Materials

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.

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

Too many variables for a simple chart.



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 and 3s would be especially welcome)
 * Milling cutter
 * actual feed / speed and the unit of measure (mm/sec in/min etc)
 * whether or not you had dust collection active
 * any active cooling
 * material, including source

Excellent discussion of feeds, speeds and guidelines and more: http://community.carbide3d.com/t/need-some-help-w-this-gcode/746/8

http://www.hainesengineering.com/rhaines/cnc/cnc_info_speed.htm

http://community.carbide3d.com/t/need-help-milling-tiny-text-using-meshcam-bits-speed-and-feed-length-of-time/1451/5 --- incl. guidelines for brass.

Toolpaths: https://www.cnccookbook.com/3d-cnc-milling-machining-cam-toolpaths/

Choosing materials: "What Happens If You Machine the Wrong Metal Alloy or Temper?" https://www.youtube.com/watch?v=rm-qSytjFnI

Feeds and Speeds

Opensource

 * http://brturn.github.io/feeds-and-speeds/
 * HSM beta: http://brturn.github.io/feeds-and-speeds/beta.html
 * http://brturn.github.io/feeds-and-speeds/instructions.html

Online

 * https://map.harveyperformance.com/
 * http://ugracnc.com/cnc-spindles/milling-speed-and-feed-calculators
 * http://www.mitsubishicarbide.net/contents/mmus/enus/html/product/technical_information/information/formula2.html
 * http://micro100.hsmadvisor.com/
 * https://www.cnccookbook.com/cnc-feed-rate-calculator/
 * http://www.iscar.com/ita/Calculators.aspx?units=M
 * http://www.armtoolingsystems.com/metric_milling_formulas.php and http://www.armtoolingsystems.com/english_milling_formulas.php
 * http://www.carbidedepot.com/formulas-milling.htm
 * https://www.deanza.edu/manufacturing/speeds_feeds.html
 * American Machinist: Speeds/Feeds Conversions Calculator --- converts to/from SFM to RPM, IPM to IPT, IPT to IPR
 * cncprogramming.martinchick.com
 * custompartnet: Milling Speed and Feed Calculator --- wants Feed Per Tooth and SFM --- seems to be from: http://www.custompartnet.com/quick-tool/ which lists a number of other specific calculators
 * http://www.custompartnet.com/calculator/milling-horsepower
 * http://www.custompartnet.com/calculator/step-over-distance
 * Dapra's Speed and Feed calculators --- seems to be specific to their endmills
 * http://www.daycounter.com/Calculators/GCode/Feed-Rate-Calculator.phtml
 * http://www.destinytool.com/speeds--feeds.html
 * easycalculation.com: Milling Speed and Feed Rate Calculation --- notable for having the code available for embedding in other sites --- wants speed, diameter, chip load, number of flutes and will calculate speed and feed rate (backwards?) c.f., http://www.custompartnet.com/quick-tool/ above
 * http://janproducts.com/Speeds_and_Feeds_calc.html
 * http://jjjtrain.com/vms/calcualtors/_01.html --- graphical representation w/ dials unfortunately limited by slider-only input which makes specific number entry difficult
 * https://www.kennametal.com/en/resources/engineering-calculators/miscellaneous/speed-and-feed.html.html
 * http://littlemachineshop.com/mobile/speeds_feeds.php
 * http://www.monstertool.com/monster_tool_calculators.html --- (SFPM, Chip load) very simple on-line form which allows one to enter known values, then select unknown values to be calculated
 * http://www.productivity.com/resources/calculators/ --- calculates SFM, IPM, RPM, Chipload, Feed per Revolution, Material Removal Rate, Radial Chip Thinning
 * https://www.whitneytool.com/SpeedAndFeedCalculator.aspx
 * http://www.hispeedcorp.com/resources/speed-feed-calculators/hsm-machining

Spreadsheet

 * CNC Chip Thinning Calculator
 * Chip Load Calculator Excel spreadsheet --- also displays formulas and sample calculations
 * The Feeds and Speeds of CNC cutting tools --- includes download link for another Excel spreadsheet
 * Google Spreadsheet: Router Feedrate Calculator (Imperial)
 * http://www.practicalmachinist.com/vb/cnc-machining/free-end-mill-feed-speed-calculator-v10-222002/

Desktop or Mobile App

 * FSWizard (suggestion for using this w/ the SO3 is to limit cutter force output to 2--3 lbs. and to have at least 0.001" chip load per tooth.) --- free on-line version discontinued, only desktop and app versions now available w/ 30 day demo period

https://www.sandvik.coromant.com/en-gb/knowledge/machining-calculators-apps/pages/machining-calculator-apps.aspx

Android: https://play.google.com/store/apps/details?id=com.beta.fswizard_lite&hl=en_US

Apple Store

 * https://itunes.apple.com/us/app/cnc-machinist-calculator-pro/id1037668281
 * https://itunes.apple.com/us/app/machinists-calculator/id687225532
 * https://itunes.apple.com/us/app/machinist-calculator-sfm/id373899555

Calculators

 * TI-36
 * TI-85 --- noted as having many conversions
 * slide: http://www.niagaracutter.com/speed-feed-slide

Endmill selection tool

 * Onsrud Router Bit Search for plastics

Endmill-specific

 * http://www.endmill.com/pages/training/spdfeed.html

Login required

 * http://www.sgstool.com/content.aspx?contentId=tool-wizard --- requires registration

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

A notable calculator is G-Wizard listed at: Commercial_Software. See: https://community.carbide3d.com/t/does-sfm-matter/13487/12 for a description of use.

There are also physical calculators: Calculated Industries 4088 Machinist Calc Pro 2 Advanced Machining Math with Materials

In addition, one needs to decide upon a cutting depth advancement, 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. See also References, Feeds and Speeds below.

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

The S1 and S2 both give good finish passes at around 1 pound cutting force per FSWizard. Roughing passes, maybe up to 10 pounds depending on how aggressive you want to be. Edward (Ford, the machine's designer) has posted an aluminum milling video with the S3 with good finish and parameters that FSWizard spits out about 4 pounds for. 

http://community.carbide3d.com/t/meshcam-s-f-vs-doc-s-f-vs-gwiz/3848/2

404

 * Speeds and Feeds and Considerations when cutting metal

Conversion Utility
CNC Speed Converter

Math and Physics Calculations
http://www.toolingpro.com/milling-calculator.php --- in addition to the typical calculations, includes horsepower calculations.

http://www.sandvik.coromant.com/en-gb/knowledge/materials/workpiece_materials/the_specific_cutting_force

http://www.daycounter.com/Calculators/Lead-Screw-Force-Torque-Calculator.phtml

Measuring Cutting Force
https://www.youtube.com/watch?v=0cxNjo59PWA

Charts
Cutting Force (lbf) and MRR (cubic inches/min.) vs Power (Watts), Endmill Diameter (in) - Collet Type, and Workpiece Unit Power (Watts/cubic inches/min.)

https://www.amanatool.com/pub/media/productattachments/Insert-V-Groove-Speed-Chart-v8.pdf

Overview
The feed rate (speed at which the machine head moves in XYZ space) and the speed rate (number of revolutions per minute the cutting tool revolves around its axis) need to be proportional to each other, so as to have the machine cut out suitably sized chips. If a calculator suggests one be greater or lesser than allowed by your machine, reduce or increases the other proportionally (w/in the limits of your machine’s frame and linear motion setup) so as to bring the other into range.

Typical starting values:


 * RPM higher speeds improve edge quality finish
 * Cut Depth/Step Down: The traditional guideline is 1/2 the diameter of the end mill. 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) Reasoning for shallow vs. deep passes
 * Stepover: 1/3--1/10 the diameter of the end mill --- discussion of step over for ball end mills and finishing: https://www.reddit.com/r/CNC/comments/4bx2fp/how_to_go_about_high_finish_quality_3d_milling/
 * 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% (a useful guideline is one-fourth the feed)
 * If ramping in at ~45 degrees then 75% to 100% depending on material and endmill

The G-Wizard suggestion for plunge rate is to divide feed rate by # of flutes.

Cutting Formula
In contrast to the usual cutting formula, this simpler one has been suggested:

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. 

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.

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.

The whole thing needs to be really stiff to cut steel. If the deflection at the tip of the cutter (cutter plus whatever it is attached to) is more than the thickness of the chip, (feed per tooth) then it is guaranteed to chatter, and not cut well. This is why milling machines are HEAVY.

http://www.routerforums.com/cnc-routing/32970-feeds-speeds-needed-red-oak.html

Metric: http://www.endmill.com/pages/training/spdfeed.html

Horsepower Unit Factor
If known, this may be used to calculate the spindle horsepower needed for a cut:

Material removal rate (in³/min) × Unit power (hp/in³/min) = Spindle horsepower (hp)

see: http://www.custompartnet.com/calculator/milling-horsepower

Material Properties

 * 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.
 * https://www.makeitfrom.com/ --- curated database of engineering material properties that emphasizes ease of comparison

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.

