One of the more scary machines in the Fablab of Waag Futurelab is the big Shopbot CNC mill. With a spindle turning up to 18.000 rpm, this machine can send objects flying, reel in hair or clothing, or create a shower of sparks in less than a literal blink of an eye. Because of this, I’ll start with some general warnings:

1. Never turn your back on the machine during operation!
2. Watch out with long hair. Wear it in a bun, not a ponytail!
3. Watch out with loose clothing. Roll up your sleeves, tuck in shirts, and ditch your tie!
4. Always check if all the machine is clear of obstructions before operation!
5. The machine has no Z limit sensor!! When manually operating the toolhead, use extreme caution lowering the Z!
6. Don’t touch the carriage of the machine during operation. It might be tempting to rest your hand on Y carriage rail, but if your hand gets trapped in the moving gantry, the machine will chew right through it!

Prepare CNC for milling:

1. Turn on computer –> log in as fablab
2. Turn on CNC main board (not spindle) with the big red turn knob
3. There are only 2 programs to use: Vcarve and Shopbot
4. Open Shopbot (the CNC has to be on before opening shopbot)
5. Press “K” on the keyboard for manual toolhead movement (arrow keys). –> EXTREME CAUTION WHEN USING THE Z MOVEMENT (with PgUp/PgDn), there is no Z limit sensor, so the machine will ram the spindle through the floor when asked to do so.
6. Move the toolhead so there is enough clearance to swap milling bits
7. Lower the dust skirt by loosening the butterfly nut on the back of the toolhead
8. Use the spindle wrench to loosen the collet nut on the spindle
9. Remove the collet from the collet nut, select a new milling bit and matching collet
10. (A) Mount the collet inside the collet nut first, you have to feel a click!
11. (B) Then push the milling bit inside the collet assembly
12. Take note of the length of the milling bit sticking out of the collet, as you won’t be able to mill any deeper than this value
13. Mount the collet assembly in the spindle and fasten with the collet wrench, raise and fasten dust skirt

A short explanation of milling bits:

CNC milling bits have a couple of features:

1. Diameter (thickness of the milling bit) - 5mm is standard
2. Flutes (the number of threads) - more flutes are more precise but lower the cutting speed
3. Nose contour (ball nose or flat nose, called “end mill”)

Prepare Vcarve:

1. Open Vcarve
2. Create new file –> Job setup
3. Job size (X & Y): The width and length of your material
4. Material (Z): The height (thickness) of your material. Set “Z zero” to the bottom for 2D milling
5. XY Datum position: The origin point for this job. This is set to the bottom left corner of the shopbot by default
6. Units –> mm. Modeling resolution –> leave these settings. Press “OK”
7. Choose a milling bit from the tool database, and fill in the diameter of the milling bit at “Diameter(D)”
8. Fill in the following parameters:
   1. Pass depth: The maximum amount of material taken away in one pass. Set this to half the diameter of the milling bit (except when milling foam)
   2. Step over: The amount of overlap between passes of the toolhead. The lower stepover -> higher overlap -> smoother finish -> longer milling time
   3. Spindle speed: The spindle has a max of 18.000 rpm, use this setting for milling wood. The actual spindle speed is entered on the control box (V7-4X). Use the 2 worn up and down buttons to increase or decrease the spindle rpm
   4. Feed rate: The X/Y speed of the toolhead. When milling wood with a 2-flute end mill, set to 50-60mm
   5. Plunge rate: Z speed of the toolhead. Set to 20mm

Prepare files for milling (VECTOR):

1. Import file (.dxf, .ai, .pdf) –> File –> Import –> “Import Vectors”

2. Create a toolpath. Depending on you job type, select one of the following toolpaths:

3. Drilling toolpath - This toolpath is useful for pre-drilling screwmarks to fix your material to the CNC sacrificial layer. 2. Start depth: the Z point where the mill starts milling. Set this to 0, if you want the mill to start at the very top of your material

   1. Cut depth: How deep this toolpath needs to be drilled. Use a very shallow cut depth for pre-drilling screwmarks, ~2.0mm is sufficient.
   2. Select the drilling hole in the vector file –> create a drilling toolpath with matching settings –> select “calculate”

4. Profile toolpath - This toolpath prepares milling for lines, for instance when cutting out parts from plate material.

   1. Select the cutting lines in the vector file, MAKE SURE THAT NONE OF THE DRILLING HOLES ARE SELECTED. If the toolhead passes one of the screws once the material is fixed to the sacrificial layer, this will result in sparks, potentially leading to a fire or explosion.
   2. Cut depth: Same as material thickness, if you want the part to be cut all the way through. Start depth is 0
   3. Step over: if you are milling a single line, there is no step over!
   4. Tabs: THIS IS IMPORTANT! If you were to mill a simple circle from a plate of plywood, what would happen when the mill has almost cleared the circle free from the rest of the material? The moment the circle is free, it is no longer fixed to the sacrificial layer, so it would be sent flying by the spinning mill. We want the part to remain attached to the rest of the material, while cutting away ~95 percent of the profile. The “tabs” feature creates a few points where the mill will leave a little material untouched, similar to how the parts of a scale model need to be cut off of a plastic sprue before assembly.
   5. It is preferable not to put tabs at the corners of your model, but rather along straight edges
   6. Select “calculate”
   7. Save your toolpaths as seperate files, a DRILLING_TOOLPATH and a MODELNAME_TOOLPATH

   

