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

Changing inflow velocity direction deteriorates lift and drag

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 23, 2013, 07:28
Default Changing inflow velocity direction deteriorates lift and drag
  #1
Member
 
Bart A.
Join Date: Feb 2012
Posts: 45
Rep Power: 5
ziggo is on a distinguished road
I'm running a 3D simulation in Fluid and have found that when I change the inflow velocity direction my results are terrible.
I have a three dimensional wedge in a spherical domain. From the side it looks as in image 1. Image 1 also shows the how the domain is meshed.
This situation gives me acceptable lift and drag results w.r.t. the wind tunnel data I have.

Image 1:


When I change the inflow velocity direction the error from the CFD simulation grows w.r.t. the windtunnel data.

If I change the inflow direction for example to the direction shown in image 2 the difference between the CFD and the data is around 20%.

Image 2:



If I change the direction even more, the error becomes larger.

I define the velocity on the velocity-inlet using xyz-components. For the first image this is
Code:
x = 0, y = 0, z = -26
and for the second image this is
Code:
x = 0, y = =8.9, z = -24.4
I also make sure that Fluent calculates the CL and CD values with the correct direction vectors. So for the first image the CL components are:
[CODE]
x = 0, y = 1, z = 0
[\CODE]
And for the second image the CL components are:
[CODE]
x = 0, y = 0.94, z = -0.34
[\CODE]

How can I make sure that for every velocity direction I get reasonable results as in the situation shown in image 1? Do I need to rotate the geometry instead, re-mesh and keep the velocity parallel to the z-axis?
ziggo is offline   Reply With Quote

Old   July 23, 2013, 13:11
Default
  #2
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
Do you really have measurement data for arbitrary angles of attack for the wedge?
What happens if you turn the wedge instead of changing the inflow direction?
How did you validate the results for the zero AoA case? Grid dependency study performed?
Is the flow turbulent? If yes, which kind of turbulence model and wall function do you use?
How about the pressure outlet? Imagine you change the angle of attack to 90, then only half of the geometry gets an inflow velocity which clearly doesnt correspond to an undisturbed flow. Consider a free stream boundary or a velocity BC for the whole outer boundary instead.
flotus1 is offline   Reply With Quote

Old   July 24, 2013, 08:24
Default
  #3
Member
 
Bart A.
Join Date: Feb 2012
Posts: 45
Rep Power: 5
ziggo is on a distinguished road
- Yes, I have wind tunnel data for the wedge from 10 to 55 degrees of attack for every 5 degrees. Image 1 shows the 55 degree angle of attack situation.
It's actually one element of a tetrahedral kite (the image shows 4 elements). From the side it looks like a wedge.

This image show show I defined the angle of attack alfa:


- I haven't tried this yet as this means I have to re-mesh everything again. This costs more time than changing the inflow direction.

- The zero AoA case is actually the 55 degree AoA case shown in image 1. I did a grid convergence study with four different mesh sizes and found that increasing the number of cells after a certain threshold only changed my force coefficients by ~1%. So I used the threshold mesh.

- Yes the flow is turbulent. I use the standard k-epsilon model.

- The 90 degree case would indeed cause a problem, but as I will not be using that case I thought I would be OK with a pressure outlet.
I'm not familiar with other boundary conditions so I'll investigate those.

- The flow simulations for all the cases where the flow was not coming straight from the left did not converge because the residual for the continuity did not go down. Also I kept receiving messages that there was a reversed flow in ### faces. Is this maybe a pointer that I should change something?
ziggo is offline   Reply With Quote

Old   July 24, 2013, 08:39
Default
  #4
Senior Member
 
flotus1's Avatar
 
Alex
Join Date: Jun 2012
Location: Germany
Posts: 1,098
Rep Power: 19
flotus1 will become famous soon enoughflotus1 will become famous soon enough
I mentioned the problem with the "90" AoA only to make it more evident. This problem still exists with all AoA higher than 0 (55 in your case).
In fact that is why you get the messages about reversed flow at the outlet. Because for these cases, there would actually be a reversed flow at some portions of the outlet.

The solution is still the same:
Use a free stream or velocity boundary condition for the whole outer boundary.
flotus1 is offline   Reply With Quote

Reply

Tags
angle of attack, fluent 14, lift and drag

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
Display lift and Drag in paraview SamerAli OpenFOAM Paraview & paraFoam 1 May 16, 2013 12:51
direction vectors for lift and drag in fluent nauman55 FLUENT 6 September 10, 2012 10:34
Drag & lift coefficients for a velocity inlet BC tsi07 FLUENT 4 May 30, 2012 08:59
lift and drag ceofficient problem icemaniac178 CFX 6 August 17, 2011 18:40
Correct lift but wrong pressure drag - possible? zx Main CFD Forum 4 July 27, 2007 23:38


All times are GMT -4. The time now is 05:26.