Cnc Carved 3d Lampshade
Introduction: Cnc Carved 3d Lampshade
I really hated the old plastic lamp we had hanging in our family room, so I made a better one!
Supplies
* Cnc
* Fusion 360
* 1x6 oak boards
* 1/4x6 aspen boards
* 3" long 1/4" endmill
* 1/8" endmill
* Lamp hardware
* Lots and lots of spare time and patience
Step 1: Modeling the Lampshade
I fired up Fusion360 and got started with a 14" square. I made an offset plane 10" up and made a 9" circle. I told it to Loft from the square to the circle, and had the basic shape. After doing a Shell with 1" thick walls, I had a lampshade.
Next I made some cylinders, and used Combine to subtract them and swiss cheese the model. The next step was to slice the model into 5 levels each 2" tall, and slice the 4 sides apart. The 2" height was chosen because that is as tall as I can get through with the 1/4" endmill. 668
I selected each side and did a fillet to get the cool 3d curves between levels.
We now have 20 separate pieces, each exactly 2" tall.
Step 2: What Are Registration Holes?
They are holes drilled through the part and into the spoilboard underneath that allow you to flip the part over and get it back into the exact same spot, which is a requirement for all two sided carving.
Most people put registration holes through a frame, and leave the part attached to the frame with tabs until it's done. I didn't want to go that route, so I decided to put mine through the middle of each part.
Step 3: Adding Registration Holes to the Model
I created a sketch on the top of the part, marked the centerline, drew a circle slightly larger than 1/8", and mirrored the circle to the other side.
After extruding the circles through the part, I have 2 holes exactly spaced from center going all the way through the part.
Step 4: Bottom Setup
We're going to flip the part over, because cutting it from the bottom first gives me a slightly larger surface area to glue it back down after the flip.
The setup here flips the Z and X axes, and very importantly choses a model box point for origin. Choosing a stock box point instead would result in the second carve being off center.
I've added .4" to each side of the stock, because the bit needs some room to move around. Otherwise the endmill bumps into the stock and then messes up the carve.
Step 5: Bottom Toolpaths
I created a 3d adaptive clearing toolpath.
I'm going to use an extra long (3 inch) 1/4" endmill, because it turns out a normal 2.5" long endmill isn't quite enough to cut through 2" of wood.
Under geometry I'm setting rest machining from the setup stock.
The cutting heights go from model bottom to stock top. The retract and clearance heights are both stock top plus 1/8" because I have almost no clearance with the extra long bit.
I'm using a .02" rough stepdown, .005" fine stepdown, and the smoothing option. That will clear out everything it can reach from this side up.
Next I have created a 2d bore toolpath.
It's setup for a 1/8" endmill, and choosing the 2 holes we made for registration.
For the heights, its going to cut from the hole top down to the hole top minus 1/2" because my 1/8" endmill only has 1/2" of cutting length.
Step 6: Top Setup and Toolpath
Ok for this setup, we can stick with model orientation, and choose the box point in the same corner as the origin.
We're not adding any stock to the model because we've already cleared the space around the part.
So just like the bottom, I'm using a 3d adaptive clearing toolpath with the 1/4" endmill.
This time the rest machining is set to "from previous operation" so it knows what's already been carved.
Heights are the same, with 1/8" for retract and clearance.
The stepdowns are still .02" and .005" with the smoothing checked.
And that should do it for the software side!
Step 7: Preparing Stock Blanks
I'm using a red oak 1x6, which is of course 3/4" thick.
I cut off two pieces about an inch longer than the piece I'm carving.
The whiter colored wood is aspen 1/4"x6. 220