Difference between revisions of "Materials"

From ShapeOko
Jump to: navigation, search
m (Metals: Spelling - tram -> trim)
Line 217: Line 217:
* single flute, up-cut cutter (e.g., Onsrud O-Flute), starting point 18,500 rpms on the spindle, feed rate of 85 inches per minute.
* single flute, up-cut cutter (e.g., Onsrud O-Flute), starting point 18,500 rpms on the spindle, feed rate of 85 inches per minute.
* Work holding: spoil board and spray glue technique.  
* Work holding: spoil board and spray glue technique.  
** secure your spoil board to the machine, tram an area slightly larger than your work piece.  
** secure your spoil board to the machine, trim an area slightly larger than your work piece.  
** use a spray adhesive such as 3M Super 77 --- follow the directions
** use a spray adhesive such as 3M Super 77 --- follow the directions
** Apply some weight for a few seconds to make sure you get good adhesion.
** Apply some weight for a few seconds to make sure you get good adhesion.

Revision as of 19:54, 9 January 2015

Primary consideration is how fast the flutes of the cutter move against the material. A secondary consideration is the direction of rotation of the cutting tool (typically clockwise) and the interplay between the movement of the spindle and material, Climb vs. Conventional Milling.

The perfect cutting is not too slow, not too fast, not too shallow and not too deep.[1]

Forum user danimal wrote up an excellent overview: Re: Seek and Feed rates, depth passes w/ an in-depth usage strategy.

The values below may be used in configuring milling operations when using a CAM program to generate G-code to make a cut, but unless your machine is essentially identical to the machine which they were used on, can be considered as only very general guidelines. All values should be verified and tested on a scrap of material first, then one should adjust to match desired chip size and surface finish and time required for completion.

Please share any instances of success or failure along w/ the specifics of:

  • your machine and its configuration, esp. any upgrades (but information for stock Shapeoko 2s would be especially welcome)
  • endmill
  • actual feed / speed
  • whether or no you had dust collection active
  • any active cooling
  • material, including source

Feed and Speed Calculators

While several online tools exist for calculating linear movement (feeds) and spindle RPM (speeds):

Onsrud Router Bit Search for plastics
Chip Load Calculator Excel spreadsheet
Feed Rate Calculator (online)

These tools are intended "... for industrial machines that assume that there is no slop, twist, or flex in the machine."[2]

In addition, one needs to decide upon a cutting depth advancment, and the amount of stepover (how much each toolpath overlaps, see the Glossary). Using a smaller cutting depth advancement is one suggested strategy for coping w/ the design's lack of rigidity.[3]

See also References, Feeds and Speeds below.

Interesting discussion of materials suitable for cutting on a Shapeoko and their characteristics in: Re: Material Advice.


Typical starting values:

  • Cut Depth/Step Down: The traditional guideline is 1/2 the diameter of the end mill[4]. Another school of thought is to start shallow and work deeper until the sound of the cut changes (typical values this way are 0.3mm (harder plastics (acrylics)) or 0.6mm (wood)[5]
  • Stepover: 1/3--1/10 the diameter of the end mill[6]
  • Plunge Rate: (Note that your Endmill must be capable of centercutting)
    • harder materials (steel and cast iron and harder alloys): 8 to 10% of feed rate
    • softer materials (softer aluminum alloys and brass, denser/harder plastics and composites, exceptionally hard woods): 15 to 20%.
    • softest materials (most plastics and varieties of wood): 30 to 50%

Cutting Formula

In contrast to the usual cutting formula, this simpler one has been suggested[7]:

Chip load is a physical thing. It's the thickness of the thickest part of the chip that the cutter generates. If your cutting feeds are set up right (i.e. actually generating chips), you should be able to straighten out a chip (carefully! they can be sharp) and measure the thickness. That would be your chip load. I like to keep chip load constant, since the thickness of the chip has a huge amount to do with where heat goes, where cutting forces go, and ultimately the cleanliness of your cut and the life of the tool. I'll always start with the chip load to get a feed rate. Here's how that works:

Feed = [chip load]*[#of flutes]*[RPM]

You'll notice that cutter diameter doesn't come into play there. If you add it to your formula, you're going to come out with really weird numbers. Basically, I say I want each tooth of my cutter to take off a certain amount of material, say 0.004". Now let's say my cutter has two flutes, so every time it rotates I have two chips being removed. In order to remove 0.004" per flute, I have to move the cutter by 0.004*2, or 0.008" per revolution. Now I can multiply that out by my spindle RPM (12000, because why not) to get 0.008*12000 or 96 inches/min. You'll notice units cancel out to a sane unit of IPM for feed. "But Jeremy," you say, "If I'm trying to run my poor little 1/16 cutter through acrylic at 96 IPM it won't last two seconds! That's just too fast!" Well, I hear you. The thing is, it's not too fast. It's actually the appropriate speed to get a good cut. (I'm not vouching for 0.004" necessarily being an appropriate chip load for acrylic. I'd actually suggest something more along the lines of 0.002" to 0.003", but that's a discussion for another time.) The thing at this point in time that will break your cutter is excessive cutting forces, which come from the last variable in our cutting equation: depth of cut.

