# Simulation Forums

Find Simulation answers, share expertise, and connect with your peers

Find Simulation answers, share expertise, and connect with your peers

44 Views, 7 Replies

03/08/2018 7:38 AM

Hey folks, I'm trying to do a fairly straight forward aerodynamic analysis on our Dodge Neon race car that we are thinking of adding a front air splitter and rear wing to. I'm trying to establish a baseline of drag and lift/downforce with the unmodified car and then play around with different wing and splitter configurations to maximize downforce with the lowest addition of drag.

Anyway, I've created a basic model of the car including some rough cutouts for engine and undercarriage and ran a model to convergence. I'm trying to use Wall Results to compute the forces on the car body and the center of force - from which I should be able to resolve the force on the front and rear wheels. I thought this would be fairly easy. When looking at forces on the car body though I'm getting confused.

There is a cryptic comment in the wall calculator help section:

*To remove very low wall pressures (which may indicate the on-set of cavitation) from the force calculation, check the Cutoff Pressure box, and specify a minimum pressure value. This value will be assigned to all locations with pressures that fall below the Cutoff. *

I have found that doing this makes an enormous difference in the forces I am seeing and the location of the forces.

For what it's worth, a manual calculation of drag in the direction of travel (z in my model) based on Fd - 1/2 p CD A X V^2 predicts a drag force of around 125 lbs at 85mph with reasonable values for CD and A. So I'd expect to see a Fz of around 125 lbs.

I'm running my model at 85 MPH and it's half the car so forces in the Z and Y will need to be multiplied by 2.

With NO cutoff pressure set - I'm seeing a FZ of 226 lbs - much higher than my manual calculation predicts. The model also predicts a FY LIFT of around lbs - this isn't the direction I was expecting - I was assuming a downforce but I guess the car is somewhat teardrop shaped so is it possible that I'm actually seeing lift? The model also predicts a FX of 257 lbs which makes no sense to me at all. this implies that the car is being sucked away from the Slip/Symetric wall on the center YZ plane??? Seems very weird.

I arbitrarily set the cutoff pressure to .25 PSI and re-ran the study. I had absolutely no idea what pressure to set that at so this was totally random. I'm now seeing a FZ of 112 lbs - Much closer to the 125 lbs predicted by my manual calculation. The FY is STILL predicting the car is experiencing lift but it's reduced to a lift of 34 lbs. And the FX has reversed direction and is now predicting a force inward of 5lbs. Seems more reasonable and is presumably offset by an equal force on the other side of the car.

Likewise, when I compare where the center of force is for an analysis run with and without cutoff pressure I see a huge change in location - something like 5 feet!

So my questions:

Am I doing anything wrong with my analysis you can see?

Does it make sense that a passenger car is experiencing LIFT at 85 mph and now downforce?

Clearly setting cutoff pressures makes a huge difference in the analysis. What should I do to generate the most accurate numbers for a passenger car at 85 mph?

Link to design files (had to remove this

Screen shots of wall results follow as well.

Thanks so very much in advance for any guidance!

Report Inappropriate Content

Message 1 of 7 ( Views: 44 ) 03/08/2018 3:46 PM

Hi @davef_dci,

There are a few things that might improve your simulation.

1. Run to complete convergence. Set iterations to 1000 and let automatic convergence assessment stop the simulation for you.

2. Try using SST k-omega turbulence model with 8 wall layers, 0.6 layer factor and 1.3 gradation.

3. A surface wrap on the car might make meshing easier.

I think that possibly the air channels through the head lights and grill may be causing higher forces due to trapped air becoming pressurized. I would Close these off in CAD.

Cutting off the pressure I think only makes sense when trying to avoid cavitation, you are simulating air so there is no chance of cavitation. Uncheck Cutoff Pressure and work on getting an accurate result.

Hope that helps a bit.

