CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > FloEFD, FloWorks & FloTHERM

Car external aerodynamic with wheel spinning issue

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 15, 2016, 13:58
Default Car external aerodynamic with wheel spinning issue
  #1
Member
 
Join Date: Nov 2014
Posts: 79
Rep Power: 7
hokhay is on a distinguished road
Hi all, I am now to FloEFD and vehicle aerodynamic simulation. I am trying to compute lift and drag for a car with wheel spinning. I use local region averaging method to simulate wheel spin. The rotation region is slightly larger than the wheel, so its boundary sits between wheel arch and the wheel.

The result that I get is very different from the result I got with simple closed wheel with rotating wall instead of local region rotation. I have noticed the pressure difference between inside and outside of the rotating region is very large, especially at location where air flow is tangential to the rotating region.

https://www.dropbox.com/s/2mz6s4t7cdtx2lv/Preview%20wheel%20centre.bmp.bmp?dl=0
https://www.dropbox.com/s/ac0zh7p0ll...x.bmp.bmp?dl=0


Could anyone tell me what have I done wrong? What is the best method for wheel spin simulation please?

Thank you
Jason

Last edited by hokhay; May 16, 2016 at 04:23.
hokhay is offline   Reply With Quote

Old   May 23, 2016, 04:48
Default
  #2
New Member
 
A. Lindgren
Join Date: Feb 2016
Posts: 6
Rep Power: 5
Vejby is on a distinguished road
The "averaging" approach for rotating regions is not really suitable for this case. It is only good when the flow is mainly axis-symmetric.
The "sliding" approach is better in this kind of case, but unfortunately a lot more demanding also.
Vejby is offline   Reply With Quote

Old   August 18, 2016, 05:23
Default
  #3
Senior Member
 
Boris Marovic
Join Date: Jul 2009
Posts: 584
Rep Power: 18
Boris_M will become famous soon enough
Hi,

It depends how the rotating region is setup and the flow is entering the rotating region.

But first to your setup of the rotating region.
The rotating region in general should not only tough a surface of enter into a stator surface that is not fully rotational around the body. In your case I cannot fully tell if the upper part of the rotating region in your first image is just touching the fender, if it has a tiny gap or if it reaches into it. Either way, it is not ideal to set it up this way.
The best setup you can do is to create the rotating region in the way that it cuts through the rubber. It is only important to have the spokes of the rims inside the region as they are not a disc or a cylinder but like fan blades. Every fully rotated surface without any holes or gaps in it over its 360° rotation can be modeled with the rotating wall. As soon as you have ribs or fan blade like extrusions from the center going out or anything that is not a rotated wall, it should be included in the rotating region. The only exception is that it has to rotate. If a stator wall such as the road or the fender is reaching in it but not rotating ad is not a 360° rotated wall like a duct of a ducted fan, it should not reach into the region.

The reason for the rotating wall is that it basically applies a moving boundary layer instead of moving the wheel. If a duct of a ducted fan (so the shroud) is reaching into the rotating region, you can simply apply stator wall to it and fix the boundary layer instead of having it moving. But this does not work for single protrusions into the rotating region that are not rotating such as the street or the fender. The rotating or stator wall are only influencing the boundary layer, this is a valid approach for a rotating cylinder wall such as the outer wheel surface that touches the street. But the street should not be inside the rotating region as it does not actually rotate and the stator would only freezes the boundary layer but still rotate the protrusion of the street into the rotating region. If it is a duct for a ducted fan, it doesn’t matter if the geometry of the duct wall is rotated as it is a 360° fully in the rotating region and not a single sided protrusion. If the walls are defined as stator then the fluid velocity is zero there and everything is fine.


If you create the rotating region that it cuts into the rubber and therefore only includes not 360° fully rotated geometries that actually rotate, then you can use the rotating wall for all the 360° rotated surfaces that actually do rotate and are not included or partially included in the rotating region to apply the rotation of the boundary layer. This then will solve the pressure issue you are having.

The other thing is that the averaging plane approach works only if you have axial or radial flow. The flow in radial direction should be over the circumference the same. The reason is that this approach averages the flow over the circumference and therefore a flow like in this case of a car would enter the cylindrical surface on one side and exit on the other side and if you average +5m/s on the one side and -5m/s on the other you would get 0m/s (to put it simple). So this approach will not work for tangential flow, only the axial or radial flow if averaging in radial direction is not causing any errors which it does in your case.

If your rim would sit in the middle of the wheel, you could use a rotating region that does not extend over the wheels from and rear surface and only includes the rim so that there is only the possibility to flow axial but in your case the rim is slightly outside of the outer wheel side. Maybe the error is small but it is not ideal.
I attached an image with a highlighted rotating region as you should apply it and apply all the other surfaces that are not inside the rotating region as well as those who cut the rotating region with a rotating wall.

The sliding mesh is now basically rotating the actual geometry and the limitation of only axial or radial flow does not apply, but the limitation of the size of the rotating region and not intersecting stator protrusions into it does still apply. Otherwise you would see the bit of the road entering the rotating region actually rotating around the wheel as if cut off at the rotating region boundary and glued to the wheel while it is rotating around the center.
However as already mentioned by Vejby, it is computing intense as you need to do it in transient. This sliding mesh is by nature a transient simulation.

I hope this helps,
Boris
Attached Images
File Type: jpg example.jpg (112.7 KB, 25 views)
Boris_M is offline   Reply With Quote

Reply

Tags
car aerodynamics, wheels

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] External mesh crawls into car model. Holes in STL model? MadsR OpenFOAM Meshing & Mesh Conversion 8 October 26, 2013 11:21
error while solving external aerodynamics Praveenreddy FLUENT 0 December 6, 2007 21:44
External Flow Prediction around a Car Body S. Main CFD Forum 5 June 5, 2007 23:40
Please help about car body aerodynamic analysis Tayfun Toraman FLUENT 2 November 30, 2004 09:52
Aerodynamic analysis of car Vikas Kumar Main CFD Forum 3 April 10, 2003 16:15


All times are GMT -4. The time now is 07:24.