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I’m Kevin Kennedy and welcome to Learn Shapr3D in 10 Days for Beginners. On day one, we’ll design this 3D printable one-handed book holder. This object helps you hold back the pages with your thumb. You’ll learn how to set units of measurement, create 2D sketches, turn your 2D geometry into a 3D body, and how to soften edges.
This course assumes you have no prior experience with Shapr3D. I’ll be using Shapr3D for Mac OS, but it’s important to note that the core functionality and workflows are the same across all Shapr3D platforms. This includes iPad, macOS, and Windows.
We’ll start with a new Design file. Select the ‘New Design’ plus symbol in the upper righthand corner.
We’ll want to adjust the unit of measurement before we start to sketch. Change Units from the View dropdown menu on Mac or select the Units in the Title Bar.
We’ll select millimeters for this design.
We can also close the Sidebar, which is called the Items Manager. Hiding it will give us the maximum size to focus on our design.
We’re now ready to create a 2D sketch. In Shapr3D, everything starts with a sketch. Sketches are the foundation of your 3D models.
To start sketching, we’ll select Sketch from the menu. Notice we’re provided with geometric shapes to help us quickly sketch out our designs. You can break down the contour of this book holder into circles and arcs.
We’ll start with the center circle using the Circle command. Generally, you’ll want to look directly at the sketch by selecting a face of the Orientation Cube, or we can press the Spacebar, and it will automatically reorient for us.
Looking at this from an orthographic view will help us better apply sketch dimensions and constraints.
Start the circle by selecting the center origin point. A dimension input will appear as you drag your mouse cursor away from the origin. This first circle represents the hole for the user’s thumb. You can define a measurement specific to you. I’ll use 12mm for the radius of this circle, followed by the Return key to commit the value.
To Zoom in and out, pinch with your fingers on a trackpad, or scroll your center mouse wheel back and forth to zoom in and out.
We need another circle to represent the outer contour of the design. Another way to quickly access the circle command is to type “Circle,” followed by the Return key.
I’ll define this as 20mm, followed by the Return key.
At any time, we can edit these dimensions by selecting the value. Let’s change this to 17.5mm.
Next, we need to create the circle on the left. We can draw a circle anywhere on the left, making the radius 6.5mm.
At any time, press the Escape key to clear the active command. You may need to select sketch geometry, then use the center point or the directional arrows to move it around.
Notice Shapr3D will help us snap to other elements in our sketch, such as the X, Y, or Z-axis.
To define the distance between the circle on the left and the center of our other circles, we can hold the Shift key and select each center point. We can then place the dimension and set it to 39mm.
In its current state, our sketch geometry can move around freely. To make our sketches more precise, we can utilize constraints in addition to the sketch dimensions.
Constraints are rules that restrict the movement of sketch geometry. You can fully define a sketch with a combination of constraints and dimensions. To fully define a sketch means it will only update if you alter the dimensions or constraints.
I’ll press CMD + Z to undo the recent changes. Locate Constraints on the righthand side of the interface.
Notice we have a setting to turn on Auto-Constraints, where Shapr3D will help define them for us. However, I encourage you to get familiar with manually applying constraints. You’ll then better understand the use of automatic constraints.
We’ll start defining our constraints by locking down the center of the larger circles. With the center selected, we can use the Lock constraint. Notice Lock is also available near the selection. Locking the point will ensure it doesn’t move unless we intentionally unlock it.
Comparing the two points, you’ll see that locked sketch points are darker in color. Unlocked sketch points will remain white. The color of sketch geometry will help you keep track of geometry that is not yet defined.
Our small circle on the left can still move around. To further define this, we can use the line command to draw a horizontal line connecting the center points of each circle.
After selecting the two points, we can press the Escape key to clear the command.
We can add a horizontal constraint to this line to ensure it remains along the axis. The horizontal constraint will also keep our small circle defined. The circle can only change location if we decide to update our Sketch dimension.
Go ahead and change the sketch dimension to test this out. Creating a habit of testing your sketches as you go will help you avoid long-term problems. Be sure to undo or change the dimension back to 39mm.
To finalize our sketch, we need to create arcs that connect to each circle. The bottom two arcs will meet in the middle, resulting in a pointy edge that fits in the seam of a book. Sketch a vertical line starting at the origin point, with a length of 22mm.
We can also apply a vertical constraint to the line, ensuring it remains vertically.
