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

 March 25, 2013, 15:04 Freewheeling radial fan #1 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 7 I am simulating a freewheeling fan using the frozen rotor model. The goal is to compare the messured static pressure rise and the torque in dependence of the volume flow. The model has an inlet tube to the opening of the fan. The massflow is set at this boundary. the fan has a big sourounding cylindrical volume so that the flow can expand. while the shroud has a diameter of about D the sourounding volume has a diameter of about 4xD. The boundary faces of the sourounding volume are set as "openings with static pressure =0, entrainement and zero gradient turbulence". When comparing the results of pressure and toruqe with experiment it is obvious that the calculated results are a factor of 2 to small (pressure and torque). In Post you can see that the fan tries to suck and drag a lot of sourounding air with itself. We checked all the physic settings the pressure, y+ is between 25 and 100, sst-turbulence, etc.. Even the mesh independence check did not show any significant changes. Could it be that the openings are still to close to the happening scene or is there anything else anybody observed trying to run a freewheeling fan? Thanks in advance!

 March 25, 2013, 18:17 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 Are you sure the rotor is being compared to the experiment properly - has it settled down to a steady state?

 March 26, 2013, 15:08 #3 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 7 The flow starts in a big box and is suced into the fan at the top of the box. The static pressure in the box is measured using drilled holes in the walls. The pressure distribution in the box is pretty homogeneous (only very small variation). Officialy the flow is is transient! ;-) but... we calculated for a big number of iterations and the pressure monitor shows a periodic behaviour around and averag value. but the variation of the pressure never gets into the range of the expected experimental value. Also if we compare the calc. torque with the experimental value we get a torque that is abou 30% too small. From my understanding this means that we have to less pressure losses in the fan (right?). Could wallfriction cause such a big difference? Are there any other big influences that could be caused by the turbulence models and would improve the description (for example curvature correction,...)? I appreciate any idea!

March 26, 2013, 17:52
#4
Super Moderator

Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 13,808
Rep Power: 107
Quote:
 Could wallfriction cause such a big difference?
Yes, absolutely.

This is an FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

 March 27, 2013, 14:26 #5 Member   Benny Join Date: Apr 2012 Posts: 40 Rep Power: 7 Today we ran a simulation using a sand roughness of 1mm (pretty rough wall ;-). We could observe an increase of the torque and the pressure drop that is in the order of the missing pressure difference. But we will also have a look again into the mesh because the curvature of the blades is pretty big so strong separations could be possible. Ansys support told me that especially the "exit flow" of the fan and the "sourrounding volume" is pretty important. They observed that it could be possible that some closer details like walls must be modelled to get the correct exitflow. We also try to run a laminar turbulence transition calculation. Quick handcalculation shows that 30% of laminar flow could be possible.

 March 27, 2013, 17:52 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 13,808 Rep Power: 107 If the flow is 30% laminar and presumably 70% turbulent then you might want to consider the transitional turbulence model. There is no laminar rough wall model, for a laminar flow you have to model the bumps directly to get a rough wall model.

 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 seza FLUENT 2 December 27, 2013 04:52 r.sirait ANSYS Meshing & Geometry 3 June 4, 2012 01:57 fidan FLUENT 3 March 6, 2008 21:42 Paal Main CFD Forum 3 August 5, 2002 05:12 Alan Davis Main CFD Forum 7 April 24, 2001 12:15

All times are GMT -4. The time now is 18:59.