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Create Your Workspace
Create Your Workspace
Open OnShape, Login or Sign Up
Open OnShape, Login or Sign Up
Sign Up if you haven’t already
You can use your student email
Doesn’t have to be a student account
Using for "Fun"
Select the Free plan
Create a new document
Create a new document
In your home page
Create (top left)
Select Document
Document Name: “LCVT - Your Name - Demo Saber”
Click Create public document
Get familiar with the workspace
Get familiar with the workspace
Default Sketch Planes
(Top, Front, Right)
Features Tab
Parts Tab
Views Manager
Tools bar
Buttons
Buttons
Left-Click
Select features
Hold and drag to select multiple features
Click on empty space to deselect
Right-Click
Edit features
Hold and drag to rotate view
Scroll Wheel
Zoom in/out
Hold and drag to translate view
Make sure your units are in inches!
Make sure your units are in inches!
Reference Pipe Setup
Reference Pipe Setup
You'll begin by creating a quick part in OnShape. This part will act as the steel pipe these parts will eventually be glued on.
NOTE: This part should NOT be exported at the end. It is only for reference as you model the actual lightsaber parts.
Create a sketch on the Top Plane
Create a sketch on the Top Plane
Select Sketch in top left
Select the Top plane in Features tab or click on the plane in the workspace.
Hide the Front and Right planes by clicking on the eye icon next to them.
Draw two circles on the Top Plane
Draw two circles on the Top Plane
Select Top face in the views manager.
Select Center point circle sketch tool in the top left.
Click on the origin in the center of the workspace. Then click again off to the side to create the circle.
Create another circle at the origin. Make it slightly larger.
Select the Dimension tool at the top (or press the "d" key).
Click on the outer circle once, then click off to the side.
Set the dimension to 1.125 in and press Enter.
Set the diameter of the inner circle to 1 in.
Press Esc to deselect the Dimension tool.
Extrude the ring created by the circles
Extrude the ring created by the circles
Select the Green Check Mark to complete your sketch.
Select the Extrude tool.
Click on the outer ring created by the two circles.
Set the Depth to your pipe length.
Recommended pipe lengths (inches):
9-10: Short, one-handed
10-11: Standard one/two handed
12+: Long, two-handed
Rename the part
Rename the part
You’ve just created a part representing the steel pipe that your parts will go on.
This part should not be exported for 3D printing. It only acts as a reference.
Press Shift + 7 to view your part in isometric view.
Right-Click on the part in the Parts tab.
Rename the part to Steel Pipe
You may hide the part while you work on the rest of your hilt.
Demo Hilt
Demo Hilt
This demo hilt will cover some basic CAD features and the design rules you'll need to follow for your own hilt model.
Part 1: Pommel
Part 1: Pommel
We will build our demo hilt from the buttom up. This first part, starting from the top plane is the pommel.
Create a new sketch on the Top plane
Create two circles at the origin
Set their diameters to 1.16 in and 1.5 in.
Extrude the sketch 1.5 in.
Create a sketch and select the top face of the extruded part.
Add two circles at the origin.
Use the Equal constraint tool and select both the inner ring of the extruded part and the smaller circle you just created.
Set the diameter of the other circle to 1.6 in.
Extrude by 2 in.
Create a Sketch on the Front plane.
Create a Center point rectangle near the bottom, vertical with the origin.
Set the height to 0.75 in and the width to 0.5 in.
Set the distance from the center of the rectangle to the bottom to 0.75 in.
Extrude the sketch by 1 in.
Select New instead of Add to turn this extrusion into a new part.
Apply a Chamfer of 0.2 in to the top and bottom corners of the extrusion.
Click on Circular pattern and select the new part.
Click on Axis of pattern and select the cylindrical side of the pommel.
Select Add.
Click on the rest of the pommel for the Merge scope
Set the Instance count to 6.
Add a Fillet to the top corner of the pommel.
Leave the Radius to 0.1 in.
Finally, rename the part to Pommel.
Part 2: Grip/Body
Part 2: Grip/Body
This part shows how to use the Linear pattern tool to create a common grip style for lightsabers.
Create a new Sketch on the top surface of the pommel.
Create two Circles centered in the middle.
Use the Equal constraint to set one of the circles equal to the inner diameter.
Set the other circle equal to the outer diameter.
Extrude the sketch by 0.3 in, and create a New part with it.
Add a 0.1 in Chamfer to the top and bottom corners of the extrusion. This should create a ringed tooth shape.
Click on the Linear pattern tool and select the new part.
Click on Direction and select the top surface of the part. The linear pattern direction will be perpendicular to the face.
Set the Distance to 0.3 in and the Instance count to 10.
Select Add and set the Merge scope to the new part.
You have completed the grip!
Don't forget to rename the new part!
Part 3: Emitter
Part 3: Emitter
This emitter uses the extremely powerful Revolve tool. This tool can save you a ton of time and allow you to create more complex shapes.
Create a new Sketch on the Front plane.
Create a long vertical line along the center.
Select the line and then click on Construction to turn it into a construction line.
Add another Line off to the side of the construction line.
Use the Coincident constraint to set the bottom of this line to the top of the grip.
Set the distance between the two lines to 1.16 / 2 in.
Add the following lines:
Note: The exact dimensions or lengths of these lines do not matter. You will give them specific dimensions later.
Define each line using this picture as reference:
Make sure each line is solid black, indicating it is fully defined.
Do not leave any lines blue. Undefined lines may be accidentally manipulated during future operations.
If you're having trouble defining all the blue lines, try these techniques:
Drag undefined lines to see which part of them is undefined
Use horizontal or vertical constraints. Some lines may be diagonal.
Click on the Revolve tool and select the face we created with all of the lines.
Set the Revolve axis to the center construction line.
Select New to create a new part.
Add a 0.2 in Chamfer to the bottom inner corner of the thick bit.
Add a 0.1 in Fillet to the top outer corner of the thick bit.
Part 4: Button & Blade Retention Holes
Part 4: Button & Blade Retention Holes
Once your model is complete, add the holes for the button and blade rention screw.
Start a new Sketch on the Right plane.
Face the Right side and line up your mouse with the center.
Create two circles. One near the middle and one close to the top.
Set the diameter of the button circle to 14.3mm.
Type "14.3mm" will automatically convert to inches when you click the check mark.
Set the diameter of the retention screw circle to 11/64 in.
Set the distances from the top of the hilt to the center of each circle as shown.
Click Extrude and set it to Remove.
Toggle the direction to cut the holes on the Right side.
Check Merge with all to cut the holes through all parts (including the pipe).
Part 5: Final Touches & Prep for 3D-Printing
Part 5: Final Touches & Prep for 3D-Printing
Hollow out the middle and double check the design rules guide.
Create a new Sketch on the bottom surface of the hilt.
Draw 1 circle at the origin. Set the diameter to 1.16 in.
Click on Extrude, select Remove, and set the merge scope to include all parts except for the Steel Pipe.
Instead of Blind, set the End type to Through all.
This will cut through anything in that direction.
This removes any residual features inside the hilt like those generated from the circular pattern.
Final Product
Final Product
You now know the basics to create your own hilt.
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