2017 front wings downforce compared to 2010

[Dipesh1995]

Yep, I understand what you’re saying and I agree. I’m kinda clutching at straws at the moment because redesigning the tunnel is a lot of a CAD work. I’m still gonna test a simple wing just to make sure I’m not setting up the CFD incorrectly otherwise I’ll have to redesign the complete wing

[Vyssion]

Yep, I understand what you’re saying and I agree. I’m kinda clutching at straws at the moment because redesigning the tunnel is a lot of a CAD work. I’m still gonna test a simple wing just to make sure I’m not setting up the CFD incorrectly otherwise I’ll have to redesign the complete wing

Yeah I totally understand You may not need to totally redesign it though!! To be honest, it may be possible to swap some of the aerofoil profiles you currently have, out for some more traditional racing ones, and to just play with AoA, slot gap and overlaps until you get something that works. Your design works in freestream, which means that you CAN get it to work in ground effect too; just needs some tweaking due to the physics going on I'm sure that there are plenty of people besides me who would enjoy analyzing your images as you progress!!

[Dipesh1995]

Yep, I understand what you’re saying and I agree. I’m kinda clutching at straws at the moment because redesigning the tunnel is a lot of a CAD work. I’m still gonna test a simple wing just to make sure I’m not setting up the CFD incorrectly otherwise I’ll have to redesign the complete wing

Yeah I totally understand You may not need to totally redesign it though!! To be honest, it may be possible to swap some of the aerofoil profiles you currently have, out for some more traditional racing ones, and to just play with AoA, slot gap and overlaps until you get something that works. Your design works in freestream, which means that you CAN get it to work in ground effect too; just needs some tweaking due to the physics going on I'm sure that there are plenty of people besides me who would enjoy analyzing your images as you progress!!

https://photos.app.goo.gl/9IpIN49T17udhins2

Ok so I went back to basics and tested a 2-element wing with the following specifications to make sure I'm setting the CFD up correctly :
Span: 900mm (each half)
Main Plane aerofoil chord: 400 mm
Flap aerofoil chord: 286 mm
Footplate height from ground: 50 mm
Main plane height from ground: 80 mm

I ran it in freestream first and it worked as expected.

As soon as I ran it in ground effect, convergence of Tke became poor, in general, the convergence of all the residuals became poorer and the edge vortex is about to disappear as shown by its core velocity and direction shown in the images (vortex moving inboard in a similar fashion to the complex wing) with that stagnant bubble of flow reappearing in the contour plot. I've changed the mesh type from polyhedral to trimmer and changed the turbulence model from SST to realisable K Epsilon yet the issue remains. My Y+ is between 0.28 and 1 in all regions of the wing with blended wall function. I know I have a some trailing separation on the flap but certainly not enough to cause the stagnant bubble.

I'm setting something up incorrectly and its affecting the wing when its in ground effect so that I think that maybe points to the ground plane physics. I've set the ground plane as wall with slip condition and left everything else as default.

I don't exactly why its doing what its doing because the adverse gradient is certainly not as strong as the complex wing and the fact that separation bubble only appears near the endplate and not in the inboard region of the wing.

Out of desperation, I also went ahead and the changed the wing from having a no-slip condition to a slip condition to remove the boundary layer and the problem still existed despite have zero surface separation on the aerofoils.

One positive thing is that the wing generates 4294 N of downforce and 335 N of drag.

[Vyssion]

https://photos.app.goo.gl/9IpIN49T17udhins2

Ok so I went back to basics and tested a 2-element wing with the following specifications to make sure I'm setting the CFD up correctly :
Span: 900mm (each half)
Main Plane aerofoil chord: 400 mm
Flap aerofoil chord: 286 mm
Footplate height from ground: 50 mm
Main plane height from ground: 80 mm

I ran it in freestream first and it worked as expected.

As soon as I ran it in ground effect, convergence of Tke became poor, in general, the convergence of all the residuals became poorer and the edge vortex is about to disappear as shown by its core velocity and direction shown in the images (vortex moving inboard in a similar fashion to the complex wing) with that stagnant bubble of flow reappearing in the contour plot. I've changed the mesh type from polyhedral to trimmer and changed the turbulence model from SST to realisable K Epsilon yet the issue remains. My Y+ is between 0.28 and 1 in all regions of the wing with blended wall function. I know I have a some trailing separation on the flap but certainly not enough to cause the stagnant bubble.

