CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > ANSYS Meshing & Geometry

Vehicle aerodynamics-Flow analysis

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

Like Tree1Likes
  • 1 Post By MachZero

Reply
 
LinkBack Thread Tools Display Modes
Old   July 10, 2013, 11:15
Default Vehicle aerodynamics-Flow analysis
  #1
New Member
 
Anand
Join Date: Jul 2013
Location: India
Posts: 9
Rep Power: 3
Anand Sis is on a distinguished road
Hi everyone...
I've been trying to model the flow around a car with an aim to determine the aerodynamic lift and drag induced and the local velocity near the rear of the vehicle(almost at a point where the leading edge of a spoiler will come) to a fair level of accuracy.
I tried to add prism layers around the vehicle body and near the ground...I've attached the screenshot of the settings i gave...plus the rough mesh i got without the prism layers
My problem is that am not able to generate the prism layers as ANSYS Meshing seems to freeze after sometime but it doesn't crash

I've tried running it for hours but its still frozen ...it seems to get stuck at "Modelling interior for part"...
Any reason that anyone might know ?..i don't think its because of my low end system...coz its not using more than 2.5GB of my system memory(I got 8gigs) !
Attached Images
File Type: jpg ANSYS settings.jpg (52.0 KB, 20 views)
File Type: jpg mesh.jpg (106.0 KB, 32 views)
File Type: jpg mesh close.jpg (99.6 KB, 27 views)
Anand Sis is offline   Reply With Quote

Old   July 11, 2013, 02:27
Default
  #2
siw
Senior Member
 
Stuart
Join Date: Jul 2009
Location: Portsmouth, England
Posts: 435
Rep Power: 12
siw is on a distinguished road
Are you using the pre prism generation, rather than the post prism generation? If so you could then preview the prism mesh (before it makes the volume filling tetrahedral elements). This might help in working towards solving your mesh issue. I cannot recall if this works of the first aspect ratio optio but you ould change to smooth transition or first layer height, for instance.
siw is offline   Reply With Quote

Old   July 11, 2013, 07:20
Default
  #3
Member
 
Join Date: Aug 2011
Posts: 49
Rep Power: 5
MachZero is on a distinguished road
Ansys meshing is super finicky and super buggy. I have loads of problems with it. What version are you using? V 14.5 was supposed to be worlds better but I noticed in 14.5.7 all sorts if bugs and freeze ups. When I have these issues I delete the meshing cell and start from scratch. Then as I'm rebuilding I has controls one at a time and mesh. This helps to find the problem. It wouldn't surprise me if there was a bug in their code that wasn't happy because you has 3 face sizings in a row. I've had a bug caused by something similar.

By the way, why are you modeling the interior?
MachZero is offline   Reply With Quote

Old   July 11, 2013, 09:04
Default
  #4
Far
Super Moderator
 
Far's Avatar
 
Sijal Ahmed Memon (turboenginner@gmail.com)
Join Date: Mar 2009
Location: Islamabad Pakistan
Posts: 3,885
Blog Entries: 6
Rep Power: 37
Far will become famous soon enoughFar will become famous soon enough
Send a message via Skype™ to Far
Try ICEM CFD it is much faster and robust along with Tgrid.
Far is offline   Reply With Quote

Old   July 11, 2013, 12:16
Default
  #5
New Member
 
Anand
Join Date: Jul 2013
Location: India
Posts: 9
Rep Power: 3
Anand Sis is on a distinguished road
Quote:
Originally Posted by MachZero View Post
Ansys meshing is super finicky and super buggy. I have loads of problems with it. What version are you using? V 14.5 was supposed to be worlds better but I noticed in 14.5.7 all sorts if bugs and freeze ups. When I have these issues I delete the meshing cell and start from scratch. Then as I'm rebuilding I has controls one at a time and mesh. This helps to find the problem. It wouldn't surprise me if there was a bug in their code that wasn't happy because you has 3 face sizings in a row. I've had a bug caused by something similar.

By the way, why are you modeling the interior?
@MachZero. Am using V14.0 and yes i used 2 face sizings. I had actually followed a video tutorial from youtube where an Ahmed body had been meshed using a similar approach flawlessly. I had considered mine as a simple geometry and assumed it would work. I guess it was not that simple for Ansys meshing after all !!
And regarding the interior, i was trying to include the volume of fluid between the wheel arch and the tires as well...i guess that's what u meant ? May be that small volume had been creating problems for me
Anand Sis is offline   Reply With Quote

Old   July 11, 2013, 12:45
Default
  #6
New Member
 
Constantine
Join Date: Jun 2013
Posts: 4
Rep Power: 3
ConstantineTheGreat is on a distinguished road
Quote:
Originally Posted by Anand Sis View Post
I've been trying to model the flow around a car with an aim to determine the aerodynamic lift and drag induced and the local velocity near the rear of the vehicle(almost at a point where the leading edge of a spoiler will come) to a fair level of accuracy.
If you want to simulate the flow around a car why you build a mash inside a vehicle and its wheels?
Try to exclude the interior of the vehicle from the area calculation
ConstantineTheGreat is offline   Reply With Quote

Old   July 11, 2013, 12:53
Default
  #7
New Member
 
Anand
Join Date: Jul 2013
Location: India
Posts: 9
Rep Power: 3
Anand Sis is on a distinguished road
Quote:
Originally Posted by ConstantineTheGreat View Post
If you want to simulate the flow around a car why you build a mash inside a vehicle and its wheels?
Try to exclude the interior of the vehicle from the area calculation
I tried to include the volume of air between the wheel arch and the tires as i sd. The mesh you see doesn't include the entire wheels. That's how it should be..right ?
Anand Sis is offline   Reply With Quote

Old   July 11, 2013, 13:57
Default
  #8
Member
 
Join Date: Aug 2011
Posts: 49
Rep Power: 5
MachZero is on a distinguished road
I think I misunderstood the image you showed. You have a symmetry model and this is a side view, isn't it? I was under the impression you tried to mesh the volume of the interior of the car. My
Mistake.
One thing I have noticed is that sometimes inflation can't run ansys meshing into the ground as it appears to have done to you. It looks like you have a very fine mesh around the tires. I bet this is where meshing messes up. Please try placing a coarse mesh on the wheel, and all over, then try. If that works you can reduce the mesh size from there
Anand Sis likes this.
MachZero is offline   Reply With Quote

Old   July 22, 2013, 06:24
Smile
  #9
New Member
 
Anand
Join Date: Jul 2013
Location: India
Posts: 9
Rep Power: 3
Anand Sis is on a distinguished road
Thanks everyone for your replies. I had found out the cause of the error. It was a problem with my geometry, where the wheels met the bottom surface. The lowest part of the tires had a very small angle between them and the ground,because of which prism layers could not be generated.The solution adopted for this was cutting the lowest part of the tire using design modeler four millimeters over the surface. Then, the tire was extruded on the Z direction(vertical) connecting the tire and the ground and then the prisms could be generated.
Anand Sis 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
Review: Reversed flow CRT FLUENT 0 July 20, 2012 13:03
Steps for analysis of a flow rskrishna87 CFX 15 February 1, 2011 11:08
Can 'shock waves' occur in viscous fluid flows? diaw Main CFD Forum 105 November 20, 2009 04:19
how to do this blade passage flow analysis ? manish CFX 2 January 16, 2006 03:58
Coolant flow analysis - IC engine Frank FLUENT 2 May 19, 2002 15:59


All times are GMT -4. The time now is 17:28.