CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Axial fan simulation problems

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 12, 2015, 17:11
Default Axial fan simulation problems
  #1
New Member
 
Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 3
adinacatslowo is on a distinguished road
Hello everyone

Currently I'm dealing with some problems during the axial fan simulation. My task is to remodel existing fan, working in coal mine - here it is: http://www.grupamarat.pl/eng/marat/fans/ to obtain characteristics that the mine wants. First I want to obtain the characteristic of the working fan and then optimize it to get new one.
Since it is a pretty large model I decided to simulate it with periodic (one passage). To have an equal arrangement of the pressure at the outlet I decided to move it about 6 diameters after the diffuser.
The problem is that the total pressure, static pressure fluctuates between 4400 and 4600 Pa like on the attached pictures, and the dynamic pressure is constantly rising. I have made 1000 itterations and the pressure doesn't stabilize. I don't know what I'm doing wrong, so if you can help I would be very grateful.
Attached Images
File Type: jpg 1.JPG (25.1 KB, 24 views)
File Type: jpg 3.JPG (38.8 KB, 21 views)
File Type: jpg 5.jpg (39.7 KB, 26 views)
File Type: jpg 6.JPG (60.3 KB, 23 views)
Attached Files
File Type: docx Solver.docx (64.9 KB, 11 views)
adinacatslowo is offline   Reply With Quote

Old   April 12, 2015, 18:13
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
This looks like an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria
ghorrocks is offline   Reply With Quote

Old   April 13, 2015, 04:00
Default
  #3
New Member
 
Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 3
adinacatslowo is on a distinguished road
Is it possible that I get those oscilations of pressure because I'm doing calculations only on one passage (1/10 part of engine and rotor and 1/12 part of stator and difusser?
adinacatslowo is offline   Reply With Quote

Old   April 13, 2015, 06:10
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
If this is a steady state/frozen rotor simulation (which it appears to be) then no.

I think the FAQ describes the best approach - make sure your mesh is good, your convergence tight enough. You might need to use larger time steps or the other tricks in the FAQ.

Also I see you are using 4 domains. What are the 4 domains? An image of your model would be useful.
ghorrocks is offline   Reply With Quote

Old   April 13, 2015, 07:15
Default
  #5
New Member
 
Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 3
adinacatslowo is on a distinguished road
I attached the picure of the model. I didn't feat on one page, so my model has 5 dotains (engine, rotor, stator, difusser and the longrst one the extension)
I tried to simulate on bigger timescale factor (5) but it's still oscilating. I'm using Auto timescale and it is 0,1/w
If it come to the mesh I know that the rotor and stator should have pretty thick mesh, but on the other domains I use mesh with max element size 15 mm + inflation on the wall (7 layers, first layer 2 mm, growth rate 1.1)
Attached Images
File Type: png CFX.png (51.3 KB, 29 views)
adinacatslowo is offline   Reply With Quote

Old   April 13, 2015, 07:26
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Why 5 domains? Shouldn't it be 3? That is a stationary inlet and outlet domain and a rotating domain in the middle? Extra domains just means extra interfaces and you want to minimise them.

Please post an image of your mesh.
ghorrocks is offline   Reply With Quote

Old   April 13, 2015, 08:00
Default
  #7
New Member
 
Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 3
adinacatslowo is on a distinguished road
I used 5 domains so I can each domain mesh independently.
Edit
But I think I can minimaze it by merging difusser and extension together 4 domains are the absolute minimum
Attached Images
File Type: jpg 7.jpg (50.6 KB, 22 views)
File Type: jpg 8.jpg (43.7 KB, 17 views)
File Type: jpg 9.jpg (51.2 KB, 14 views)
File Type: jpg 10.jpg (50.0 KB, 16 views)
File Type: jpg 11.jpg (52.6 KB, 11 views)

Last edited by adinacatslowo; April 13, 2015 at 10:56.
adinacatslowo is offline   Reply With Quote

Old   April 13, 2015, 18:08
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your mesh quality is not very good:

* There is a big jump in mesh size from the inflation layers to the volume mesh. You should make mesh size continuous from the inflation layers to the volume mesh.
* You appear to have meshed a face and swept it around. This works well for your annular regions, but for the regions which go to the rotation axis means you get horrible quality elements near the axis. For domains which extend to the axis this annular sweep mesh is not a good choice, better to use a normal 3D mesh.
ghorrocks is offline   Reply With Quote

Old   April 13, 2015, 18:25
Default
  #9
New Member
 
Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 3
adinacatslowo is on a distinguished road
Thanks for the advise I will try to apply then and see what results I get.
If it comes to the mesh of those "big" domains like engine and diffuser what would be the min lenght of the element and first layer of inflation to get good results. Is there any good rule or practice for this?
adinacatslowo is offline   Reply With Quote

Old   April 15, 2015, 05:54
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,838
Rep Power: 100
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Read the documentation on advice for flow modelling. It has good tips on this area. But remember that a lot of these issues are problem dependant so it is best if you test it yourself on your model to determine whether it is an issue for you or not.
ghorrocks is offline   Reply With Quote

Old   April 16, 2015, 02:52
Default
  #11
New Member
 
Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 3
adinacatslowo is on a distinguished road
I had made some improvements in the mesh quality (sweep, inflation, and size of the mesh outlet/inlet so that face mesh on the two domains next to each other would have almost the same size) and the results are much better (there is still a little oscilation on the pressure but only around 50 Pa from 300th iteration to the end - almost nothing if the fan gives around 4600 Pa.
I still can't get the convergance but I this its because I'm doing Steady-State (my computer won't handle Transient) or I'm not calculating the optimal point of the fan.
adinacatslowo is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Fan simulation with inlet and outlet duct chaudhry_hashim STAR-CCM+ 0 June 27, 2014 08:59
Fan flow simulation in open air idiroft CFX 5 June 10, 2014 07:34
Thrust in Axial flow fan for different inlets acoustica CFX 8 April 24, 2014 03:44
Axial fan or blower cooling a hot object with recirculation mariconeagles96 CFX 4 April 18, 2012 08:41
Propeller Fan Curve Simulation Teng_YJ FLUENT 2 February 16, 2009 20:37


All times are GMT -4. The time now is 12:15.