For weeks now I have been staring at the stapler on my desk thinking “This would be so much fun to model.” A stapler has everything; formed parts, machined parts, sheet metal parts, springs, rivets and injection molded parts. What better way to put to use some of the tools and concepts we have explored together? Every week we will build another component of the stapler until we have all the components that make the assembly. After the stapler is built, maybe can use it to try out some other functions of SolidWorks. Today we are going to begin with the base of the stapler since this is the foundation of the whole assembly.

The Base Sketch

The base is a formed metal part but we aren’t concerned with the manufacturing process for this part. Instead we will just build the part as we need it and let the manufacturers decide how to make it. First we need to create a horizontal construction line starting at the origin. Press ‘S‘ on your keyboard to access the Shortcut toolbar and click on the Line fly-out to access the Centerline button.

With the centerline tool active, click the origin and drag the line horizontally while still holding the mouse button down. The stapler base is just over 6″ long so watch the number to the right of the pointer. There is no exact number you a trying to hit just as long as it it more then 6″. When made the line long enough, release the mouse button; there will be no need to hit ESC if you held the mouse button while creating the line.

Next, we want to enable the Dynamic Mirror mode. This will enable us to mirror our sketch entities while we are sketching them. Click Tools -> Sketch Tools -> Dynamic Mirror.

You will be able to tell that the Dynamic Mirror mode is enabled because our centerline changed to a symmetry line. A symmetry line is shown as a centerline with two small lines perpendicular to the centerline on both ends.

With the Dynamic Mirror mode enabled we can begin to sketch our base outline using arcs. Press ‘S‘ on your keyboard and select 3 Point Arc from the Arc fly-out.

Starting at the sketch origin, sketch out the shape shown below on one side of the symmetry line with three arcs. As you sketch each arc it is automatically mirror on the other side of the symmetry line.

. While holding the CTRL key on your keyboard, click the two adjacent arcs and click the Make Tangent button in the context toolbar. Do the same for the other two arcs at the other end of the profile. This will clean up the ends of the profile to appear to be one continuous arc.

Using Smart Dimensions, dimension the rest of the sketch as shown below. Since the arc segments the make the ends of the profile, we only need to add one dimension to each side.

All that is left to do in this sketch is the define the two arcs at the top and bottom of the profile. Since the start and end points of the arcs are fully defined we could just specify the radii of the arcs and the sketch would be fully defined but that would not suit our needs. We can care less what the radii of these two arcs are in reality, in fact all we care about is the over all height of the profile. With Smart Dimension enabled, hold the SHIFT key on your keyboard and select both the top and bottom arc to dimension the distance between the outermost edges.

Lastly, we just need to add fillets to the four corners of the profile. Once again press the ‘S‘ key on your keyboard and select the Sketch Fillet tool in the toolbar.

Set the Fillet Radius to .25 and ensure that the Keep constrained corners is enabled.

Click the points at the four corners of the profile to add radii on each corner.

Use Instant3D to Extrude

With the sketch created and fully defined we are now ready to make our extrusion. Instead of using clicking the Extrusion tool as most are tempted to do we are going to build our part using Instant3D. Instant3D is a new tool in SolidWorks 2008 that allows you to quickly create and modify part geometry by using Drag Handles in conjunction with On Screen rulers.

First, ensure that the Instant3D button is enabled in the Features toolbar of the CommandManager. Without the Instant3D button enabled, you would not be able to do any of the cool things I am showing you here. You would be force to use the same old extrusion tools and where’s the fun in that?

Rotate the view to a perspective view and select any sketch segment. An arrow, or Drag Handle, will be displayed on the segment.

Grab the arrow and drag to extrude the base to a length of 0.3″ by hovering over the on-screen ruler while dragging. NOTE: If you haven’t done so already, it would be a good idea to read my post on the on-screen ruler since it discusses how to achieve precise extrusions.

Upon releasing the mouse, a small context toolbar will be available. Click the Draft button.

After clicking the Draft button, an angle on-screen ruler will be displayed. Drag the value to 6°. Of course, you can still edit the extrusion and adjust and value including the Draft in the Extrusion PropertyManager.

Cut Extrude with Instant3D

With the base feature created, it is time to add the features that will be used for the Anvil and the Arm Bracket. Instant3D isn’t just for creating bosses, it is also great at creating cuts. In fact, play around with the the tool and you will see that depending on which direction you drag the Drag Handle you will create either a Boss or Cut. First we need to create a sketch to work with for the first cut. Select the top face and click the Sketch button on the context toolbar.

Once again press ‘S‘ on your keyboard and click the Center Rectangle button in the Rectangle fly-out.

Draw a rectangle approximate where shown on the larger side of the part.

Dimension the rectangle as shown below.

Notice how we didn’t dimension the position of the rectangle yet. I normally like to constrain sketches with relations prior to adding other dimensions. In this sketch the only relation that will work is to add a Horizontal relation between the sketch origin and the center of the rectangle, that is the reason we went with the Center Rectangle. Click the Origin of the sketch and the center point of the rectangle and select the Horizontal relation in the context toolbar.

Since there were no other relations we can add to the sketch, we can add one final dimension to fully define the sketch. Apply a dimension to the sketch as shown.

Not it is time to create the cut extrude. Just like before, exit the sketch and select a sketch segment to show the Drag Handle.

This time, instead of dragging the sketch up to create a boss, we drag the sketch into the part to create a cut. Drag the handle over the on-screen ruler to ensure that the cut dimension is precise. Create a cut extrude 0.06″ deep, as shown below. NOTE: You may find in necessary to zoom in enough in order to be able to actually achieve the 0.06″ dimension.

After releasing the mouse, click the Draft button on the context toolbar.

Set the draft to be 2.5° by using the angle on-screen ruler.

Wow! This is Long!

This has got to be one of my longest post to date…. and you know what? It’s not over yet. In order to maintain your sanity, I am breaking up this post into two parts. The second half will be available real soon.

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