Many places will have fundamental rules of thumb for how deep you should cut with your CNC router. They'll say "cut at 1/2 your cutter diameter," or something along those lines. Ignore that for these models. I don't trust something that simple, as its bound to be overlooking something. In this case, proper chip and cutter loading. There are a lot of ways to use a lot of math to calculate how deep you should cut, but at the end of the day you're still using a shapeoko machine, which is quite flexible. What I'm saying is, every machine will be different and hard to predict. Start shallow (won't hurt anything) and work down deeper and deeper until it sounds like your cutter is really loading down, then back off a shade and remember that value. I usually suggest starting with 0.012" depth per pass for harder plastics (acrylics) and 0.024" for woods. Those will be very light cuts, and you can play with increasing them more and more until you're happy with how the cut goes. [8]

Suggesting that one should modulate the cutting depth (the afore-mentioned working w/ a light and delicate touch).

One thing to understand is that depth (axial depth, along the cutter) vs width (radial width, or stepover) is very different in traditional machining as opposed to cnc routing. In traditional machining, you tend to start out with a block of material slightly oversize of the actual part. You then whittle it away to reveal the part hidden inside, which usually involves very deep axial cuts with a very shallow radial cut. This is the opposite of routing, in which we're cutting parts out of sheets, so most of the time we have no choice but to have 100% radial engagement (full width of the cutter is cutting). This is less than optimal, and means that we have to cut shallower to compensate. Most "rules of thumb" for cut depth don't quite grasp the fact that you are more or less locked in to 100% width of cut. You can't choose an optimal depth and adjust the width to compensate as normal. You can implement various strategies to do that when cutting parts out of a sheet or panel, but it really doesn't make any sense in that context because it's much less efficient from a cycle time perspective.[9]

An exercise for the reader:

Take the feeds and speeds for a small endmill in a particular steel alloy, then calculate the force needed to make that cut, a specific engagement. Then, calculate it out as a kinematics problem.[10]


  • MatWeb Material Property Data --- searchable database of material properties includes data sheets of thermoplastic and thermoset polymers such as ABS, nylon, polycarbonate, polyester, polyethylene and polypropylene; metals such as aluminum, cobalt, copper, lead, magnesium, nickel, steel, superalloys, titanium and zinc alloys; ceramics; plus semiconductors, fibers, and other engineering materials.

Dimensional Stability

Note that different materials will respond to cutting in different ways, and will ultimately be cut with differing levels of accuracy. Discussion in: Re: Accuracy: Not sure if this is a MakerCAM issue.

Feeds and Speeds

Sortable table
Material Surface speed Bit Feed Speed Cut Depth Stepover Cooling/lubricant Spindle Notes
Aluminum 1/8" four flute solid carbide endmill 400mm/min 30,000 RPM 0.2 mm 50% WD40 generic dremel
UHMW single or double flute 1/8" end mill 762--1524 mm/min (30--60ipm) 11,000 RPM 1.5875 mm (1/16" @50-60ipm) or 3.175 mm (1/8" @30-40ipm) ? none generic dremel
HDPE double flute 1/8" end mill, 1/2" cutting length 355mm/m 11,000 RPM 1mm 50% none generic dremel, Dremel 4000
Polycarbonate (Lexan) double flute 1/8" end mill 1000mm/m 20,000 RPM 1mm 2mm none ?
Acrylic double flute 1/8" end mill 400mm/min 20,000 RPM 2.032 mm (0.08" Plunge Rate: 75mm/min.) n/a (through cut) none ?
Plywood 2 flute 1/8" Carbide 700--1000mm/m 20,000--30,000 RPM 0.7mm--2mm 2mm none stock spindle, DW660
Basswood 2 flute 1/8" Carbide, 1/2" cutting length 710 mm/m 25,000 RPM 1mm 40% none Dremel 4000 (conservative)
MDF 2 flute 1/8" Carbide 2400mm/min (conservative) 30,000 RPM 1.5mm (very conservative) none DW660
33kg/m^3 Foam 6--12mm ? ? 5 to 10 mm 50% none ?


Ideally when milling metals one would use an upcut bit, so as to clear chips --- however, given the narrower bits which a Shapeoko is likely to be using, plunge depth is typically limited to 0.25mm (0.01") which ameliorates the difficulty of clearing chips. Even so, some users have found it helpful to increase the width of cuts to aid in chip clearance as noted in Re: ORD Bot Hadron.

