Last week we started to Make a Thing in Solidworks. We got as far as sketching and extruding the base. This week we’ll make the back portion. We’ll use some of the same techniques in Part I and a few new features such as 3D filleting and the Hole Wizard.
As you know, this is not the first ‘Making a Thing’ tutorial. In case you missed them, the softwares previously covered in the 3D Printering series are:
- AutoCAD Part I
- AutoCAD Part II
- Blender Part I
- Blender Part II
- Autodesk 123D
- FreeCAD Part I
- FreeCAD Part II
- Solidworks Part I
Picking up where we left off, the next step is to make the back portion of the shape. To do this, start by rotating the view to see the rear face of the part. We want our sketch to be on the rear face so select the rear face by clicking on it. Once it is highlighted, select Sketch from the Sketch Tab.
A new line will show up in the Model Tree (in this case it is called Sketch2). Right click on this and click on the Normal To icon. This will rotate the view to be perpendicular to the face the sketch will be on.
Now that we are looking at the rear face of the part, we can draw the back portion, which is basically a tombstone shape with tapered sides. Start by drawing a circle. It can be any size and any location as it will be dimensioned later. Like in Part 1, I will intentionally sketch the shape out of proportion to show how the geometry will change when adding dimensions and constraints.
The tapered lines should be tangent to circle. To do this, select the Line Tool from the Sketch Tab, start the line on one of the top corners of the rear face. Then hover over the circle near the point where the line would be tangent to the circle. A yellow box with a tangent symbol will appear. Clicking at this time will make the line tangent to the circle. Do this for the other side. Then draw the last 3 lines. Hovering over the corners of the rear face will make the lines snap to those points. On the Sketch Tab, select the Trim Tool and click on the bottom portion of the circle to delete it.
From the sample drawing, we know that the center of the arc is 7/8″ above the top face of the portion we have already drawn and extruded. Use the Smart Dimension Tool to add a dimension from the center of the arc to the top face of the extruded part. Then enter “7/8” as the desired distance and the sketch will move to satisfy that requirement. Click on the arc to specify its radius. Enter 5/8 or 0.625.
The radius is currently not centered over the rear face. To center it, left click on the top of the rear face and select the midpoint. Then hold shift and select the center of the arc. A window will pop up, select the vertical line to make the arc centered over the rear face.
The sketch is now complete. Click Exit Sketch from the Sketch Tab.
NOTE: The 7/16″ through-hole could have been drawn on the sketch and it would have created a hole when the sketch was extruded. After that, the counterbore would still have to be added. We will create both the hole and counterbore in one step later.
To extrude the part, select the sketch (Sketch2) on the Model Tree, then on the Features Tab, select Extruded Boss. In the Boss-Extrude dialog box, type in 0.5 or 1/2 to specify the length to extrude. Click the green check mark to make it happen.
To make the hole and counterbore we’ll try something new. Select the Hole Wizard from the Features Tab. This tool will allow us to make the hole and counterbore at the same time. In the Hole Specifications Dialog Box, select the following:
Hole Type: Legacy Hole
Type: Counterbored (adds a counterbore)
End Condition: Through All (makes the hole go through the entire part)
Enter the dimensions from the sample drawing for the Hole Diameter, Counterbore Diameter and Counterbore Depth.
NOTE: We can’t change the hole Depth because we specified “Through All” for the End Condition. If we selected “Blind” and added a depth of 2 inches, the hole would go into the part 2 inches deep.
Now that the hole and counterbore dimensions are specified, we need to determine where the hole will be. While still in the Hole Specifications dialog box, click on the Positions Tab. Then select the face of the part where the hole will be placed. Position does not mater right now.
A representation of the counterbored hole will be placed on the part. We know it is not in the correct spot. To make the hole concentric with the arc of the back portion of the part, click on the asterisk at the center of the previewed hole, then hold shift and click on the arc of the part. A little window will pop up. Clicking on the icon made of two circles will make the two selected features concentric with one another. Hit the green check mark to finish the operation.
Remember in Part 1, we left a couple fillets off of the drawing so that we could add them later. On the Features Tab, there is a Fillet Tool. Selecting this will open a dialog box where you can enter the desired radius of the fillet. The sample drawing stated these fillets were 1/8 inch. Enter that and click on the corners that need to be radiused. Solidworks will show a preview of the fillets. Click the green check mark to accept the preview.
That’s it! Here’s the final product:
This Hackaday Column is called 3D Printering and in order to print the part, the file must be saved in .stl format. This is as easy as File-Save As. Select .stl from the file type list.
That concludes the Solidworks ‘Making A Thing’ tutorial. Happy modeling and printing!
3D Printering is a weekly column that digs deep into all things related to 3D Printing. If you have questions or ideas for future installments please sending us your thoughts.