Galleries

 * Early tests with different materials --- aluminum, bakelite, particleboard, rubber

Feeds and Speeds

 * https://en.wikipedia.org/wiki/Speeds_and_feeds
 * http://www.mmsonline.com/articles/start-with-the-right-speeds-and-feeds --- includes table of horsepower needed to cut various materials
 * http://www.onsrud.com/xdoc/FeedSpeeds
 * https://www.toolstoday.com/images/CNC-Feed-Rate.pdf
 * http://www.cncroutershop.com/us_en/calculate-feeds
 * http://www.pdsspindles.com/engineering-speeds
 * http://www.precisebits.com/tutorials/calibrating_feeds_n_speeds.htm --- technique for determining optimal feed based on spindle r.p.m. and test cuts
 * http://makezine.com/2014/03/21/cnc-routing-basics-toolpaths-and-feeds-n-speeds/
 * Bits__Speeds__Feeds_01-38344.pdf
 * http://www.woodworkingcanada.com/r5/showkiosk.asp?listing_id=5161481
 * CNC Cookbook
 * http://carbide3d.com/blog/2016/feed-and-speeds-part-1/ --- guest post by Bob Warfield of CNC Cookbook on the Carbide 3D blog.
 * http://carbide3d.com/blog/2016/feed-and-speeds-part-2/
 * http://www.cnccookbook.com/CCCNCMillFeedsSpeeds.htm
 * http://www.cnccookbook.com/CCCNCMillFeedsSpeedsSurfaceFinish.htm
 * https://www.cnccookbook.com/trochoidal-milling-feeds-speeds/
 * https://www.nyccnc.com/speeds-feeds/

https://www.sandvik.coromant.com/en-gb/knowledge/milling/milling-holes-cavities-pockets/pages/slicing-trochoidal-milling.aspx

Cumulative
Feeds and Speeds

Official Feeds and Speeds
Interactive Tableau: https://public.tableau.com/profile/willadams#!/vizhome/Carbide3DCNCFeedsandSpeeds/Sheet1?publish=yes

Shapeoko 3

 * http://docs.carbide3d.com/support/supportfiles/S3_feeds_250.jpg --- Metric version: http://community.carbide3d.com/uploads/default/original/2X/0/0e65e6d346b92b71ce0b7211e3f734823b256d9a.jpg Online Excel version

Please note that the values for a Shapeoko are copied into the page below at the appropriate points.

Note: RPMs have been regularized against the Router Speed Chart (see below) using the Dewalt dial setting as the standard. Please verify on your machine with a test cut.


 * M/M == Meters / Minute
 * SFM == Surface Feet / Minute
 * CPT == Chip load Per Tooth
 * MRR == Material Removal Rate

Calculations done using http://www.productivity.com/resources/calculators/

Shapeoko 3 (Carbide Create)
Carbide Create has two notable sets of feeds and speeds for the Shapeoko --- build 433 uses a chipload-based calculation, while 440 and later use a set of pre-calculated feeds and speeds which are intended to be quite conservative, so as to minimize problems.

Shapeoko 3 (Carbide Create 433)
In Carbide Create build 433, feeds and speeds could be automatically calculated based on chipload. This was discontinued in later builds (see the section below). For posterity, the calculated feeds and speeds were copied out to Materials Carbide 3D Carbide Create.

Shapeoko 3 (Carbide Create 440 and later)
In Build 440, Carbide Create began using a series of tables for tooling and feeds and speeds. Formatted as CSV files, they may be readily modified and shared.

Nomad 883

 * http://docs.carbide3d.com/support/supportfiles/Nomad883_feeds_125.jpg


 * M/M == Meters / Minute
 * SFM == Surface Feet / Minute
 * CPT == Chip load Per Tooth
 * MRR == Material Removal Rate

Calculations done using http://www.productivity.com/resources/calculators/

Problematic:


 * Plastic
 * Acrylic
 * 1/8″ #101 or #102
 * mm (″)
 * 1.429 mm (0.056″)
 * 9000
 * 881.38 mm (″)
 * 220.345 mm (″)
 * cu. cm ( cu. in.)
 * Carbide Create
 * cu. cm ( cu. in.)
 * Carbide Create
 * Carbide Create

Material Monday
Winston Moy has begin a series of YouTube videos on #MaterialMonday.

A central tenet of this series is an acknowledgement that the hobby CNC routers need different numbers for different sorts of paths. Thus far he has done:

Aluminum (Material Monday)
Shapeoko 3:

https://www.youtube.com/watch?v=RH4AXz_rtPo

Nomad 883 Pro:

https://www.youtube.com/watch?v=H0jQ997wcn4

(not part of the series: https://www.youtube.com/watch?v=szo5FFmJzv4 )

Brass (Material Monday)
Copper and brass sheets:

https://www.youtube.com/watch?v=VLOkXeQR_CU

Nomad 883 Pro:

https://www.youtube.com/watch?v=mhqjhD0XJl0

Copper (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=eekR8zs3WD8

Cast Acrylic (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=SV-L59RwCIo

Delrin (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=6vWtCtglXf8

HDPE (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=SiLWI62N5pc

Expanded PVC (Material Monday)
Shapeoko 3:

https://www.youtube.com/watch?v=hbbV0K37UVQ

Machinable Wax (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=iO9pw_tLYBs

MDF (Material Monday)
Shapeoko:

https://www.youtube.com/watch?v=Hq8lmk4Zrgk

Renshape (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=GQOlxf5P8NY

Tool Steel (Material Monday)
Nomad 883 Pro:

https://www.youtube.com/watch?v=Ta_KiG_5etU

Stainless Steel (Material Monday)
Shapeoko 3:

https://www.youtube.com/watch?v=QYkDKkfUuFs

Wood (Material Monday)
Shapeoko:

https://www.youtube.com/watch?v=cjoNGACBkks

Roughing Passes
Forum discussion: http://www.shapeoko.com/forum/viewtopic.php?f=7&t=5952&p=45452

Boring Holes
Discussion and experimentation: http://www.shapeoko.com/forum/viewtopic.php?f=7&t=6834&p=53873

I made a test piece with 30, 6mm holes, using 2d pocket, bore and circular tool paths. All three strategies was tested with and without finish passes. With climb and conventional. And any combination. And I also tested boring conventional with 0.3mm stock to leave and then a contour/profile path at full depth to finish off the hole. I haven't gone through the numbers thoroughly yet. But so far a few things I've noticed.

It seems Gadgetman was on to something with single-cut operations vs choosing a roughing and finishing two part strategy. All my best holes (size, roundness and finish) were made by single operations that did the full diameter at once!

Secondly using conventional milling produced the best results. Some with climb milling was ok as well, but the general result was that anything concerning climb milling (be it complete single cut operations or used as finis passes) gave a little worse result.

I had little luck with the any variation of the circular path, and it also does a very annoying z up movement with every completed Z level.

The best two were simply 2D pockets (normal pockets) and bore cut as a single conventional milling operation. Those two produced the best looking holes and finish and was closest to spec. Of the two I think I prefer bore, since it's quicker to set up and quicker to cut.

The ones I did as a rough bore with a finishing contour pass came out pretty bad, too small and with lots of chatter.

Coolant
Ideally, all the heat of a cut will be carried away by the chip — this is not always possible, so for some cuts in certain materials, coolant will be used.

It may be applied in various ways, either through drip or mist systems (see Upgrade Overview) or one may fashion a dam or well in which to pour it.

Discussion:

http://community.carbide3d.com/t/is-this-coolant-ok-for-cutting-titanium/1312

Paraffin: http://community.carbide3d.com/t/coolant-lubricant-for-cutting-aluminium/1313/5

Cutting Oil
http://www.precisebits.com/products/chemicals/cutting_oil.asp

Testing Cuts/Materials
To actually test feeds and speeds for a material, esp. note the technique mentioned above:


 * http://www.precisebits.com/tutorials/calibrating_feeds_n_speeds.htm --- technique for determining optimal feed based on spindle r.p.m. and test cuts

Or this technique:

...Use a simple 3 x 3 matrix method to judge DOC and speed. Make 9 small square (pocket)s in a piece of the wood, and vary the speed and feed across the 9 (also) varying the DOC and feed. When a DOC and feed looks good, check to make sure the chips are little C shapes instead of dust or burnt dust. 

It is always a good idea to test and prove out a G-code path, esp. the first time one uses it. One can of course do an “air cut”, one anxious user piled up flour and had the endmill drag through that, or one can use a less expensive material (poplar rather than walnut, aluminum rather than brass).

The industry-standard for this is machinable wax, a combination of wax and a compatible plastic, usually polyethylene (used in plastic bags and many food containers).

See below for feeds and speeds which are specific to this material, and other details, but it should be possible to use the G-code intended for the final material.

Foam (testing material)
Home Depot: Foamular by Dow Corning --- .125" end mill at about 7500rpm, 75-85 IPM, 37 plunge, 90% stepover, 100% step down

Chipload
A given endmill, in a specific material will have a chipload suggested by the manufacturer. Unfortunately, these don't directly apply to the less-rigid machines typically used by hobbyists.

For aluminum: The most important thing is to make sure chipload is at least 0.001 (0.0008 for 1/16) minimum. If cutting under 50% diameter you need to use a chip thinning calculator to see actual chip size.

https://engineering.stackexchange.com/questions/2413/high-spindle-speed-low-tool-pressure

1/8" endmills
Suggested generic chiploads:


 * Plastic: 0.75mm (0.03")
 * Hardwood: 0.25mm (0.01")
 * Softwood: 0.5mm (0.02")
 * Aluminum: 0.05mm (0.002")

Lakewood Carbide recommendations:

(these should be conservative and are based on smallest from the larger recommendation and largest from the smaller from their chart)


 * Plastic: 0.0010 -- 0.0020 inches
 * Aluminum: 0.0009 -- 0.0016 inches
 * Brass: 0.0008 -- 0.0015 inches

1/4" endmills
Lakewood Carbide recommendations:

(these should be conservative and are based on smallest from the larger recommendation and largest from the smaller from their chart)


 * Plastic: 0.0020 -- 0.0030 inches
 * Aluminum: 0.0015 -- 0.0020 inches
 * Brass: 0.0015 -- 0.0018 inches

V endmills
https://community.carbide3d.com/t/v-bit-feeds-and-speeds-poll/17077

Router Speed Chart
Note that these speeds are all approximate, and should be verified on your system w/ a test cut.

Official chart for Carbide Compact Router:

1: 10,000

(1.5: 12,000)

2: 14,000

(2.5: 16,000)

3: 18,000

(3.5: 20,500)

4: 23,000

(4.5: 25,000)

5: 27,000

(5.5: 29,500)

6: 32,000

RPMs are from users who have measured the speeds on their units, or extrapolated linearly.

