It has been quite a while since the last tutorial about the stapler. The last component of the stapler we created was the Staple Cradle.  Before moving on to another area of the stapler, we will need to build one more component to complete the Staple Cradle.

Today we are going to build the front plate of the staple cradle. The front plate is a sheet metal component that covers the gap in front of the Staple Cradle. The cover is a real simple part that is held in place by pressing tabs into the sides that coincide with holes we added in the previous model.

Since we have covered making simple sheet metal parts before, we are going to explore another technique to create a sheet metal part. Instead of starting with a sheet metal Base Flange, we are going to make a solid model then convert it to a sheet metal part. Then we will create two configurations of the part. One configuration will show the part as it is made, the next configuration will be the installed state of the part.

The Sheet Metal Form Die

To save time, I am ommitting the step where the form die is being made. Instead, you need to download it here: Cradle Front Dimple Form (110). If you are interested in how to create a form tool, check out the post when we created the forming tool for the Arm Brackets.

After downloading the zip file that contains the form die, save it in your forming die folder of the Design Library. It doesn’t matter which folder you save the tools into as long as it is designated as a Forming Tools Folder. To make it easier for me to remember, I created a separate folder just for the stapler models but you are free to save them anywhere.

The Base Feature

With the forming tool downloaded and saved to the Design Library, we can begin with the cover piece. Create a new part model and name it Cradle Cover, Stapler. I mentioned earlier that we are not going to begin with a sheet metal feature, instead we will begin the part with a regular Extruded Boss/Base. Then we will convert it to a sheet metal part. This approach has quickly become my favorite approach to creating sheet metal components. I think by the end of this tutorial you will know why.

So, let us get started by creating the base feature:

1. In the new part file, press S on your keyboard to access the Shortcut Bar. In the Shortcut Bar, select the Extruded Boss/Base button.

2. Since a sketch has not been created yet, you are asked to select a plane that will be used to create the feature cross section. In the Graphics Area, select the Top Plane.

3. Now it is time to create our first sketch. Press the S key on your keyboard and select the downward pointing arrow next to the Rectangle button. In the flyout, select the Center Rectangle button.

4. For the center of the rectangle, select the sketch origin. Move your mouse away from the origin to create an undefined rectangle. Using the dimensions in the image below, fully define the sketch that will be used to create the base feature.

5. Click the Exit Sketch button in the Confirmation Corner (the upper right corner of the Graphics Area) to exit the sketch and to initiate the Extruded Boss/ Base tool.

As you can see, after selecting the Exit Sketch button the Extruded Boss/Base tool is automatically initiated. That is exactly why I began the model by selecting the extruded command before creating a sketch. Of course, you can still opt to create a sketch first then initiate the Extruded Boss/ Base command. It will just require one extra mouse click but every saved mouse click is time saved in the overall scheme of things.

6. To mix things up a little bit more, instead of entering a value into the Boss-Extrude PropertyManager, we are going to specify the extrusion depth using an on-screen ruler. select the vertical arrow, by clicking and holding the left mouse button. As you drag the arrow, ruler next to the mouse pointer will be displayed. Move the mouse directly over the tick marks and drag the extrusion to a depth of .450.

7. After achieving the desired depth of the extrusion, release the left mouse button. Then click the green check mark in the Boss-Extrude PropertyManager to exit the command.

8. Press S on your keyboard and this time select the Extruded Cut button.

9. When prompted to select a plane, face or existing sketch; select the front face of the model.

10. Press CTRL-8 on your keyboard to make the sketch plane normal to the viewing plane.Select the Line tool from the Shortcut bar. Begin the line by selecting the lower left corner of the rectangle face. Make sure the the corner is highlighted with an orange dot and the Coincident relation icon is shown next to the mouse pointer. If you the starting point is not coincident with the corner, the final sketch may not act as expected.

For the second endpoint of the line, click the upper edge of the rectangle and make sure that you are not selecting a corner.

11. Now it is time to fully define the sketch, press S on on your keyboard and select the Smart Dimension tool. Select the line you just sketched. Then select the left edge of the rectangle, being careful not to select a corner. The dimension previewed will change to an angle dimension. Place the dimension above the sketch and set the angle to 10°.

At this point the sketch should be fully defined. If you look on the Status Bar below the Graphics Area, you should see the words “Fully Defined”. If you see Under Defined or Over  Defined, double check your sketch dimensions and relations. If the Status Bar displays the “Fully Defined” statement, exit the sketch by clicking the button in the Confirmation Corner.

12. After exiting the sketch the Cut-Extrude will be displayed. This time, since the sketch is an open profile, the only option that is available is the Flip Side To Cut option. Look in the Graphics Area and make sure that the arrow is pointing towards the smaller section of the rectangle. If the arrow is pointer towards the largest side, select the Flip Side To Cut option. Click the green check mark to cut the material and to close the PropertyManager.

13. Now we need to add a couple of radii before we convert our model into a sheet metal part. In order to add the fillets, it might be helpful to rotate the view slightly to the right to give better access to the edges on the angled face of the part. Press and hold the middle mouse button or scroll wheel and move the mouse to the right. Once you see both the top and bottom edges of the angled face, release the middle mouse button.

14. Select the Fillet tool in the Shortcut Bar. In the Items to Fillet section of the Fillet PropertyManager, set the radius to .075. Then select the bottom edge of the angled face. Click the green check mark to apply the radius to the specified edge.

