The SolidWorks Geek

Picking up where we left off on Friday, we are going to be finishing up the stapler cradle today. If you missed the first part of this tutorial, you can find it here. In the first part of this tutorial we started building the staple cradle using standard features that we will then convert to a sheet metal component.

Finishing up the Cradle Model

The next feature, is the cut out that the staples will pass through when the stapler is in use. As the staples are fed down the cradle, they will be individually pass through this opening and formed with the anvil.

1. Select the top face of the cradle and click Insert Sketch in the Context Menu.
2. Press ‘S‘ on the keyboard and select Line from the Shortcut toolbar.
3. Starting at one of the inside corners, roughly sketch out the shape shown below.
4. If you didn’t do so when creating the sketch, make the various points and lines Coincident and Collinear with the edges of model by selecting and sketch entities and edges while holding CTRL. Then select the appropriate relation in the PropertyManager.
5. We need to make the sketch symmetrical, instead of using construction lines, we are going to achieve this with relations. First, select the two line segments labeled “a” while holding the CTRL key and select the Equal relation from the PropertyManager.
6. If all of the other sketch segments are either horizontal or vertical, There is no need to make the two segments labeled “b” equal. Instead, select both segments while holding CTRL and select the Perpendicular relation from the PropertyManager (The relations can also be selected in the Context menu)
7. The last relations we need to add will be to the segments labeled “c“. Select both of the “c” segments and select the Equal and Collinear relations from the PropertyManager.
8. Next, press ‘S‘ on the keyboard and select Smart Dimensions from the Shortcut toolbar.
9. Place the .038″, .063” and .075″ dimensions as shown below.
10. Select Extruded Cut from the Features toolbar.
11. Change the End Condition for Direction 1 to Through All.
12. Click the green check mark.

Now we need to cut out a corner relief for when we convert the part to sheet metal and while we are at it, it is also a good time to make clearance for a future component.

1. Select the front face of the cradle and select Insert Sketch from the Context Menu.
2. Press ‘S‘ on the keyboard and select Corner Rectangle from the Rectangle fly-out in the Shortcut toolbar.
3. Starting at the lower-left corner of the face, draw a small rectangle and do the same of the lower-right corner.
4. Press ‘S‘ once again and select Center Rectangle from the Rectangle fly-out in the Shortcut toolbar.
5. With the center of the rectangle near the middle of the part, draw a rectangle approximately where shown.
6. Before we can start placing dimensions we should add as many relations as possible to the sketch. First, select the top line of the center rectangle and the top edge of the part while holding CTRL on your keyboard. Then select, the Collinear relation from the PropertyManager.
7. Select the centerpoint of the rectangle and the sketch origin while holding the CTRL key and select the Vertical relation from the PropertyManager.
8. Select the two top segments, of the lower two rectangles while holding the CTRL key and select the two relations Equal and Collinear from the PropertyManager.
9. Now it is time to add those dimensions. Press ‘S‘ on the keyboard and select Smart Dimensions from the Shortcut toolbar.
10. Make the top rectangle .165″ wide by .090″ tall.
11. Since we made the top segments of the two lower rectangle Equal and Collinear, we only need to add a couple of dimensions. First, make the height of one of the lower rectangles .045″. Then make the distance between the two .450″.
12. The sketch should now be fully defined, if not you need to go back and make sure you added all of the appropriate relations.
13. Select Extruded Cut from the Features toolbar.
14. Change the End Condition of Extrusion 1 to Up to Surface and select the highlighted surface below. This is the face we created in the cut feature earlier.
15. Click the green check mark.

We are almost done with adding all of the features. All that is left to do is add two holes on the bottom surface of the cradle. Once again, I am not exactly sure as to the purpose of these features. My best guess is that that are used by a fixture during the assembly process.

1. Select the face on the bottom surface of the cradle and select Insert Sketch from the Context menu.
2. Press ‘S‘ and select Center Circle from the Circle fly-out in the Shortcut toolbar.
3. Draw two circles, approximately where shown, on the surface.
4. While holding the CTRL key, select the center of the circles and the sketch origin.
5. Select the Horizontal relation from the PropertyManager.
6. Select both circles while holding the CTRL key and select the relation Equal from the PropertyManager.
7. Once again, Press ‘S‘ on your keyboard and select Smart Dimensions from the Shortcut toolbar.
8. Select one of the circles and make the diameter .156″
9. Select the right edge of the part and the circle on the right. Enter the dimension value of 1.700″.
10. Select both circles and make the distance, between them, 3.250″
11. Click Extruded Cut from the Features toolbar and change the End Condition of Direction 1 in the Extrude PropertyManager to Up to Next.
12. Click the green check mark.

The actual part is now complete. We can now convert the part into a sheet metal part.

Converting Solid Model to Sheet Metal

In the Sheet Metal toolbar, select Insert Bends. If you do not have the Sheet Metal toolbar in your CommandManager, right-click one of the tabs and select Sheet Metal.

The first thing we need to do is specify the fixed face of the model. Imagine that you placing this part in a fixture, this is the face that you will be clamping down when you bend the part down to make a flattened pattern.

In the model, select the bottom-inside face of the part.

Set the Bend Radius to be .015″. This value will vary depending on your parts you are trying to bend. Sometimes you may encounter errors when trying to create a sheet metal part from a solid that can be remedied by playing with this value. Click the green check mark.

Looking in the FeatureManager, you will now see three new features for the sheet metal part. The first feature, Sheet-Metal4, makes the part a sheet metal part. The next feature, Flatten-Bends4, creates a flattened version of the converted part. The last feature, Process-Bends4, bends the flattened pattern back into a sheet metal form.

Add Forms to Side of Cradle

Now that we have converted the part into a sheet metal component, we can use sheet metal forms to complete the part. In the attached zip file([download#10]), you will find the form that you need to use for this model. Place the form in your Sheet Metal Forming Tools folder in your design library. If you do not know how to do this, you can go here for more information.

1. Drag the Staple Cradle Form Die from the Forming Tools folder in the Design Library directly onto one of the inside faces of the cradle.
2. Press ‘S‘ on your keyboard and select Smart Dimensions from the Shortcut toolbar.
3. Make the vertical construction line 2.950″ from the outer edge of the part and make the horizontal construction line .198″ from the top edge.
4. Click the green check mark.
5. Repeat steps 1-4 for the other inside face of the cradle.

The staple cradle is now complete and ready to go into your assembly.

Wow… That Was Long…

Well, it took a few days but I finally managed to finish this post, thank you for sticking in there. Let me know what you think about the new approach to my tutorials. They take a little longer to write but they are meant to give you, the reader, the whole story. Ciao!