The SolidWorks Geek

As promised, we are back with part two of creating the base for our stapler. If you miss the first half of this post make sure you go back and read it since it introduces you to Dynamic Mirrors, Instant3D and a different approach to modeling. So with out further a due, one to the stapler base.

Even More Cut Extrudes with Instant3D

Using the same methods described in the previous half of this post, create the sketch show below using 3 Point Arcs made tangent to each other. If you enabled the Dynamic Mirror mode, as describe earlier, you should have only need to draw one half of the sketch. Remember when dimensioning the overall of the sketch, hold SHIFT on your keyboard while selecting the arcs.

Cut extrude the created sketch using either Instant3D or a regular Cut Extrude 0.06″ deep, as with the previous sketch on the other side of the part. Also, be sure you set the draft angle, as we did with the previous cut extrude, to be 2.5°. Even though this part is not an injection molded part, it is meant to be stamp which will require a small amount of draft.

Filleting the Edges

If you haven’t been able to tell yet, I almost exclusively use the shortcut toolbar to access my most common tools. In a part you can access the Feature tools on the shortcut bar by pressing ‘S‘ on your keyboard.

For the outside edge of the part, on the top side only, create a Fillet with a radius of 0.1″.

Using the FilletXpert

On the inside edges of the cut extrudes we are going to use the FilletXpert to make selecting the edges quicker and easier. Earlier this week I briefly describe the usage of the FilletXpert tool, make sure you check it out! In the Fillet PropertyManager click the FilletXpert button, shown below.

Make sure the radius dimension and set to 0.1” and select one of the corner edges of the rectangle cut. As describe in my earlier post on FilletXpert, on clicking the edge a small context toolbar will be displayed allowing you to designate which edges you wish to be included in the current set. Click the button shown below, since all four of the corner edges will be selected then click the green checkmark to accept the fillet created.

Using the same process, apply a 0.025″ radius to the bottom edge of the extrusion and select the button shown. This will apply the same radius to the bottom edge of the second extrusion on the other side of the part.

Lastly apply a 0.065” radius to the upper edge of the extrusion and select the button shown.

The part is already starting to look recognizable, pretty cool don’t you think?

Shell the Part

We are almost done, I swear. Now it is time to shell out the part, since this is meant to be a stamped part. Click the Shell button in the Features toolbar.

Set the thickness of the material to be 0.06” then click the area designated Faces to Remove.

Click the bottom face of the part to be removed when creating the shell. Otherwise, the part will be a hollow part, which is not the effect we are looking for at this point.

Now there is a constant thickness of 0.06″ around the part.

Apply the Final Cuts

Now with the Shell applied to the part we can create our cut outs for attaching the rivets for the Arm Bracket and the Anvil. We couldn’t create these cutouts prior to the Shell operation since the shell would just create a wall where the cut outs were created. First create a sketch on the bottom surface of the rectangle feature per the dimensions shown below and make a extrusion that cuts through the part.

Create another Cut Extrude on the bottom surface of the round feature using the dimensions below. I created the outline of the sketch using an offset from the Tangent edge of the bottom radius.

That’s All Folks!

With those final Cut Extrudes the base part is now complete. We now have a part designed to be stamped and formed that we can mass produce for our stapler.

Look at the FeatureManager, nice and clean with not a bunch of unnecessary features. The cleaner your Feature Tree, the easier it is to make revisions.

Well Folks, that just about does it for this special two parter. I hope you have learned some new tools and techniques that you can then turn around and use in your day to day usage of SolidWorks. If you interested, I am making the model created for this post available for download here: [download#2]. All models created for the Friday Modeling Series will be available for download. You may pass them on to anybody but please do not use them for any commercial purposes without my prior approval.