Forum discussion full of suggestions: Re: Aluminum.

Strategy for cutting thin sheets: http://www.reddit.com/r/CNC/comments/2jdjdf/tips_for_cutting_thin_metal_with_a_cnc_machine/clbltfl

  • single flute, up-cut cutter (e.g., Onsrud O-Flute), starting point 18,500 rpms on the spindle, feed rate of 85 inches per minute.
  • Work holding: spoil board and spray glue technique.
    • secure your spoil board to the machine, trim an area slightly larger than your work piece.
    • use a spray adhesive such as 3M Super 77 --- follow the directions
    • Apply some weight for a few seconds to make sure you get good adhesion.
  • Machine
  • to remove the work piece, use a propane torch to heat your piece until it's too hot to touch, this will loosen the adhesive.
  • Use a chisel to carefully pry your work piece from the spoil board, solvent will clean any remaining adhesive.

One consideration when cutting electrically conductive material is that the electronics must be shielded from the chips --- ensure that your controller is in an enclosure which will protect it.


When milling aluminium, you have to know which alloy you're milling. Aluminium is like wood : milling oak, pine or balsa wood is not the same. For instance in aluminium you have series (1000 to 8000), each of which uses different elements (specified in parentheses below) to achieve differing mechanical properties.

  • 1000 essentially pure aluminum, can be work hardened
  • 2000 (copper)
    • AU4G (2017) is really good at machining : you can take deep passes (~0.3 to 0.5mm) at something around 500 to 800mm/min (20 to 23 ipm). This aluminium will resist to the heat and won't melt.
    • 2024 --- very strong and is used a lot in some aerospace applications. Its ok to work with, I'd say its in the middle. Its not gummy like some other alloys but it doesn't produce the best finishes and will take a little longer to mill over say 6061-T6[12]
  • 3000 (manganese) can be work hardened
  • 4000 (silicon)
  • 5000 (magnesium)
    • 5052 available in sheet --- machinability only fair
  • 6000 (magnesium and silicon) easily machined
    • 6060 is really different. It's much softer and melt faster and stick on the endmill, making it worse. You have to take smaller passes (0.2mm) at high feedrate (around 1000 to 1200 mm/min, or 40 or 47ipm). Using a 1 flute endmill usually give better results.
    • 6061 most commonly used aluminum alloy (in the U.S.) --- 6061-T6 nice to machine and forgiving. Can be milled without coolant or lubricant if the feed rate, depth of cut, and spindle RPM are set correctly.[13] 6082 is very similar and more common in Europe.[14]
  • 7000 (zinc) can reach the highest strengths of any aluminum alloy
    • 7075 also gives good results when milling, but is difficult to cut on a Shapeoko[15]

These are not the same values as the best suited feed and speed in industry.[16]

One thing which will make a big difference is to choose an end mill especially designed/made for cutting aluminum. Characteristics of such include:

  • upcutting flutes
  • reducing the number of flutes to reduce the effective feed rate[17]
  • special coatings to prevent material from adhering to the bit[18]
    • ZrN (Zirconia Nitride)[19] --- described as “for aluminum only”
    • TiB2 (Titanium Diboride)

Depending on the aluminium alloy you're milling, the material can melt and stick to your endmill. If this happens, try to change the cut parameters: fewer flutes, lower RPM, faster feedrate, also try coolant while milling (WD40, water or aluminium specific coolant fluid). This is less likely to happen with harder alloys such as 2017.[20]

Discussion of techniques and strategies in: Re: Success and Some Failure milling Aluminum. See also CNCCookbook: 10 Tips for CNC Router Aluminum Cutting Success.

Doing the finishing pass as a climb cut will give a better finish on an extraordinarily rigid machine and bit. Using a roughing pass wider than cutter is advised.[21]

If aluminum “galls” on an endmill, a bathroom drain clearing product (such as Draino®) may be used to remove the material (please check the chemistry of this first against the composition of your end mill and its coating).

An afternoon with aluminum --- detailed discussion of tool paths, finish and various

6061 plate

This is available from Inventables.

Forum discussions here:


Narrow Belt Clip

.02" aluminum 6063

  • Feed: 500mm/min (this could probably be increased)
  • bit: 2 flute 1/16" bit.
  • Cut Depth: .01" (Cut in 2 passes)
  • Plunge: 75mm/min

T6 plate

Re: Vote for your favorite ShapeOko spindle solution!

