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2010 Camaro Body Tutorial
First a little info about this tutorial. This tutorial assumes you know the basics of modeling as
well as your way around SolidWorks. It is best that you have some surfacing experience and
understand what each of the surfacing tools do before you tackle a project like this.
Understanding basic sketching principles, the how and why of sketch relations and the use of
projected curves is a must and will not be covered in detail here. Don’t expect to be a surfacing
expert by completing this tutorial. It’s more of a procedural guide on the approach to modeling
a car body since it seems to be one of the harder topics. This is the first time I have drawn this
car and I will be writing this document every step of the way so any mistakes or errors we
encounter are actual problems I run across during the model. Also this is only the third car I
have modeled in SolidWorks and the fourth car overall so I am still learning myself. Good Luck.
The first step to modeling anything based on a current product is obtaining as many photos (or the real object) as you can. When modeling a car it is essential that you have a good set of blueprints. You need to have a side, front, back and top view. If you don’t there will be a lot of guess work involved and your job will be that much harder. You can work off of photos, but there will be perspective that will throw things off if you aren’t aware of it. If you are designing a part based on artist sketches it is also important that you have these reference prints to work off.
Before you get started there is a nice feature called Auto-Trace within the sketch picture. While this won’t really help you out with the car, if you have a nice high contrast sketch of a consumer product it may be just what you need. Auto-trace can be turned on from the Tools>add-ins menu. It will appear within the sketch picture dialog, but I am not going to go into that here. Just be aware of it and play around with how it works because it might come in handy one day.
The first step in the actual modeling process is laying out your blueprints. Make sure you use your standard planes and take the opportunity to rename the sketches for your own benefit later. Drawing something like a car will leave your feature tree a mess so take any chance you can to make folders and name sketches or features. Especially if you have to roll back the end of part marker or make adjustments. This is also helpful if someone else needs to work with your model.
Setting up Blueprints
Start a sketch on the Right Plane. You will want to use the Sketch Picture button to add your Right blueprint image. If the Sketch Picture button isn’t on your Sketch tab you can add it by right clicking on the sketch ribbon somewhere, customize and add it. Also you can go up to the Tools menu, Sketch Tools>Sketch Picture. Setting up these blueprint images so they line up is extremely important to the quality of your model. If each image has a different scale or border you will need to ensure they are lined up. These Camaro blueprints are pretty good but others may not be. Make note of the transparency option in the Sketch Picture dialog. I prefer to leave the picture backgrounds as is but you can alter them. It’s really a personal preference. The Right image will be placed automatically but you can move it while the Sketch Picture dialog is open. I like to leave the bottom left corner of the picture
at the origin. Also note while you are in the Sketch Picture dialog that 6 handles will appear around the border of your image. These handles will stretch the image so be careful you don’t grab them. OK the sketch picture and exit the sketch.
Start a sketch on the Front Plane and follow the same procedure for adding the Front Blueprint image. My preference is to move this image so that it is centered on the origin. This allows me to mirror surfaces across the Right Plane later on in the process. Be very careful not to stretch/scale the image as you move it. Since we are not exactly replicating the car getting it close will be just fine.
Follow this same procedure for the Top Blueprint image on the Top Plane. For the Back you will want to create an offset plane based on the Front Plane. This isn’t really necessary but I like to keep the back image at the back of the car.
Notice my feature tree. I’ve added a Back Plane for the back blueprint image. I’ve also added a folder called Blueprints and all of my named blueprint sketches are within this folder.
Since the Camaro is a new car you have the benefit of using the manufacturer’s website. If you go to www.chevy.com you can “build your own” Camaro. Inside here you can rotate the car 360degrees. This is a valuable asset when trying to figure out body lines and I recommend you do this when possible.