To finish our sketch, we’ll create the two arcs on the left, we’ll then mirror them over to the right.
With the arc command, we can snap to the circle on the left, as well as the larger circle. You’ll also have to select the final position of the arc or define radii. Don’t worry about the placement at this point.
The arc command is still active. We can select the bottom of the circle on the left, followed by the endpoint of our vertical line.
After placing this arc, use the Tangent constraint to limit the position of the arc, ensuring it remains tangent to our circles. Tangency will provide us with smoother geometry.
Press Escape to clear out the Arc command.
You may have noticed that constraints are disabled or grayed out, and they become active based on the geometry you select. We’ll shift-click the circle on the left and the top arc, followed by the Tangent constraint. Notice this makes the arc tangent with the circle, and the tangent constraint icon appears in the sketch.
We’ll repeat this for the remaining three endpoints of each arc.
Once complete, we have many constraint icons in our sketch. These can be toggled on and off with the Show Constraints option. At times, you may want to hide these to focus on other sketch elements.
This design is symmetrical, which means we can save time by mirroring the sketch. In Shapr3D, you can Mirror both 2D sketches and 3D bodies.
Locate the Mirror command in the Transform menu. Once active, we can select each arc and the small circle. The mirror command then needs a mirror plane or item. With our sketch, we can use the vertical line. Notice this mirrors the geometry, speeding up our workflow.
Keep in mind that mirrored sketch geometry does not include any existing constraints. You will want to apply the preferred constraints or add symmetry constraints to fully define your sketch.
Instead, I’ll undo and let’s take a look at mirroring the solid body.
We can use the Orientation Cube to look at this sketch from a perspective.
From the Tools menu, select the Extrude command. Extrude is one of the most used commands across many CAD programs. It allows us to choose a 2D sketch to turn into a 3D body by extruding it to a specified distance.
You’ll see that our sketch geometry has a blue background highlight. The blue background signifies our sketch is fully-closed, which is a requirement to turn our sketches into a 3-dimensional body.
Notice we’ll have to select each closed object. Because we intend to mirror this, we don’t want anything past the centerline, so we’ll need to cancel.
We can use the Line command and another vertical constraint to close off the profile. Let’s also make sure to align the endpoint of our arc with the Y-axis.
Once complete, we can head back to the Extrude command.
After selecting the desired closed profiles, define a value for the Extrude distance or drag the arrow up or down.
I’ll make this 10mm, followed by selecting Done.
We can now use the Mirror command to mirror this solid 3D body.
Double-click on a 3D body to select the entire body, then we’ll define the inner planar face as the mirror plane.
Notice this mirrors the 3D body.
After completion, you’ll find these are two separate 3D bodies, as indicated by the line running down the center.
We can use the Union command from the Tools menu to join the two bodies together. Union often makes it easier to modify your 3D bodies with other features, as we’ll see in a second.
We’ll want to finish this design by rounding over the sharp edges, resulting in a better 3D print.
With the Chamfer/Fillet command from the Tools menu, we can select the vertical edge. This feature lets us drag towards the model to create a Chamfer and away from the model to define a Fillet or rounded edge. I’ll make this first Fillet 0.5mm.
We can also apply a Fillet by selecting a planar face, which lets us quickly apply a Fillet to all edges. By previously unioning the bodies, we made it simpler to Fillet the entire edge. I’ll select the top face of the model and then reorient the model with the Orientation Cube, helping us choose the bottom face.
We can then apply the final Fillet of 1.5mm.
Lastly, we can export the file from the File menu and Export. You can also use SHIFT + CMD + E. The Export dialog will present us with many file types sorted by usage and format.
Select 3D Print and choose STL or 3MF, whichever you prefer. Define the name, and you’re all set and ready to save it to your local computer, where you can then import it into your preferred slicing software.
Last but not least, you may be wondering how to save your file. Shapr3D has automatically saved the file as you’ve been designing. We can head back to Home and to the Designs tab, where we can right-click to Open, Rename, Duplicate, or Delete files. I suggest renaming the file before moving on to the next project.
Shapr3D will soon release the ability to sync your designs across platforms, allowing you to continue designing on their iPad, Windows, or Mac applications.
Be sure to subscribe for more free Shapr3D lessons and check out ProductDesignOnline.com for more resources. Then, click on this YouTube playlist to view the rest of the ten days.