11 Replies Latest reply on Jan 7, 2016 12:05 PM by Boyko Tchavdarov

    How to calculate Drag Coefficient of a Car

    Peter Pedro

      I am very new into Solidworks Flow Simulation. I want to undergo a flow simulation of my car like a wind tunnel testing in real life. I've done the steps coming from the forum and some other sources but none of them has the answer on how to calculate the Drag Coefficient of the car using the formula. I am new into simulations and I am learning it bit by bit in some point. The attach photo is the formula for the Drag Coefficient, I want to know how to calculate the drag, fluid density, velocity, reference area. I want to explain this in my thesis defense concerning how did I get the Cd of my car using the formula.


      I've tried something with global goals, and surface goals but I think I didn't get to where I want it to be.


      Hope you guys can help me out step by step into this. I'm going nowhere.


        • Re: How to calculate Drag Coefficient of a Car
          Amit Katz

          Does your drag force calculated value make sense? How does it compare to primitive bluff bodies (ie spheres, egg shapes) with comparable characteristic lengths at the same free stream velocity? Let's take it step by step and see where the problem is.

          • Re: How to calculate Drag Coefficient of a Car
            Amit Katz

            These huge column-like images are a little bit of a pain to work with with the way this forum is set up, I think it would be easier in the future to just upload your screenshots individually.


            Your process looks OK for a first step, but now it's time for a sanity check. How long is your car? Knowing the characteristic length and the free stream velocity of the wind will allow a rough estimation of the drag and lift forces, that way you can check if you are on the right track.


            I also find it handy to never run the simulation without first meshing the model and check the mash by hand using cut plots. If you upload your projects with all the settings that you set we can help you find where the errors are (if there are any.)


            Finally, an easy way to check your front sectional area would be to make a sketch on a plane parallel to the front of your model. You can use the "Convert Entities" sketch tool, which projects lines and edges from your geometry onto the sketch. Then once your section is all sketched out you can use the Evaluation tools to calculate the area inside the section.

              • Re: How to calculate Drag Coefficient of a Car
                Peter Pedro

                Sure, I'll keep that in mind.


                My cars length is 3073 mm and height in 801 mm. Here are my 3d models. One is with the original mesh in my trials and the other model is a new export with more meshes.

                Thanks a lot everyone. It would be difficult for me to try and solve this alone. If you could provide the step by step procedure (would be nice if there's a screenshot as well) on how to calculate the drag coefficient using the formula and how to get the frontal area. You guys are a great help to me right now. Thank you


                @Seckin Uslu

                Thanks a lot. Here are my models.

                  • Re: How to calculate Drag Coefficient of a Car
                    Amit Katz

                    OK, I haven't had time to look at your mesh yet, but something is definitely wrong with the simulation. Let's look at two extreme examples under the same conditions. First of all the Reynolds number for your flow is ~ 1e7, so we're well within the fully turbulent domain.


                    Extreme case 1: brick

                    If your car was a square brick, 3m x 0.8m x 0.8m, the most un-aerodynamic shape I can imagine, the drag coefficient is ~ 2.05 and the resulting drag force at 50 m/s is about 2000N


                    Extreme case 2: aerodynamic body

                    If by some happenstance you designed the most perfectly aerodynamic shape possible, with a Cd of 0.04, the drag force will be about 30N (here for the sake of argument I just assumed the x-sectional area is a circle with diameter 0.8m)


                    Now, the software calculate your drag force as a whopping 37.5 thousand Newtons, so something is waaaaaaay off. It's time to go back to the software and figure out why your simulation didn't work.

                    • Re: How to calculate Drag Coefficient of a Car
                      Amit Katz


                      I finally had a chance to run your model. The first thing I noticed was that it was about 10x as big as you thought it was (30 meters long instead of 3.) This was the reason why the forces were so large. I can only assume there was some unit error involved in exporting or importing the STL files. By the way, most CAE software that I've run into doesn't play well with STL files, I recommend sticking with Parasolid when possible. I'm guessing your created this model in a NURBS type environment, that's not usually what CAE is built around.


                      I used the scaling feature to shrink the model down to 10% of the original size and got to work.


                      Once I had the solid geometry in the software, the rest was cake. I used a projected sketch to get the cross-sectional area:

                      car drag1.PNG


                      I added a floor with a 50 m/s moving wall boundary condition to simulate a road (since this is a car and not an airplane.) It's important to have this wall with the same velocity as the air, otherwise the simulation will develop a boundary layer that will interfere with the aerodynamics of the vehicle.


                      Finally I ran a rough simulation that gives reasonable numbers, although I wouldn't rely on these since it's just a quick and dirty first pass.

                      car drag2.PNG


                      Good luck!

                  • Re: How to calculate Drag Coefficient of a Car
                    Boyko Tchavdarov

                    My general piece of advice when calculating Drag:

                    Always use a simple benchmark model case  that contain the essence of your problem (similar topological main surface that contribute to the drag AND the same surface finishing !) in comparison to experiment data to tune the mesh resolution AND the MODEL roughness of the surfaces.


                    Accurate aerodynamic drag of a car is not easy to calculate even in a fully developed turbulent flow and very difficult in relatively low Re.
                    Keep in mind that Flow Simulation utilize algebraic wall function which is quite universally applicable to small and large Y+ values on which the drag depends very strongly. It means that NOT always finer mesh will give you better results than a bit more coarser mesh. For that reason tuning the mesh (as well as the MODEL roughness value) by first running the benchmark model is absolutely necessary.