Earlier this week, I revisited the techniques I discussed in my video Splitting a Part in SolidWorks. I left off at splitting the part into two solid bodies and that is where will be picking up from today. If you missed the first part of this article, I would strongly suggest you go back and read it here.

Finishing the Bottom Half

Now that part has been split, we will no longer be needing the radiated surface. We cannot delete it because it would cause our split feature to fail. Instead, we must hide it from view by selecting the surface and clicking Hide in the Context Menu. You will be able to find the surface for future use in the Surface Bodies folder in the FeatureManager.

Now, we are going to be adding a lip for mating on the bottom half of the egg. In order to get to the bottom body, we are going to hide the top half from view by selecting the top half and clicking Hide from the Context Menu.

The bottom half of the egg can now be finished by extruding a lip from the face that was created by the split.

Create an extrusion from the face of the split that is .030″ thick from the inside edge extruded .050″ high.

1. Select the face of the split egg and create a sketch.
2. Select the inside edge of the face and select Convert Entities from the Sketch toolbar.
3. Click Extrude Boss/Base from the Features toolbar.
4. Set the Extrusion Depth to be .050″ from the face of the split.
5. Select Thin Feature in the PropertyManager and enter the Thickness to be 0.030″.
6. Click the green check mark.

Hiding and Showing Solid Bodies

With the bottom half finished, you need to switch the solid bodies that are visible. In the Solid Bodies folder, you can see the two solid bodies we created earlier. The shaded icon represents a visible body and the outlined icon means the body is hidden.

Click on the visible body in the Solid Bodies folder and click Hide in the Context Menu.

Then select the other body and click Show in the Context Menu.

Finishing the Top Half

Since the lip on the bottom half of the egg was an extruded boss, we will need to create a cut on the top half of the egg.

Create an cut extrude from the face of the split that is .030″ thick from the inside edge extruded .050″ deep.

1. Select the face of the split egg and create a sketch.
2. Select the inside edge of the face and select Convert Entities from the Sketch toolbar.
3. Click Extruded Cut from the Features toolbar.
4. Set the Extrusion Depth to be .050″ from the face of the split.
5. Select Thin Feature in the PropertyManager and change the type to Two-Direction.
6. Set Thickness1 and Thickness2 to both be .030″.
7. Click the green check mark.

With the half finished, show both of the solid bodies. If you section the egg longitudinally, you can see the two halves and how they fit together.

Saving Solid bodies Externally

With the two halves of the egg completely modeled, we can save the parts externally. To save the parts , click Insert -> Features -> Save Bodies.

In the Save Bodies PropertyManager, you will see the two newly created bodies listed in the Resulting Parts section.

To specify the path and filename for the two bodies, double-click the first file in the Resulting Parts section.

In the Save As window, specify the location and filename for the first part.

Do the same for the second part.

In the graphics area, the individual parts will be highlighted pink and the callouts will display the full path for each part.

The files listed in the Resulting Bodies section will also be updated to display the name you specified in the Save As window. Click the green check mark and the files will be created and saved externally.

In the FeatureManager a new feature for the Save Bodies is displayed. If you delete or modify this feature, the externally saved parts will be effected.

In the new files, the FeatureManager shows how the the part is externally linked to the parent model. As with Derived Parts, Any changes made to the child part will not be reflected in the parent but changes to the parent part will update the child.

Eggs-ellent Tool!

Hopefully, if you tend to design many plastic parts you will find this technique helpful. Also, if you seen the original video you will notice that I followed different steps to achieve the same outcome. This should illustrate that, in SolidWorks, there are more ways then one to do anything.

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