FreeCAD Tutorial 1d: Design of an Electronic Box, Concluded

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Link to: Tutorial 1c (prev)

Introduction

This tutorial concludes the sequence for designing a sample electronics box to demonstrate how to use FreeCAD.

In the previous tutorials, most of the basic tools have already been addressed. In the steps that follow, knowledge of these tools will be assumed. If you are unfamiliar with any of these tools, you may want to review the previous entries in this sequence.

In the series leading up to this one, we designed the E-box with a number of mounting features that permit a small circuit board to be mounted. The geometric constraints that were demonstrated allow for the dimensions and mounting features to be changed around to fit circuit boards of different sizes with different mounting footprints.

One important feature that hasn't been placed yet is a pass-through to get wires in and out of the box. We will design this next. We will also design a raised-text label for the outside of the box.

Design the Pass-Through

This feature uses tools that have already been introduced previously. Click on one of the longer side walls of the box. For this lesson we select the face whose normal vector points in the +Y direction.

Use the () "Sketch" tool to open a new sketch. Using the () "Circle" tool define a 1/2" circular hole in the upper half of the box. Close the sketch.

Select the () "Pocket" tool to turn the circle into a hole. Make the depth of cut something deeper than the wall thickness.

Note: In the previous tutorial we mentioned a bug with the () "3D Fillet" tool. If this bug were expressing itself, this hole wouldn't appear as shown above.

Select the same face and open a new sketch. Use the () "External Geometry" tool to select the circle from before. You will need to create a second circle in this sketch identical to the first. After that, sketch another circle somewhat bigger in diameter. If you make it 0.7" then the wall thickness will match out standard wall thickness of 0.1".

Close the sketch. Use the () "Pad" tool to raise this sketch into a 1" long sleeve.

This pass-through isn't terribly sophisticated, but it would carry some wires in to the circuit board. In a future tutorial we will add more features to this pass-through to grip the wires more securely.

Raised-Text Label

FreeCAD is an application comprised of a group of smaller applications (called Workbenches) that are able to pass data between each other. To create a raised-text label for the box, we need to use the Draft workbench.

To keep things clean, open a new document from the "File" menu. Select the () "Draft" workbench from the pull-down menu along the upper edge of the window.

Up to now we have only used the () "Part Design" workbench and the () "Sketcher" workbench. This workbench contains tools that aren't duplicated in the other two.

You will see a new graphic window open that looks a little bit different from the previous ones. In the upper left of the window, there is a button that indicates the working plane, (XY) by default. Click on the button to select the (XZ) plane.

The reason we need this plane is because we seek to place a label on the face opposite the one where we placed the pass-through. This face is oriented perpendicular to the Y-axis, hence it is the (XZ) plane.