Metals
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. Note that downcut bits are intended for woodworking and may present a combustion hazard in some metals, and will certainly be quickly dulled from re-cutting chips if used w/ metals.

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, tram 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.
 * 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.
 * Alternately 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.

The typical (ideal?) technique would be to find the Surface Feet Per Minute (SFM) (available in references such as: http://niagaracutter.com/techinfo/millhandbook/speedfeed/sfm.gif ) for the metal in question, then calculate:

RPM = (SFM*3.82) / Cutter diameter in inches

Discussion on Reddit: https://www.reddit.com/r/CNC/comments/3fnqt3/what_makes_a_given_cnc_machine_better_for/ctqbdbj

Considerations for jewelry: https://www.reddit.com/r/CNC/comments/406scf/total_newb_here_i_would_like_to_create_an/cys764k

Identification
Metals may be colour-coded --- one company's system: http://www.westlakemetals.com/opencms/export/westlakemetals/downl/METAL_COLOR_CODESa.pdf

Aluminium
Suggested chipload 0.001": https://community.carbide3d.com/t/my-first-aluminum-part/19223

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 is alloyed with different elements (specified in parentheses below) to achieve differing mechanical properties.

McMaster-Carr: About Aluminum

Alloys which are readily anodized include 5083 and 6061.

Aim for 0.001 to 0.0007" chip load 0.00075 in/tooth (12.5 in/min) or better yet, to 0.001 (18 in/min) @9000 RPM suggests.

A further consideration is whether or no the material has been heat treated.


 * 1000 essentially pure aluminum (99% minimum by weight), can be work hardened
 * 1050 not good for machining --- report of success w/ single flute endmill: http://community.carbide3d.com/t/1050-aluminium-how-to-cut/9473/3
 * 1100 --- machinability poor
 * 2000 (copper)
 * 2011 --- machinability excellent
 * 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. It's ok to work with, I'd say it's in the middle. It's 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 If welded, loses its temper and strength.
 * Brinell Temper 0 Hardness 47
 * Brinell Temper T3 (solution heat treated then cold rolled) Hardness 120
 * Brinell Temper T4 Hardness 120
 * 3000 (manganese) can be work hardened
 * 3003 --- machinability poor
 * Brinell Temper 0, Hardness 28
 * Brinell Temper H18, Hardness 55.
 * 4000 (silicon)
 * 5000 (magnesium)
 * 5052 available in sheet. machinability only fair (poor) Cuts usually look gummy on scrap/drops, easily welded.
 * Brinell Temper 0, Hardness 47
 * Brinell Temper H34 Hardness 68
 * Brinell Temper H38, Hardness 77
 * 5086 --- machinability poor
 * 5251 not good for machining
 * 5456 --- machinability poor
 * 6000 (magnesium and silicon) easily machined
 * 6020 --- machinability excellent
 * 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. 6082 is very similar and more common in Europe. Thickness for plates is typically Imperial measure.
 * Brinell Temper 0, Hardness 30
 * Brinell Temper T6, Hardness 95
 * 6063
 * Brinell Temper T0, Hardness 25
 * Brinell Temper T6, Hardness 73
 * T651 --- contains internal stresses which will deform a machined piece if annealing is attempted.
 * 6082 medium strength alloy with excellent corrosion resistance, machines well in T6 and T651 temper Thickness for plates is typically metric measure.
 * 6101 --- machinability poor
 * 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
 * Brinell Temper 0, Hardness 60
 * Brinell Temper T6, Hardness 150
 * 8000 (other elements)

Brinell Temper:

(Note that these denote a tempering process rather than a specific Rockwell hardness)


 * 0 = Fully annealed (soft)
 * H## = Strain hardened (medium)
 * T# = Solution treated (hard)

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

2 lb./hr. material removal rate on an SO3.

Discussion of difficulties w/ guidelines: http://community.carbide3d.com/t/s3-6061-aluminum-cut-fail/894/3

Technique for deriving feed and speed and depth of cut by observing a cut: http://community.carbide3d.com/t/carbide-3d-end-mills-chipload/1748/5

MeshCAM settings: http://www.shapeoko.com/forum/viewtopic.php?f=30&t=7804&p=61754#p61754

Discussion of adjusting feed/speed, using coolant, air to clear chips, and tendency of chips to heat, elongate, and weld: http://community.carbide3d.com/t/so3-first-cuts-in-aluminum/6170/6

Tutorial Videos
Winston Moy has begun a #MaterialMonday series:

Shapeoko 3 #MaterialMonday: Aluminum




Nomad 883 Pro #MaterialMonday: Aluminum
Winston Moy has begun a #MaterialMonday series:



Other: Aluminum
https://www.youtube.com/watch?v=PWMIHLF6D6Y

https://www.reddit.com/r/hobbycnc/comments/7kywdb/settings_i_use_for_machining_aluminum_with/

Finishing Passes
...using a climb cut for finishing passes produces a nice finish in aluminium (6082)

Faster and shallower
Some hold that aluminum should be cut extremely shallow and extremely fast, having even made the statement: "Whatever you're doing, go even shallower and even faster".

Drilling holes
http://community.carbide3d.com/t/holes-how-do-you-drill-in-aluminium/4245/5

Endmill considerations
One interesting observation is that ball end end mills work better.

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
 * special coatings to prevent material from adhering to the bit
 * ZrN (Zirconia Nitride) --- described as “for aluminum only”
 * TiB2 (Titanium Diboride)

Additionally, a radius endmill has been noted as reducing vibration.

Length matters, w/ shorter bits reducing chatter.

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.

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.

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).

Horsepower Unit Factor (Aluminum)
0.25

Aluminum starting point
1/4" carbide, Adaptive Clearing, 33k RPM, 60 IPM, 0.1" stepover, 0.063" doc also did 1/8" carbide, 33k rpm, 30 ipm, 0.05" stepover, 0.02" doc

Shapeoko 3
Using the upper pair of mounting holes on the spindle carriage plate may reduce chatter. 2F end mill at 12ipm with 5 speed (DWP611).




 * Material: 1/8" Thick, 6061 Aluminum
 * Feedrate: 60ipm (1524mm) --- conservative 80ipm was achieved
 * Depth pass: 0.0625" (1/16") (1.5875mm)
 * 45% overlap
 * Plunge Rate: 20ipm (508mm)
 * Bit: 3 Flute, 1/4" Square end Mill, HSS
 * CAD: Autodesk Inventor 2014 Professional
 * CAM: MeshCAM v6 Pro
 * Router: Dewalt DW611 (Speed set to 4)

.25" depth of cut, .025" stepover, and 60IPM feed. This makes nice long dagger shaped chips, and seems to cause the least chatter of all while still keeping a .5in^3/min material removal rate.

1/8" 3 flue 45 deg helix upcut mill made for aluminum. Tin coating is good. You should be making little flakes/chips not powder. I run about 550mm/sec .5mm DOC and stepover. 20kRPM on DW611

http://www.shapeoko.com/forum/viewtopic.php?f=35&t=6631&p=53672

I cut a "grill" into the "protection plate" that covers the electronics of the shapeoko 3 to mount an 80mm fan, i did it no problem without lubricant. My settings: 2 flute 8mm carbide bit 1000mmpm Stepown 1 mm Overlap 3 mm Dewalt set on 5

6061 (1' x 1/2"), 1/4 x 4flt coated ball. Spindle 16k, feed: Slot: 2"/min, Front angle: 11"/min, Top: 22"/min

http://community.carbide3d.com/t/created-my-aluminum-fixture-with-s3-and-nomad-pro/945/5

rough on shapeoko3: 25 ipm, 0.3mm doc, 150mm plunge waterline finish on nomad: 8ipm, 0.3mm doc, 150mm plunge parallel finish: 4ipm, 50mm plunge




 * 0.25" dia. cutter
 * 300mm/min (11"/min)
 * 0.5-0.75mm (0.02"/0.03") depth of cut

1/2" 6061 aluminium --- 3 flute1/4" End Mill at 600mm\min, 200mm\min plunge, around 14,000rpm, 0.2mm DOC... awesome finish, and good looking chips.

0.1mm depth per pass at 560 mm/min 4 flute high speed steel endmill

AlTiN coated 5/64 2 flute flat end mill. Feed was 12ipm doc was .012 spindle speed set on 1 plunge feed was 6.5ipm. No lubricant. 

T6 6061
http://community.carbide3d.com/t/s3-6061-aluminum-cut-fail/894/28


 * Mill Bit 2FL SE REG SQ - TiALN
 * Plunge rate 3 in/min
 * Depth per pass at 0.020 (conservative)
 * Feed rate a little to 36 in/min
 * Speed set to 5.5 on the Dewalt, guess, could be 26,000 rpm

http://community.carbide3d.com/t/aluminum-feeds-and-speeds-in-carbide-create/1853/5

combination of a 3mm 2flute 45 Helix cutter at 16000-17000 Rpm with a .17mm DoP with a feed of 400mm/min

1/8" thick 6061-T6 alu. Plate Feed 215mm Depth 0.2mm Plunge 27mm Bits 1/8" 2 flute carbide and V-bit

http://community.carbide3d.com/t/pics-attached-help-creating-a-cpu-water-block-mount-adapter-for-g4-cube-i-have-a-nomad-pro/2321/6

Shapeoko 3: 16,000 RPM (DeWault on the SO3), 0.015" DOC, 0.04" stepover, and 30 IPM with an 1/8" 2 flute coated end mill.

Detailed notes on a cut in 0.0625" thick plate: http://community.carbide3d.com/t/aluminum-cut-was-good-now-bad-any-advice/8012/7

0.015 DOC at 15 IPM, then start increasing it by 0.005 and another 5 IPM, until it starts to make too much chatter/noise. Every machine/set up is a little different…find YOUR sweet spot.... 10k to 15k rpm

Carbide 3D Shapeoko 3 (6061 AL)
The feeds and speeds below were published by Carbide 3D in a pixel image chart published to the Support | Tooling section of docs.carbide3d.com:


 * DOC: 0.76
 * RPM: 17500 (Dial setting: Dewalt: 1.5, Makita: 2.9)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 762 mm/min
 * Plunge: 254 mm/min

Nomad 883 (6061 AL)
.25mm depth per pass, and 200mm feed rate. plunge rate is .25mm.

