Though introduced on an iPad Pro, most CAD users will prefer to use the software on a workstation.
Shapr3D is professional CAD software for use on the go. If you don’t have it, download a trial license. It will give you full access to all the tools you need to do product concepts, designs, visualizations, and documentation.
This tutorial is about how to use the interface with a traditional mouse and keyboard. Later tutorials will cover using a touchscreen with a stylus or pen.
The goal of this tutorial is to create a simple part. Working through this tutorial will give you experience with sketching, manipulating the view, the general interface arrangement and some workflow practices.
Using a Traditional Mouse Setup with Shapr3D
Shapr3D was originally developed to be used on the iPad Pro. Since then, it has been ported to Microsoft tablets, as have Apple- and Windows-based laptops and desktops. The developers at Shapr3D have worked hard to make a mouse and keyboard interface feel as natural as possible. They appear to have achieved that objective.
Other Versions
You may have seen Shapr3D demonstrated in various versions. Some YouTube videos show it with elements of the interface in different places on the screen or with somewhat different functionality. When you download Shapr3D, you’ll always get the latest released version, and most of the information from older videos should be easily translated into the version of the interface you will get now or in the future.
Tutorial
This tutorial assumes you are using a mouse with a keyboard on a Windows PC, but you can also use other devices including iPads and Macs, in many form factors. Check for your device compatibility here.). You can still follow this tutorial with those devices, but the steps will be slightly different.
1) Download and install Shapr3D from the Shapr3D website on your device. As long as your device is compatible, this should be a straightforward process.
There is a beta version available, which is introducing history-based modeling, but I recommend the standard installation.
2) When you open Shapr3D, click the “+” icon in the upper right to create a new project. This will put you into a new workspace.
3) Notice when you hover the mouse over interface items, the tooltips will appear. Click on the sketch icon on the left side.
4) This brings up a display of the three standard planes in the middle of the screen. Click the XY plane on the bottom. You can see the axes labeled in the orientation cube in the upper right.
5) The view now changes so you are looking down on the Top plane and the icons on the left switch to show all of the sketch tools. Shapr3D also automatically turns on the line tool so that you don’t have to select that.
6) Using the units button in the upper right, make sure you are set to millimeters.
This area will also allow you to lock the grid so that it always stays the same size regardless of the zoom state. By default, the display size of the grid changes as you zoom the view in and out.
7) Using the Snap (magnet icon) settings, make sure all the snap settings are turned on. Snapping to the grid makes sketching much easier. You can apply dimensions later that don’t correspond to the grid spacing, but it is easier to start with these options turned on.
8) Using the Constraint Settings (gear icon), make sure that Auto-constraining is turned on and Show All is enabled for Constraint Visibility. This allows you to create and see geometric constraints that keep the sketch behaving properly, such as horizontal, tangent, parallel and symmetric.
9) Starting from the Origin (where the colored axes intersect), start sketching a horizontal line toward the right. Sketches automatically chain (meaning that a new line starts when you finish the previous one) until you have completed a closed loop.
Notice that in my sketch there are symbols for perpendicular and horizontal. Also notice that the line I drew on the right is not straight vertical up and down. If you make a mistake like this, it is easy to fix. Press Back (to get out of the line command), click the slanted line, and pick the horizontal/vertical tool on the right side. The line will snap to the closest one.
Note also that you can use the hot key shift V instead of clicking the button. Hot keys are convenient and fast when you have a full keyboard and have learned the software.
10) You can place dimensions as you sketch or when the sketch is complete. There is no special tool for dimensions in Shapr3D, so you can just click on the sketch element you want to dimension and a dimension box will pop up. Use the dimensions shown in the illustration.
To recenter the view, click the top face of the orientation cube, use the scroll wheel on your mouse to zoom in or out or drag the middle mouse button (MMB).
11) To get the angle dimension, click on the angled line, then shift+click the vertical line next to it.
12) Click on the origin point where you first started the sketch and notice that the entire sketch can be dragged around the screen. Drop that point back onto the origin and click on the lock icon. This locks that point so that it cannot be moved unless you unlock it.
13) Press ctrl+1 to set the view to an isometric view. You can also get this by clicking on the corner of the orientation cube.
Notice that the dimensions go away because you are no longer editing the sketch and the enclosed loop of the sketch turns blue. Click inside the blue area and drag the arrow up. Use a distance of 6 mm. This can be done by dragging or keying in the value. Click in the blank space to clear the selection.
Congratulations, you’ve made your first solid in Shapr3D!
14) Notice that there are no sketch fillets in the sketch tools. That is because fillets are generally better applied as features rather than in the sketch. There is a tool for sketch arcs but not for fillets. It is best practice to get accustomed to using fillet features, and as you will see, applying them to the 3D model is much easier than doing so in 2D sketches.
15) Next, we need to add the back plate. For this, we will sketch on the front plane. The easiest way to do this is to click the front face of the orientation cube, then click the sketch icon in the tools on the left. There are many ways to achieve this, but follow the procedures for sketching and dimensions from the previous steps.
Note: If you have sketched a line accurately and want to place a dimension but don’t want to change it, you can click the line, then hover over the dimension and the lock icon will appear. Clicking on the Lock will use the current dimension without the need to key it in again.
16) Press ctrl+1 to get out of the sketch and get into an isometric view. Click inside the blue enclosed area and use the straight arrow to pull it to a 6 mm thickness. (The curved arrow will revolve or tilt the sketch.)
17) Now notice that the new extrusion is a separate solid. (It is listed as body02 in the Items list on the left side). In some situations, this is what you want – but not this time. To join this with the first body, click the small cube icon next to the 6 mm dimension and select Union.
18) Now we can apply fillets to the corners. In the isometric view, you can select all four corners as shown. To do this, click the first corner, then shift+click the rest of the corners.
19) From here, you can key in the value for the fillet radius or drag the arrow away from the model to create four filleted corners.
20) Next, click on the top face of the bottom flange and press the spacebar to open a new sketch. The view swings normally to that face. Change from the line tool to the circle tool. Place one circle near each filleted corner, as shown in the illustration.
To draw a circle, click the center and drag out the radius. Make the two circles roughly equal in size.
21) Select both circles (drag a fence around them or select one and shift+select the second) and apply the equal sketch constraint.
22) Next, select one circle individually and shift+select the fillet edge next to it and apply the concentric constraint. Remember that you can use the hot keys, which are listed in the tooltip. In this case, concentric is Shift+C.
Do this for both circles.
23) Press ctrl+1 on the keyboard, select inside both blue circles and drag them all the way down through the model as cut holes.
24) Follow these same steps to make holes in the top flange. Your model will look like this when completed.
There is much more to the Shapr3D software, but this should be enough to whet your appetite. As you can see, it’s very easy to use and the interface is very streamlined, allowing you to work quickly. This lets you spend more time on the design and less time figuring out CAD.