All the best,

David

Report Inappropriate Content

Message 2 of 7 ( Views: 32 ) 03/08/2018 7:20 PM

Say David,

Very helpful. Sorry to be needy but a few questions.

a) I will run to convergence. thanks. the model is a bit slow on my machine but I understand the need.

b) You wrote: *Try using SST k-omega turbulence model with 8 wall layers, 0.6 layer factor and 1.3 gradation *I found options for SST k-omega under the physics of the solver but:

A) there are 5 different k-omega options including SAS, RC, Des, etc. Does it matter which one I use?

B) I don't see options for wall layers, layer factor and graduation. Instead, I have options for:

Length Scale

Wall Parameter

Turbulence intensity

Ven Dreist Constant

Kappa

Inteligent wall forumation

Far Field TKE

Far Field Omega

CMu

CE1

CE2

RNG Beta

RNG Eta

RNG CEO

Are you able to help map your suggestions to these parameters or am I missing something here?

c) Do I need to adjust the CAD model or the mesh or just re-run with this selected under Physics?

d) Looking for a bit of stylistic advice. I imported the CAD model in as a "negative" of the car cut out of a wind tunnel modeled in Solidworks. WOuld you generally recommend importing a solid and building the wind tunnel in native Autodesk? Is that a better approach?

e) The surface wrap function is really cool. Didn't know that existed. I didn't have any real issues importing or meshing my part but will a surface wrap result in a model that runs faster? If it improves performance or results I will use this surface wrap. If it doesn't impact performance I'd probably just stay where I am. What would you advise?

f) Your point about the open spaces in the headlight and grill are valid but this reflects the actual car - we've removed the headlights and positioned our air intake in that space and are also drawing air in through the radiator at the grill and headlights. You may have noticed that i've modeled a very crude engine and underbody to try to get some indication of the losses that occur in these areas. One objective was to help us select locations for these intakes as we do have some flexibility - but perhaps that should be a second model. I was thinking the model would be more accurate if it included air swirling through the headlight holes, over the engine and under the car - but perhaps this creates more errors that accuracy. Do you have a gut feel?

Thank you very much for you help. I am very grateful.

Report Inappropriate Content

Message 3 of 7 ( Views: 29 ) 03/09/2018 1:00 AM

FYI I re-ran the analysis using SST-k omega and accepting the default settings. Total force in the Y direction on the car (side of the car) was 265 lbs OUT of the car. Again, presumably this would be offset by an equal force on the other side but it seems very weird that the analysis is indicating the sideways force is outward - I really would have expected this to be inward. This just gives me pause and makes me wonder if I have some fundamental error. See attached image. Am I looking at this the wrong way?

Dave

Report Inappropriate Content

Message 4 of 7 ( Views: 24 ) 03/09/2018 8:02 AM

Hi Dave,

**b) You wrote: Try using SST k-omega turbulence model with 8 wall layers, 0.6 layer factor and 1.3 gradation I found options for SST k-omega under the physics of the solver but:**

** A) there are 5 different k-omega options including SAS, RC, Des, etc. Does it matter which one I use?**

Stick with the standard SST k-omega (no extra letters) the other models are for some specific situations but the standard is good for external aerodynamic situations.

**B) I don't see options for wall layers, layer factor and graduation.**

Sorry i should have been more clear. Wall layers are a meshing option. The mesh elements in the boundary layer region link closely with the effectiveness of turbulence models. You will see the option under options in mesh edit.

**d) Looking for a bit of stylistic advice. I imported the CAD model in as a "negative" of the car cut out of a wind tunnel modeled in Solidworks. WOuld you generally recommend importing a solid and building the wind tunnel in native Autodesk? Is that a better approach?**

** **

This approach is a good one. You have more control over your tunnel geometry in CAD than in CFD.

** **

**e) The surface wrap function is really cool. Didn't know that existed. I didn't have any real issues importing or meshing my part but will a surface wrap result in a model that runs faster? If it improves performance or results I will use this surface wrap. If it doesn't impact performance I'd probably just stay where I am. What would you advise? **

It may create a more regular mesh on the car which could be beneficial but if you are making progress with your current setup then stick with it..