I'm setting something up incorrectly and its affecting the wing when its in ground effect so that I think that maybe points to the ground plane physics. I've set the ground plane as wall with slip condition and left everything else as default.

I don't exactly why its doing what its doing because the adverse gradient is certainly not as strong as the complex wing and the fact that separation bubble only appears near the endplate and not in the inboard region of the wing.

Out of desperation, I also went ahead and the changed the wing from having a no-slip condition to a slip condition to remove the boundary layer and the problem still existed despite have zero surface separation on the aerofoils.

One positive thing is that the wing generates 4294 N of downforce and 335 N of drag.

Are you able to supply a plane section image of your mesh please? With all the refinement around aerofoils etc etc? Also, a y+ surface plot?

Couple of things pop out to me:

• You changed the turbulence model from SST to realizable k-eps which is fine, however, you no longer need a y+
  so low. What you have of 0.28 -> 1.0 is something you would have for SST "without" wall functions. If you are running realizable k-eps WITH wall functions, then you can get away with a y+ of 60-100 pretty safely.

• The curvature of the edge vortex travelling inboard isn't that erroneous a thing; you have a larger pressure differential between the underside of the wing and the outside of the endplate in ground effect have in freestream. So streamline curvature is to be expected.

• The "bubble" you mention isn't really one at all - its just a slice of the vortex as it rolls inboard

• The adverse pressure gradient is not as strong as the other wing, true - but that doesn't mean it still isnt strong enough to separate. But for the most part, at least from your images you supplied, the wing is 98% attached - the tiny bit at the trailing edge of the flap element is all

• At around iteration 400 ish, there is a spike in the residuals... Did you change any under-relaxation parameters to force a convergence? Or what caused that?

• This may just be the colour discretization that is making it look this way, but are your cell sizes the same size as some of those blocky bits within the big blue region?

Numerical instabilities often appear due to a badly defined problem, a poor quality mesh and/or the wrong solver settings. The instabilities can mean diverging residuals occur, or it can mean that they just kind of "hover" and get stuck. Diverging residuals often imply that there is an increasing amount of imbalance in the conservation equations (mass, momentum, etc.)
Maybe give these a shot?

• If you're not already, try and solve for a first order discretization schemed solution

• Check how many cells you have that are of a high aspect ratio or high skewness and refine those regions or remesh

• Note: you can't improve the cell skewness by using adaptive mesh refinement - i.e. by modifying the existing mesh to make it "better"

[jjn9128]

I'm not a CFD methodology engineer so I bow to Vyssion's expertise in this area, I've also not used Star for a long time. It would be good to see your mesh though, as someone who studied wakes for a living I'm a bit sensitive to mesh fidelity in the far field, as Vyssion says this could be colour discretization making it appear worse, but I think not. The far field is as important as boundary layer fidelity for simulation accuracy.

On visualizing the vortex, rather than using streamlines you could plot an isosurface of Q criterion or lambda2, both will show the vortex better than the seeded streamlines, because where you seed will vary how the vortex looks. Even an appropriately chosen isosurface of static or total pressure can show the vortex core in the wake. You could also slice the wing orthogonally to the flow to see how the vortex develops around the endplate as you progress chordwise along the wing and beyond. If you plot streaklines on the surface as well you should see the roll up of the main vortex on the inner face of the endplate and the tip of the wing, the roll up of the outer endplate votex, and the footplate vortex, as well as any separation issues on trailing edges ...etc.

I would also be careful about how you present data to engineers, we're a curmudgeonly bunch (I certainly am, one of Vyssion's lecturers was also my examiner and he was grumpier than me!!!) - it comes from critical analysis of everything you do. Your Cp contours are between -22 and 0.7, is there a point on the wing with Cp=-22?? That seems erroneous to me so automatically I'm skeptical of your results. Also is there no stagnation point on the wing or endplate? The specificity of the numbers has me suspect they're auto-generated to the limits of the simulation output, so what is the issue here? I would take note of what Vyssion suggests about setup and have another go.

