CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Autodesk Simulation CFD

Ahmed Body Validation Study – Autodesk CFD

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   June 2, 2020, 22:38
Default Ahmed Body Validation Study – Autodesk CFD
  #1
New Member
 
Nik
Join Date: Jun 2020
Posts: 1
Rep Power: 0
Nik CFD is on a distinguished road
I am currently conducting a validation study on Autodesk CFD on the experimental work described in the following paper: https://www.researchgate.net/publica...ns_on_the_aero...


My computational model features a nearly identical setup to the one described in the paper. The only difference is that the paper suggests a slip boundary condition on the ground (bottom of the domain) upstream of the Ahmed body in order to achieve a boundary layer of a set thickness. I found that removing this slip boundary condition in Autodesk CFD helped to achieve the desired boundary layer thickness. Other prominent features of my computational setup are summarized below:

Domain Size (length/height/width): 15m/1.87m/1.4m
Ahmed Body: 25°
Boundary conditions: (1) inlet: velocity = 40 m/s (2) outlet: pressure = 0 Pa (3) Ceiling (top) and sides of the domain: slip/symmetry
Convergence: “tight”
Turbulence model: SST k omega
Boundary layer setup: number of layers = 15, layer factor = 0.8, layer graduation = 1.5, wall blending = on. (Please note: I have tried a variety of different setups but, this combination achieves the lowest y+ values).

Additionally, I have experimented with a variety of refinement boxes and refinement surfaces. I calculate my force values using Autodesk’s built-in wall calculator.


My “best” results are as follows:

1) A surface refinement is applied to the Ahmed body to decrease its element size by a factor 0.15 from the Autodesk’s baseline auto size. This corresponds to 4,468,821 fluid elements. This model achieved y+ values up to 2.3 with the majority of the Ahmed body being below a value of 1. Furthermore, the model achieved a drag force of 47.0 N and a lift force of 15.60 N. This corresponded to Cd of 0.424 and a Cl of 0.141

2) A surface refinement is applied to the Ahmed body to decrease its element size by a factor 0.25 from the Autodesk’s baseline auto size. Additionally, refinement is applied to the Ahmed body’s front and rear panels. This corresponds to 2,784,143 fluid elements. This model achieved y+ values up to 2.2 with the majority of the Ahmed body being below a value of 1 – this is better than the mesh setup discussed in best result #1. Furthermore, the model achieved a drag force of 46.3 N and a lift force of 14.3 N. This corresponded to Cd of 0.418 and a Cl of 0.128

3) Four refinement boxes were applied: 2 are in the streamwise direction to aid the transition from the wall layer to the rest of the domain and 2 are around the Ahmed body. No direct surface refinement was applied. This corresponds to 5,077,823 fluid elements. This model achieved y+ values up to 4.482 with the majority of the Ahmed body being above a value of 1. Furthermore, the model achieved a drag force of 48.3 N and a lift force of 7.53 N. This corresponded to a Cd of 0.435 and a Cl of 0.0679


I should also note that on the Autodesk CFD forum, an Autodesk technical expert provided a geometry file and computational setup. Running this provided geometry following his computational setup and guidance yielded even worse results (drag force = 75.8 N, lift force = 25.4 N, which corresponds to Cd = 0.684 and Cl = 0.228). The Autodesk technical expert states in his post that the forces will be on the high side but, the flow trends will remain the same. Link: https://forums.autodesk.com/t5/cfd-f...rofile.languag...


The experimental values presented in the paper stated above feature a Cd of 0.299 and a Cl of 0.345. Neither my work nor the work suggested by the Autodesk technical expert matches (or even comes close) to the target values.


Any suggestions on how to improve my simulation to match those target values would be greatly appreciated!
Nik CFD is offline   Reply With Quote

Old   July 22, 2020, 20:42
Default
  #2
Member
 
Join Date: Jun 2011
Posts: 79
Rep Power: 11
CFDfan is on a distinguished road
Quote:
Originally Posted by Nik CFD View Post
I am currently conducting a validation study on Autodesk CFD on the experimental work described in the following paper: https://www.researchgate.net/publica...ns_on_the_aero...


My computational model features a nearly identical setup to the one described in the paper. The only difference is that the paper suggests a slip boundary condition on the ground (bottom of the domain) upstream of the Ahmed body in order to achieve a boundary layer of a set thickness. I found that removing this slip boundary condition in Autodesk CFD helped to achieve the desired boundary layer thickness. Other prominent features of my computational setup are summarized below:

Domain Size (length/height/width): 15m/1.87m/1.4m
Ahmed Body: 25°
Boundary conditions: (1) inlet: velocity = 40 m/s (2) outlet: pressure = 0 Pa (3) Ceiling (top) and sides of the domain: slip/symmetry
Convergence: “tight”
Turbulence model: SST k omega
Boundary layer setup: number of layers = 15, layer factor = 0.8, layer graduation = 1.5, wall blending = on. (Please note: I have tried a variety of different setups but, this combination achieves the lowest y+ values).

Additionally, I have experimented with a variety of refinement boxes and refinement surfaces. I calculate my force values using Autodesk’s built-in wall calculator.


