FreeCAD Tutorial 1b: Design of an Electronic Box, Continued

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Link to: Tutorial 1a (prev)

Link to: Tutorial 1c (next)

Introduction

This tutorial is the second in a series teaching basic CAD sketching and modeling tools using the open-source package FreeCAD.

In the previous tutorial, we designed a simple hollow box. In this tutorial we will start to add the features that will give it its function: A sample electronics enclosure that could be made on a 3D printer.

In this page we will explore more aspects of sketching, especially those that add features to the surfaces of a simple model, and the addition of geometric relations between features so that changes to the model's dimensions will carry through more smoothly.

The pace of this tutorial will be somewhat faster than the previous one because knowledge of tools already presented will be assumed.

Add Mounting Lugs

The box will need to be mounted to a surface, so the first feature we will add will be a pair of mounting lugs on the bottom of the box.

We will use a slightly inefficient process for designing them in order to examine some of the tools for adding dimensional constraints to features in the design. As you get more experience, hopefully some of the easier ways to design these features will become evident.

Open a New Sketch on the Bottom Surface

With the box displayed as it was at the end of the previous tutorial, rotate the view so the box bottom is visible. To do this, use the () orientation icon in the upper-right corner of the window.

Click on the box bottom to select the plane, and hit the () sketch icon to open a new sketch.

If you are unfamiliar with this operation, please review the previous tutorial.

To prepare the sketch for input, you will need to incorporate some geometric elements from the existing part. Click on the () "External Geometry" selection tool and use it to select the two vertical edges on the left and right sides of the box bottom. The cursor should appear as illustrated below. The two endpoints should appear in purple and the line should get a nearly invisible purple dashed highlight.

References to these lines should appear in the "Elements" list of the sketch, listed as "External."

Sketch the Mounting Lugs

Select the () rectangle tool and choose the "Centered Rectangle" option.

As you hover the cursor over the X-Axis, the cursor should acquire a () "Point-On-Object" icon to indicate that clicking there will cause the rectangle center point to "snap" to the axis. Drag the mouse diagonally over to the box edge and again the "Point-On-Object" icon should appear so you can attach the rectangle edge to the box edge.

Make rectangles like this on both sides of the box.

Add Fillets to the Lugs

Now that the retangles have been created, we need to round the corners. Select the () "Fillet" tool.

Move the cursor over the four external corners and click on them in sequence. As you click on each corner point, the square corner should be replaced by an arc with a default radius.

After creating the four fillets, expand the () "Dimension" tool popup menu by clicking on the () adjacent to it. Move down the menu and select the "Constrain Radius" tool.

Dimension the Mounting Lugs

Select the () "Dimension" tool. Click and release the LEFT mouse button on one of the lines of one of the lug rectangles. Drag the cursor sideways to lay out a set of dimension lines. Click the LEFT mouse again to place the dimension lines on the sketch. Do this for the other side perpendicular to the first one.

Change the dimensions of the rectangle to 5/8" on each side.

Hold down the -CTRL- or the -SHIFT- key and click on the top horizontal segments of each rectangular lug. The entries in the "Elements" list should be highlighted.

Select the () "Constrain Collinear" tool. The line that hasn't been dimensioned should snap to the same vertical location as the other one. Since this is a "Centered" rectangle, the lower line should automatically snap to the same vertical location as the lower line on the other side.