!! Safety instructions !!

Make sure you never bump into screws (fire).

Check material of leftover screws/metal pieces!

Write down how many screws you put in.

Setting up your file in VCarve Pro

  1. Turn on computer.

  2. Open VCarve pro.

  3. Create a new file.


Setting up the material


  1. Job size (X & Y): Measure the width and height of the material.

You can either use the correct full-size width/height of the material, or trick the machine in thinking the material is smaller than its original size.

  1. Material (Z): Set Zero at the bottom. Except when using foam/wax/3D milling: When you don’t want to cut all the way through the material.

Measure the thickness of the material. Use a caliper.

  1. XY Datum position: ! Important, always double check ! Set the orientation point. Use the bottom-left corner (See blue dot on the picture).

  2. Units: Use mm

  3. Modeling resolution: Not important, is used for rendering.

  4. When finished, press “OK”

Always keep the orientation of the CNC in mind. X-axis should be the side parallel to the wall, Y-axis should be the “open” side. XY datum position should be the bottom left corner. When sitting behind the CNC-computer, line up the computer to correspondent with the right orientation.


Opening the CAD file
  1. Go to “File -> Import -> Import vectors”


Sometimes when you import a file lines disconnect. You can fix it in the VCarve.

  1. Check if there are no open/duplicate vectors. Delete if needed.


  1. Go to “Edit object -> Join vectors (with tolerance)” to connect lines.



  1. Use “Transform object” to move or rotate objects.
Types of mills

When choosing a mill there are a few things to consider.

  1. Diameter: Thickness of the mill. The thicker the mill, the faster and less precise. The thinner, the slower but more precise. Standard is 5mm

  2. Flutes: The number of threads of the mill. The more flutes, the more precise the milling, but also more slow.

One flute: For rough/prototype work. Fast, but not very neat.

Two flutes: Standard, more precise.

Four flutes: For very precise work. Slower.

The flutes are important for the speed of the machine, because the mill needs to drain the material. The more flutes, the more difficult to drain the material.

  1. Tips: We mostly work with two kind of tips; End mill (flat) or Ball nose mill (rounded). We generally use the square end mills. Ball nose mills are used for milling contoured surfaces.


5mm 2 flute end mill


3mm 4 flute ball nose mill


6mm 1 flute end mill


6mm 2 flute ball nose mill


Open the toolpath menu



We create different toolpaths for the milling.

The order of the toolpaths should be as following:

1 - drilling toolpath

2 - pockets toolpath

3 - inner cutting toolpath

4 - outer cutting toolpath

1 - Drilling toolpath


Use this toolpath to make holes for your screws to hold down the material when milling. Use the same size for the holes as for the mill. (If mill size is 5mm -> drilling hole size should also be 5mm)

  1. Select the drilling holes. (When using Vector selection order the machine will mill the holes in the order of selecting)

  2. Set start depth and cut depth

Start depth - If starting on the top of the material (most cases) start depth is 0. (Except for when drilling in a pocket)

Cut depth - You don’t want to cut all the way through because you want the screw to hold onto something. (2/3 of the material thickness is good)

  1. Select the tool (mill)

When pressing select the tool database will open. Select the desired tool and settings.


Tool info

Name - Name of the tool

Tool type - select End mill or Ball nose. (or other type you’re working with)


Diameter - Diameter of the mill using.

Cutting Parameters

Pass Depth - Depth for every vector per pass (you always use multiple passes) (half of the diameter of the mill). If using a 5mm mill pass depth is 2.5.

Step over - Distance between each pass of the machine tool head. The larger the step over, the faster the job but the less precise. 100% step over is no overlap. 50% is half overlap. The lower the step over, the smoother the surface.

Larger stepover: rough milling, fast prototypes.

Small stepover: nicer material, nice finish, precise work.

30% is roughly in the middle - Good startpoint

Feeds and Speeds

Spindle speed - 18000 for wood (maximum speed).

Feed rate - 50 - 60 mm for wood with 2 flute end mill. Smaller diameter -> Go slower. Check with Henk and other presets (trial and error) more flute; go slower (not completely sure). If milling foam (easier for mill) 100 - 120 mm per second.

Plunge rate - Speed of going down, always on 20.

  1. Peck drilling - Doing down in steps. (don’t need to use) (look up when to use)

  2. Dwell at the bottom of each drill pass - Mill will stay down a little bit longer. Result is more neat.

  3. Press calculate and then close.

2 - Pocket toolpath


  1. Set start depth and cutting depth

  2. Select tool

  3. Clear Pocket:

Offset (square spiral) or raster (side by side). Works well with vectors, but not with 3D shapes.

Cut direction - Climb or conventional. (doesn’t matter)

Raster angle - Set raster angle to match only moving the head of the machine.

Profile pass - Nice to do at the end to avoid ugly bits.

Pocket allowance - Will mill the pocket either smaller or bigger than the vector. (To make thing fit loosely or tightly)

3 - Profile toolpath


  1. Set start depth and cutting depth

  2. Select tool

  3. Machine vectors - Where to place mill.

  4. Seperate last pass - makes cut smoother.

  5. Tabs !! Important !! - Little nudges to connect everything to abound pieces moving during milling and being sucked up by ventilation. Preferably no tabs on corners.

After creating toolpaths

Save the file and name the toolpaths. Make sure the drilling toolpath is separate from the other toolpaths.

Clock icon - Check how long milling takes

Floppy icon - Save toolpaths Save files separately. Set metric system. Save file in map.

!! Safety break - Check your file !!

