How to calculate the drag of a car. Are the values correct?

[joseflambley3]

Hi,

Im trying to get a base line for the drag cofficient of a car model so that I can investigate how different mods would effect it.

Im very new to the software and I've only worked out how to use it via youtube tutorials and websites so my knowledge is quite low.

I have run the wind tunnel test with a wind speed of 60mph. I then ran 300 iterations as the plot seemed to level out at this point.

I then went to use the wall calculator and got:

FX -84N

FY -1600.56N

FZ 245N

using a calulator online this gives me a ruff estimate 2.47 which seems quite wrong

Is the negative values due to the model back to front? Is my answer massively wrong due to my bad calculation or have I set the enviroment up wrong?

Any help appreciated, please remember Im very new :).

[joseflambley3]

Hi,

Im trying to get a base line for the drag cofficient of a car model so that I can investigate how different mods would effect it.

Im very new to the software and I've only worked out how to use it via youtube tutorials and websites so my knowledge is quite low.

I have run the wind tunnel test with a wind speed of 60mph. I then ran 300 iterations as the plot seemed to level out at this point.

I then went to use the wall calculator and got:

FX -84N

FY -1600.56N

FZ 245N

using a calulator online this gives me a ruff estimate 2.47 which seems quite wrong

Is the negative values due to the model back to front? Is my answer massively wrong due to my bad calculation or have I set the enviroment up wrong?

Any help appreciated, please remember Im very new :).

[John_Holtz]

Hi @joseflambley3 . Welcome to the CFD forum.

I have the same question for you! How did you calculate the drag coefficient? In other words, 

1. What is the formula that you used?
2. What are the input values (and units) that you used?
3. Where are your calculations?

Once we know whether your basic calculation is correct, then we can begin to explore the setup of your analysis. Some example questions about the analysis would be:

1. What directions are X, Y, Z? (The axis is not shown in your figures. 😞)
2. Your image hides what we want to see: the volume of air! What does it look like? (Your Fusion model, .f3d, has a hollow car that allows air to flow in and out of the car, so we do not know what your CFD model looks like.)
3. What type of boundary layer mesh did you create?
4. What type of turbulence model did you use?

This forum post may also provide some suggestions. See Solved: How to calculate drag coefficient of wing? - Autodesk Community - CFD (and also the link included in the forum to this YouTube video Review NACA0012 2D Airfoil Model in Autodesk Simulation CFD - YouTube.)

John

[John_Holtz]

Hi @joseflambley3 . Welcome to the CFD forum.

I have the same question for you! How did you calculate the drag coefficient? In other words, 

1. What is the formula that you used?
2. What are the input values (and units) that you used?
3. Where are your calculations?

Once we know whether your basic calculation is correct, then we can begin to explore the setup of your analysis. Some example questions about the analysis would be:

1. What directions are X, Y, Z? (The axis is not shown in your figures. 😞)
2. Your image hides what we want to see: the volume of air! What does it look like? (Your Fusion model, .f3d, has a hollow car that allows air to flow in and out of the car, so we do not know what your CFD model looks like.)
3. What type of boundary layer mesh did you create?
4. What type of turbulence model did you use?

This forum post may also provide some suggestions. See Solved: How to calculate drag coefficient of wing? - Autodesk Community - CFD (and also the link included in the forum to this YouTube video Review NACA0012 2D Airfoil Model in Autodesk Simulation CFD - YouTube.)

John

[joseflambley3]

Thanks so much for the reply,

Here is a google drive link to the design study folder: https://drive.google.com/drive/folders/1qG2S3kSjKEMQG1uUZMgUh3r5hsFLnb1F?usp=sharing

(I would upload directly this but the file type is not supported)

I used the formulae in this article: https://clickprintchem.wordpress.com/2019/11/09/tutorial-using-autodesk-computational-fluid-dynamics...

and converted 60 mph to m/s, used there value for density of air, and used a ruff front area of around 1.43m2

for setting up my test I followed this tutorial: https://www.youtube.com/watch?v=nS9SfKLdkw4&t=629s

Im not sure what turbulance model I used so probably the default and the air volume I'm not sure either.

With regards to the model being open, for me the model is closed if I open via the simulation section in fusion but if i export it to a step file then the front is open

Thanks for the help

[joseflambley3]

Thanks so much for the reply,

Here is a google drive link to the design study folder: https://drive.google.com/drive/folders/1qG2S3kSjKEMQG1uUZMgUh3r5hsFLnb1F?usp=sharing

(I would upload directly this but the file type is not supported)

I used the formulae in this article: https://clickprintchem.wordpress.com/2019/11/09/tutorial-using-autodesk-computational-fluid-dynamics...

and converted 60 mph to m/s, used there value for density of air, and used a ruff front area of around 1.43m2

for setting up my test I followed this tutorial: https://www.youtube.com/watch?v=nS9SfKLdkw4&t=629s

Im not sure what turbulance model I used so probably the default and the air volume I'm not sure either.

