This is really important because these pictures are going to be our reference. If they aren\u2019t orthogonal, the points on the side view won\u2019t match up with the points on the top view, no matter how much image manipulation we do.<\/p>\n
That being said, with all of the cameras and technology that we have at our fingertips today, this should be easy, right? Errrrr\u2026 turns out not-so-much. Well, I suppose it depends on your circumstances. I\u2019ll show you a picture to explain mine:<\/p>\n
Without distraction or interruption, however, the technique is quite simple. All you need to do is take a zoomed-in picture from as far away as possible. This imitates an orthogonal lens and, at least in my case, is the closest I can get. I also recommend taking these pictures during daylight hours unless you have a well-lit house and a long corridor. I learned this the hard way so that you don\u2019t have to! I made sure to get TOP, BOTTOM, FRONT, BACK, LEFT, and RIGHT images, but technically that\u2019s a bit overkill for this project since there is a lot of symmetry in this model.<\/p>\n Step 2: Rotate, Crop, and edit. <\/strong><\/em><\/p>\n The first two steps are necessary in order to make sure the pictures will line up, and the \u201cedit\u201d step is a trick I use \u2013 I like to remove the background to make it even easier to line my pictures up. This also helps me because I really zoom in and I can find the imperfections\/non-orthogonal bits of my pictures as I go. Like I said earlier, the pictures are close, but not perfect. You can use any photo editing app to do this as long as you have the ability to Rotate, Crop, and Remove Background. I like to use GIMP because it is free and it even allows you to crop directly to content after you remove the background, but my husband swears by photopea.com which is also free and doesn\u2019t require an installation. Here are some of the photos I collected and edited:<\/p>\n We\u2019re off to a good start! Now the fun part \u2013 we get to open SOLIDWORKS!<\/p>\n Step 3: Add your pictures to a new SOLIDWORKS part.<\/strong><\/em><\/p>\n Take a few measurements and add your pictures to your SOLIDWORKS model, being sure to scale as you go. A trick I used here was to create a 3D sketch first with a \u201ccage\u201d around the exterior measurements that I took. This made it easy to visualize where each picture should be. I also created planes for each sketch picture to match and inserted my pictures directly onto these planes (Tools<\/strong> > Sketch Tools <\/strong>> Sketch Picture<\/strong>). The simplest way to scale these pictures is to set the Width or Height in the properties box and move them using the X and Y positioning boxes.<\/p>\n Here\u2019s what it looks like so far:<\/p>\n Off to a good start! Now let\u2019s get to modeling.<\/p>\n Step 4: Choose a place to start and dig in.<\/strong><\/em><\/p>\n This is the second-to-last step, but it is a big one. My goal in this next section is to step through most of the techniques used to finish the mechanical design using the reference pictures. If I attempted to step through every single thing, you would be reading a chapter book, so I won\u2019t do that. You\u2019re welcome. However, if you do want more details about any of it, feel free to comment below or send me a message on LinkedIn.<\/p>\n Because we have so many perfectly imperfect photos, it is important to pick one or two as your \u201cdefault\u201d \u2013 as in, if things aren\u2019t matching up, you know where to go. I chose the LEFT side view as my default and FRONT as my backup for most things. Another tip before we dig in to the nitty-gritty is to organize features into folders in your FeatureManager Design Tree. This is a good idea for any model that is going to have a large number of features because it allows you to quickly edit specific sections as needed without looking through a thousand features first. Also, for the reference pictures specifically, it allows you to very quickly turn them on\/off by suppressing the Folder itself rather than having to find and Shift + Select the group of sketches. For reference, here\u2019s what our FeatureManager Design Tree looks like so far:<\/p>\n The first part of the car we are going to work on is the hood and the technique I used here involves surfacing. Many moons ago I recreated a Delorean using 99% surfacing, so I figured this would be a fun way to start things off.<\/p>\n We\u2019re going to create a Surface Loft, so we need two sketches. Looking at our LEFT side view, we can see that these sketches will need to be on non-default planes, so let\u2019s create those first. Sketching on the Right plane, I created two lines representing the start and end of our loft.<\/p>\n From here, I selected the lines individually and used the shortcut key (S<\/strong>) to select the Plane<\/strong> feature. The first reference is the line and the second reference is a plane \u2013 in this case we can select the RIGHT plane and make sure to select the Perpendicular relation.<\/p>\n Another trick to use here is to take advantage of symmetry. I only traced half of the vehicle, making sure to add a tangent relationship to a horizontal construction line at the middle so that, once mirrored, the surface would look smooth. From here, we can use the Surface Loft<\/strong> command, selecting the two sketches we made to loft between and then Thicken<\/strong> them, using the FRONT view as a reference for how much to thicken them. At this point, I realized the fatal flaw in this technique: our front and back edges end up being curved.<\/p>\n I could have gone back and finished tracing\/creating sketches that would have allowed me to do a normal loft, but at this point, I was committed to the technique, so I went back and added a few steps to correct this. First, I rolled back in my tree to right after the surface was created and used Surface Extend<\/strong> to create a larger surface than needed.