Tracing in the 21st century Is 3D.
SOLIDWORKS is a powerful tool that millions of people use every day to design all sorts of products across all sorts of industries. There are a handful of design methods used to create 3D geometry inside of SOLIDWORKS. Some use the “bottom-up” method, which is where parts are created and then assembled independently from each other. Others use the “top-down” method, where all the parts are formed in an assembly. Others use hybrids of these two, while still others just drop already existing models into their assemblies as though they were virtual “name-withheld” building blocks. All of these methods are creating a virtual model of a product or system. But what happens when a product already exists in the real world and there are no virtual models of it? How do we reverse engineer a product that has a digital counterpart? To do that, we start from scratch.
Starting from scratch is not difficult for any of the above scenarios. We will show a method for parametrically modeling parts from scans and imported data.
21st Century Tracing
Everyone and anyone who has ever drawn with a pencil, crayon, pen, and so on, knows that drawing in 2D is not very difficult. As children, we were taught to stay inside the lines during after-nap coloring time. We graduated to follow the lines in order to better replicate our drawings. From that point, people diverged. One group focused on freehand drawing, creating new, unique geometries that weren’t perfect but were close enough. The other group focused on perfection. Transparent paper was used to lay over the original geometry and trace it until the two layers of paper were indistinguishable. Both groups came together to make parts in 3D with SOLIDWORKS.
The first step in bringing a real-world product into the digital world is to have a picture or scan of the product. If you are making a 3D model and have access to 2D views, you can import those views. As seen below, here is a cutting tool that will be used to show how to import views into SOLIDWORKS. Note that the three standard views were taken in real life: the top view, the front view and the side view that would normally be used in a SOLIDWORKS drawing.

A quick tip for this part of the import is to have the object of interest with some sort of scaling device. The front view above has the cutting tool on top of a standard sheet of letter-sized paper. Then both are on a dark wooden tabletop. Because we know that a standard sheet of letter paper is 8.5ʺ by 11ʺ, we can use that as our defined scalar inside of SOLIDWORKS. From here, we can create the first sketch in SOLIDWORKS. Using the front plane, create two lines perpendicular to each other and dimension them to the appropriate 8.5ʺ x 11ʺ as shown in Image 4.

Exit that sketch and create a new sketch on the front plane. Then go to the dropdown menu and choose TOOLS-> SKETCH TOOLS-> SKETCH PICTURE (Image 5). The reason we put the picture onto a new sketch is so that we can scale the picture against the original, dimensioned lines (Image 6). Using the scale arrows of the picture, we adjust the front view picture such that the piece of paper in the background aligns with the 2D lines from the first sketch. Exit this picture sketch. Create a new (third) sketch on the front plane. Finally, you can start tracing the geometry of the cutting tool.
A few tips on this. First, use whatever sketch tools you feel are necessary to properly trace the outline of that geometrical dimension—front plane in this example. This is the hybrid approach mentioned earlier. Trace until your sketch is good enough. Then freehand and dimension the sketch as best you can. In this example, we use a spline to blend into the top arc. Then a straight, angled line for the blades front end. The trace (when dimensioned) had that angle at a length of 1.058642 inch, but the edge is probably 1.00 inch, so the dimension needs to be adjusted.


Once this front plane sketch is good enough, repeat the sketches on the top plane. However, to make things a little smoother, the first top plane sketch (sketch # 4 in this succession) should use boundaries that you defined in your front view trace. These construction lines will allow better scaling when you go to insert the top picture on the second top plane sketch. Then, trace on the third top plane sketch. Wash, rinse and repeat until you achieve the right plane. Image 8 shows these construction lines tangent to the top view sketch and side view sketch.

Now that the wireframe has been developed for the tool, it is easy to make it a solid model. There are many methods that can be used to create a solid model, but most users would opt to use surfaces for this model because there are ergonomics to consider—the tool has to fit comfortably in the hand.
This can be somewhat of a challenge as using surfaces in SOLIDWORKS is more of an advanced skill. The trick to making this model manageable is to divide the tool into multiple sections, surface those sections and then knit the entire structure and check off the Created Solid in the knit feature.
STP Right Up
Advanced surfacing techniques also play a vital role when importing non-native files in SOLIDWORKS. A new function was released in SOLIDWORKS 2017 that allows the software to create a container part that links to a non-SOLIDWORKS file format called 3D Interconnect. This function takes the place of importing non-native files.
Tip: If you are using product data management (PDM), be sure to keep the original file in the vault with the SOLIDWORKS file; otherwise, you run the risk of reference issues later on down the road.
To turn off this feature and go to System Options -> Import -> uncheck Enable 3D Interconnect (Image 9). Turning this feature off allows you to use the regular import function and bring non-native files into SOLIDWORKS.

With 3D Interconnect disabled, you can import a non-native file in the traditional SOLIDWORKS manner.
Select a new part from your template, resolve surfaces (if it’s an STP file) and then the model will have a single feature called IMPORTED and, invariably, it will have the dreaded yellow color associated with a warning. Run the Import Diagnostics Tools to show gaps and surface errors. The best first step is to Attempt to Heal All. Maybe it works, maybe it doesn’t. Then you can try to heal/repair individual surfaces. Sometimes it just creates more surface errors. Finally, you can delete those surfaces and the gaps list starts to increase (Image 10). This is a great place to start trying to manually repair the model.

Once faces have been deleted, it’s time to close out of Import Diagnostics and start manually repairing the model. The good news is that the surfaces that were giving you issues are now deleted. You can also delete additional surfaces as necessary. It is highly recommended that you familiarize yourself with 3D sketches in SOLIDWORKS whether you are a beginner or a power user. They will save you countless hours when recreating surfaces from an imported model (Image 11). Another quick tip is to fully delete surfaces (Image 12) instead of trying to delete and patch. Otherwise, for imported models, you will fall down a rabbit hole.


Once you have reestablished the wire frame, use the Fill Surface feature in the surfaces toolbar and select your 3D sketch entities. After you have those surfaces to your liking, use the knit feature, as before, and select Make Solid. Every model is different, but if you approach all of them with a one-step-at-a-time mentality, the process is straightforward.
Tip: Most 3D models sent to you are STP files because it has become the industry norm. The thing with STP files is that they are a surface model. If you want to avoid the issues with surfaces altogether, ask for a Parasolid model. These have the file extension *.x_t. SOLIDWORKS uses the Parasolid kernel for its geometry so that any file saved as .x_t will open with no surface issues at all.
Using SOLIDWORKS to virtually create models of real-world parts can at first seem daunting. Using the Sketch Picture command will allow you to trace sketches from scans or pictures. Using 3D Sketch in combination with deleting surfaces will allow you to fix imported models with faulty geometry. These are but two of many methods available to create parametric models from scans or imported data.