SolidWorks Tutorial 1d: Design of an Electronic Box, Continued

Link to: CAD Main Page

Link to: Tutorial 1c (prev)

Introduction

This tutorial concludes the basic introduction to SolidWorks, using an electronics box (E-Box) as an example. In the previous tutorials, we designed a simple box, starting from zero ; followed by adding mounting lugs, with attention to geometric relations and continuing with other mounting features, using feature copying and pasting.

There are still a few features to be designed to complete the box. An important feature that is frequently forgotten is a pass-through for the wires needed to activate the circuit board. After that, we will place a label in raised lettering on the box.

Because this tutorial has been preceded by several others, many of the operations used here have already been presented. To keep the pace up, we will assume the reader is familiar with these details.

Create the Pass-Through

Select one of the long walls of the box and open a sketch on it. If this process is unfamiliar, please review Tutorial 1b.

Sketch a circle on this plane, centered on a line somewhat above the center of the side of the box. The diameter should be about 0.2 inches larger than the girth of the bundle of wires and connectors that will plug into the circuit board. In this example, we make this circle 3/4 of an inch in diameter.

Exit the sketch and with it selected, click on the "Features" tab and select "Extruded Boss/Base."

Extrude this sketch to a height of one inch and hit the () green check-mark to accept.

Select the top surface of the extruded cylinder and open a sketch. Draw a circle centered on the face with a diameter equal to the girth of the wire bundle passing into the box.

Exit the sketch and select "Extruded Cut" from the "Features" tab. In the pull-down menu under "Direction 1" select "Up To Surface." The yellow preview of the cut should pierce through to the box interior.

Select the () green check-mark to accept.

Label the Box

This section shows how to put raised text on a planar surface.

Select the long face opposite the pass-through and open a new sketch. The first feature to add to the sketch is a line that directs the text. Draw a line lengthwise across the face and select "For Construction."

Once the guide line is placed, select the () "Text" tool under the "Sketch" tab.

When to tool opens up, the first field in the window in the left margin says "Curves." Select the guide line that you just drew so that a reference to it appears in that field.

Type the text for the label in the "Text" field. Click on the radio button that says "Use Document Font" and press the "Font..." button. This will open a dialog box that allows you to change the font parameters to make the label have the right appearance.

Close the sketch and with the sketch selected, open the "Extruded Boss/Base" tool in the "Features" tab. Set the extrusion height to a number that isn't too large. In a 3D printer, the text will be built with a support structure that will need to be carved off when the part is finished.

Hit the () green check-mark to accept.