<\/p>\n Then I rolled back to the end (after thickening) and used the Cut with Surface<\/strong> command, along with the two planes we originally created, to cut away the extra. This leaves us with two beautiful planar faces at the start and end of our hood. Here\u2019s what the hood looks like after applying Mirror<\/strong> to the half we created:<\/p>\n Way better! Now all that\u2019s left to complete this feature is to add a couple of fillets, although we can easily leave this as the last step in modeling (this is often advantageous, but in this case, it is fine to add them now). Either way, it\u2019s all good in the hood.<\/p>\n The next portion of the car I modeled was the grill, but I used simple extrudes and cuts here, so let\u2019s move on to the front bumper.<\/p>\n The technique I used here involves the massively useful Intersect <\/strong>command. We begin this technique by sketching the basic shapes we see in the bumper from the TOP and FRONT views. I sketched these on the default TOP and FRONT planes.<\/p>\n Now we extrude each shape out past the point where the material actually exists, making sure to un-check the Merge<\/strong> box in each feature. We get this crazy thing. Don\u2019t panic \u2013 it will get better, I promise!<\/p>\n Now it is time to activate the magical Intersect<\/strong> command. After activating the command, we want to select all of the bodies we just created and click the Intersect<\/strong> button after selecting Create both<\/strong> in the properties box. Then we can start clicking in the graphics area to remove excess material. I find this to be the simplest way of getting exactly what I want, especially with a large number of bodies, but we could have also checked and unchecked boxes in the Regions to Exclude<\/strong> area of the properties box. Once we have exactly what we want, we can select Merge result<\/strong> and hit ok.<\/p>\n Now all that\u2019s left is to Mirror<\/strong> our body on the RIGHT plane, add a quick Extrude<\/strong> for the connector (traced from the BOTTOM reference picture), and add some fillets to get rid of sharp edges.<\/p>\n Beautiful and fairly simple really, considering all of the shapes we created with a single command!<\/p>\n The next part of the car I decided to tackle was the front fender. I could have used the Intersect<\/strong> technique again, but because it was so simple I decided to just use the Extrude<\/strong> and then Cut-Extrude<\/strong> technique here. From the LEFT side, I traced the profile and used the Extrude<\/strong> command to draw out a solid close to the correct size.<\/p>\n From here, I traced the profile from the TOP, and cut away the excess material using a Cut-Extrude<\/strong> by selecting Flip side to cut<\/strong> in the command and selecting the body we just created under Feature Scope<\/strong>.<\/p>\n Next, I added a couple of fillets to match the original side profile before running into an issue! Due to the imperfectness of our pictures, the profiles didn\u2019t line up correctly, resulting in an unwanted flat face at the front.<\/p>\n Yikes! Luckily, this is a super easy fix. All we have to do is right-click on the face and go to Delete Face<\/strong>, being sure to select Delete and Patch<\/strong> in the properties box.<\/p>\n Instant fix! Now, all we need to do is add a couple of fillets, Mirror<\/strong> our body, and move on to the next feature.<\/p>\n At this point, I basically used the techniques we discussed above to create a bunch more geometry \u2013 wheels, the windshield, the side panel, the dash, steering wheel, side step, floor, front axle, back axle, back bumper, and the back panel\/bumper were all fairly straightforward with few new techniques of note, so let\u2019s fast forward a bit to the floodlights because these are a bit more interesting. Just to catch you up, here\u2019s our model so far:<\/p>\n For the support portion of the floodlights, I started by tracing the profile for the first segment from the LEFT side view and then from the TOP view (modified slightly so that things line up later) like so:<\/p>\n Then I selected the sketches and used the Project Curve<\/strong> command to project the first sketch onto the second sketch, essentially defining their intersection. Here\u2019s what the resulting curve looks like:<\/p>\n This is perfect, *except* it is obviously missing a portion. I got around this by creating a 3D Sketch<\/strong>, selecting the curve and using Convert Entities<\/strong> to bring it over, and then drawing in the portion that was missing manually, being sure to double-check my sketch against my reference pictures. I also took advantage of the fact that we can Mirror<\/strong> within a 3D Sketch<\/strong> now to complete the curve on the other side.<\/p>\n Beautiful! Now it is time to Sweep<\/strong> some actual material into existence. Many moons ago we would have had to first create a profile consisting of a circle at the end of our path, but today SOLIDWORKS makes it incredibly easy with the Circular Profile<\/strong> option inside of the Sweep<\/strong> command. I opted for this, obviously, setting it to a diameter of 1.25in based on the reference pictures. Then I repeated the process for the second support beam and reused the same paths (using Convert Entities<\/strong> in two additional 3D<\/strong> sketches) to create the T-joint.<\/p>\n Gorgeous! Creating the Flood Lights themselves was actually pretty basic, so I won\u2019t go into a ton of detail here except to say that I used a Revolve<\/strong> to create the connector and I used a Circular Pattern<\/strong> to create the detailed cuts around the edges of each light. I also went ahead and added fillets.