[jon g]

I need some help as I am clearly doing something wrong. I can't seem to get results for loads that correspond anywhere near to what experience and simple theory would suggest.

To keep things simple I have done a thin airfoil theory suggests a lift for this study of 15 but i only get 6N

Its not only this study but all the ones I have done so far including analysis of a race car. where the drag and downforce seem to be much lower than some old wind tunnel data

This example is of a NACA0012 airfoil I got the co-ords and performance data (attached) from ABBOT & DOENHOFF the theory of wing sections That I have borrowed.

This airfoil has a nearly linear lift co-efficent up to 12 deg
at 10 degrees Lc is 1.0

for the study attached chord is 0.1 m air density is 1.2 KG/m^3 ( and checked by showing it in a cut plot )

for an air velocity of 50 m/s 1/2 rho V^2 = 1.2*0.5*50^2 =1500N/M^2

chord=0.1m domain width= 0.1m so plan area =0.01M^2

Expected lift at Lc=1 = 15N

result from the study is 6N

This value changes slightly if if make the domain larger and improve the mesh resolution but only a small bit
the pressures are what I would expect the max and min relative pressures are +1692Pa and - 2018

I have attached the study and a few pictures.

would be really pleased to recieve some help and advice

Jon G
wing performance.jpg

wingcoords.jpg

SURFACE LOADS.jpg

cover.jpg

NACA0012-10DEG.zip

[Boris_M]

If that is the mesh in one of the images you show, then it is no wonder that you won't get accurate results. We are talking about external aerodynamics with a very aerodynamic body. It is not a large assembly of parts like in an electronics box where there is so much disturbance that aerodynamics is not your main concern.
Here it is the core you are interested in and therefore the mesh should resolve that core interest.

Please have a look at the Best Practice Guide for external aerodynamics at the download link below. This should help you get a better understanding of how to set up such cases better for accurate results:
http://www.floefd.com/download/BPG_External_Aero.zip

Regards,
Boris

[jon g]

Many thanks for that. Had an interesting time reading it very informative
have tried much refined mesh with no real changes to results which was dissapointing

on page 19 it shows how to force the thin boundary layer approach by creating support_config.txt file have tried this with no success have put the file in several places ie the project folder where the study is and the results folder and in the program file folders in caase that helps.
I havent seen a change in the results so i suspect it is not working

It seems too simple to just add a small text file next to the study files.

Be really pleased if you could help

Many thanks Jon


this is the code I have used in support_config.txt
block_begin redefine_a_i_arrays
I[29]=2.
block_end

[Boris_M]

Hi Jon,

Nope, works like a charm and that's how it is meant to be. You need to put it into the project folder (i.e. the folder named 1 or 2 etc.) depending on the project you are simulating.
The software checks automatically for that file and if it finds it with the right command, then the setting is used. You can easily check it by using a surface plot and the parameter Boundary Layer Type. 1 is Thick boundary layer and 0 is Thin boundary layer and if you have values in between, then it is automatically selecting depending on the mesh and the boundary layer.

Did you use the same Reynolds Number to compare the simulation?

We use the NACA 0012 in every QA run of the software as it is one of the default validation airfoils and it gives good results.
We run it at Mach 0.3 and 0.8 for different angles and compare not only lift and drag, which is something everyone can get for a wide range of bodies quite good, but also the pressure coefficient profile along the wing surface.
We are comparing NASA and AGARD experiments in the QA and the error is between 0.15 and almost 3% for the lift.

Also, it is best to move the air, not the wing for the AOA. It will keep the mesh the same for the whole AOA sweep.

If you send me the model I can have a look at it if you like.

Regards,
Boris

[jon g]

Many thanks am making progress at last
did some new models and runs:
with chord at 1m and air speed of mach 0.3 100m/s and 5deg AoA results were 99 % of expected had changed the boundary layer type to 1
running again with boundary as type 0 get 94% of expected answer

Going back to the 100 mm chord model with type 1 boundary layer 50m/s ( mach 0.15) got 90 % which is ok but maybe reynolds number is low 3.3 e+5 put velocity up to 200 m/s
mach 0.58 reynolds 1.3 e+6 results came out at 104 %

zip added with a solidworks model attached. cant send the results folder as its too big
If you think I am doing ok will push on with trying to sort out the main project
many thanks for all your advice. as you said the support file works a treat.

Many Thanks Jon

[Boris_M]

Looks good.
If you run into local supersonic regions with the airfoil it makes sense to use adaptive mesh refinement to better resolve the shock region as it influences the lift and drag.

I think this looks good and you can continue.
Make sure you meet the same reynolds numbers as otherwise the flow will be different and results probably won't match anymore.

Regards,
Boris