  • Feed: 30ipm
  • bit: 1/8 carbide altin endmill
  • Cut Depth: .025"

2017A and 7075 (harder)

Forum discussion here:

Re: Suggested feeds and speeds for Aluminum

  • Bit: 2 flute 1/8" carbide endmill w/ 45 degree helix.
  • Feed: 600mm/min
  • Speed: 20--25,000
  • Plunge: 100 or 150 mm/min
  • Step Down: 0.4mm


From: Aluminum 7075-T6 spindle mount

  • Bit: 2 flute 1/8" carbide
  • Feed: 350mm/min
  • Speed: 10,000 rpm
  • Plunge: n/a (ramp-in only)
  • Cut depth: 0.2mm for slots with 100% bit engagement, 0.4mm for finish pass
  • Lubrication: used cutting oil only on the pockets
  • Bit: 2 flute 6mm carbide endmill
  • Feed: 400mm/min
  • Speed: 6730 rpm
  • Plunge: n/a (ramp-in only)
  • Cut depth: 0.2mm for slots


  • Feed: 200mm/min
  • Step Down: 0.4mm

WD-40 lubricant.[24]


1/8" carbide cutter at 150mm/min. 0.2mm depth of cut per pass using DW660.[25]


cut on my SO2, with a feed rate of 300mm/min and a 0.1mm depth of cut... Dremel. I used a speed of around 15000 rpm and plenty of WD40 as lubricant. The thing that made the biggest difference to the finish was blasting all the chips out with air at regular intervals. ... On the down side, it blasts small chips of aluminium and WD40 all over the place, so there is plenty of cleanup required afterwards...[26]

Softer alloys

Forum discussion here:

Re: Suggested feeds and speeds for Aluminum

  • Bit: 1 teeth 3mm mill
  • Feed: 800--1200mm/min
  • Speed: 10--13,000
  • Plunge: 100 mm/min
  • Step Down: 0.2mm
  • Cooling/Lubricant: a lot

10mm 6160 aluminum plate

Carbon Fiber Plates and Aluminum Bearing Blocks

400 mm/min feed 20000 RPM 1/8" four flute solid carbide endmill. Spiral plunge lots of tap magic cutting oil throughout the milling. 0.25 mm pass depth.

1/2" aluminum plate

Aluminum spindle mounts for Makita RT0701c

1/8" single flute spiral end mill from Inventables. Step down was .2mm per pass, feed rate of 400mm/min. Makita's speed was set to about 3-1/3 on the dial, which goes up to 6. I used some silicone spray initially, but I ran out and cut most of the job dry, periodically vacuuming chips out of the cut.

Aluminum Knob

1/4" 4 flute bit.

Feed was 15 ipm and 1 ipm Z. 0.01" per pass too. Very conservative. Used cutting oil occasionally.

15 ipm with step down .01 on 1/2 aluminum[27]

Aluminum flashing

Cutting Stencils in Aluminum Flashing

Aluminum (from Easel)

  • Speed: 25
  • Depth Increment: 0.005"


Tough, strong alloy with excellent corrosion resistance, however not easy to machine.[28] Datasheet.[29]


  • Speed: 10
  • Depth Increment: 0.015"

Cast Iron

6000 r.p.m. (theoretical)


Weld Steel

Speaking of pushing my machine hard, by pure accident I've actually been able to cut 22 gauge weld steel in a single pass at 7 IPM. It was smoking quite a bit but the machine was marching along without missing steps or jerking. I'll never do that again though, but it was cool to see the machine pushed to its limits.[30] The intention was to make a 0.005" pass.[31]

Stainless Steel

Forum post discussing this: Cutting stainless steel?

One user, danielfarley was successful using an 800W spindle w/ settings of: carbide tool - two flutes, 2mm wide, 100--140 mm / min, used some WD-40 as lubricant... although some tooling works better with no lubricant.[32] Unfortunately, this has a potentially high cost in tooling, w/ endmills only lasting for cutting of a single (small) part in this instance.[33]


More successful was forum user dottore in An afternoon with stainless, making a "turner's cube" on a much upgraded Shapeoko 2 (Makita RT-0701, aluminum bed, belt drive Z-axis w/ Acme screw, cooling system, &c.).


Brass is available in a wide variety of alloys each w/ markedly different characteristics, Engraving Brass (CZ120 / CW608N) which has 2% lead added to it, or Free Machining Brass (CW614N / CZ121) which has 3% lead content are “lovely to machine”.[34]

DW660. 0.063" straight 3-flute bit[35] Feed 5in/min drop 5in/min drop distance 0.015"[36]

353 engravers brass


Two flute:

  • bit: 2 flute 1/8"
  • feed rates: 4in/min
  • plunge rate: 0.015 drop down
  • step over: 60%

Three flute:

  • bit: 3 flute 1/16"
  • feed rates: 10in/min
  • plunge rate: 0.02" drop down
  • step over60%

3 flute straight bit 0.063" diameter 0.01" stepdown 5"/min feed rates [38]


Good overview of plastic machining characteristics here: Boedeker Plastics: Guide to Plastics Machining. See also Basics of Plastic Selection for Machining.