When you plan out the approach to modeling this car you need to look at the hard lines of the body and find good places to break up your surfaces. The door and front fender keep the same bodylines but the rear fender flares out. So at a first glance I want to model the door and front fender first. Sometimes it’s best to start with the roofline or the glass but I think the side of the body will give the most trouble so I want to tackle it first. Start a new sketch on the Right Plane and we are going to layout the top ridge of the fender/door. Start by drawing a spline from the front edge of the fender to the back edge of the door like below.
Now use the spline handles to control the curve and match the shape of the body. I ended up with my handles like this.
Keep in mind when making these splines that the body lines on other parts like the front nose cone will end up with a tangent relation. Make sure your handles are reasonable in their direction to account for this. End the sketch and start a new sketch on the Top Plane. We want to draw the same body line we just did, only from the Top View. In some cases (such as this) I like to use Convert Entities on that first sketch onto the top plane and make it a construction line. The reason I do this is so I can add a horizontal relation. It helps me early on in the model to know my blueprints are in a reasonable spot and that my project curves will hit where I want them to. Again you only want to draw the start and end of your spline. Make them horizontal from the endpoints of your converted construction line and make sure they hit the same spot on the blueprint image as our original sketch.
Sketch on Sketch will allow you to take two 2d sketches and create a 3d curve where they meet. Sketch on face will be used later possibly for things like sweep paths for window seals. This allows you to take a single 2d sketch and project it onto a 3d surface. Make sure you use Sketch on Sketch for now until otherwise noted.
Select both sketches and create your first bodyline. Now for some reason these projected curves often aren’t visible when a sketch blueprint is there so you may need to rotate the model or hide some of the blueprint sketches to see this curve. If you select the curve in the window or in the feature tree it should be easier to see. Also take this opportunity to rename Curve1 to something meaningful and notice that both 2d sketches are consumed by the Curve1 feature because they are children to it. Once we use this curve along with others to create a surface this will happen again. I named mine Fender Door Ridge.
From here on out I will give you very general guidelines to help, but the point is to learn and not regurgitate. I won’t be telling you to OK the sketch, it’s just implied. If I use something new I will point it out but the procedure is the same from here on out for the majority of the body. The next curve will be the front edge of the fender. In a new sketch on the Right Plane I draw a vertical line. I select the end point of the line and the 3d curve from the previous step and add a coincident constraint. Here it’s important to note the pierce constraint. An example of the pierce constraint would be drawing a 2d sketch where a 3d curve will intersect this sketch at some point. Pierce will make your sketch intersect this 3d curve. In this case our 2d sketch is on the Right plane while our curve never intersects this plane, so coincident must be used. Also you may notice if you select the endpoint of your 3d curve that you have no relation options. This is because the endpoint doesn’t lie on the plane. However if you select the entire curve it will be “projected” but not actually drawn in your sketch. Make sure after you apply the coincident relation that you try to move your line all the way to the end of your curve. If you are not at the endpoint it will cause issues with your surfaces so this is important. Another thing you could do is use Convert Entities on your 3d curve or you can go back to the 2d curve on the right plane. This is possibly a more stable method because it allows you to pick an end point. This way if you go back and edit curves they will more than likely update better. I will let you make the call on how you do this because part of learning is finding out what works and what doesn’t. It’s a good idea to create a new part and play around with these projected curves and watch what happens when you make changes.
The second 2d sketch this time is on the front plane and not in the top plane. The reason for this is simply the direction of curvature of the model. If you look at this from the top it would be a straight line and you would not accurately mimic the curve. It will be up to you to decide which views to sketch in and it will take a bit of practice to pick up on this. Be prepared to do it wrong several times. Some compound curves may also require you to try a few different methods. There is nothing wrong with trial and error, so don’t get frustrated if you have to get it wrong a few times.
The first thing I do is create a 2point spline. Before I mess with the handles I apply a coincident relation between the endpoint of the spline and the 3d curve (either by selecting the curve and converting, then using it as a construction line, or simply applying it to the curve. Remember it’s up to you to find out which works best. Making sure that both 2d sketches intersect the 3d curve at the same point will ensure your Projected Curve will be in the right spot. Go ahead and adjust the curvature to match the blueprint.