With regards to the model being open, for me the model is closed if I open via the simulation section in fusion but if i export it to a step file then the front is open

Thanks for the help

[John_Holtz · Accepted solution]

Here are the answers to my first set of questions:

1. What is the formula that you used? F=0.5*density*velocity^2*Cd*Area
2. What are the input values (and units) that you used?
   1. density ~ 1.2 kg/m^3
   2. velocity = 60 mph ~ 27 m/s
   3. Area ~ 1.43 m^2
3. Where are your calculations?
   1. 1600 N in Y (the flow direction) = 0.5*(1.2 kg/m^3)*(27 m/s)^2*Cd*(1.43 m^2)
   2. Therefore, Cd = 2.52. This agrees with your estimate of 2.47.

Your calculations are correct, so the CFD analysis is inaccurate. (The main reason I asked the questions is so that all the other readers do not need to do the same research to check the calculations.)

Here's the longitudinal cross-section through the middle of the car. These are the main problems that I see.

1. The air should not exist inside the volume of the car and should not be connected to the outside volume. (I assume that all drag calculations like this are with the windows of the car closed.) The CAD model is the "shell" of the car which means the air volume is outside and inside the car. You want the car to be solid so that the air volume has a big hollow where the car should be (1).
2. You will need a larger volume downstream to allow for turbulence and to get the artificial boundary condition farther from the model. (You can change that volume after taking care of other things in order to reduce the runtime.)
3. There is a boundary layer mesh at the wall, but it is hard to see around the outline of the car. (The boundary layer at the top and bottom is easy to see. BTW, you could make the top, bottom, and sides of the air volume a slip condition since you do not need a boundary layer there.) I hope that other readers will comment on the size of the boundary layer as far as whether it is too thin, need more layers, and so on. (I suspect it needs to be thicker with the more elements. See the Help for Wall Layers.) At the very least, I suggest using the "Enable wall layer blending" so there is a smoother transition from the small boundary layer and the large elements in the "free" stream.
4. I hope that other readers will comment on the turbulence model. (Solve > Physics > Turbulence). I do not know if k-epsilon is sufficient to calculate the drag at these speeds or whether one of the SST turbulence models is required. The forums post and webinar links in my previous reply will give good information if no other readers have suggestions for your particular model.

I have attached a support share file (.cfz) of the model in case other readers have some feedback. (The support share file includes all the input but not the mesh or results. This makes the filesize relatively small.)

John

[John_Holtz · Accepted solution]

Here are the answers to my first set of questions:

1. What is the formula that you used? F=0.5*density*velocity^2*Cd*Area
2. What are the input values (and units) that you used?
   1. density ~ 1.2 kg/m^3
   2. velocity = 60 mph ~ 27 m/s
   3. Area ~ 1.43 m^2
3. Where are your calculations?
   1. 1600 N in Y (the flow direction) = 0.5*(1.2 kg/m^3)*(27 m/s)^2*Cd*(1.43 m^2)
   2. Therefore, Cd = 2.52. This agrees with your estimate of 2.47.

Your calculations are correct, so the CFD analysis is inaccurate. (The main reason I asked the questions is so that all the other readers do not need to do the same research to check the calculations.)

Here's the longitudinal cross-section through the middle of the car. These are the main problems that I see.

1. The air should not exist inside the volume of the car and should not be connected to the outside volume. (I assume that all drag calculations like this are with the windows of the car closed.) The CAD model is the "shell" of the car which means the air volume is outside and inside the car. You want the car to be solid so that the air volume has a big hollow where the car should be (1).
2. You will need a larger volume downstream to allow for turbulence and to get the artificial boundary condition farther from the model. (You can change that volume after taking care of other things in order to reduce the runtime.)
3. There is a boundary layer mesh at the wall, but it is hard to see around the outline of the car. (The boundary layer at the top and bottom is easy to see. BTW, you could make the top, bottom, and sides of the air volume a slip condition since you do not need a boundary layer there.) I hope that other readers will comment on the size of the boundary layer as far as whether it is too thin, need more layers, and so on. (I suspect it needs to be thicker with the more elements. See the Help for Wall Layers.) At the very least, I suggest using the "Enable wall layer blending" so there is a smoother transition from the small boundary layer and the large elements in the "free" stream.
4. I hope that other readers will comment on the turbulence model. (Solve > Physics > Turbulence). I do not know if k-epsilon is sufficient to calculate the drag at these speeds or whether one of the SST turbulence models is required. The forums post and webinar links in my previous reply will give good information if no other readers have suggestions for your particular model.

I have attached a support share file (.cfz) of the model in case other readers have some feedback. (The support share file includes all the input but not the mesh or results. This makes the filesize relatively small.)

John

[joseflambley3]

Hi,

Thanks for the help. I ended up using a different turbulence model outlined in the webinar, I added some wheel arches, I used layer blending, added some more wall layers, made the test enviroment longer, added the slip condition, used fusion to get a better value for the cross sectional area and got a final value of 0.61.

However I ran the simulation for 300 iterations and I don't think that was quite enough for the plot to converge, but this is way closer and Im going to leave another run overnight and see what I get.

Once again thanks for pointing me in the right direction.

[joseflambley3]

Hi,

Thanks for the help. I ended up using a different turbulence model outlined in the webinar, I added some wheel arches, I used layer blending, added some more wall layers, made the test enviroment longer, added the slip condition, used fusion to get a better value for the cross sectional area and got a final value of 0.61.

However I ran the simulation for 300 iterations and I don't think that was quite enough for the plot to converge, but this is way closer and Im going to leave another run overnight and see what I get.

Once again thanks for pointing me in the right direction.