There is a heat issue with all plastics, the idea is to remove as much material in one rotation of the spindle as possible then move on. If you dwell in one place too long your bit will heat up and the material will heat up, leading to distortion, bad smells, and dull bits. Single flute bits will help.

Info: When milling plastics you want "chips" to come off the bit. If you find that you are instead getting "threads" of material you need to either increase your speed or increase your depth (preferably not both). You will notice a difference depending on the direction your mill is going. If you get a lot of "chatter" (bit seems to hop) while milling uphill (where bit is turning into the material) you'll want to slow your job down slightly.


Go a bit slower and a bit lighter in ABS than HDPE.[40]

3 or 5 in/min and a plunge depth of 0.05"[41]


  • Bits: roughing path with a 1/4" end mill and a finishing path using a 1/16" ball nose mill
  • Feed: 800 mm/min feed speed
  • Cut Depth: 1/16" @50-60ipm or 1/8" @30-40ipm
  • Stepover: 10% step over
  • Material Thickness: Varies (Tested 1/8" - 3/4")

Forum post: Han Solo trapped in Delrin?

According to some machinists, Delrin must be allowed to rest for about 24 hours after initial machining, and then the last finish cut (0.001") to precise dimension can be taken. Very sharp tools, lots of coolant, and temperature limits are recommended.

Further information:


  • Bit: single or double flute 1/8" end mill (with center point for drilling!)
  • Feed: 30-60ipm
  • Speed: generic dremel turned up to 11
  • Cut Depth: 1/16" @50-60ipm or 1/8" @30-40ipm
  • Stepover: ???
  • Material Thickness: Varies (Tested 1/8" - 3/4")
  • Wikipedia Link


Plastic that can easily be found in your local supermarket as a white cutting board (but also available in other colors). Only limitation is they are typically quite thin, usually not greater than 1/4"(6mm) thickness. Thicker material is available (9mm or so is sold as "half-inch" cutting boards), while larger boards in half-inch or even 3/4" thickness are available from specialty suppliers or online.

Forum posts discussing (very conservative) specifics of cutting it here.

  • Bit: double flute 1/8" end mill
  • Feed: 355mm/m (very conservative 1,500--2,700 mm/min has been suggested --- one can trade off speed for cutting depth)
  • Speed: 11,000 RPM (Dremel 4000 set to 11)
  • Cut Depth: 1.5mm (as much as 2.5mm may be feasible at slower speeds)
  • Stepover: 30%

We did some tests at Inventables and these settings worked successfully[42]:

DIA = 0.0625 Step over% = 60 Step down = 0.045 Spindle Speed = 12,000 Feed Rate = 60 Plunge Rate = 30

DIA = 0.125 Step over% = 60 Step down = 0.062 Spindle Speed = 12,000 Feed Rate = 60 Plunge Rate = 30

One datapoint, Improbable Construct notes "2 flute 1/8" endmill, 40% step over, 1/16" cut depth, 27000 RPM, at a feed speed of 1200 mm with good results. Of course that was with dual Y motors and the double X mod."

Another datapoint: 30in per minute on the feed rate, and .125 on the depth per pass.[43]

A further note: "With HDPE you want to use conventional milling. It does leave a fuzzy, stringy edge when you use climb milling."[44]

Rubbing the pieces w/ a towel after machining will help remove errant flecks/strands.

Two-Color HDPE

the following settings worked best with a straight fluted bit. Upcut bits make a huge mess of things.

  • 40% stepover
  • 0.05" step down
  • 20IPM Feed
  • 10IPM Z-Feed
  • Clockwise on the engraving[45]

Polycarbonate (Lexan)

  • Bit: double flute 1/8" end mill
  • Feed: 1000mm/m
  • Speed:20,000 RPM
  • Cut Depth: 1mm
  • Stepover: 2mm


Lengthy discussion of the difficulties of milling acrylic and some solutions: bit getting "sucked" down.

Notes from IC for cutting his dust shoe:

  • Bit: double flute 3.175mm (1/8") end mill
  • Feed: 400mm/min
  • Speed: 20,000 RPM
  • Cut Depth: 2mm (0.08")
  • Stepover: n/a (through cut)
  • Plunge Rate: 75mm/min.