Nomad 883 (#122)
http://community.carbide3d.com/t/why-am-i-breaking-my-bits/2875/8


 * Depth per Pass: 0.102mm
 * Stepover: 0.356mm
 * Spindle speed: 9200 RPM
 * Feedrate: 190.068mm
 * Plungerate: 25.4mm

or


 * Depth per Pass: 0.003"
 * Spindle speed: 10000 RPM
 * Feedrate: 6" feed
 * Plungerate: 2" plunge

ShapeOko 1/2
Forum discussions here:


 * Aluminum
 * Feed: 160 mm/min
 * Plunge: .2 mm
 * Speed: 20,000 RPM (DW 660)
 * Shapeoko cutting metal — aluminum, includes specifics for bit, depth, stepover, feed and use of a cooling solution.
 * Bit: 2 flute 1/8" endmill.
 * Feed: 12ipm
 * Speed: generic dremel turned on high (30k RPM?)
 * Cut Depth: .0125"
 * Stepover: .0625" (50% of bit diameter)
 * Cooling/Lubricant: liberally applying WD40 as the job was being cut
 * Milling Aluminum - First Results
 * Re: Belt on outside (about milling parts for same)
 * Re: Shapeoko cutting metal (post with link to
 * Milling aluminum with the Shapeoko 2
 * Bit: single flute spiral upcut 1/8" endmill. Available from Inventables.
 * Feed: 500 mm/min
 * Plunge: 300 mm/min
 * Cut Depth: 0.1 mm
 * Speed: Maximum speed (bundled generic rotary tool)
 * Coolant: cutting fluid (mineral oil or water should work)
 * .071 6061 Aluminum sheet BMW Motorcycle Strobe mount
 * Tool: Flat carbide endmill .0625
 * using a small Dremel
 * step .003
 * Feed: 12inches /Min
 * Plunge :6 /Min
 * 1/8" thick aluminum and 3/8" thick aluminumRe: Made some aluminum parts for a 3d printer
 * Bit: 2 flute center cut end mill (from Inventables) --- Dewalt DW660 spindle --- max. speed 30,000 r.p.m.
 * Feed: 500mm/min feed
 * Plunge: 100mm/min plunge
 * Step Down: .2mm step down
 * accuracy was +/-.2mm over 3inches
 * 1/8" 6061-t6 aluminum
 * Niagara C330 1/8" 3 flute TiAlN coated end mill
 * .2mm DOC
 * 650mm/min feed
 * 100mm/min plunge
 * HSM (high speed machining) techniques to pocketing 6061 with a Shapeoko 2
 * Toolpath: Helix to depth, 0.5mm constant engagement adaptive clearing (trochoidal) toolpath
 * End mill: 4-flute variable helix TiAlN carbide
 * Speed: 17.5K RPM
 * Feed: 450mm/min (18ipm)

Engraving
30 degree 1/8" shank v-bit. 8ipm (203.2mm) feed, 3ipm (76.2mm) plunge rate with 0.008" (0.2032mm) plunge per pass.

6060
Nomad
 * Tool Diameter: 3mm
 * Shaft: 6mm
 * Coating: DLC (Diamond Like Coating)
 * Flutes: 3

F&S:


 * 10000 rpm
 * 250mm/min
 * stepover: 1,4 mm
 * DOC: 3 mm
 * Stickout: 30mm (incl. the 5mm shaft which does not hurt)

Cooling: Low tech air cooling (Fish tank pump), no fluid

http://community.carbide3d.com/t/the-mother-off-all-mills-for-aluminium-milling-nomad/6525

10,000 rpm I was able to take a 0.2mm DOC with a 10mm bit at something like 2000mm a min. To get a better cut I changed DOC to 0.1mm

6063
Termed architectural aluminum, it may be identified by the profile having square edges (usually other grades have slightly rounded edges similar to steel angle). Inexpensive and easily extruded.

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

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

7075
http://www.shapeoko.com/forum/viewtopic.php?f=35&t=6631&p=53775#p53773

1/8in endmills at 40IPM .05 step over, and .032 depth of cut in 7075 AL.

standard length ones at 20IPM, .05 stepover, and .032 depth

1/4" chamfer mill at 20IPM with .05" stepover.

Image of MeshCAM settings at: http://community.carbide3d.com/t/knife-handle-project-overview-and-files/422/3

7075-T6
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

5052

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

WD-40 lubricant.

500mm/min, .3mm per pass with a 1 flute 1/8 carbide endmill, at speed 3 on a DW611

Shapeoko 3


 * 1/4 #201-Z
 * Dewalt Spindle 17500 RPM (setting 1.5)
 * DOC: .010
 * Feedrate: 40ipm
 * Plungerate 3.5ipm


 * 1/8" #102-Z
 * Lubricant/coolant
 * Dewalt Spindle: 16000 RPM (setting 1)
 * DOC: .010
 * Feedrate: 20ipm
 * Plungerate: 3.5

5083
Tough, strong alloy with excellent corrosion resistance, however not easy to machine. Datasheet.

6062
1/8" carbide cutter at 150mm/min. 0.2mm depth of cut per pass using DW660.

6082
Experiments in aluminium (6082) cutting on an eShapeoko

3 flute, 45deg flute, carbide, 4mm diameter ... 21k RPM, dry, climb cutting ... Spiral downcut along a 1mm radius, .4mm per revolution (leading to a 6mm hole) ... feedrate of 500mm/min with a forward step of 0.5mm (12% tool engagement)

6082 (Shapeoko 3 with spindle)
From: http://community.carbide3d.com/t/first-time-with-aluminum/4910/26


 * 6mm end mills: 0.75mm DOC 800mm/min and 290 hertz on my 3 phase spindle 16390 RPM (1.5 setting on the Dewalt, between 2.75 (15722.5) and 3 (16870) on a Makita)
 * 3mm end mills: 0.4mm DOC 750mm/min (same RPM)

1050A
Least expensive alloy. Likely available as sheets.

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...

10mm 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.

unknown alloys
1/8" carbide, 33k rpm, 30 ipm (10IPM if you are taking full width passes), 0.05" stepover, 0.02" doc for adaptive clearing.

From Easel:


 * Speed: 25
 * Depth Increment: 0.005"

http://www.shapeoko.com/forum/viewtopic.php?f=5&t=6134&start=10#p51513

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.

New Makita Mounts

1/4" 2 flute carbide endmill, Makita up to 4.5, .002" depth per pass at 25--30ipm

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

Aluminum flashing
Cutting Stencils in Aluminum Flashing

Thin sheets
Superglue. I use a thick (>4mm) piece of aluminium larger than what I need to cut, clamp that to the wasteboard and then dab a few drops of standard cyanoacrylate superglue on the thin sheet and slap it to the larger, thicker piece. Then I break out my 1.2mm 1-flute endmill (http://www.ebay.com/itm/1-20mm-0472-sin ... 58a7df7885) and run it at a feed rate of400mm/min, plunge 100mm/min and a pass depth of 0.2mm. The spindle... runs at full tilt. When I'm done all I have to do is give the thin sheet a good whack sideways and it pops right off the larger sheet. 

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

T6 plate
Re: Vote for your favorite ShapeOko spindle solution!
 * Feed: 30ipm
 * bit: 1/8 carbide altin endmill
 * Cut Depth: .025"

Horsepower Unit Factor (Bronze)
0.50

Copper
Use very sharp cutters with copper. Many alloys (and the element itself) are "gummy" and difficult to machine.

3-4 IPM 0.015 cut depth at the low end of the DW611's speed range with lubricant --- Copper sign


 * Speed: 10
 * Depth Increment: 0.015"

Ascertain that if a copper alloy, it does not contain beryllium. (Note that such alloys are normally only used for non-sparking tools for certain industries.)

Nomad: "For brass and copper I use Plunge rate 170 m/m, Feedrate 400 m/m or more 10% / 20% and depth 0.07 mm. whit 0.063" cutter. And I use Alcohol for coolant to and the cuts are better ."

1/16" carbide flat with DOC 0.07mm. Feed 400 mm/min Plunge 170 mm/min RPM 19000 and coolant Trichloroethane whit good ventilation.

Horsepower Unit Factor (Copper)
0.50

MaterialMonday Nomad Copper
https://www.youtube.com/watch?v=eekR8zs3WD8

Cast Iron
6000 r.p.m. (theoretical)

Horsepower Unit Factor (Cast Iron)

 * Gray Cast Iron: 0.50
 * Ductile Cast Iron: 0.56
 * Malleable Cast Iron: 0.67
 * Chilled Cast Iron: 1.67

Titanium
Potential for ignition. Will not be extinguished by water (which will actually increase the flames).

http://community.carbide3d.com/t/nomad-made-custom-titanium-multi-tool/642

https://community.carbide3d.com/t/titanium-lets-get-wild/12909/20

http://www.americanmachinist.com/features/cool-tips-cutting-titanium

Horsepower Unit Factor (Titanium)
1.67

Grade 5

 * 2in/Min
 * Step down .002"
 * Dewalt speed 1
 * small 1mm flat endmill

Horsepower Unit Factor (Steel)

 * Steel 150 BHN: 1.00
 * Steel 300 BHN: 1.25
 * Steel 500 BHN: 2.50
 * 300 Series Stainless Steels: 1.00
 * PH Series Stainless Steels: 1.33

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. The intention was to make a 0.005" pass.

1018 cold rolled steel

 * Endmill: 1/4" carbide
 * Spindle speed: 12000 RPM
 * Feed: 70 in/min.
 * Plunge: 18/min.

