FreeCAD Tutorial 1a: Design of a 3D Printed Electronic Box

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Introduction

FreeCAD is a free, open-source CAD package that was under development for years; and recently it has produced a "release" version. By attracting developers from all over the design community, FreeCAD has assembled an impressive collection of features and add-ons.

This tutorial is an analog to the SolidWorks series that begins with SW Tut 1a. We will design an electronic box (E-Box) following the sequence there as closely as possible. It assumes no previous experience with CAD, though you may want to review another page that discusses the tools for navigating the design space.

To get started, please visit the FreeCAD download site if you haven't already done so.

You may also want to download the PDF user manual and look at it. It gives detailed instructions on how to install the package. You may also want to look at the navigation options on pp. 31-32 if you are used to a particular set of mouse actions to zoom, pan and rotate the view.

The modeling operations used in this tutorial are are described in the manual starting on page 80. Please note: The lesson here is just what is needed to get started designing relatively simple objects. Many more tools are available than these, and you will be left to explore them for yourself.

Load FreeCAD and Open a Sketch

Double-click on the FreeCAD icon (or shortcut) on the desktop. The window will show a startup dialog as shown below. Click on New File - Parametric Part to create a new part.

When you open new part, a blank window in the FreeCAD interface should appear.

This interface can be a little bit perturbing to someone who is used to the more verbose SolidWorks tool bars. In the interest of preserving real-estate on the screen, FreeCAD has chosen to leave text labels off of their tool icons, so you need to memorize the familiar ones you want to use. Tool "hints" exist and give you a text description if you hover the cursor over a tool icon.

When you open a sketch, the first window displayed allows you to pick one of the three cardinal planes in the design space in order to start the first sketch in the part design. Later you can add sketches to planes of the part under design, but you have to bootstrap off of something to get started. Click on one of the planes, it doesn't really matter which at this point.

Note: FreeCAD has an important architectural component. If you are designing a house, you probably want to ground it on the X-Y plane.

After selecting a plane, FreeCAD opens the "Sketcher Workbench" which is a member of the "Part Design Workbench." These take the place of the tabs in the SolidWorks toolbar.

Sketch a Framed Rounded-Corner Rectangle

You will see a large array of sketching tool icons, several of which will be used later in this tutorial sequence. For the first step, please select the "Rectangle" tool as shown below.

FreeCAD presents many options for drawing rectangles. For this example design, you will want to select a rounded, framed, centered rectangle.

With this tool selected, the appearance of the cursor will change as it moves around the window. Three appearances are shown below.

Part a shows the cursor when it is traveling around an open section of the window. It shows the X-Y location and a thumbnail of the type of rectangle being drawn.

Part b shows the cursor when it is traveling over one of the cardinal axes of the sketch plane. Besides the location and thumbnail of the rectangle type, it also shows a () "Point On Object" icon to indicate that clicking the cursor there would cause the feature to "snap" to the axis.

Part c shows the cursor when it is traveling over the origin of the sketch plane. Besides the location and thumbnail, it also shows a () "Point Coincidence" icon to indicate that clicking the cursor there would cause the feature to "snap" to the origin.

Click on the origin, as in part c above. Drag the mouse diagonally in some direction. You will see some edit boxes with dimension lines appear next to the growing rectangle. One of them will automatically be selected for editing.

Without clicking the mouse again, type in sequence: 4.5" -ENTER- 2.5" -ENTER- 0.25" -ENTER- -0.1" -ENTER- The first number specifies the width and the second specifies the height of the rectangle. The third specifies the corner radius and the fourth specifies the frame thickness. A minus sign in the last parameter tells the system the offset rectangle is moved inwards from the original.

No other work is needed to complete the desired rectangle. We could have manually dimensioned these after clicking the rectangle into place, but this is easier. We will observe how to do that later in this sequence.

Double-click on one of the indicated dimensions and change the value around to see how to manipulate the edit boxes. You can also drag the dimension labels around to make their location more appealing. Drag the label for the frame thickness away from the edge of the rectangle to make it more legible

Click on the "Close" button in the upper left to close the sketch.

Extrude the Box Sides

When you close the sketch, the system exits the Sketcher and returns to the Part Design Workbench.

The part design tools will be displayed in a row of colorful icons across the top of the window and there is an outline of the design history in the left margin. At the bottom of the list there is a reference to the sketch we have just produced.

If the sketch is selected the entry is highlighted in blue and a table of data is displayed.

To raise the sides of the box into the third dimension, we use the () "Pad" tool located on the extreme left of the tool bar. When you click on that tool icon, the display shows a preview of the shape with a default value for the extrusion length. Set the length (i.e. height) of the box sides to 1.5 inches.