On your wing geometry and going back to basics, you really need to think about the center-of-pressure of your wing, peak loading, how that affects the pressure gradient...etc. You may be getting a fair amount of downforce but the plan area of the wing is massive, and as I said I'm skeptical of the results anyway. Check out some old aerofoils used for an old 2-element wings in F1 - a Gottingen GOE795 for the mainplane coupled with a Benedek B-8356-b flap with the flap overlapping to ~20-25% of it's chord. Or there's a MSc paper from Delft, can't recall the students name, with the Cartesian coordinates for an old Toyota wing. Or even try some NACA 4 digit aerofoils.

We both think it's great that you're enthusiastic and want to encourage you, sorry if it feels like a double assault, we mean well!

[Vyssion]

We both think it's great that you're enthusiastic and want to encourage you, sorry if it feels like a double assault, we mean well!

Definitely

We both love this stuff and it's fun for us. It's awesome what you have done, and we want to help you get it working properly so that it is TOTALLY AWESOME!!

[Dipesh1995]

https://photos.app.goo.gl/9IpIN49T17udhins2

Ok so I went back to basics and tested a 2-element wing with the following specifications to make sure I'm setting the CFD up correctly :
Span: 900mm (each half)
Main Plane aerofoil chord: 400 mm
Flap aerofoil chord: 286 mm
Footplate height from ground: 50 mm
Main plane height from ground: 80 mm

I ran it in freestream first and it worked as expected.

As soon as I ran it in ground effect, convergence of Tke became poor, in general, the convergence of all the residuals became poorer and the edge vortex is about to disappear as shown by its core velocity and direction shown in the images (vortex moving inboard in a similar fashion to the complex wing) with that stagnant bubble of flow reappearing in the contour plot. I've changed the mesh type from polyhedral to trimmer and changed the turbulence model from SST to realisable K Epsilon yet the issue remains. My Y+ is between 0.28 and 1 in all regions of the wing with blended wall function. I know I have a some trailing separation on the flap but certainly not enough to cause the stagnant bubble.

I'm setting something up incorrectly and its affecting the wing when its in ground effect so that I think that maybe points to the ground plane physics. I've set the ground plane as wall with slip condition and left everything else as default.

I don't exactly why its doing what its doing because the adverse gradient is certainly not as strong as the complex wing and the fact that separation bubble only appears near the endplate and not in the inboard region of the wing.

Out of desperation, I also went ahead and the changed the wing from having a no-slip condition to a slip condition to remove the boundary layer and the problem still existed despite have zero surface separation on the aerofoils.

One positive thing is that the wing generates 4294 N of downforce and 335 N of drag.

Are you able to supply a plane section image of your mesh please? With all the refinement around aerofoils etc etc? Also, a y+ surface plot?

Couple of things pop out to me:

• You changed the turbulence model from SST to realizable k-eps which is fine, however, you no longer need a y+
  so low. What you have of 0.28 -> 1.0 is something you would have for SST "without" wall functions. If you are running realizable k-eps WITH wall functions, then you can get away with a y+ of 60-100 pretty safely.

• The curvature of the edge vortex travelling inboard isn't that erroneous a thing; you have a larger pressure differential between the underside of the wing and the outside of the endplate in ground effect have in freestream. So streamline curvature is to be expected.

• The "bubble" you mention isn't really one at all - its just a slice of the vortex as it rolls inboard

• The adverse pressure gradient is not as strong as the other wing, true - but that doesn't mean it still isnt strong enough to separate. But for the most part, at least from your images you supplied, the wing is 98% attached - the tiny bit at the trailing edge of the flap element is all

• At around iteration 400 ish, there is a spike in the residuals... Did you change any under-relaxation parameters to force a convergence? Or what caused that?

• This may just be the colour discretization that is making it look this way, but are your cell sizes the same size as some of those blocky bits within the big blue region?

Numerical instabilities often appear due to a badly defined problem, a poor quality mesh and/or the wrong solver settings. The instabilities can mean diverging residuals occur, or it can mean that they just kind of "hover" and get stuck. Diverging residuals often imply that there is an increasing amount of imbalance in the conservation equations (mass, momentum, etc.)
Maybe give these a shot?