Again, and I won’t always mention this; apply that coincident relation with the 3d curve so you know the end point is coincident. When you try to drag the spline to the end of your 3d curve the little coincident icon will appear, but if you don’t convert the line, updates later may cause you problems, hint hint.
For the second sketch I’m going to give the top view a shot since there is some curvature in this view. We will not be able to do this for the part of the door below centerline because it is hidden in the top view, but for this edge it should work just fine.
Next we complete the 4th^ 3d curve which will be done from the side and top views. Don’t worry about the wheel arc just yet as we will trim the surface for that. If you try to create the surface with the arc already cut then it will produce some unwanted geometry. We are going to make this curve before the back edge of the door in our feature tree. This will let us go back and edit that back edge to meet the bodylines properly or maybe create a new 2d sketch on the front plane. Only time will tell.
For the front edge of the fender go ahead and use Convert Entities and make it a construction line. Then apply a coincident constraint between a spline and its end point. At a first glance you may think this bodyline is straight but once you draw your spline you will have to edit the handles a little bit to match it. When you are drawing your top view curve don’t worry about the wheel arch. Try to get the underlying geometry to line up.
Pay attention to the curves on the blue print, especially the nose cone lines.
After you make this 3d curve (and name it), roll the end of part past the door back edge curve you created. Now notice how short it is of our body midline. So it looks like the top view we used for it just isn’t going to work. What I did was delete the 3d curve for the back door edge and moved the sketches to the end. I also deleted my top view sketch that was used for the back edge of the door.
We know from looking at pictures and rotating the “build your own” model on the Chevy site that this door line appears to be close to the same arc as the front edge of the fender. Keep in mind you do not want your lower spline handle to be vertical; we still need a crisp body line. Once we make the surface (and the bottom part of the door) we can edit this spline if we feel it doesn’t look right.
To make this projected sketch work out we need to go back in and edit our side view sketch to make sure that it is coincident with our door midline 3d curve. Then our new projected curve should look good.
This is a very important part of the model, the first surface. This surface can be Lofted, Boundary or filled. And although it might seem like they would all be the same, each one may produce a different result. We don’t have any other surfaces so we aren’t worried about constraints with surrounding surfaces, but make use of the zebra striped previews in each surface to see any differences.
Lofted, make note of the green handles on the loft profiles. You can manually move these from one side to the other. Each profile needs to have these on the same edge or the loft will try to twist.
If you rotate a filled surface around you will notice it will not work. The issue is that all 4 edges are curved in several directions. It makes it hard for filled surface to work. This would work well if we had a surface that we needed to trim and fill. Without the use of surrounding surfaces to apply tangent or curvature relations, filled surface is very unstable. For this surface I chose a Boundary Surface. Loft and Boundary surfaces will be nearly identical in this instance. The benefit comes in the needed curves to create the surface. Loft needs a start and end profile. Boundary can be created with two curves; one could be a guide similar to a sweep only your profile doesn’t need to be 2d.
Because the bottom half of the front fender shape is a little different than the door, we are going to go ahead and cut the wheel arch from the surface we just made so we can start filling it some more panels.
When you draw the sketch to cutout the arch draw it large enough so we can also use it to cut the lower part of the fender later. There is no point to make the same sketch twice so we want to ensure we have enough to use later. Unfortunately it’s not a simple arc, but a spline can fit this shape by just using its end handles.
A common mistake here would be to use multiple points to make the arc but this will yield bad results in your surfaces. Use the Trim Surface command to trim away the wheel arch from our surface. Also as another note, if your surface has blue edges like mine below, this means your 3d curves are visible. You want to be very careful when making surfaces that you select the edge of the surface and not the 3d curve. The 3d curve will not allow you to make use of tangent or curvature face constraints.