<\/p>\n Now that we have most of the external car parts\u00a0 (besides seats, which were also created using the techniques previously discussed), it\u2019s time to move on to the internals. This part was actually a bit trickier since our reference pictures don\u2019t show everything inside the vehicle, but also critical since we are planning on adding in our electrical components and then modifying them in subsequent blogs. The trick I used here was to actually go back to the physical car and look at it\u2026 with my eyes. This required getting up, which was a good idea at this point anyway, so it was a win-win. I then approximated some of the sketches and measured some parts using digital calipers.<\/p>\n For the battery compartment in the front of the car, I started by hovering over the hood and hitting TAB<\/strong> to hide it. Then I sketched out the approximate shape that I saw after looking under the actual hood and extruded it to a depth based on the LEFT side reference picture. Next, I used the Shell<\/strong> command, selecting to remove the top face and extruded a top to the compartment using existing geometry and using Convert Entities<\/strong>.<\/p>\n Fairly straightforward so far, right? Next, I added what I\u2019m called the \u201cunderbelly\u201d \u2013 again using the partial information we get from the side view \u2013 before moving on to the pedal and the area that houses the electronics from this and connects to the battery area in the front. The rest of the conduit was fairly simple after going back and forth, but I do want to mention one place that I made a mistake the first time using the Shell <\/strong>command. Essentially my technique was to Extrude<\/strong> the conduit and then Shell<\/strong> it out to create a path for our wires, but the timing of the Shell <\/strong>matters. Make sure you can visualize the end product before hollowing it out because you might want to combine multiple bodies before activating this command. Here\u2019s what most of our conduit looks like in isolation and then in the context of our whole vehicle.<\/p>\n Now that our car is pretty much done, it\u2019s time to add some details to the back and front bumpers. Jumping into a BACK view (Ctrl 2<\/strong>) we can trace the geometry from our reference picture.<\/p>\n From here we can use the Split Line<\/strong> command, being sure to select the appropriate faces along the back bumper, to split our faces and prepare them for painting. I repeated this on the front and added some fun text at my daughter\u2019s request.<\/p>\n The final piece I added in was a custom unicorn horn \u201cwindshield wiper,\u201d again at my daughter’s request, using a simple Extrude<\/strong> and some Fillets<\/strong>.<\/p>\n We\u2019re done! We made it! Now it\u2019s time to make it shiny and give it a paint job.<\/p>\n Step 5: Give your vehicle a dream paint job.<\/strong><\/em><\/p>\n There are so many different ways to add appearances, but the way I like to do it is mostly from the graphics area. All we need to do is click on a part of the car we want to \u201cpaint\u201d and then select the largest relevant area to paint. What I mean by this is that we want to first apply to the part, then to bodies, then features, and finally faces if we are getting really specific. I\u2019ll give you an example.<\/p>\n The majority of the car is going to be one color \u2013 blue, as selected by (you guessed it) my toddler. Let\u2019s start with that by clicking anywhere and selecting the part before grabbing our blue appearance from the task pane.<\/p>\n This turns our entire car blue!<\/p>\n Now we can start getting a bit more specific. The seats and the window\u2019s glass are separate bodies, so we can apply an appearance at this level. The same thing goes for most of the grill, so we can apply an appearance and get more specific with the lights and turn signals later.<\/p>\n Next, we can apply to specific features (the wheels and the headlights require this), and finally any faces that need to be unique. This technique ensures that we are being as efficient as possible. I also want to mention that we can copy\/paste appearances between sections as needed as well using the same menu.<\/p>\n Fantastic! Our new coat of paint looks awesome.<\/p>\n The last thing we want to do is add some decals (NEEDS MORE UNICORNS), but let\u2019s wait until we are in SOLIDWORKS Visualize to do this since we need to reapply there anyway. Note: I added a unique appearance to the unicorn horn in preparation for exporting so that applying a decal would be easier in Visualize.<\/p>\n With our SOLIDWORKS Visualize tab activated, we can go ahead and click Export Advanced<\/strong> to jump into Visualize. Applying decals in Visualize is easy \u2013 all we need to do is activate the Appearances tab and right-click in the background > New Decal<\/strong> > Image\u2026<\/strong> before selecting the picture we want to use.<\/p>\n![\"\"](\"https:\/\/blog-assets.solidworks.com\/uploads\/sites\/4\/ec201-scaled.jpg\")
<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/center>I repeated this for the second plane before switching to a FRONT view and opening a sketch on the plane we just created that is closer to the front (I renamed this to \u201cGrill Plane\u201d in my tree for the sake of organization and sanity). Now we get to trace the front of the hood! Note: it is important here to trace our reference picture in a FRONT view rather than in a view normal to the angled sketch plane that we just created. I tend to personally gravitate towards using lines and arcs here instead of splines, but you could use splines just as easily. Here\u2019s what my trace looks like:<\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n<\/a><\/p>\n