• If you're not already, try and solve for a first order discretization schemed solution

• Check how many cells you have that are of a high aspect ratio or high skewness and refine those regions or remesh

• Note: you can't improve the cell skewness by using adaptive mesh refinement - i.e. by modifying the existing mesh to make it "better"

https://photos.app.goo.gl/uSOOSy3sLcsxVuZI2

I haven't refined the wake region signficantly. I've also included a slice contour of the x- velocity of the vortex tunnel of the complex wing so you can make direct comparison between the two wings near the end plates.

Since my Y+ is quite low and I'm using the blended wall function, presumably, I'll have to reduce the surface refinement of the wing and focus on refining the wake region of the wing.

At around 400 iterations, I changed the mesh type and turbulence model.

Also, how do I plot surface streamlines on STAR, I've looked around the web and can only find seeded streamlines?

[Dipesh1995]

I'm not a CFD methodology engineer so I bow to Vyssion's expertise in this area, I've also not used Star for a long time. It would be good to see your mesh though, as someone who studied wakes for a living I'm a bit sensitive to mesh fidelity in the far field, as Vyssion says this could be colour discretization making it appear worse, but I think not. The far field is as important as boundary layer fidelity for simulation accuracy.

On visualizing the vortex, rather than using streamlines you could plot an isosurface of Q criterion or lambda2, both will show the vortex better than the seeded streamlines, because where you seed will vary how the vortex looks. Even an appropriately chosen isosurface of static or total pressure can show the vortex core in the wake. You could also slice the wing orthogonally to the flow to see how the vortex develops around the endplate as you progress chordwise along the wing and beyond. If you plot streaklines on the surface as well you should see the roll up of the main vortex on the inner face of the endplate and the tip of the wing, the roll up of the outer endplate votex, and the footplate vortex, as well as any separation issues on trailing edges ...etc.

I would also be careful about how you present data to engineers, we're a curmudgeonly bunch (I certainly am, one of Vyssion's lecturers was also my examiner and he was grumpier than me!!!) - it comes from critical analysis of everything you do. Your Cp contours are between -22 and 0.7, is there a point on the wing with Cp=-22?? That seems erroneous to me so automatically I'm skeptical of your results. Also is there no stagnation point on the wing or endplate? The specificity of the numbers has me suspect they're auto-generated to the limits of the simulation output, so what is the issue here? I would take note of what Vyssion suggests about setup and have another go.

On your wing geometry and going back to basics, you really need to think about the center-of-pressure of your wing, peak loading, how that affects the pressure gradient...etc. You may be getting a fair amount of downforce but the plan area of the wing is massive, and as I said I'm skeptical of the results anyway. Check out some old aerofoils used for an old 2-element wings in F1 - a Gottingen GOE795 for the mainplane coupled with a Benedek B-8356-b flap with the flap overlapping to ~20-25% of it's chord. Or there's a MSc paper from Delft, can't recall the students name, with the Cartesian coordinates for an old Toyota wing. Or even try some NACA 4 digit aerofoils.

We both think it's great that you're enthusiastic and want to encourage you, sorry if it feels like a double assault, we mean well!

On visualizing the vortex, rather than using streamlines you could plot an isosurface of Q criterion or lambda2, both will show the vortex better than the seeded streamlines, because where you seed will vary how the vortex looks.

Yep, I'll have a go at that.

Your Cp contours are between -22 and 0.7, is there a point on the wing with Cp=-22?? That seems erroneous to me so automatically I'm skeptical of your results. Also is there no stagnation point on the wing or endplate? The specificity of the numbers has me suspect they're auto-generated to the limits of the simulation output, so what is the issue here?

The Cp numbers are based on reference numbers set under field functions. At the moment, the reference velocity does not match the inlet velocity and the density is set at 1 kg/m^3 which is clearly wrong. I haven't yet changed them until until I get the flow behaviour around the wing correct at which point I will. Its annoying that STAR doesn't set them up automatically within field functions. The downforce and drag figures are independent of this error because they are based on the actual density and inlet velocity and thus the figures I get are based on the wing geometry, meshing, physics etc

On your wing geometry and going back to basics, you really need to think about the center-of-pressure of your wing, peak loading, how that affects the pressure gradient...etc. You may be getting a fair amount of downforce but the plan area of the wing is massive, and as I said I'm skeptical of the results anyway. Check out some old aerofoils used for an old 2-element wings in F1 - a Gottingen GOE795 for the mainplane coupled with a Benedek B-8356-b flap with the flap overlapping to ~20-25% of it's chord. Or there's a MSc paper from Delft, can't recall the students name, with the Cartesian coordinates for an old Toyota wing. Or even try some NACA 4 digit aerofoils.