My “best” results are as follows:

1) A surface refinement is applied to the Ahmed body to decrease its element size by a factor 0.15 from the Autodesk’s baseline auto size. This corresponds to 4,468,821 fluid elements. This model achieved y+ values up to 2.3 with the majority of the Ahmed body being below a value of 1. Furthermore, the model achieved a drag force of 47.0 N and a lift force of 15.60 N. This corresponded to Cd of 0.424 and a Cl of 0.141

2) A surface refinement is applied to the Ahmed body to decrease its element size by a factor 0.25 from the Autodesk’s baseline auto size. Additionally, refinement is applied to the Ahmed body’s front and rear panels. This corresponds to 2,784,143 fluid elements. This model achieved y+ values up to 2.2 with the majority of the Ahmed body being below a value of 1 – this is better than the mesh setup discussed in best result #1. Furthermore, the model achieved a drag force of 46.3 N and a lift force of 14.3 N. This corresponded to Cd of 0.418 and a Cl of 0.128

3) Four refinement boxes were applied: 2 are in the streamwise direction to aid the transition from the wall layer to the rest of the domain and 2 are around the Ahmed body. No direct surface refinement was applied. This corresponds to 5,077,823 fluid elements. This model achieved y+ values up to 4.482 with the majority of the Ahmed body being above a value of 1. Furthermore, the model achieved a drag force of 48.3 N and a lift force of 7.53 N. This corresponded to a Cd of 0.435 and a Cl of 0.0679


I should also note that on the Autodesk CFD forum, an Autodesk technical expert provided a geometry file and computational setup. Running this provided geometry following his computational setup and guidance yielded even worse results (drag force = 75.8 N, lift force = 25.4 N, which corresponds to Cd = 0.684 and Cl = 0.228). The Autodesk technical expert states in his post that the forces will be on the high side but, the flow trends will remain the same. Link: https://forums.autodesk.com/t5/cfd-f...rofile.languag...


The experimental values presented in the paper stated above feature a Cd of 0.299 and a Cl of 0.345. Neither my work nor the work suggested by the Autodesk technical expert matches (or even comes close) to the target values.


Any suggestions on how to improve my simulation to match those target values would be greatly appreciated!
Deleted message

Last edited by CFDfan; July 25, 2020 at 17:43. Reason: use full blown solid model model (not a half) and you'll get quite different results
CFDfan is offline   Reply With Quote

Old   August 3, 2020, 12:08
Default
  #3
Senior Member
 
siara817's Avatar
 
siamak rahimi ardkapan
Join Date: Jul 2010
Location: Copenhagen, Denmark
Posts: 220
Rep Power: 14
siara817 is on a distinguished road
A question: Did you try K-epsilon as well?
__________________
Good luck
Siamak
siara817 is offline   Reply With Quote

Old   September 14, 2020, 17:12
Default
  #4
New Member
 
Mike Stroup
Join Date: Sep 2011
Posts: 12
Rep Power: 11
Mithrandir is on a distinguished road
Wow.....

<crickets>

Bueller..... Bueller??
Mithrandir is offline   Reply With Quote

Old   September 21, 2020, 02:00
Default very good
  #5
New Member
 
AL
Join Date: Sep 2020
Posts: 1
Rep Power: 0
hannahberry is on a distinguished road
I think the problem with which your article came up makes perfect sense. We have helped me quite a lot in finding related information.
geometry dash
hannahberry is offline   Reply With Quote

Old   September 28, 2020, 14:40
Default
  #6
New Member
 
Apolo
Join Date: Jul 2009
Posts: 18
Rep Power: 13
ApoloV is on a distinguished road
@Nik CFD
A bit of a long read but some background and notes that should help

When we've done ahmed body we should be able to get within 10% on the Drag Coefficient.

As you noted y+ and mesh quality will be critical here. What we offer in the interface is just 1-15 boundary/wall layers as most general purpose users will fall in that range for their needs.

For advanced users, or those going more in to validation studies like this we do offer methods for increasing mesh control.
These are done by using flags to the specific scenario.
The Flag Manager is found under the Design Study Tools drop down menu

mesh_enhance_layers allows you to add any number of wall layers. For example in doing a NACA0012 validation we found that a minimum of 30 layers was required, with 60 layers correlating better to published test data.

mesh_enhance_thick is an overall thickness multiplier in the event you need the total thickness to be larger than the UI limited 1.2
Again in that NACA 0012 validation with a nominal thickness (in UI) of ~0.6, we leveraged a thickness multiplier of 400%

Additionally, depending on the version you're using will impact this next statement.


The forum post referenced was from 2012 using CFD 2013. At that time we did not have any SST turbulence models. Running RNG, or K-e would have been the norm and using Mesh adaptation to try and improve the mesh quality while staying within y+ limits of the turbulence models.

Since then we've had a number of solver changes both on turbulence models as well as advection schemes. I didn't run the file linked in v2013 but at that time I wouldnt doubt that James did get a decent correlation. Sadly he didn't post specific numbers. That said it's a bit hard to take his file and run with today's solver as his was tuned based on the solver from 2013. While overall the approach can still work there will be changes that need to be done, especially given his RNG run and if you used those same settings for SST

In CFD 2015 we introduced a variant of SST with Hellsten curvature correction. This in 2015 was flag driven but later became a selectable turbulence model from the Interface. This can better predict the separation on the rear of the ahmed body and does help further improve drag results.
Result Image - https://a360.co/2HOsFrl

Last edited by ApoloV; October 5, 2020 at 11:07. Reason: add image
ApoloV is offline   Reply With Quote

Reply

Tags
ahmed body, autodesk cfd, drag coefficient, mesh

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
Pump CAD + experimental data for CFD verification study bemism Main CFD Forum 0 July 20, 2017 16:30
Ahmed body 2D -Questions about mesh independence, Y plus value and others treviusss FLUENT 0 July 6, 2017 08:52
ICEM Ahmed Car body Parms ANSYS 1 December 22, 2016 22:19
CFD Study of a Diffuser lemat1 Main CFD Forum 9 December 7, 2009 08:45
Starting Point to study CFD and code writing Lynn Main CFD Forum 3 November 23, 2005 05:31


All times are GMT -4. The time now is 01:28.