Hot rolled steel
30 ipm, 10 plunge, .015 depth of cut, .2 step over.

Stainless Steel
Forum post discussing this: Cutting stainless steel?

http://community.carbide3d.com/t/making-a-stainless-steel-watch-case-and-back-on-the-shapeoko-3/5468/13

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. Unfortunately, this has a potentially high cost in tooling, w/ endmills only lasting for cutting of a single (small) part in this instance.

303
Created for its machining characteristics.

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.).

304

 * 1/4" thick 304 stainless steel about 2.5" x 3" each
 * 3/16 carbide bit
 * .015 doc for roughing, then .01 doc for penetrating the circles, then .007 doc for the profile cut.

Engraving

 * 1/8" ball end mill
 * depth ~.005".
 * 5 ipm
 * step down .0025"

HSS (unhardened)
https://www.reddit.com/r/shapeoko/comments/5pusjt/s03_carbide_can_cut_steel_possibilities_are/dcxx9xz/

Unhardened HSS. 5mm diameter tool blank.

For facing the shaft, I used 10ipm with a 0.01" depth of cut to fix the horrid hacksaw edge.

For slotting/notching: Feed rate of 15ipm, 0.005" cut depth.

Using a 1/4" 4 flute carbide from Kodiak (AlTiN coated).

Carbide 3D Shapeoko 3 (Steel)
Use coolant.


 * DOC: 0.51
 * RPM: 17500 (Dial setting: Dewalt: 1.5, Makita: 2.9)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 305 mm/min
 * Plunge: 127 mm/min

Carbide 3D Nomad 883 Pro (Steel)

 * DOC: 0.002"
 * Feed: 2.5"
 * Plunge: .5

Brass
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”.

List of alloys and their characteristics: http://www.emachineshop.com/machine-shop/Brass/page322.html 353, 360 and 385 noted as suitable for machining on a CNC router.

My MeshCAM Notes for machining brass

Discussion of machining brass tags: http://www.shapeoko.com/forum/viewtopic.php?f=7&t=6477&p=50695 Finished results in Engravering Brass (CZ120) http://www.shapeoko.com/forum/viewtopic.php?f=30&t=8371

HSS tooling preferred.

Recommended machining parameters for copper and copper alloys --- reference .pdf from copper.org

DW660. 0.063" straight 3-flute bit Feed 5in (127mm)/min drop 5in (127mm)/min drop distance 0.015" (0.381mm)

Horsepower Unit Factor (Brass)
0.40

260
Available from http://www.ksmetals.com/18.html Alloy 260 1/2 hard ASTM B36 Likely difficult to machine.

353 engravers brass
DW660

Two flute:


 * bit: 2 flute 1/8"
 * feed rates: 4in (101.6mm)/min
 * plunge rate: 0.015" (0.381mm) drop down
 * step over: 60%

Three flute:


 * bit: 3 flute 1/16"
 * feed rates: 10in (254mm)/min
 * plunge rate: 0.02" (0.508mm)drop down
 * step over60%

3 flute straight bit 0.063" diameter 0.01" (0.254mm) stepdown 5" (127mm)/min feed rates

360

 * 1.5mm 2 flute carbide end mill
 * stepdown: 0.15 mm
 * RPM: 24000
 * Feed: 330 mm/min.
 * Plunge: 165mm/min.

http://community.carbide3d.com/t/my-first-foray-into-brass-a-keyhole-escutcheon-for-a-blanket-chest/6405/9


 * DOC 0.1 mm.
 * Feed 400 mm./min.
 * Plunge 100
 * RPM 16000
 * #112 tool
 * Coolant: Ethanol (Datron)

Carbide 3D Shapeoko 3 (360 Brass)

 * DOC: 0.51 mm
 * RPM: 18000 (Dial setting: Dewalt: 2, Makita: 3)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 635 mm/min
 * Plunge: 279 mm/min

Small tools (Nomad)
http://community.carbide3d.com/t/1-64-endmill-in-brass/5896/9

smallest diameter square end mill I use is 1/32 My settings for that are: .250mm DPP, .200 step, 300mm feed, 100mm plunge, and .040 OAD.

The 10k rpm limit makes running smaller end mills unacceptable.

For smaller details, I use a 20 degree tapered end mill, with a .004 tip. MeshCam thrives when I'm running these small details. Tool settings: .127mm DPP, .020mm Step, 200mm feed, 100mm plunge, .050 OAD.

http://community.carbide3d.com/t/carbide-3d-tool-112-1-16-endmill-speeds-feeds/6024/4

.062 endmill at the following settings: depth per pass: .400mm stepover: .750mm feed rate: 400mm plunge rate:100mm RPM: 10,000

Nickel Silver
Leaded nickel silver (C792) machines the same as 360 brass. Other alloys (C752) are more difficult.

Lead
Note that lead will bio-accumulate, and dust must be handled with that in consideration. Any cutting or fabrication involving fumes or the potential for fumes must use suitable exhaust hoods and filtration.

Carbide 3D Shapeoko 3 (Lead)

 * DOC:   1.65
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1270 mm/min
 * Plunge: 508 mm/min

Magnesium
Potential fire hazard and once ignited burns at over 5,000 degrees F.

Horsepower Unit Factor (Magnesium)
0.25

Carbide 3D Shapeoko 3 (Magnesium)
Fire Hazard


 * DOC:   1.02 mm
 * RPM: 17500 (Dial setting: Dewalt: 1.5, Makita: 2.9)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1016 mm/min
 * Plunge: 381 mm/min

Mokume gane
A multiple layering of various metals, it is reported to cut similarly to sterling silver.

Nomad 883: 9000 RPM, a feed rate of 12.300". Carbide's #112 with a depth per pass of 0.008".

Silver
https://community.carbide3d.com/t/micro-end-mills-0-2mm-0-5mm-feed-speed/12814/16 --- screengrab of settings

https://community.carbide3d.com/t/cutting-pure-silver-for-jewelry/15551/4

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


 * http://www.sgstool.com/PDF-speedfeeds/SGS-Speeds-Feeds-GP.pdf
 * Machinist-Materials, Plastics Comparison Table
 * Guidelines for Machining Engineering Plastics
 * https://www.curbellplastics.com/Research-Solutions/Plastic-Properties
 * http://www.pepctplastics.com/resources/plastic-part-design-guide/basics-of-plastic-selection-for-machining/
 * Sawmillcreek Forum: Plastic Comparisons of Delrin, Acrylic, and Lexan
 * http://www.pepctplastics.com/resources/plastic-part-design-guide/Machinability-of-plastics/ --- graph charting relative ease or difficulty of machining various plastics
 * http://www.dotmar.com.au/machinability.html --- list rating plastics from 1--20 in terms of machinability
 * http://www.boedeker.com/fabtip.htm --- fabrication guidelines
 * https://www.reddit.com/r/CNC/comments/47xjg6/cheapest_machinable_plastic_to_make_fixtures/

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.

If instead of cutting the plastic adheres to the endmill, stop and rework the feeds and speeds.

When engraving plastics, coating the surface w/ WD-40 may allow easier removal of waste material which sticks at the cut edges: Re: Engraving plastics

https://www.reddit.com/r/CNC/comments/44xkqo/cutting_plastic_material_and_rates_to_use/

https://www.reddit.com/r/CNC/comments/765948/cheapest_machinable_plastic/

Amount to leave for a finish cut

 * 1/8" Cutting Edge Diameter (CED): 0.015" -- 0.030"
 * 1/4" 0.030" -- 0.080"
 * 3/8"--1/2" 0.060 -- 0.125"

never less than 0.015"

ABS
Heats and melts easily above 125 degrees F. Slow speeds, medium tooth cut. Easily worked by hand.

Will fume if heated, wear respiratory protection.

Go a bit slower and a bit lighter in ABS than HDPE.

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

Cutting ABS with Onsrud tool


 * RPM: 1200 (300W DC Spindle)
 * Tool: Onsrud 63-701 1/16" Solid Carbide One Flute Upcut O Flute
 * Step down: 0.015625 -- 1/32"
 * Feed: 10--15 IPM
 * Plunge: 5--10 IPM

3mm ABS sheet milling and routing:


 * Machine: eShapeOKO, dual Y motors (1.5NM torque steppers)
 * RPM: 6000 (Kress 1050 FME spindle)
 * Tool: 2mm Carbide 2 flute end mill
 * Feed: 2000 mm/(? sec)
 * Plunge: 300 mm/(? sec)

1/16"
 * 16000 RPM (Makita at 2.75, 1 on DeWalt)
 * 800mm/min
 * 1.2mm max depth.

Carbide 3D Shapeoko 3 (ABS)

 * DOC: 1.78 mm
 * RPM: 17000 (Dial setting: Dewalt: 1.5, Makita: 2.8)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 559 mm/min

Delrin
Delrin is the DuPont brand name for Acetal (Polyoxymethylene (POM)). Moderately expensive plastic which machines extremely well. Suited for use in bearings and wear applications (it was originally developed as a replacement to the plectrums in harpsichords). Can be machined to tight tolerances, and will wear for long periods without lubrication. Suggestion is twice the DOC and feedrate as 6061 aluminum. Other machinists note it works much like soft brass.

less strong than nylon, moderate stiffness

https://www.reddit.com/r/CNC/comments/49obi1/working_with_delrin_and_teflon_tips_on_good/


 * 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?

SO3: 15krpm at 40ips feed rate with an 1/8" carbide flat end mill

Nomad settings: http://community.carbide3d.com/t/notes-on-the-journey-nomad-pro/1303/3

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.

