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

Wind Tunnel Setup

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 15, 2011, 21:58
Default Wind Tunnel Setup
  #1
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 6
aerospace_guy_ is on a distinguished road
Hi All,

I've tried to find a solution for my problems in the tutorials and documentation, but I can't seem to find anything which I can apply to this situation.

I have created our solar car aero-shell in Solidworks, and created a tunnel around it. for these tests the car has no wheels so it is floating 12cm from the bottom of the tunnel. I've attached a picture of my mesh setup to clarify this. I realize the mesh is not as dense as it should be, but these are simply my initial tests.

The domain has been created using a composite of the two 3D regions, the car, and the tunnel. the inlet speed is 25m/s, the outlet is 0 static pressure. The walls are free-slip, the ground is a no-slip wall moving at 25m/s and the car is a no-slip wall. I am using the k-epsilon turbulence model.

I am using local parallel solution with 7 threads. when I try to run the solution the solver stops with the following error:
2 isolated fluid regions were found in domain composite

I figured it simply didn't like the fact that the car was separate from the ground, so I tried using an expert parameter to skip checking for isolated domains. when I did this I was presented with the following error:
Error interpolating results onto the new mesh

I have obtained results by doing the blunt body tutorial, with my geometry cut in half along the plane of symmetry substituted in, so I suspect my problem lies in not setting up the separated car correctly.

any help would be much appreciated. please let me know if you require more information from me.
Attached Images
File Type: jpg Car with mesh.jpg (31.5 KB, 44 views)
File Type: jpg tunnel view.jpg (34.5 KB, 39 views)
File Type: jpg CFX-pre setup.jpg (34.7 KB, 38 views)
aerospace_guy_ is offline   Reply With Quote

Old   February 16, 2011, 06:04
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Firstly a minor point: I would recommend using the SST turbulence model. It has superseded the k-e model for many types of flow and I think this is one flow which would benefit from it.

Secondly a major point: The isolated fluid regions error means you have mesh regions which are not connected. This means you have a meshing error to fix. It is not the floating car, somewhere in your mesh is a region of mesh which is not connected to the rest of the mesh. This is a major problem and you MUST fix it.

Let me guess - have you meshed the region inside the car? If so you have to delete this region as it will not be connected.

Finally, a minor point: Your geometry is symmetric and the flow is likely to be symmetric too. Might as well chop it in half and use a symmetry plane.
ghorrocks is offline   Reply With Quote

Old   February 16, 2011, 17:31
Default
  #3
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 6
aerospace_guy_ is on a distinguished road
Thanks for your quick reply!

I've taken a look through the documentation I have regarding volume mesh generation today. I still can't seem to figure out how to tell CFX-mesh not to mesh inside the car, or how to go about deleting the part of the volume mesh inside the car.

in regards to the symmetrical flow, I know this test is symmetrical, and as I have run the simulation using a plane of symmetry. however, once I figure out how to run the car like this, I will be analyzing versions of the car which includes asymmetrical intake duct placement.

thanks for the tip regarding k-epsilon turbulence, I'm fairly new to CFD and I was using it because a friend of mine said it gave fairly accurate results.
aerospace_guy_ is offline   Reply With Quote

Old   February 16, 2011, 20:38
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
If you have modelled the vehicle as surfaces then you will have isolated mesh regions inside the car. Instead you want to cut the vehicle out of the block, so the vehicle is a void. This is how the blunt body mesh is made.

SST turbulence model will also allow you to use the turbulence transition model. For accurate drag prediction on a body like this you might need it as I suspect the transition points on your vehicle could be a fair way back from the front and therefore the laminar flow region is significant.
ghorrocks is offline   Reply With Quote

Old   February 16, 2011, 23:48
Default
  #5
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 6
aerospace_guy_ is on a distinguished road
Thanks so much for your help! the solver is running now. The solution looks like it's converging, but we'll have to see in a few hours how it does.

I noticed you were from Australia, I don't know if you're interested in solar car racing at all, but this car will actually be racing in the World Solar Challenge from Darwin to Adelaide in October.
aerospace_guy_ is offline   Reply With Quote

Old   February 17, 2011, 21:51
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The solar car race gets national news coverage here. I am not personally involved with it at all, but I watch it on the news.
ghorrocks is offline   Reply With Quote

Old   February 18, 2011, 00:06
Default
  #7
Senior Member
 
Joshua Counsil
Join Date: Jul 2009
Location: Halifax, Nova Scotia, Canada
Posts: 366
Rep Power: 9
Josh is on a distinguished road
Steve -

Are you from Calgary U?
Josh is offline   Reply With Quote

Old   February 18, 2011, 17:31
Default
  #8
New Member
 
Steven
Join Date: Feb 2011
Location: Calgary, Canada
Posts: 13
Rep Power: 6
aerospace_guy_ is on a distinguished road
Thanks again for all your help. I've been able to run some simulations. the results are quite different than the simulations we ran last year, however the last results were obtained on a computer running FLUENT. Do you know how the results from CFX and FLUENT might differ. As far as I can tell the domain set up and turbulence models are the same, the mesh sizing is similar in both cases, but CFX is giving me drag numbers which are 14% lower than that which we obtained in FLUENT.

lastly, I've been trying to use the function area_z()@Car to find the cross-sectional area of the car for Cd calculation. The z axis is perpendicular to the front of the car, but when I use this to find the area, I get areas which are on the order of 10^-10 m^2. It works fine for the inlet and outlet, returning 25m^2 for both. Do you know what I might be doing wrong?

@Josh, yes I am from the UofC
aerospace_guy_ is offline   Reply With Quote

Old   February 21, 2011, 01:30
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Both CFX and Fluent should converge on the correct answer. There is no systematic bias in either code, or one would be more "accurate" than the other and the less "accurate" one would go out of business very quickly.

I suspect the difference you are seeing is in regards to the turbulence model. Did both models use the same turbulence model?
ghorrocks 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
how to setup 3d wind tunnel bukm CD-adapco 9 December 13, 2014 16:06
wind tunnel results vs fluent pixie Main CFD Forum 1 August 20, 2009 08:02
how to consider perforated wind tunnel wall in CFD simulation littlelz CFX 4 June 11, 2009 05:51
Virtual Wind Tunnel in FLUENT ND FLUENT 0 April 7, 2006 07:43
Wind tunnel modeling Pandu CFX 3 May 19, 2003 21:49


All times are GMT -4. The time now is 20:40.