Toolhead homing, material preparation

1. Turn on the CNC mainboard (if not on already)
2. Open Shopbot
3. Home the X and Y axes. This part is rather easy (read: safe) compared to homing the Z axis. Check that the machine is clear of obstructions and hit the XY zero button
4. Home the Z axis. CAUTION: because the Z axis does not have an endstop sensor, this operation is far more dangerous than home the X/Y, double check every step of the Z homing process:
   1. Put the toolhead in manual mode (“K” on the keyboard) and put the toolhead roughly above the area you’ll later position your material
   2. Take the metal levelling plate from the side of the toolhead
   3. Check if Shopbot recognises contact between the leveling plate and the milling bit: manually touching the mill with the leveling plate should light up the “stop-input-1”:
   4. Carefully place the leveling plate under the milling bit. Make sure the plate is directly under the bit!
   5. SLOWLY lower the toolhead with PgDn until the milling bit is ~5 cm above the plate
   6. Press the Z zero button to home the Z axis
   7. Raise the toolhead and move it out of the way
   8. Place your material, make sure it is level. Heavy slabs of wood will stay in place because we’re only drilling shallow holes, but lighter materials might need to be fixed with double-sided tape
   9. Move the toolhead exactly where you want your job origin point to be
   10. Make a piture of the coordinates in shopbot, this is your origin! If the machine loses power, you can still manually reset the toolhead to these coordinates if you have documented them
   11. Go to " (Z)zero" –> home(x,y). This resets all coordinates in shopbot to 0

Starting job

1. In Shopbot, go to “open” –> “load path” –> load your DRILLING_PATH. A paper-ish notebook-style window should appear
2. Turn on the spindle with the key attached to the collet wrench. The socket for the key is on the right side of the shopbot under the red turning knob
3. Turn on the vacuum machine (inside the closet)
4. Set the spindle control box to the desired spindle rpm
5. Check to see if there is any wobble in the milling bit, this might indicate that it is incorrectly seated
6. If you press START, the mill will start the loaded job. It is a good habit to keep a hand near “spacebar” before starting a job, since that is the key that immediately pauses the job if needed.
7. Press START, and carefully inspect the behavior of the mill. The mill should now drill 2mm deep holes in your material
8. After the mill has completed the path, turn off the spindle and move the toolhead out of the way with “K”
9. Carefully drill “woody” screws in the pre-drilled holes to attach your material to the sacrificial layer. MAKE SURE YOU DO NOT MOVE THE MATERIAL
10. Make sure the screws are not sticking out above the material
11. Load your profiling path named MODELNAME_TOOLPATH
12. Turn on the spindle
13. With a finger on spacebar, hit START. The mill should now start cutting your final model

IF THE TOOLHEAD HITS A SCREW: STOP THE MILLING JOB IMMEDIATELY, TURN OFF THE VACUUM MACHINE, AND PULL THE DUST BAG OFF THE VACUUM MACHINE. A FIRE-EXTINGUISHER IS KEPT NEXT TO THE SHOPBOT, NEAR THE WINDOW

Toolpath for 3D file:

1. Open Vcarve
2. Import STL: “import component” –> “3D model”
3. Milling 3D models consists of 2 operations, a ROUGHING PATH and a FINISHING PATH. The former takes away the most material, leaving a rough finish, while the latter takes precise passes to leave a smoother finish.
4. Roughing path:
   1. Select “Roughing toolpath” from the toolpath operations list.
   2. Pass depth for foam can be much higher than 0.5x the bit diameter. So you can enter any value less than the length of the milling bit extending from the splindle/collet
   3. Step over can be set to the lowest setting for a roughing pass, since it doesn’t need to leave a smooth finish. Set to 90 (since 0 is the most step over)
   4. Spindle speed for foam can be ~12.000
   5. Machining limit: Set to model
   6. Machining allowance: The amount of material left to the finishing path, or when only doing a roughing path on a part that will be sanded afterwards
   7. Roughing strategy: Z level or 3D raster. According to parsons: Z level uses a type of pocketing that follows the shape of your model. It’s more efficient, but leaves more stock material, making it a better choice for soft materials. 3D raster follows the topology of your model. It removes more stock material, but takes longer to machine. This is a better choice for hard materials. https://makingcenter.parsons.edu/wp-content/uploads/2021/02/How-To-3D-Rough1.pdf
   8. Select calculate, check the preview window
5. Finishing path:
   1. Select “Finishing toolpath” from the toolpath operations list.
   2. Step over: 0.5 (around 10%), a lower value will take longer to machine, but will leave a smoother finish
   3. Area machine strategy: This dictates the machining direction. Set this to CLIMBING, as CONVENTIONAL is the same direction as loosening the collet nut.
   4. Select calculate and check the preview
   5. Save both toolpaths as separate files. A ROUGHING_PATH and a FINISHING_TOOLPATH

Milling my box:

During my box milling assignement, a couple things went wrong:

1. During the execution of a drilling toolpath, I became worried my material was not positioned properly. I decided to stop pause the job, but didn’t realise that the spindle was still milling in the wood. This experience leads to the following addition to the rule of having a thumb ready at spacebar during a job:
   1. Spacebar is not an emergency shutdown. Pressing spacebar at any given moment of panic does not mean you can sit back and relax again. Preferably, you wait with pausing the job until the spindle is executing a travel move (i.e. the milling bit is traveling through air, not through wood). If that is not possible, it is important to shut down the spindle shortly AFTER pausing the job. Don’t shut off the spindle BEFORE pausing the job, as that means the shopbot will try to ram a non-spinning milling bit through the material.