O-flute bits are recommended.[46]

Makita RT0701 16in/min feed, 0.08" step down[47] at speed 2 (~12,280 r.p.m.)[48]

10mm cast Acrylic using 6mm Single Flute bit 2mm depth 400mm/min Feed speed.[49]

Cast Acrylic: DW660: single flute end mill, 30000 rpm, 300mm/min feed rate, 75mm/min plunge. Pass Depth 0.0625[50]

Extruded Acrylic: Stock Shapeoko 2 w/ stock spindle, maximum speed, feed rate 380--400mm/ min and plunge rate 100 mm/ min., Step down 0.8mm with better results.[51]

Acrylic and Polycarbonate: 600 Watt router, 30,000 rpm, feedrate of 1500 mm / min, plunge rate of 800 mm / min.[52]

Some users have reported difficulties w/ the above settings: 660 and 30000 RPM issues --- please test w/ scrap and report specifics.

Fabrication Notes

Extruded acrylic tends to "store" energy and may randomly crack if one presses in a part as a friction fit. This happened when I.C. tried pressing in the magnets on his DWP611 shoe and broke a couple.[53] A further issue is that it will have two separate optimal feed/speeds for cutting, one along the extrusion axis, the other at 90 degrees to it.[54]

The edges may be polished after cutting by rapidly passing an open flame over them and quickly allowing the material to melt and cool.

You may wish to consider misting the material w/ water[55] and/or dishwashing liquid[56] as a coolant or applied to the bit as a lubricant[57]

Further Notes and References

  • 14,500 r.p.m. and 200 i.p.m. or 18,000 and 250 i.p.m.[58]
  • Plastics Distributor® & Fabricator Magazine: Achieving Premium Finishes When Routing Acrylic
  • Plexiglas = Perspex = Acrylic = PMMA = Polymethylmethacrylate
  • Cast vs. Extruded --- usually cast has a paper protective film, while extruded has plastic[59]
    • Cast PMMA is essentially pure polymethylmethacrylate and machines well using, when possible, tools with zero top rake and a very sharp cutting edge. Brand new HSS cutters are a good option.
    • Extruded PMMA has chemicals added to it to aid in extrusion and does not machine as nicely, tending to melt. There is a possibility of stress cracks and crazing after machining as noted above[60]

Extruded Polystyrene


  • Bit: 1/8" end mill
  • Feed: 1000mm/min
  • Speed: 6,000 RPM
  • Cut Depth: 2mm (0.08")



  • Feed: 200--300 in/min
  • Speed: 5,000 RPM

Using a Dewalt DW660 on a ShapeOko 2, Riley Porter was able to cut 3/8" plexiglass[61] with the following settings:

  • Bit: 2-flute 1/8" carbide upflute w/ 1/4" shank[62]
  • Feed: 600 mm/min
  • Speed: Full speed
  • Cut Depth: 1.75mm (was supposed to be 1mm)

Extruded plexiglass

Stock shapeoko 2 with dremel 4000 (grbl 0.9)

  • Feed xy: 1000mm/min
  • Plunge Z speed: 250mm/min
  • Speed: 13-15,000 RPM
  • Cut Depth: 0.5mm
  • Bit: 1-flute 1/8" carbide upcut spiral [63]

Note: Extruded plexiglass is not easy to mill. The above combo is what gave me best results after some experimentation. A two flute straight cutter can be used but will cause more melting.


13--15,000 RPM --- Spiral O shape bit suggested.


available as boards and trim pieces at home center. Mentioned for cutting in 25mm thickness.[64]


alupanel (HDPE layer caught between 2 0.3 aluminium sheets) http://www.shapeoko.com/forum/viewtopic.php?f=30&t=4394


See Guesstimating Feed Rates for a technique for using Janka hardness numbers to derive a first approximation for cutting a harder wood.

For shallow pockets, a down cut spiral bit results in cleaner top edges.[65]


  • Depth Increment: 1mm
  • Cut Feedrate: 710mm/min (conservative)
  • End mill: 2 flute .125 end mill
  • Speed: 25,000 r.p.m.
  • Stepover: 30%
  • Spindle: Dremel 4000

These measurements work for other soft hardwoods too, like Alder and may be a good starting point for softwoods.


  • Speed: 30
  • Depth Increment: 0.028"


  • Speed: 28
  • Depth Increment: 0.045"

Hard Maple

Forum post showing a cut in hard maple using a Dewalt DW660 here.

Forum user cchristianson posted the following numbers in Re: First real project! dimensional letter shop sign: 24 in (609.6mm)/min for feed with 5 in (127)/m plunge @ 1/16" passes (1/8" 4 flute end mill). The same values were used for a very hard mahogany as well.

1/4" router bits at 60 in/min and a .060" deep pass through maple with no issues.[66]

  • Speed: 28
  • Depth Increment: 0.028"


  • Bit: 2 flute 1/8" endmill.
  • Feed: 562.5mm[67]
  • Speed: 26,000 R.P.M. (likely too fast --- Harbor Freight Trim Router)
  • Cut Depth: 1.5mm
  • Stepover: 40%

Theoretical: 1/4 inch carbide bit try 12-18000 rpm and 762--2,286mm/min (30--90 ipm). 1/8 inch depth per pass. Leave about .01 inches for a full depth finish pass at the lower ipm range. Depending on the machine you may need faster or slower. You might also need a different step down.


