Power: 17 |
In case anybody interested in centrifugal/radial fan simulation here you can download (.res file) and have a look at it:
https://fetchcfd.com/view-project/39-Radial-Fan |
|
Thread Tools | Search this Thread |
Display Modes | |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
How to build current blower fan model in Flotherm | eric0722 | FloEFD, FloWorks & FloTHERM | 3 | January 2, 2021 02:36 |
Centrifugal fan as a momentum source | siw | CFX | 3 | August 20, 2015 05:48 |
Radial velocity and tangential velocity on centrifugal fan, | johnnyp | FLUENT | 2 | May 24, 2013 07:10 |
How to model flow of centrifugal fan? | Peter | Main CFD Forum | 0 | April 2, 2008 06:07 |
centrifugal pump and centrifugal fan | Mangesh | Main CFD Forum | 3 | January 3, 2006 11:21 |