Carbide 3D Shapeoko 3 (Delrin)

 * DOC: 2.03 mm
 * RPM: 20500 (Dial setting: Dewalt: 3.5, Makita: 3.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 813 mm/min

Further information

 * Dupont Delrin (acetal resin) Design information
 * http://www.practicalmachinist.com/vb/cnc-machining/machining-delrin-173503-post1048423/#post1048423

UHMW

 * 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

Tips for cutting: http://community.carbide3d.com/t/help-machining-hdpe-i-think/5965/5

Carbide 3D Shapeoko 3 (UHMW)

 * DOC: 2.54
 * RPM: 17700 (Dial setting: Dewalt: 1.5, Makita: 2.9)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1905 mm/min
 * Plunge: 559 mm/min

HDPE
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. Much larger and thicker panels are available from specialty plastics shops, sign shops and possibly local hardware stores.

Lighter than Delrin and will not hold the same machining tolerances.

Note that boards which are molded (as opposed to cut) may be swollen or otherwise out of dimension along the edges, or somewhat shrunken towards the center, depending on how they are cooled coming from the mold.

Will distort under pressure when clamping: http://community.carbide3d.com/t/flipping-job-strategy/3719/4

Adhesive: http://solutions.3m.com/wps/portal/3M/en_US/Adhesives/Tapes/Products/~/3M-Scotch-Weld-Structural-Plastic-Adhesive-8005?N=6081374+3293241357&rt=rud

Temperature/memory: https://www.reddit.com/r/CNC/comments/7jlqr7/does_hdpe_have_a_memory/

Excellent post showing a variety of endmills cutting out gears: https://community.carbide3d.com/t/hdpe-milling-gears/19358

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%

Tests done with an eShapeOKO with dual Y motors (1.5NM torque) and a Kress 1050 spindle:


 * Bit: 4mm 2 Flute carbide end mill
 * Feed: 2000mm/minute
 * Plunge: 300mm/minute
 * Speed: 9000 (Kress set to '2')
 * Cut Depth: 3mm

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

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

.25" end mill 4 flute (I run 2 flute at 150 ipm (up to 180 ipm can be done but chatters along Y-axis) - .130" doc - .1 stepover - 160ipm - 16k rpm [https://www.facebook.com/groups/unofficialshapeoko/permalink/321308161610483/?comment_id=321320864942546&comment_tracking=%7B%22tn%22%3A%22R3%22%7D)

.125 end mill 4 flute - .04 doc - 150ipm - 16k rpm

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.

single flute 0.063, 0.125 and 0.25 carbide bits ~15,000 RPM 0.05" Step 20-30 IPM


 * Bit: 1 flute 1/8" upcut
 * Feed: 1300mm/min.
 * Plunge rate: 250mm/min.
 * Cut Depth: 3mm
 * Spindle: Kress 1050

1/8 single flute carbide end mill. 30 imp, 10 plunge, .1 depth of cut, .4 step over. dewalt set to 2.5 (very conservative) Video.


 * 1/8 O-Flute endmill
 * 0.1” dpp
 * 90 ipm feed
 * 40 ipm plunge
 * Router at “2” on the Carbide Create router ~12k

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

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

Nomad
http://community.carbide3d.com/t/cutting-hdpe-faster/5182/7

Carbide 3D Shapeoko 3 (HDPE)
The below feed and speed rating was published by Carbide 3D on the pixel image chart published to Support | Tooling on the docs.carbide3d.com pages:


 * DOC: 3.18 mm
 * RPM: 21500 (Dial setting: Dewalt: 4, Makita: 4)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 2032 mm/min
 * Plunge: 1016 mm/min

Black HDPE cutting board works at 1.75 on a Makita w/ a 1/8" endmill.

Usage notes (Carbide 3D HDPE)
"... around 1 or 2 on the DWP611 speed and I feed about 750mm/min with a two-flute carbide end mill. I find I can do about a 4mm maximum depth cut before I start having rigidity issues, but for roughing a full plunge slot at this speed I get significant chatter in the Y direction, where my SO3 is least rigid." 

"The 34 mm/sec with a 1/4" flat cutter at 3.17 mm step was way too fast. Router speed makita at 3. Had a perfect cut at 12 mm/sec, 3.17 step and router at 4 makita with 1/4 " flat carbide3d cutter. 1/2" hdpe in 4 passes."

"6.35mm square endmill (#201 from Carbide3D) => 12000 RPM + 1250 mm/min"

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

recycled HDPE
SO3: http://www.shapeoko.com/forum/viewtopic.php?f=7&t=166&p=57325

Corrugated Plastic (Coroplast)
160 ipm. Dewalt on 1. I'm cutting 10mm in 3 passes with good results.

Starboard
Also note Starboard, a form of HDPE with additives to make it tougher and more UV resistant.

http://community.carbide3d.com/t/online-source-for-plastics-e-g-hdpe-delrin-acetyl-pvc-etc/1306/9

Nomad
King Starboard HDPE5

http://community.carbide3d.com/t/experience-milling-hdpe/462/2

food safe, >100 degree C melting point, easy to machine

King Starboard HDPE5. I don't know if that differs from what you have.

But if it helps, I was using the .125" endmills that came with the nomad (so, 2 flute). 7500 rpm spindle speed 68.3 in/min cutting feed rate (feed per tooth .0046") 17.075 in/min plunge feedrate .03" stepdown All climbmilling

f:1960; DOC:3; WOC:2,2; 22000 RPM; MRR 12.94 mc3/min; with a 2 flute carbide endmill

Polycarbonate (Lexan)

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


 * Bit: 1 flute 1/8" upcut
 * Feed: 800mm/min.
 * Plunge rate: 250mm/min.
 * Cut Depth: 0.5mm
 * Spindle: Kress 1050

0.188" Lexan 1/8" 2-flute end mill DOC 0.03" 19,000rpm (3 on the 611) feed rate of 20ipm

Machining Polycarbonate - Nailed it!

Machining holes: 2-flute 1/8" end mill, 40 IPM, DWP611 speed at 1, depth per pass 0.04", and following up with 2 finishing passes (one climb, one conventional)

Engraving: 30-degree engraving bit with 0.0118 tip (0.3mm) (Amazon) Max depth 0.020". Depth per pass 0.020". Feed at 80 IPM. DWP611 speed at 1.

Nomad with tiny endmills in polycarbonate
spindle speed constant at 10000rpm. For 0.1mm flat end mill, I plucked in the feed rate as 76.5mm/min and the plunge rate as 2mm/min and for 0.2mm flat end mill, I used the feed rate and plunge rate as 186mm/min and 7mm/min respectively. 

Carbide 3D Shapeoko 3 (Polycarbonate)

 * DOC: 2.03 mm
 * RPM: 18000 (Dial setting: Dewalt: 2, Makita: 3)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1397 mm/min
 * Plunge: 635 mm/min

Acrylic
Available in two different forms as noted below, cast and extruded.

Single flute cutter, routers likely need lowest possible speed setting.

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

[https://www.quora.com/What-are-the-best-ways-and-practices-to-clean-acrylic-or-plastic-parts-after-precision-CNC-milling Quora: What are the best ways and practices to clean acrylic or plastic parts after precision CNC milling? (and answers)]

inexpensive in some forms, moderately strong and stiff like acetyl, generally transparent, but low toughness and can be a bit annoying to machine

Note that what is sold as 0.25" thick acrylic is typically manufactured to metric 6mm (0.236"). Thickness tolerance for typical manufacture is 0.02", engineering plastics are available w/ tighter tolerances (0.005" from McMaster-Carr).

O-flute bits are recommended.

Trochoidal milling: 3mm endmill feed - 1750mm/min DOC - 10mm plunge - 650mm/min trocoidal stepover - 12.5% trochoidal width - 50% http://community.carbide3d.com/t/trochoidal-milling-is-amazing/6063/7

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. 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.

Finishing Notes
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 and/or dishwashing liquid as a coolant or applied to the bit as a lubricant

https://www.facebook.com/groups/unofficialshapeoko/permalink/392408684500430/

Cast Acrylic
Moderate tensile strength with good abrasion resistance, but low impact resistance (tends to split or crack under shearing forces). Handle carefully due to its brittle nature. Easily shaped with application of heat (150--250 degrees F).

Will melt under heat generated by friction from incorrect feed, speed or endmill selection. Endmill selection can be critical for successful cutting.

Commonly Available Colors: Clear, Opaque (White, Grey, Black, Red, Yellow, Blue, Green), Solid Tints (White, Grey, Bronze, Red, Blue, Green, Yellow, Amber), Fluorescent/UV Tints (Amber, Red, Green, and Blue)

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

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

single flute 0.063 and 0.125 carbide bits ~15,000 RPM 0.05" Step 20-25 IPM

Makita on dial 1, 1500mm/min with a 2-flute 1/16″ bit and a doc of 0.25mm

Extruded Acrylic
Often used as a glass replacement, excellent optical clarity, even when thick. Smooth surface.

Less impact resistance than polycarbonate.

Produces more fumes and is even more brittle than cast acrylic.

Similar machining characteristics to cast acrylic, with all difficulties exacerbated, will split or crack under shearing forces.

Can be shaped by heat like cast acrylic (but at slightly lower temperatures)

Usually seen as bars, rods, tubes, balls, and discs.

Commonly Available Colors: Clear

Extensive notes on cutting: https://www.facebook.com/groups/unofficialshapeoko/permalink/328563164218316/

1. If you have designed multiple parts in Carbide Create, but your goal is to cut them from varying thicknesses, I find I’m happiest using multiple files, each with a different stock thickness.

Seems like Carbide Create was gracious enough to zero my retract height when I changed stock thickness. Down one “O” flute 1/8” bit 😉

2. Go thick. I don’t mean buy a foot thick slab and try to mill it down to what you need. I needed to cut a lens that will likely be sanded on both sides to increase the opacity. So I got some extruded acrylic from the big blue box store that was double what I needed and have accounted for that change in my overall design

3. “O” flute up cut and somewhere between 1 and 3 for dial setting on the Makita. It was doing an amazing job until the retract height thing got me and snapped it clean off. There was a bit of build up, but it’d get to a thickness then fling off. After this broke, I switched to a straight cut but it didn’t do nearly as nice a job and really failed to eject the chips.