Forum post showing small, detailed cuts in pine (including a Harley Davidson logo) here.

Forum user atrueresistance reported success in So Close, 80 lines left any suggestions

Forum user Junior483 noted success using the same settings as for MDF.[68]

Stock Shapeoko 2 w/ Altocraft spindle: Plunge depth 0.03125", feed rate 5 inches per minute --- seemed to tax the spindle. Suggest shallower plunge.[69]

(CamBAM settings)

  • Depth Increment: 0.03
  • Cut Feedrate: 35 (40 was too fast)
  • Depth Plunge: 10
  • Tool Diameter: 0.125 (2 flute .125 end mill)
  • DW660


MDF (medium-density fibreboard) is a relatively easy material to cut. It's soft and evenly composed, so the bit should have no trouble working through it at a consistent pace. The main concern when cutting MDF is that cutting will yield a lot of airborne sawdust (which, due to how MDF is made, can be harmful to to inhale). Wearing a dust mask is certainly not a bad idea.

You should also be aware of burning issues while cutting MDF. If your cuts are making the wood darker and/or producing a smell, try using a faster feed rate or a better bit (a 2-flute carbide endmill works very well). Faster feed rates prevent the bit from staying in one place for too long, which is a factor in overheating.


  • Three inch MDF Box Forum post with speed and bit specifics here.
    • Bit: 2 flute 1/8" endmill.
    • Feed: 100ipm
    • Speed: ???
    • Cut Depth: ???
    • Stepover: ???
  • Simple triangles (Blog post)
    • Bit: 2 flute 1/8" carbide endmill
    • Feed: 400mm/min (conservative)
    • Speed: 30,000rpm (DW660 standard)
    • Cut Depth: 7.5mm (entire 1/4" sheet)
    • Stepover: ???
  • 2D wing shape (Blog post) (Video)
    • Bit: 2 flute 1/8" carbide endmill
    • Feed: 400mm/min (conservative)
    • Speed: 30,000rpm (DW660 standard)
    • Cut Depth: 1.5mm (very conservative)
    • Stepover: ???
  • Signs carved out of MDF: here


AngusF noted in Re: How to mount DW660?, “1/8" end mill cutting Baltic birch plywood at a 0.7mm depth per pass, I will miss steps at 800mm/min, but not at 700. I'm still using the stock spindle...”

With a DW660, double X, Y drive shaft, this gives a fairly clean edge.

  • Material: 1/4" nominal (4.8mm - 5.2mm actual) Birch Ply from Home Depot
  • Bit: 2 flute 1/8" Carbide
  • Feed: 1000mm/m
  • Speed: 30,000 RPM
  • Cut Depth: 2mm
  • Stepover: 2mm

From: Re: Mudsharks' #0054 Upgrade using a Proxxon rotary tool:

  • Material: 1/8" birch plywood
  • Bit: 1/16" 2 flute endmill
  • Feed: 150mm (Probably could go 200)
  • Speed: 15,000 RPM
  • Cut Depth: 0.8mm
  • Stepover: n/a (through cut)

Makita Compact Router.

  • Material: 3/4" Baltic Birch
  • Feed: 38in (965mm)/min.
  • Speed: 30,000 RPM
  • Cut Depth: .06in (1.524mm)



Plywood forms can be tough to cut. One tactic is to use a down-cut spiral bit for the first half of the cut, then switch to an upspiral --- this may be of use w/ other forms of plywood.

Available in 3 forms:

  • carbonized --- sort of reddish brown color. Soft, about as hard as typical plywood
  • natural --- blonde to yellowish blonde in color. About 15--20% harder than maple.
  • strand-woven --- as hard as Ipe

Following is from an article on Easel:

  • Speed: 762mm/min (30 inches per minute)
  • Depth per pass: 0.7112mm (0.028")[71]

Red Oak

  • DW660[72][73]
  • Speed: 1,000 mm/min
  • Depth per pass:1.5 mm


  • Speed: 32
  • Depth Increment: 0.04"



Abrasive and dusty. Potentially hazardous.



May contain quartz which will dull bits.


Slate - (Metamorphic Stone) A fine -grained rock formed from clay, sedimentary rock shale and sometimes quartz. Hardness scale: 3

Engraving slate for an art project


Copper circuit board cut on the forums here. Further discussion here.

Inventables blog post; http://blog.inventables.com/2014/02/circuit-board-milling-on-shapeoko-2.html

Especially clean Double Sided PCB cut "using a 0.3mm end mill with lots of WD40 on the board.... (F)eedrate is 4ipm and depth is 0.005 inches."