When changing a file - Always calculate again! Never change anything after checking. (No no recalculations etc. You don’t want anything changed because maybe you don’t notice a screw having a different location/or other dangerous situations occurring) Breathe, don’t hurry.

Make sure the drilling toolpath is separate from the other toolpaths.

Triple check your settings. Watch 3D view.

!! Safety break - Before using the machine !!

Always tie your hair.

Put on safety goggles.

Optional: Use ear protection on longer sittings.

Make sure there are no obstructions near the machine (no pieces of wood leaning onto the machine).

Check sacrificial layer, sand if needed.

Setting up the CNC Milling Machine

  1. Turn on the red button on the side of the machine.


  1. When the machine is turned on; Open Shopbot3.


  1. Locate keypad for moving the milling head by pressing K.


  1. Use keypad or arrows (keep x and y position in mind) to move milling head.

  2. Move z-axis by using page up/page down.

Change the milling bit
  1. Use butterfly screw to move skirt.


  1. Use tools to loosen the mill.



From left to right: Mill - Nut - Collet

  1. Push collet out of the nut to release mill.

  2. Choose the right collet for the mill


  1. Put collet into the nut until satisfying click.

  2. Put mill into the collet - Push all the way through the grip.


  1. Keep the length of the milling bit in mind when setting up file!


  1. Screw nut onto the machine head and secure with the tools - make it really tight but don’t overdo it.


  1. Put skirt back up - all the way.

  2. Place material on the machine. Make sure surface underneath is flat.

  3. When using small piece of wood: use drill to secure a screw so the piece doesn’t move when milling the drilling toolpath (on a place where the milling bit doesn’t go!). Make sure material doesn’t lift. Keep number of screws used in mind.

  4. Calibrate the machine, find absolute zero (press zero X/Y button).- Then press ok


  1. Press K and move mill head to the material origin (bottom left - check file).


  1. Take a picture of the coordinates - in event of a power shortage/emergency button pressing etc; you’ll need to re-enter the origin


  1. Open tab Zero -> click zero [2] axis (X & Y)


  1. Zero the z-axis. Zero on table surface since we put the zero in the file on the bottom. Choose a nice flat place.

  2. Use the metal plate to check connection with milling bit. Check if inp 1 lights up.



  1. Put metal plate directly under milling bit.


  1. Press ok. Don’t remove the aligator clip.

  2. Open keypad with K. Press page up ! No other button !

  3. Put away metal plate.

  4. Check file one more time.

  5. Load part file (folder) - open the screw toolpath file.

  6. Use key to turn on spindle


  1. Check if spindle spins straight.

  2. Turn on ventilation.



  1. Check ventilation room.

  2. Put in goggles.

  3. And when completely ready: Press start!

Holes will be drilled!

Stay close to the spacebar - if anything goes wrong: the mill will stop moving (not spinning) when you hit spacebar.

  1. Turn off spindle and ventilation.

  2. Press k to open up keypad and move milling head to make space to put in screws.

  3. Secure screws.

We prefer to use woodies since those won’t break. If the woodies are too long use the box with “schroeven kort”.


  1. Load second file.

  2. Turn on spindle and ventilation.

  3. Press start (keep spacebar in touch).

The remaining toolpaths will be milled.

After using the CNC milling machine

  1. Turn off ventilation and spindle.

  2. Move milling head.

  3. Take out screws. Count how many screws you take out.

  4. Close the Shopbot software.

  5. Turn off ventilation in the back.

  6. Switch the machine off.

  7. Vacuum the table.



To do:

Look into shopbot settings because of non circulair circle.

Look into offset - lower feed rate - gcode.

The intern box

After learning how to work with the CNC, it was time to make something!

First assignment: The Intern Box

Prepping in Fusion360

I struggled a lot with Fusion 360. I wanted to make hamer tenons and make my box parametric.

I drew the hamer tenon on one face of the box but i couldn’t get the tenon on the other face to align.

I decided to go a little simpler and make normal finger tenons.


Then i projected the face on a sketch (By creating a new sketch on the upper component and then selecting the face as the sketchplane) and saved the sketches as a DXF file



Setting up VCarve

I found a nice piece of plywood opened up VCarve

I measured the plywood and entered the measurements in VCarve. (122089012mm)

Then i imported the DXF files and fitted them on the board.


Because the pepper was too small i transported it to the top of the box and enlarged it.

I still needed a smaller mill for the pepper so i decided to mill only the pepper with a 3mm mill.

Then i made circles for the screw holes

I set up 4 different toolpaths:


Settings for each toolpath:

Screw hole toolpath:


Pocket toolpath (for the lid of the box): I gave this toolpath 1mm offset. It fitted perfect.


Profile toolpath (cutout of the main parts): I gave this toolpath .3mm offset. Could have used a bigger offset. I placed notches on all sides of the faces. Because i was going to mill the pepper separately i gave the top face extra nudges.


Profile toolpath (pepper):

I also gave the pepper nudges.


All toolpaths (except the pepper) were done with this 5mm end mill setting:


The 3mm (pepper) mill settings:


Time to CNC!

Michelle helped me set up the CNC, since i almost forgot to make a picture of the coordinates.


I first used the “schroeven kort” but they didn’t wanted to be screwed, and one broke, so we changed to the woodies instead. Those worked perfect.

And then the moment was finally there:


I was a little scared while watching the machine. Stayed very closely to the spacebar.


Sanding, sanding, sanding

Because of the plywood being a cheap and low quality material, the wood chipped quite a lot. The pepper was done with a smaller mill and slower feed rate, and came out nicely. I used a dremmel and sanding paper to smooth the chips




And then the pepperbox was done!