# Axial fan simulation problems

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

April 12, 2015, 17:11
Axial fan simulation problems
#1
New Member

Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 4
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
 1.JPG (25.1 KB, 25 views) 3.JPG (38.8 KB, 22 views) 5.jpg (39.7 KB, 27 views) 6.JPG (60.3 KB, 24 views)
Attached Files
 Solver.docx (64.9 KB, 12 views)

 April 12, 2015, 18:13 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,456 Rep Power: 104 This looks like an FAQ: http://www.cfd-online.com/Wiki/Ansys...gence_criteria

 April 13, 2015, 04:00 #3 New Member   Bartosz Join Date: Apr 2015 Posts: 8 Rep Power: 4 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?

 April 13, 2015, 06:10 #4 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,456 Rep Power: 104 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.

April 13, 2015, 07:15
#5
New Member

Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 4
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
 CFX.png (51.3 KB, 31 views)

 April 13, 2015, 07:26 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,456 Rep Power: 104 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.

April 13, 2015, 08:00
#7
New Member

Bartosz
Join Date: Apr 2015
Posts: 8
Rep Power: 4
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
 7.jpg (50.6 KB, 24 views) 8.jpg (43.7 KB, 17 views) 9.jpg (51.2 KB, 14 views) 10.jpg (50.0 KB, 16 views) 11.jpg (52.6 KB, 11 views)

Last edited by adinacatslowo; April 13, 2015 at 10:56.

 April 13, 2015, 18:08 #8 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,456 Rep Power: 104 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.

 April 13, 2015, 18:25 #9 New Member   Bartosz Join Date: Apr 2015 Posts: 8 Rep Power: 4 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?

 April 15, 2015, 05:54 #10 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,456 Rep Power: 104 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.

 April 16, 2015, 02:52 #11 New Member   Bartosz Join Date: Apr 2015 Posts: 8 Rep Power: 4 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.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post chaudhry_hashim STAR-CCM+ 0 June 27, 2014 08:59 idiroft CFX 5 June 10, 2014 07:34 acoustica CFX 8 April 24, 2014 03:44 mariconeagles96 CFX 4 April 18, 2012 08:41 Teng_YJ FLUENT 2 February 16, 2009 20:37

All times are GMT -4. The time now is 17:48.