The SolidWorks Geek

I know, I know… It’s been way too long since I have written an article for the stapler but I am going to make up for it today. Today we are going start a two part article on how to build the staple cradle of the stapler. I don’t know if it is really called that but it is the sheet metal part of the stapler that holds all the staples. I have done sheet metal parts on the SolidWorks Geek before but this time instead of creating a sheet metal part from native features, we are going to create a solid model that we will then add sheet metal bends to create the finished part. For this article, I am also trying a different approach to present the steps for this project to the readers, your feedback would be greatly appreciated.

Create Model of Staple Cradle

Create the base feature for the staple cradle. All of the subsequent features will be added or removed from this base feature.

1. Create a sketch on the Top Plane.
2. Click Center Rectangle in the Sketch toolbar.
3. Place the center of the rectangle on the origin of the sketch.
4. Press “S” on keyboard and click the Smart Dimensions button on the Shortcut toolbar.
5. Using Smart Dimensions, make the rectangle 5.700″ long by .595″ high.
6. Click the Extruded Boss/Base button in the Feature toolbar.
7. Make sure the End Condition Type is Blind.
8. Make the depth (D1) .565″.
9. Click the green check mark.

Cut the top of the created extrusion. This is to achieve the basic shape of the top of the staple cradle.

1. Select the side surface of the extrusion.
2. Click Insert Sketch in the Context Menu.
3. Press ‘S‘ on the keyboard and click Line in the Shortcut toolbar.
4. Select the top corner of the face and trace out the profile shown closing on itself.
5. Press ‘S‘ on the keyboard and click Smart Dimensions in the Shortcut toolbar.
6. Make the distance from the bottom edge of the face to the bottom line of the profile .450″.
7. Make the angle of the segment on the right side of the profile 60° off of the top line.
8. Make the right most point of the profile .825″ from the right edge of the face.
9. Click the Extruded Cut button in the Features toolbar.
10. In the Extrude PropertyManager, change the End Condition of Direction 1 to Up To Next.
11. Click the green check mark.
    

Shell out the part to create the basic shape of the staple cradle. After this step the model is beginning to look more like the staple cradle.

1. Select Shell from the Features toolbar.
2. In the Shell PropertyManager, set the thickness in the field labeled D1 to be 0.040in.
3. Select the Faces to Remove field in the Shell PropertyManager.
4. Select the four faces shown below. These faces will be removed when the feature is shelled out.
5. Click the green check mark.

Now this is starting to take shape.

Now we need to create the tail end of the part. This is where the rivet will tie many of the pieces of the stapler assembly together.

1. Click the side face of the part.
2. Select Insert Sketch in the Context Menu.
3. Click ‘S‘ on your keyboard and select Line in the Shortcut toolbar.
4. With the Line tool active, click the bottom edge of the face about a half an inch from the left edge.
5. Draw a short line vertically and a second segment to the left horizontally.
6. Press “A” on your keyboard to activate a tangent arc from inside the line command.
7. Click the upper edge of the face.
8. Hold the ‘CTRL‘ key on your keyboard while selecting the arc and the left edge of the face.
9. Select the Tangent relation in the PropertyManager.
10. Hold the ‘CTRL‘ key on your keyboard while selecting the arc and the top edge of the the face.
11. Select the Tangent relation in the PropertyManager.
12. Press the ‘S‘ key on your keyboard and select Smart Dimensions in the Shortcut toolbar.
13. Make the right segment in the sketch .450″ from the left edge of the face.
14. Make the bottom segment of the sketch .045″ from the bottom edge of the face.
15. Click Extrude Cut from the Features toolbar.
16. Since this is an open sketch, the only option we can change in the direction of cut. Look at the direction indicated with the small arrow near the bottom of the sketch. This indicates the direction that the feature will make the cut. If the other direction is desired, select Flip Side to Cut in the Extrude PropertyManager. Do it now and you will see the arrow flip directions.

Now we need to create the hole for the rivet.

1. Select the face and click Insert Sketch from the Context Menu.
2. Press ‘S‘ on your keyboard and select Center Circle in the Shortcut toolbar.
3. Hold the ‘CTRL‘ key on your keyboard and select the arc edge on the face and the circle you sketched.
4. Select Concentric in the PropertyManager.
5. Press ‘S‘ on the keyboard and select Smart Dimensions in the Shortcut toolbar.
6. Make the diameter of the circle .156″.
7. Click Extruded Cut in the Features toolbar.
8. Change the End Condition to Through All.
9. Click the green check mark.

When the stapler is assembled, the following cut will be used to snap another sheet metal into place.

1. Select the side face of the part and select Insert Sketch from the Context Menu.
2. Press ‘S‘ on the keyboard and select Corner Rectangle in the Shortcut toolbar.
3. Create the rectangle approximately where shown.
4. Press ‘S‘ and select Smart Dimensions from the the Shortcut toolbar.
5. Make the bottom edge of the rectangle .145″ from the bottom edge of the face.
6. Make the height of the rectangle .155″
7. Make the left segment of the rectangle .100″ from the left edge of the face.
8. Make the width of the rectangle .100″
9. Select Extruded Cut from the Features toolbar.
10. Change the End Condition in the Extrude PropertyManager to Through All.
11. Click the green check mark.

The next feature, I must admit, I have no idea what it is for. My best guess, is that allows you to see if there are any staples in the cradle.

1. Select the face of the the part and click Insert Sketch in the Context Menu.
2. Press ‘S‘ on the keyboard and select Line from the Shortcut toolbar.
3. Draw a short diagonal line
4. Press ‘S‘ and select Offset Entities in the Shortcut toolbar.
5. Select the line that you sketched.
6. In the Offset Entities PropertyManager, set the offset distance to .045″.
7. Select Add dimensions in the Offset Entities PropertyManager.
8. Select Select chain in the Offset Entities PropertyManager.
9. Select Bi-directional in the Offset Entities PropertyManager.
10. Select Make base construction in the Offset Entities PropertyManager.
11. Select Cap Ends in the Offset Entities PropertyManager.
12. Select Arcs in the Offset Entities PropertyManager.
13. Click the green check mark in the Offset Entities PropertyManager.
14. Press ‘S‘ on your keyboard and select Smart Dimensions in the Shortcut toolbar.
15. Make the two centerpoints of the slot .205″ and .320″ from the top edge.
16. Make the two centerpoints of the slot .370″ and .500″ from the right edge.
17. Select Extruded Cut in the Features toolbar.
18. Change the End Condition in the Extrude PropertyManager to Through All.
19. Click the green check mark.

More to Come…

I think that will do it for today, I find if the articles get way too long people eyes glaze over. Part two of this article will be tomorrow morning at the latest.