  • Bit: 10 degree tungsten bit
  • Feed: 20 IPM
  • Speed: 30,000 RPM (Dewalt DW660)
  • Cut Depth: 0.005 inch
  • Bit Width: 0.0025 inch (used for calculating) 0.016 inches (actual)[74]


  • Bit: 30 deg bit
  • Feed: 100 mm/min
  • Cut Depth: 0.3mm inch[75]

Stock SO2 Milling a PCB

  • Bit: 0.0157 kyocera end mill from drillman1 on ebay.
  • Feed: 10 ipm XY
  • Speed: 4 ipm Z
  • Cut Depth: 0.003" depth[76]

Tips for Milling PCBs

  1. Take a piece of thick (12+mm) MDF, roughly 150x150mm to use as a platen. Fix the platen to your wasteboard in a permanent manner (just screw it into the wasteboard if you must. Be sure to countersink the holes a few mm (3-5))
  2. Now, do one of two things:
    1. If you always use the same size copper clad blanks - make a shallow pocket in the platen that is slightly larger than your blanks. This pocket only needs to be 1-2mm deep
    2. if you use scrap copper (or various sizes). Run a facing operation across the entire platen. This will bring your work surface exactly square with the machine.
  3. Download/Install/Use the autoleveler software: http://www.autoleveller.co.uk/ - Although your platen is going to be square with your machine, the thickness of the actual copper varies across any given piece by as much as .1-.2mm. The autoleveler software will help compensate for this.[77]

Height/Depth Probing

See Grbl: Height/Depth Probing


Carbon fiber

Carbon fiber can be cut, but requires dust collection (the dust is hazardous) and is tough on bits, requiring more frequent replacement.[78] Carbon Fiber Plates and Aluminum Bearing Blocks

Carbon Fibre 3.5mm

Carbon Fibre 3.5mm


  • Feed = 300mm / minute
  • Plunge = 150mm / minute
  • Spindle = Stock shapeoko demel knock off at max
  • Stepdown = 1mm
  • Bit size = 1.5875 (0.0625 inches)[79]

Corrugated cardboard

One concern w/ cutting paper and card and fiberboard is that it will dull bits.

I cut this as a test first cut before moving onto heavier materials. I used a conical shape cutter that came with my rotary tool. It's coated with some sort of rough particles. The edges of the cuts are rather messy, which would be tricky to clean up (e.g. with sandpaper), especially in areas where little "islands" have been cut (inside the "a" and "e") as there's not much left below to hold them in place.


Discussion in the forums: What Spindle and Bit for Garolite (G10).

.125" thick G10

  • 0625" fishtail diamond-cut bits
  • Feed and speed settings: 20 ipm feed
  • 8 ipm plunge
  • DeWalt DW660 on 90%-100% throttle
  • Pass depth was .045" for a total of 3 passes with .010" of over-cut into particleboard[80]


(I have in mind to make rubber stamps, e.g. for a mini production run of home-made Christmas cards...)




Forum user Cwalster noted in post Re: Foam cutting?, "EPS and EPP ... the trick is to use HSS, flat end mills and to conventionally cut it. If you don't you get a fuzzy surface."

Forum user PsyKo noted the following settings in Re: Foam tool organizer:

33kg/m^3 Foam

Craft Foam

1/32" four flute end mill[81]

Recommended Bits



Cutting Corian

Machines similarly to hardwoods, a climb cut finishing pass may eliminate marks from chatter. For a high gloss, sand using micromesh and polish with Novus #2.

(Theoretical values)

  • Bit: 1/8" end mill
  • Feed: 750 mm/min
  • Speed: 15,000 r.p.m.
  • Cut Depth: 1 mm

v60 .5 dia bit at 55 in/min and cut in .18 in deep at 19k router speed

Mother of Pearl

Dust is like glass shards. Adhere to scrap wood using CA glue (dissolve the glue after cutting using acetone). Spread the piece w/ petroleum jelly to minimize dust.


(derived from the ShapeOko coaster file from Run Your Second Job and the MakerCAM Tutorial)

  • Bit: 1/8" end mill
  • Feed: 20--30 in/min
  • Plunge Rate: 8--10 in/min
  • Speed: unknown
  • Cut Depth: 0.1 in


Suggestion is to do it before the plaster fully cures so that it doesn't dull the bits so much.

Good dust collection is imperative.

Discussion here: http://www.sawmillcreek.org/showthread.php?213915-CNC-router-for-Plaster-Moulds&p=2227973#post2227973 and here: http://www.camheads.org/showthread.php?t=3377 and discussion about various materials here: http://www.cnczone.com/forums/haas-mills/63483-anybody-ever-milled-hard-plaster.html