[Nineties123]

Hi, I'm trying to replicate experimental data for a NACA 2415- using data from the Abbott and Von Doenhoff book- and for some reason, even though I can get to within about 10% of the lift, Ansys CFX is consistently overpredicting my drag by a ridiculous amount- around 200% in some cases.

I'm debating making my inflation larger- is that likely to help? I suspect it may be to do with the viscous drag.

I am quite new to using Ansys, so any help would be much appreciated.

[aero_head]

Hello,

What is your mean value for Y+?

The Y+ mean value should be near 1. Don't worry about low values for Y+ at the leading edge, it is more important to have the correct value (i.e. 1) of Y+ from around 1/4 chord to 100% of chord.

As well, what turbulence model are you using for your simulation?

ETA: I have heard that CFD almost always overpredicts the drag of airfoils, so just be aware of that. I think the best it can do is get the value to within ~20%-30%. It is very good at predicting lift (pressure forces) but bad predicting drag (viscous forces).

[Nineties123]

Originally Posted by aero_head

Hello,

What is your mean value for Y+?

The Y+ mean value should be near 1. Don't worry about low values for Y+ at the leading edge, it is more important to have the correct value (i.e. 1) of Y+ from around 1/4 chord to 100% of chord.

As well, what turbulence model are you using for your simulation?

ETA: I have heard that CFD almolst always overpredicts the drag of airfoils, so just be aware of that. I think the best it can do is get the value to within ~20%-30%. It is very good at predicting lift (pressure forces) but bad predicting drag (viscous forces).

Hi, I used a y+ calculator to calculate my first layer thickness and used a y+ of 1. When I looked at my y+ contour along the aerofoil surface it was mostly 1 up to towards the trailing edge. The maximum was 1.6.

I am also using a Shear Stress Transport turbulence model.

[ghorrocks]

Have you gone through the issues listed on the FAQ: https://www.cfd-online.com/Wiki/Ansy..._inaccurate.3F

Some key ones for this case:
* Is your mesh fine enough?
* Is it converged enough?
* Is your turbulence model appropriate for the condition you are modelling?
* Is your boundary conditions far enough upstream and downstream?
* Is your side boundaries far enough away to act as far fields?
* Do you have turbulence transition?
* Do you have separations?

I do not agree with aero_head, you can get drag predicted very accurately if you carefully validate your model (at least in the attached flow regimes). The turbomachery and aerospace industries routinely get extremely accurate results for airfoil modelling - but they have also very carefully validated their simulation procedures. But getting accurate drag is much harder than getting accurate lift.

[aero_head]

Originally Posted by ghorrocks

I do not agree with aero_head, you can get drag predicted very accurately if you carefully validate your model (at least in the attached flow regimes). The turbomachery and aerospace industries routinely get extremely accurate results for airfoil modelling - but they have also very carefully validated their simulation procedures. But getting accurate drag is much harder than getting accurate lift.

Good to know, thanks for clearing that up ghorrocks!

[LoGaL]

I agree whit what has been said before. Actually, for NACA airfoils, you can surely get correct results for pre-stall angle of attack. TBH 200% is too off, I think there's a not so smart mistake somewhere

[Nineties123]

Originally Posted by aero_head

Good to know, thanks for clearing that up ghorrocks!

Hi, I've just noticed that on my y+ contour, the y+ value appears to be a lot lower than 1 at the leading edge and increases up to 1.6 at the trailing edge and near the quarter chord. How do I fix this?

[Nineties123]

Originally Posted by LoGaL

I agree whit what has been said before. Actually, for NACA airfoils, you can surely get correct results for pre-stall angle of attack. TBH 200% is too off, I think there's a not so smart mistake somewhere

Hi, what would you suggest I do to fix it? I have used a y+ calculator to find the first layer thickness but on my y+ contour, the y+ value appears to be quite a bit lower than 1 at the leading edge and around 1.6 at the half chord to leading edge.

Alternatively I am possibly debating increasing the number of inflation layers.

I am currently using a SST transition model, for context.

[ghorrocks]

Why are you requiring y+=1? What are you doing which requires that?

Your simulation will not fail if you depart slightly from y+=1. I would recommend you do a mesh sensitivity study where you take your existing mesh and compare it against a y+=0.5 and y+=2.0 mesh to see if it actually makes a difference in your case. This will tell you if it makes any difference.

[LoGaL]

Originally Posted by Nineties123

Hi, what would you suggest I do to fix it? I have used a y+ calculator to find the first layer thickness but on my y+ contour, the y+ value appears to be quite a bit lower than 1 at the leading edge and around 1.6 at the half chord to leading edge.