4. Slow rpm, fast(ish) feed rate. Again, I was impressed until the retract height got me.

5. Watch that tab thickness. I set my tabs to 4x2.5 mm and in the end wish I did 2x2. I know my setup is not perfectly level, but I’m ok with that for now.

I’d probably have had zero buildup, but the first cut was very aggressive (not sure what/how to adjust this in carbide Create). All subsequent passes were perfect.

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.

2 mm acrylic from Home Depot.
 * Cut with 1/8" 2-flute spiral end mill.
 * 2 mm cut depth
 * 400 mm/min feed
 * 75 mm/min plunge
 * 12000 rpm spindle (300w Quiet cut spindle)

Carbide 3D Shapeoko 3 (Acrylic)
The settings below were published by Carbide 3D in the pixel image chart published to Support | Tooling in docs.carbide3d.com:


 * DOC: 1.52 mm
 * RPM: 19000 (Dial setting: Dewalt: 2.5, Makita: 3.2)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 635 mm/min

Feeds and speed examples
1/8" cutter single flute, 1800 rpm, feed rate of 50"/minute (1200mm/min) and plunge rate 24"/minute (600mm/min) with depth of cut 1mm. Possible to increase the depth of cut if your endmill is suitable. 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.

Using a Dremel bit:
 * Spindle speed: 3500
 * Plunge rate: F10
 * Feed: F60
 * Depth:0.7 mm passes, with one clean-up pass
 * Alternating CW and CCW cutting passes

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

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

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

Plexiglass
Acrylic is also available under the name plexiglass.

(untested)
 * 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 with the following settings:


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

eShapeoko: 21kRPM, 800mm/min at 2.5mm deep

Re: Cutting plexiglas with standard Dremmel
 * Cutter: 3mm 2 flute carbide Kyocera cutter
 * Spindle speed: 13800RPM
 * Pass depth: 0.5mm
 * Feed rate: 1200 mm/min
 * Plunge rate: 300 mm/min

See also Cutting Cheap PlexiGlass Any Luck?

https://www.reddit.com/r/CNC/comments/5nj3xh/does_anyone_have_any_advice_on_milling_plexiglass/ --- mostly suggestions for flame-polishing edges.

Further Notes and References

 * http://www.plasticrouting.com/pdf/Routing_and_Trimming_Acrylics.pdf
 * 14,500 r.p.m. and 200 i.p.m. or 18,000 and 250 i.p.m.
 * 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
 * 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
 * http://www.engraverssolutions.com/PDFs/tips&tricks-routing_acrylic.pdf
 * http://www.cutlasercut.com/resources/tips-and-advice/everything-you-need-to-know-about-acrylic
 * https://www.reddit.com/r/CNC/comments/3p8z1d/best_endmillspeeds_and_feeds_for_acrylic/

Alternatives
Polycarbonate. It costs twice as much, but it's nicer in every way.

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

Description of difficulties: https://www.reddit.com/r/hobbycnc/comments/3ty0tq/issues_with_milling_extruded_polystyrene/

Carbide 3D Shapeoko 3 (Styrene)

 * DOC: 0.76 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1016 mm/min
 * Plunge: 381 mm/min

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

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.

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

Carbide 3D Shapeoko 3 (Kydex)

 * DOC: 2.03 mm
 * RPM: 18000 (Dial setting: Dewalt: 2, Makita: 3)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1397 mm/min
 * Plunge: 559 mm/min

PEEK
https://www.bearingworks.com/uploaded-assets/pdfs/retainers/peek-datasheet.pdf

Carbide 3D Shapeoko 3 (PEEK)

 * DOC: 0.76 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 762 mm/min

Carbide 3D Shapeoko 3 (Polypropylene)

 * DOC: 2.03 mm
 * RPM: 24200 (Dial setting: Dewalt: 5, Makita: 4.5)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 2286 mm/min
 * Plunge: 381 mm/min

PVC
Available as boards and trim pieces at home center. Mentioned for cutting in 25mm thickness.

Type 1 is solid, other forms foamed.

Identified by heating a copper wire red hot, melt a bit onto the wire, then place in the flame — a green tint indicates PVC.

Note that there are safety implications for heating / burning PVC, esp. w/ a laser, due to its chlorine content and exposure to its dust (may cause asthma or other respiratory problems). See http://toxtown.nlm.nih.gov/text_version/chemicals.php?id=84

inexpensive, less strength yet-maybe 60% of nylon- and stiffness can be as good as the others, but often less, and lower toughness

PVC Foam Board
100ipm @ 15000rpm with an amana o flute 1/8”. It’s long enough to cut 3/4. I usually do 1/2” doc

Carbide 3D Shapeoko 3 (PVC)

 * DOC: 2.29 mm
 * RPM: 15820 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 889 mm/min
 * Plunge: 432 mm/min

Carbide 3D Shapeoko 3 (Sintra)

 * DOC: 3.30 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 2540 mm/min
 * Plunge: 2032 mm/min

Nylon
good strength, toughness, and moderate stiffness

good to machine provided using a sharp tool with high positive rake

eShapeOKO with Kress 1050FME spindle.

Tested on a machine with limited Z axis power so the plunge rate is constrained by the machine.

Material:


 * Cast Nylon 6 (black)


 * Dry cut - No lubrication or cooling fluids.

Tools:


 * 4mm 2 flute solid carbide end mill
 * 1mm 2 flute end mill
 * 6.3mm radius HSS corner rounding router bit.

Machine settings:


 * Feed Rate: 800mm/min
 * Plunge Rate: 150mm/min
 * Kress 1050FME Spindle: '2' (approximately 9000rpm)
 * Cut Depth: 2mm
 * Step over: 40%

With these settings Nylon 6 cuts very well with no heat problems. Most of the swarf was small flakes and there was very little 'fluff' left on the work piece. With a plunge rate limited to 150mm/minute and at the lowest speed on the Kress spindle drilling is a disaster and melts the plastic. A faster plunge rate may help.

With strong enough stepper motors the following produced excellent results with Nylon:

Tools:


 * 4mm 2 flute carbide end mill for aluminium ( This one for example)

Machine settings:


 * Feed Rate: 1500mm/min
 * Plunge Rate: 500mm/min
 * Kress 1050FME Spindle: '2' (approximately 9000rpm)
 * Cut Depth: 2mm
 * Step over: 60%

Carbide 3D Shapeoko 3 (Nylon)

 * DOC: 2.03 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1905 mm/min
 * Plunge: 1016 mm/min

Rowmark Satin
Plastic locker plates


 * 1/16 2 ply
 * Bits: .010 2 flute end mill, 1/16 2 flute end mill

Composites

 * alupanel (HDPE layer caught between 2 0.3 aluminium sheets) http://www.shapeoko.com/forum/viewtopic.php?f=30&t=4394
 * vinyl-faced 3mm dibond sheets (self.CNC) http://www.reddit.com/r/CNC/comments/2znue4/bit_choice_for_cutting_vinylfaced_3mm_dibond/

Carbide 3D Shapeoko 3 (AL/PVC Panel)

 * DOC: 3.30 mm
 * RPM: 17500 (Dial setting: Dewalt: 1.25, Makita: 2.8)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1270 mm/min
 * Plunge: 635 mm/min

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

Note that there may be variation between the product of different manufacturers, always test speeds and feeds for a given supply.

http://community.carbide3d.com/t/machining-carbon-fiber-on-the-shapeoko/2261

https://www.cnccookbook.com/machining-carbon-fiber-composites-drilling-cnc-tools/

"better using diamond cut, also known as fish tail, end mills"


 * Bit: 1 flute 1/8" upcut
 * Feed: 800mm/min.
 * Plunge rate: 150mm/min.
 * Cut Depth: 0.5mm
 * Spindle: Kress 1050

Carbon Fibre 3.5mm
Carbon Fibre 3.5mm

http://dragonplate.com/ecart/categories.asp?cID=153


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

Carbide 3D Shapeoko 3 (Carbon fiber)
HAZARDOUS


 * DOC: 1.52 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1143 mm/min
 * Plunge: 508 mm/min

Garolite/G-10
Abrasive, hazardous dust (using coolant to control this is a frequent suggestion), care must be take to prevent delamination. Diamond or carbide tooling.

Discussion in the forums: What Spindle and Bit for Garolite (G10). https://www.reddit.com/r/Machinists/comments/3cx49f/machining_g10/

http://www.precisebits.com/Reference/drillfeedspeed.asp http://www.precisebits.com/Reference/diamondcutfeedspeed.asp

Suggestion: use steel speeds and aluminum feeds

>slowed down to 20 ipm feed vs. the 60 ipm that was default in Carbide Create

G10/ Garolite Notes

0.25" endmill: 50ipm feed with a 9ipm plunge, pass depth 0.06" (this cut through the complete 0.5" of material thickness)

0.125" endmill: 27ipm feed with 9ipm plunge, pass depth 0.08" (this only cut a 1/16" deep groove for an o-ring)

Router speed: Approx 4/6 on my Dewalt DW611


 * Bit: 1 flute 1/8" upcut
 * Feed: 800mm/min.
 * Plunge rate: 150mm/min.
 * Cut Depth: 2mm
 * Spindle: Kress 1050

.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

Carbide 3D Shapeoko 3 (Garolite)

 * DOC: 2.03 mm
 * RPM: 18500 (Dial setting: Dewalt: 2.5, Makita: 3.25)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1905 mm/min
 * Plunge: 762 mm/min

Carbide 3D Shapeoko 3 (G10)

 * DOC: 2.29
 * RPM: 18500 (Dial setting: Dewalt: 1.5, Makita: 2.9)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1524 mm/min
 * Plunge: 711 mm/min

Carbide 3D Shapeoko 3 (G10 XX)

 * DOC: 2.03 mm
 * RPM: 18000 (Dial setting: Dewalt: 2, Makita: 3)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1397 mm/min
 * Plunge: 635 mm/min

Hardboard/Masonite
https://forum.shapeoko.com/viewtopic.php?t=5983

https://forum.shapeoko.com/viewtopic.php?f=7&t=9097

https://forum.shapeoko.com/viewtopic.php?f=11&t=7236

https://forum.shapeoko.com/viewtopic.php?t=3332

Phenolic
https://www.amazon.com/Phenolic-Sheet-Standard-Tolerance-MIL-I-24768/dp/B00CPRFMK4 --- noted as "Hard, Machinable, Heat Resistant, Non Conductive" c.f., macor a machinable ceramic.