15. Using the same process, add a .050″ radius to the top edge of the angled face, as seen below.

Convert a Solid into a Sheet Metal Part

Now that the solid has been completed, we can now convert it to a sheet metal part. Since we did much of the work ahead of time, the part is really easy from this point on. Before moving on, I must remind you to save your model often. I would hate to have you lose all the work you have done up to this point.

To convert a solid into a sheet metal part, do the following:

1. If the sheet metal tab is not visible in the CommandManager, enable it by right-clicking one of the CommandManager tabs and select Sheet Metal in the flyout.

2. Select the Sheet Metal tab and click the Convert to Sheet Metal button.

3. The first select that needs to be made in the Convert to Sheet Metal PropertyManager is the a fixed entity on the model. This is the part of the sheet metal part that will not move when bends are added to the part.

Rotate the part around and select the back face, as shown below.

4. After select the face, you will see a yellow preview of what the sheet metal part will look like. You can see that the material thickness seems a little thick. That is because we have not specified a material thickness yet. In the Sheet Metal Parameters section of the PropertyManager set the Sheet Thickness to .020. Also, since we are in the area, set the radius to be .005.

5. Now we need to specify how the solid should be converted into a sheet metal part. To do this we are going to specify which corners are meant to be bent. SolidWorks will then be able to determine which material will be converted and which will be removed. Make sure that the Bent Edges window in the PropertyManager is active.

Then select the left and right edge of the face that was specified to be fixed. The preview will update to show how the sheet metal part will look like when created, as seen below.

If everything looks good, click the green check mark at the top of the PropertyManager and the part will be fully converted into a sheet metal part.

Add Forms to the Sheet Metal Part

Now all that is left to do is add the tabs that are created when the part is assembled with the Staple Cradle. If you have not already downloaded form tool for this exercise, do so now and add the part to your forming tools folder. The following steps will describe how to create a “As Assembled” configuration that will be used to show the tabs only in the assembly.

1. Click the Design Library tab of the Task Pane.

2. In the top section of the Design Library tab, locate the folder where you saved the forming tool for this exercise.

3. Select the Cradle Front Dimple Form by clicking and holding the left mouse button. Drag the form tool to the front face of the part. When the preview shows the form completely on the desired face, release the left mouse button to add the form.

4. After releasing the left mouse button, a window will be displayed informing you that you need to use dimensions and sketch modification tools to define the location of the form. Move the window off to to side so that you can better access the sketch of the form. Press S on your keyboard and select the Smart Dimension tool in the Shortcut Bar. First, select the horizontal construction line originating in the center of the sketch. Then select the bottom edge of the face. Set the distance form the bottom edge to the center of the form to be .223″.

5. Select the horizontal construction line of the form sketch and then select the tangent edge on the fixed face of the part. Enter .223″ into the Modify window to specify the distance from the right face of the part.

6. With the location of the form sketch fully defined, you can select the Finish button on the Position Form Feature window.

All that is left to do is add another form to the other side of the part. There are a couple of ways to do the following step but some are definitely easier then others. For example ,if you were to add the form tool once again to the other side of the part you would find that the tab on the inside of the part is on the wrong side. That is because the form was create with the angled portion to one side of the part. You could, once you enter the form on to the face, use the Modify Sketch tool to rotate the form sketch 180°. Then fully define its location but why go through all those steps. The quickest and easiest way is to just mirror the feature to the other side. There would be no need for future modification of the feature.

7. To mirror the form feature, select the Mirror tool in the Features tab of the CommandManager.

8. Click the plus (+) next to the model feature in the upper left corner of the Graphics Area to access the Flyout FeatureManager.

In the Fly out FeatureManager, select the Front Plane. The Front Plane will be used for the mirror feature. The reason why we can use that plane is because we created the base feature with a center rectangle originating at the Origin.

9. Next, select the Feature to Mirror box in the PropertyManager and then select the form feature in the Graphics Area. The preview will show how the form will look on the mirrored side.

If the preview appears as the image above, click the green check mark to create the feature. Congrats! You just created a sheet metal part from a solid.

Add a new Configuration

Sine the formed tabs we added won’t actually be made until the part is made part of the cradle sub-assembly, we will need to add another configuration for the assembled state. To add a new configuration and configure the part correctly for the assembled and default state, do the following:

1. While holding the CTRL key on your keyboard, select the form feature and the mirrored feature in the FeatureManager.

2. Release the CTRL key and right-click one of the features. In the menu, select Configure Feature.

3. In the Modify Configurations window, select the cell labeled <Creates a new configuration>. Type “As Assembled” in the field to create a new configuration then hit the Enter key.

4. Since we only want the selected features to be visible while in the assembled configuration, click the check box in both of the cells on the default row. This will make the formed features suppressed in the default configuration. Click OK to accept the changes and to create the new configuration.

5. Now that the configurations has been created, you can test it out by switching over to the ConfigurationManager. Click the ConfigurationManager tab at the top of the FeatureManager Design Tree.

6. To switch configurations, double click on the one that you wish to show. As you switch configurations, you will see the formed features disappear and reappear.

Whew!

That was definitely a marathon exercise. If you would like to compare your model to mine, you can download it here: [Download not found]. I hope you enjoyed this tutorial, even if it was a little long. I wanted to make the first stapler tutorial of 2010 a damn good one. Until next time…have fun playing with SolidWorks.

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