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

Link to: CAD Main Page

Link to: Tutorial 1b (prev)

Link to: Tutorial 1d (next)

Introduction

This tutorial continues 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 previous tutorials in this sequence, a thin-walled box was designed with mounting lugs attached to the bottom face. The first step in this tutorial is to add some additional lugs around the top of the box that could be used to attach a lid to the box. The operations to do this are mostly the same as those used in the previous tutorial. Accordingly, we will move quickly through this first operation until we need to use some new functions.

The box is shown with the plane of the top edge selected, ready to open a new sketch.

Attach Lugs to the Box Edge

Using the () "External Geometry" selection tool select the four inside edges of the box. These are needed in this sketch to locate the rectangular features we will add.

If you are unsure of how to do this, please review the [FreeCAD_Tutorial_1b:_Design_of_an_Electronic_Box,_Continued#Open_a_New_Sketch_on_the_Bottom_Surface previous tutorial].

Select the () "rectangle" tool and draw an ordinary rectangle attached to a corner of the box. Hover the cursor over the box inside edge until the () "Point-On-Object" symbol is visible. Click and drag diagonally to the other edge and "snap" it to the edge.

Repeat this operation in the other three corners. When you have done this, hit the -ESC- key once to exit the tool. If you hit the -ESC- key more than once, the sketch will exit. You will need to reopen the sketch to continue working.

Use the () "Fillet" tool to sketch fillets in the free corners of the four rectangles.

Use the () "Dimension" tool to set the width of one of the rectangles to 0.375 inches. Also set the radius of one of the fillets to 0.15 inches. Hit the -ESC- key once to exit the tool.

Now, holding down the -CTRL- key, select the four fillets on the four hanging corners. Use the () "Equal" tool to set the radii of all four fillets equal to each other. Making this selection accurately is a little bit tricky, so it is useful now to practice it.

Now, select the eight hanging straight edges of the lugs. These are the ones that touch the fillets you just dimensioned. The length of one of these edges has been set previously. With all eight selected, click on the () "Equal" tool to fix them all to the same length.

Click on the "OK" button to exit the sketch.

With the sketch selected, use the () "Pad" tool to expand the sketch into solid lugs 0.1 inches thick. Note: If you select the "Pad" tool and the rendering disappears, you will need to click on the "Reversed" checkbox to make the image reappear with the new lugs attached.

The part is shown above with the top plane selected to open a new sketch. We could have added the upcoming features to the original sketch for the lugs, but the next step will show some new features of FreeCAD.

Cut Screw Holes in the Lugs

Open a new () sketch on the top surface. Use the () "External Geometry" tool to select the two opposite corners of one of the lugs. The points should be highlighted purple when selected.

Click on the () "Construction" toggle tool. This tool places the Sketcher into a mode where new sketched features are marked as "Construction" features. They will be rendered as dotted lines and won't be extruded into 3D with the "Pad" or "Pocket" tools.

Pick the () "Line" tool and sketch a diagonal line between the two corner points of the lug you selected. The line should appear dotted as a construction line.

Now, pick the () "Point" tool. Hover the cursor close to the center of the construction line until the () "Constrain Symmetric" icon appears next to the cursor.

Click the mouse to place a point on the midpoint of the diagonal construction line.

Repeat this action for the lug in the diagonally opposite corner of the box.

Click on the () "Construction" toggle tool again to return the Sketcher to normal drawing mode.

Select the () "Circle" tool and place circles in each of the four pads. Place the circles with the construction lines centered on the points you just placed. The circles should render in solid color to indicate that they aren't for construction. Dimension one of the circles to be 0.060" in diameter. Hit the -ESC- key once to exit the tool.

Hold down the -CTRL- key and select all four of the circles. Hit the () "Equal" tool to make all of the circles the same diameter.

Select the () "Constrain Horizontal/Vertical" tool. You click on pairs of points to align features. The tool decides whether the selected features are closer to being horizontal or vertical, and aligns them in that way. Pick the circle centers in pairs between adjacent corners to align the unconstrained circles with the ones located on the construction lines.

Hit the "Close" button to exit the Sketcher.

With the new sketch selected, pick the () "Pocket" tool. There are several options under on the "Type" pull-down menu. A few of them will do the right thing. The most reliable is to pick "To First" which projects the cut to the first surface crossed below the sketch.