**f) Your point about the open spaces in the headlight and grill are valid but this reflects the actual car - we've removed the headlights and positioned our air intake in that space and are also drawing air in through the radiator at the grill and headlights. You may have noticed that i've modeled a very crude engine and underbody to try to get some indication of the losses that occur in these areas. One objective was to help us select locations for these intakes as we do have some flexibility - but perhaps that should be a second model. I was thinking the model would be more accurate if it included air swirling through the headlight holes, over the engine and under the car - but perhaps this creates more errors that accuracy. Do you have a gut feel?**

I just feel that having these openings in the head lights might be what causes the outward forces as the air get trapped and pressurized within the car. I would be interested to see results without openings at the front of the car.

Does that help?

All the best,

David

Report Inappropriate Content

Message 5 of 7 ( Views: 20 ) 03/09/2018 11:47 PM

David,

Thanks so much for your help. I re-ran the analysis with the revisions you specified (filled in all the holes, used the SST solver, set parameters as specified, etc).

The results were reasonably close to what I had gotten using the original solver and with the holes in the model - within 10-15% or so which seems pretty good to me.

There are still two things that give me pause and make me worry that I have some fundamental error.

I manually calculated the expected "drag" on the car using the equation Fdrag = 1/2*p*Cd*A*V^2 where:

p = density of air = 1.22kg/m^3

Cd = Expected drag coefficient - published as .34 for the dodge Neon.

A = 21 ft^2 - directly from my cad model

V = 85 MPH

Using MathCad to resolve the units, this gives me an expected drag force of 132 lbf.

The CFD model is predicting a Force in the Z direction (in the direction of car travel) of 131 lbs for the HALF MODEL (with Slip / Symmetry at the centerline).

Can you please confirm that forces on a "half-model" with a Slip Symmetry constraint need to be multiplied by 2???? The software isn't doing that automatically is it???

If this is not the case that you need to double the forces on a half-model then my model is yielding exactly the same results as my hand calcs which would be **really** cool - but I'm assuming that I need to take forces into the car from the CFD analysis and multiply them by two in order to get the effect of the other side. Thus, the CFD is predicting a force in the Z direction that is double what my hand calcs predict. Ouch.

Is my reasoning that the Force directly into the car (in the Z direction) should be equal to the drag force correct or am I incorrect in this assumption?

If this is correct, can you think of a reason why the Force in the Z direction the CFD model is showing is double the hand calcs?

The other thing that gives me pause is that the HALF model is still showing a 240 lb force OUT of the centerline Slip-Symmetry plane. Again I am presuming that if I were to run a FULL model, this would be offset by an equal and opposite force on the other side netting out to Zero - but the direction of this force seems odd to me. Perhaps the half-car looks like an airfoil to the CFD and there is indeed "Lift" away from the centerline plane???

Report Inappropriate Content

Message 6 of 7 ( Views: 15 ) 03/12/2018 8:21 AM

Hi Dave,

**Can you please confirm that forces on a "half-model" with a Slip Symmetry constraint need to be multiplied by 2???? The software isn't doing that automatically is it??? **

Sadly yes you need to double the force if you are only using half the model.

**Is my reasoning that the Force directly into the car (in the Z direction) should be equal to the drag force correct or am I incorrect in this assumption?**

Yes this is correct, well it at least makes sense in my head!

**If this is correct, can you think of a reason why the Force in the Z direction the CFD model is showing is double the hand calcs? **

Couple of things:

Just as a double check, are you sure the drag force calculation is correct especially the projected area? This should be the frontal area.

Second could be inaccuracy of the wall calculator. The wall calc is quite sensitive the the mesh on the body. Maybe have a go with the surface wrapper and see if you can get a bit more regularity in the mesh on the car.

Other issues may be that the result is not fully converged or mesh independent. I.e. perform a mesh study and see if the force results change.

**The other thing that gives me pause is that the HALF model is still showing a 240 lb force OUT of the centerline Slip-Symmetry plane. **

I am a little stumped on this especially now that the air spaces gone. Maybe it is forces on the engine compartment. Maybe visualize pressure under the car to see where the large values are coming from.

All the best,

David

Report Inappropriate Content

Message 7 of 7 ( Views: 8 )