I know the CoP is bit too far forwards but this wing is just a "test component for CFD" wing so I haven't done the research into the best aerofoils for this wing (something I'll have to do once I start my FYP). Thanks for the naming a couple of aerofoils though, will definitely be useful when it comes to my FYP, at the moment. The wing took about 5 mins to create and the only target was to keep flow separation minimal.

Sorry if it feels like a double assault

No not at all, I always welcome constructive criticism; I can imagine in the F1 industry, engineers would be constructively criticising and evaluating each others work all the time in order to get the best out of each other.

[jjn9128]

Okay so a couple of things about you mesh. It looks like the boundary layer mesh is very small around the wing (explained by your low y+ value), but I can't tell how many levels there are below what I can see, or what the growth rate is - it looks close to 2?? What do you set for the mesh in star, minimum cell size and growth rate? In OpenFoam you have to work back from your maximum cell size to the minimum refinement level, i.e. for structured mesh with a maximum cell size of 1.6m with 10 refinement regions is a minimum cell size of ~1.6mm. In PowerFlow is the opposite, you set minimum cell size then the number of refinement regions determines your largest cell. For the BL I would suggest a maximum growth rate of 1.3 with about 5 layers and a minimum cell size of maybe 1mm. Maybe you can refine the cells at the leading and trailing edges and run a bigger cell over the flatter part of the wings.

I think your reference value settings may explain the maximum Cp of 0.7 but not the -22. By the looks of it your trailing edges are still sharp, but I can't see the mesh quality, maybe there are some isolated cells with high skewness or something which are showing a very negative pressure?! The area should be very small so it shouldn't affect the integrated pressures much, but it's not ideal.

You do not need a boundary layer mesh on the ground plane, which should have a moving wall or slip condition so will have no boundary layer. This will have massive implications for the cells you can run in the wake, I don't know how big your domain is but that should save you millions of cells.

[Dipesh1995]

https://photos.app.goo.gl/bth9ThCzbLcw7N2w2

Ok so I've changed the mesh and the Y+ has increased. However, as shown by the images, the Y+ is very high for the leading edge of the main plane even though I've refined the mesh a lot there.

Also, residuals convergence is still not great.

[Dipesh1995]

https://photos.app.goo.gl/dyhkiOMVHQZBgTiM2

I finally managed to a plot a "sort of" surface streamlines of the complex wing in ground effect that Vyssion wanted to see.

[Vyssion]

Ok - firstly, with regards to surface streamlines in StarCCM, I can't remember off the top of my head what the operation order is (I've been using OpenFOAM the past couple of years), but I'll post that up when I get home to check.

There's been quite a bit of quotes and post within post etc., so I'll start fresh with edits on pictures to show you what I'm referring to.

• With your y+ surface contours youre supplying, it would be much more helpful to supply one image of y+ scaled from zero to 5, another image of y+ scaled from 5 to 30, and another image with it scaled 30 to 100. Giving one image with it scaled from 0 to 127 or something that the solver just automaticaly generates isnt really helpful to us

• When I asked what that spike in the iteration convergence graph that you supplied was, you mentioned it was where you changed the mesh or turbulence equations etc. When you did that, I would say that you didn't clear the solution before hitting the solve button, else the first 400 or so steps would disappear. That is bad... Because although you are improving your mesh/solver/etc., you are using an initial condition (loosely) that is incorrect. And so your solver is attempting to find the correct solution from a wrong solution, instead of a fresh one. I would suggest attempting to run it from scratch and see how it works from there; and then running it for ~1000 iterations so we can get a full sense of what the Tke is doing.

• Having density set to 1kg/m^3 isn't really the best thing to do... most of the time, the default is 1.225 kg/m^3. I cant remember how StarCCM handles incompressible simulations, however, within OpenFOAM, what it does is solve for Pressure-over-Density, and then scales the result; so if your density is off by ~20%, then your results will be off by the same.