Alternatively I am possibly debating increasing the number of inflation layers.

I am currently using a SST transition model, for context.

if you get y+ = 1.6 it is pretty fine. Concerning increasing the number of inflation layers, what are you imposing, smooth transition or first layer thickness? If you impose smooth transition, yes, just increase the layers by 2-3 and you drop below 1 almost for sure. SST will work fine so long as your Y+ is around 1, but you won't anyways get anything wrong if you get Y+= 2 somewhere

Concerning the transition model, I have no experience with it, but if your reynolds number is high enough, stick with the normal SST, not the transition one.

What I am saying is that, considering that you are 200% off the expected Cd, you must have done some more trivial mistake, e.g. uncorrect geometry, wrong fluid properties and so on. The point is that it is not surprising you match the Lift coefficient, because for most of the bodies in attached regime, Cl = 2pi*alfa

Mind posting a pic of the mesh and some velocity contour around the airfoil?

[Nineties123]

Originally Posted by LoGaL

if you get y+ = 1.6 it is pretty fine. Concerning increasing the number of inflation layers, what are you imposing, smooth transition or first layer thickness? If you impose smooth transition, yes, just increase the layers by 2-3 and you drop below 1 almost for sure. SST will work fine so long as your Y+ is around 1, but you won't anyways get anything wrong if you get Y+= 2 somewhere

Concerning the transition model, I have no experience with it, but if your reynolds number is high enough, stick with the normal SST, not the transition one.

What I am saying is that, considering that you are 200% off the expected Cd, you must have done some more trivial mistake, e.g. uncorrect geometry, wrong fluid properties and so on. The point is that it is not surprising you match the Lift coefficient, because for most of the bodies in attached regime, Cl = 2pi*alfa

Mind posting a pic of the mesh and some velocity contour around the airfoil?

Hi, I am currently struggling to open Ansys but luckily I recorded everything I have done.

I used JavaFoil with 101 points and modified for a closed trailing edge for the NACA 2415 geometry.

Below is a link to a Google Doc file where I have included relevant images.

https://docs.google.com/document/d/1...it?usp=sharing

The contours and streamlines are for where I tested at 3 degrees AoA with conditions for a Reynolds number of 6*10^6 with conditions at altitude 2500m. I have also added the domain we are currently using (in combination with the mesh it gave us a 2% error difference on Cl and 50% difference on Cd at 0 AoA, however this swiftly changed to a 17.75% error on Cl and 37.39% error on Cd when I increased the AoA to 3 degrees)

The following are all the Mesh settings I used:

DISPLAY
Display Style: Use geometry Setting
DEFAULTS
Physics Preference: CFD
Solver Preference: CFX
Element Order: Linear
Element Size: Default
SIZING
(all of this was left as the default)
Use Adaptive Sizing: No
Growth Rate: Default
Max Size: Default
Mesh Defeaturing: Yes (this was on as a default)
- Defeature Size: Default
Capture Curvature: Yes
Curvature Mi...: Default
Curvature Nor...: Default
Capture Proximity: No
QUALITY (all of these were left as default)
Check Mesh Quality: Yes, errors
Target Skewness: Default (0.900000)
Smoothing: Medium
Mesh Metric: None
INFLATION
Use Automatic Inflation: All faces in chosen named selection
Named Selection: Wall (my aerofoil)
Inflation Option: First Layer Thickness
First Layer Height: 7.53e-06 (this number was taken from entering the altitude conditions and chord length of 1.626m into a y+ calculator for y+ of 1)
Maximum Layers: 15
Growth Rate: 1.3
Inflation Algorithm: Pre
View Advanced Options: Yes
(only change was Maximum Angle to 180 degrees)
ADVANCED and STATISTICS all left alone

I then inserted a Sizing
SCOPE
Scoping Method: Geometry Selection
Geometry selected was the entire domain
DEFINITION
Suppressed: No
Type: Body of Influence
Bodies of Influence: (Selected the internal domain)
Element Size: 1e-2
ADVANCED
Growth Rate: Default (1.2)


Any help would be much appreciated.

[LoGaL]

Hi, from all the settings I can't guess much, I just wanna see this pictures of mesh and flow.
Only thing I can say is that if you wanna lower your y+, decrease first thickness value. Growth Rate 1.3 is garbage, aim for 1.2 or 1.15

But again, if you get so grossly wrong results, I repeat that you have done some bad mistake. Show me pictures of this mesh pls