Here we are at the beginning of another beautiful Friday morning and of course you know what that means…this weeks modeling tutorial.  Last month when I started the stapler project, I thought it would be fun to model up the stapler sitting on my desk. I never expected it to attract the attention it has but it now seems to be the most popular series of The SolidWorks Geek. Your comments and questions are all great and please keep them coming. Due to the number of steps required to create the models illustrated in this series, I am constantly experimenting with the way I present the information. I try to balance the amount of information with the size of the post. From time to time, I may not spend as much time on a particular step but your comments and questions fill any gaps I may have left. So thank you, my photo may be the one shown above but this blog is yours.

Forming Tool Base Revolve

Something that all staplers have in common is the anvil. The anvil guides the prongs of the stapler and forms the familiar curled shape. Without the anvil the stapler would not hold the paper and it would just fall out. Depending on the stapler, the anvil will unusually have two forming shapes; one that curls the prongs in and the other that curls the prongs out. Today we are going to create our anvil as a sheet metal component with the indents created with a sheet metal form. So, the first thing we will need to do is create our forming tool.

The first step for creating our forming tool is to create the sketch, shown below, on the Right plane. Although there are a number of ways to create the profile, I would recommend creating the construction line first. Using the Dynamic Mirror tool I described when building the Stapler Base, sketch either side of the profile and the other side will be created automatically. Next apply the dimensions shown, to fully define the sketch.

Now it is time to create the Base using the Revolve command. We are going to be apply a cut to the part in the next step, so we do not require the full 360° of the revolution.

Instead, after selecting the top segment of the sketch as the Axis of Revolution, set the Revolve Type to be Mid-Plane and set the Angle to 90°.

Trim Excess Material

Now I admit there are a number of ways to create the following cut feature but I find this method is reduces the number of errors when making dimensional changes. Ask Matt, Josh and Ricky and I am sure they have much better ways of doing this; but this works best for me. If you created the revolve sketch on the Right plane, then create the sketch shown below on the Front plane. Then create a triangle with the two sides Colinear with the sides of the Revolve and the base of the triangle Horizontal. Since the width of the finished form is more important to me then the depth of the form, I want to add the .250 dimensions shown. The way I did this, was I made two Points Coincident with the arc of the revolve; then Coincident with the base of the triangle. If I was to adjust the .250 dimension the depth of the form will change accordinally but if I was to adjust the radius of the revolve the .250 width would be preserved.

Add Temporary Base for Fillets

As you might remember from the forming tool for the arm bracket, we need to create fillets on the forming tool that will be used to properly form the metal on our sheet metal part. In order to add these fillets we need to create a temporary base that will only be used for the base fillet. On the Bottom Face of the part create a sketch as shown below. In this case the actual dimensions of the rectangle do not actually matter as long as the resulting shape is big enough to accommodate the require fillet.

Extrude the temporary base to any thickness you desire, we will be removing it shortly.

Apply a .005” Radius to the two top edges, as shown.

Next apply a .060″ Radius to the bottom edge. The thing to keep in mind with this radius is that the radius MUST be larger then the intended sheet metal thickness, otherwise the tool will not be able to make the form in the part.

With the radii created, we can now remove the temporary base. Obviously we cannot just remove it from the FeatureManager or all of it’s children features will fail. Instead, create a sketch on an face of the base and use the Convert Entities tool to trace profile. Create a Cut Extrude with the End Condition set to Up to Next.

Create the Forming Tool

With the forming tool geometry complete, it is time to create a forming tool from the geometry. Select Forming Tool in the Sheet Metal toolbar or select Insert -> Sheet Metal -> Forming Tool.

Select the bottom face of the part as the Stopping Face. This face will be coincident to the selected face of the sheet metal part, with the form extending from the face.

Since there are no cuts being created by the forming tool, there is no need to select any faces to remove.

Keep Checking That RSS Feed…

The forming tool is complete but that is only half of the story. Keep checking your favorite RSS reader for the next part, when we create the anvil itself. It should be coming either later today or sometime this weekend. Until then, feel free to download the model of the Anvil Form, Stapler (722) to see each step for yourself.

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