• I would echo jjn9128's comment about the boundary layer mesh initial setup to just get something going. Minimum cell size ~1mm with growth rate ~1.20 and 5-7 layers. Once we get that working, we can look to see whether more layers/smaller cells are needed to resolve it properly with whatever turbulence model you want to use.

I have also annotated a couple of the images you sent through with some comments - some of which are my own OCD kicking in which don't really have much of an effect. The main three comments are the ones about the layer collapsing, the refinement steps/layers and the "messy" joints.

• Layer Collapsing: This happens for mostly two reasons; the first is that within your boundarylayer mesh settings, you have too shallow an angle set for the Feature Angle setting and so when it sees the geometry "curve"
  (I use that word loosly) around the super sharp trailing edge, the mesher attempts to collapse the boundary layers because it assumes you don't want prism layers there. The second is that the corner is just too sharp regardless. To solve this, all you need to do is put a small 1-2mm fillet on the trailing edge within the CAD before you import it.
  You may want to change the "minimum cell size" option within the prism layer options ONLY to be on the order of 0.5mm to allow the cells to get small enough to curve around it. Note that values beyond ~270° tend to increase your overall orthogonality which is bad.

• Refinement Steps 1: This one is one often forgotten, but is an extension of why there is a boundary layer in the first place. The reason you have so many cells close to the surface, is so that if there is some sort of flow phenomenon going on, you have at least two cells which you are able to see that there is a pressure differential between them, and so there must be something there. If your cells are too large, you will not be able to capture that little flow thing going on, and you will miss it. A similar thing can be said for refining cells further from the surface as well, especially at the stagnation point where you need to have enough cells to fully capture the stagnation bubble.

• Refinement Steps 2: The changes in the cell volumes should be as smooth as possible because sudden larger changes in cell size may introduce disturbances to the system. The 2:1 sze jump across refinement levels usually cannot be avoided, but having more than one "lyaer of cells" between each refinement step avoids having consecutive refinement level changes close together, which would introduce disturbances. A typical number which is a balance of limiting the total number of cells and cell size jumps is 3 layers between each refinement jump.

• Messy Joints: With this setting, it often depends on the meshing algorithm that they software uses; i.e.
  some programs prefer sharp chamfer type joints, whereas others prefer fillets to mesh over. There is usually a "tolerance" setting which controls how far away from the local cell size, the mesh is able to look for something to snap to. A simple fix is to reduce your minimum "allowed" cell size, whilst still setting the "target" minimum cell size to be some multiple bigger.

.
.
.
.
.
Thats not quite the image I was after, but it does the job I've marked where flow separation is easy to tell, however, you still have it coloured by mangitude and not x-direction only, so it may not be a "full" showcase of where it is separated.

.
.
.
.
.

In OpenFoam you have to work back from your maximum cell size to the minimum refinement level, i.e. for structured mesh with a maximum cell size of 1.6m with 10 refinement regions is a minimum cell size of ~1.6mm.

Kind of... Levels of refinement are implemented as level 0 (zero) being the base cell size with a given edge length. A level 1 is then one "level" finer than a level 0, level 2 being one level finer than 1, etc. etc. But each successive level halves the VOLUME, and NOT THE EDGE LENGTH. So when you half the volume, it is like you are taking the cube root of 0.5, which is around ~0.7937 or about 79.4% of the above refinement level's edge length.

[Vyssion]

Just thinking out loud here, we have kind of "hijacked" the thread a little bit...

[n_anirudh]

1. Refinement regions need to extend in all directions. How did you estimate your wall y+?
2. Did you do any resolution study
3. Can you attempt it with a polyhedral mesh, should it give you better control?
4. Use ke model as a starting point for kw

[Dipesh1995]

https://photos.app.goo.gl/F5Uz4rZ2uLQ0h6AF2

Ok so thats the new mesh. I've set prism stretching factor as 1.2, it was 2 before as jjn128 thought it was, presumably that's the growth rate. Minimum cell size is set as 1 mm. I'll run it tommorow to see what the Y+ is like and see whether I've sorted the messy joint out.

Just thinking out loud here, we have kind of "hijacked" the thread a little bit...

Yeah, I think we may have unintentionally