CE Grade


 * 3 flute coated carbide endmill
 * 40-50IPM (1016-1270mmPM)
 * .008" depth per pass (.203mm)
 * Dial setting #2 on Dewalt DW611

Carbide 3D Shapeoko 3 (Phenolic)

 * DOC: 2.03 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 889 mm/min

Carbide 3D Shapeoko 3 (Foamcore)

 * DOC: 2.54 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 889 mm/min

Renshape
Winston Moy has begun a #MaterialMonday series:



Carbide 3D Shapeoko 3 (Renshape)

 * DOC: 4.57 mm
 * RPM: 19000 (Dial setting: Dewalt: 2.5, Makita: 3.25)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1905 mm/min
 * Plunge: 889 mm/min

Nomad 883

 * DOC: .063" stepdown
 * RPM: 5000
 * Tool: .063" cutter for roughing
 * Feed: 40ipm
 * Plunge: 889 mm/min


 * .05" step-over

Increase up to 9000rpm to run as fast as 54ipm

Alternatives
http://www.cnczone.com/forums/general-off-topic-discussions/52041-cnc-post1433784.html#post1433784

Wood
For shallow pockets, a down cut spiral bit results in cleaner top edges.


 * Wood Handbook: Wood as an Engineering Material (Centennial Edition).
 * The Illustrated Guide to American Hardwood Lumber Grades
 * http://www.woodbin.com/calcs/wood-picker/
 * http://plesums.com/wood/choosingwood.html
 * Onsrud: Soft Wood Cutting Data: Chip Load Per Tooth Table
 * http://www.cnccookbook.com/CCCNCFeedsSpeedsWood.htm
 * https://www.reddit.com/r/woodworking/comments/5u82ag/handy_chart_of_species_for_hand_tool_work/
 * https://www.vortextool.com/images/chipLoadChart.pdf

Consider expansion: http://community.carbide3d.com/t/building-an-enclosure-with-concerns-of-heat/2967

Consider angle: https://community.carbide3d.com/t/surfacing-hint-on-wood/13096

https://www.reddit.com/r/hobbycnc/comments/7f5kux/wood_cuttingmillingis_12000_rpm_fast_enough/

Stabilized woods such as Dymondwood cut more like plastics. 3400rpm/.002 per flute with very small end mills.

https://old.reddit.com/r/CNC/comments/cngurf/any_experience_milling_hybrid_blanksepoxy_resin/

Wood Carbide 3D CC433
The following charts were transcribed from Carbide Create 433.

Wood-Hard Carbide 3D CC433
Material Wood-Hard --- settings transcribed from CC433.

Chipload per Tooth (Wood)
Onsrud recommends 0.003--0.005 for their carbide upcut endmills with normal flutes, O-flutes reduce this to 0.002--0.004

Carbide 3D CLPT (Wood)
From the official feeds and speeds charts

Carbide 3D 1/8″ endmill CLPT Nomad (Wood)
0.003055″ (bamboo) -- 0.0040760″ (mahogany) -- 0.008″ (pine)

Carbide 3D 1/4″ endmill CLPT Shapeoko (Wood)
0.00120″ (bamboo) -- 0.0012428″ (pine) -- 0.001143″ (mahogany)

Safety
http://www.wood-database.com/wood-articles/wood-allergies-and-toxicity/

Drilling
http://community.carbide3d.com/t/drilling-with-the-shapeoko/7405/13

V carving
60 degree: 40ipm 50ipm

Hardwood
https://www.reddit.com/r/CNC/comments/3f2plb/need_some_advice_on_machining_hardwood/ctktfj4

Hardwoods: 1mm endmill --- 0.5mm cutting depth with 500mm/min feed rate at 16000 rpm.

Inlay in hardwoods: http://www.shapeoko.com/forum/viewtopic.php?f=30&t=6666&p=52202

Pay attention to chips on the hardwoods. If you are making sawdust the speed/feeds are to high. You want to see discernible chips, even if they are small.

Dewalt router at 1-3 speed. .250 2 flute bits flat and ball nose, and .125 ball nose. Insert V bits from Amana. 30-50 ipm. plunge 10 ipm

I have a 2 flute, 1 inch LOC, 1/4 shaft by Bosch. I run it at 10,000rpm, 20-30 ipm feed rate, plunge about 8-11 ipm. Depth .050 or less, step over .056.

1/16 bit, 2 flute, .5 LOC, flat end mill, I run it at 10k, 20 feed rate, 6 plunge, depth .025,step over .028.



From Carbide Motion:


 * depth per pass: 0.704mm
 * step over 1.429mm
 * Feedrate: 424.180
 * plunge rate: 106.045
 * RPM: 6250

Basswood

 * 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.

Birch

 * Speed: 30
 * Depth Increment: 0.028"

Bloodwood
.5" 2 flute through bloodwood @ 0.2" stepover 0.2" stepdown 74 in/min.

Bubinga

 * 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 [http://www.shapeoko.com/forum/viewtopic.php?f=30&t=1470&p=11597#p11597 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.

chip-loads of 0.0004 - 0.005 in/tooth

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


 * Speed: 28
 * Depth Increment: 0.028"

Ipê

 * Bit: 2 flute 1/8" endmill.
 * Feed: 562.5mm
 * 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.

Carbide 3D Shapeoko 3 (Mahogany)

 * DOC: 2.54 mm
 * RPM: 19700 (Dial setting: Dewalt: 3, Makita: 3.5)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 813 mm/min

3D carving: https://community.carbide3d.com/t/0687-eagle-carved-in-mahogany/15464/6

Pine
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.

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

1/16” downcut at 1/16” doc and 60ipm at 18k rpm.

http://community.carbide3d.com/t/adaptive-clearing-on-pine/8813

3.175mm (Pine)
(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

Carbide Create:


 * Depth per Pass: 0.883mm
 * Stepover 1.429mm
 * Spindle Speed: 9375
 * Feed: 586.74mm
 * Plunge rate: 293.37mm

SO3: 3.2mm flat 2-flute 800mm/min feedrate and 500mm plunge Makita set at 3, ~16,870.

SO3: 1/8" downcut bit at 75IPM and Dewalt at 1 and .0625" DOC

SO3: extended reach 1/8" endmills --- slotting: .05" DOC at around 31 IPM (787.4mm)

6.35mm (Pine)
SO3: conservative feed and speed: 13,500 rpm, DOC 4mm, Feed 200 mm/min, 2 flutes 1/4 carbide bit.

SO3: 1/4" flat endmill at 1600mm/min, 2.5mm DOC, and 2.5mm stepover (pretty conservative)

Carbide 3D Shapeoko 3 (Pine)

 * DOC: 10.16 mm
 * RPM: 21000 (Dial setting: Dewalt: 3.5, Makita: 3.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1905 mm/min
 * Plunge: 1016 mm/min

Poplar
chip-loads of 0.0004 - 0.005 in/tooth

MDF
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, and is recommended.

Another concern is that the waste will expand somewhat when it is cut, filling a slot, which may become an issue if one needs to cut more than a pass or two. Rather than slotting, cut pockets which are at least half again the bit diameter.

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, 2 flute end mills with TiAN coating are suggested). Faster feed rates prevent the bit from staying in one place for too long, which is a factor in overheating.

http://www.pizazzsystems.com/Assets/Docs/Multimounts/Multimount%20MDF%20Panel%20Weights%20Schedule.pdf


 * Bit: 2 flute 1/8" straight
 * Feed: 1950mm/min.
 * Plunge rate: 375mm/min.
 * Cut Depth: 3mm
 * Spindle: Kress 1050

1/8" 2 straight flute, flat end: 0.024" cut depth, 64 IPM

1/8" 2 flute upcut, ball end: 0.062" cut depth, 36 IPM

1/8" upcut single flute DOC: 0.03" RPM: 11143 Feed Rate: 60ipm

Veneered MDF
https://www.reddit.com/r/CNC/comments/4ium3b/can_you_cnc_veneered_mdf/

Carbide 3D Shapeoko 3 (MDF)
The below are the settings for MDF from the pixel image chart which was initially put up by Carbide 3D on their docs.carbide3d.com Support | Tooling area:


 * DOC: 7.62 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 2032 mm/min
 * Plunge: 762 mm/min

Note that some users have specified 5080mm (200in.) successfully: https://www.facebook.com/groups/232744457133521/permalink/302749516799681/

Material Monday: https://www.youtube.com/watch?v=Hq8lmk4Zrgk

Wasteboard surfacing
Feed and Speed data: Makita router, 3/4" straight router bit (cheap Grizzly . com router bit) with 0.1 mm DOC at 30 mm/sec. Surfacing MDF waste board type cut.

Projects

 * 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

eShapeoko: 21kRPM, 1200mm/min 3.5mm deep or 21kRPM, 12mm deep feedrate of 500mm/min

Plywood
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...”

1.8mm depth of cut, and 1200 mm/min feedrate

Compression bit from Toolstoday Router Bits and Saw Blades: "1/8 compression at 40ipm at full depth cutting 1/4 plywood all day, dewalt speed 3. you can go faster, but it wont be as smooth a cut."

"1/8" Whiteside RD1600 downcut bit at 70 ipm 35 plunge and .0625 DOC, #1 on the Dewalt. I get excellent tool life, and very little finish work."

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)

130ipm


 * Bit: 2 flute 1/8" straight
 * Feed: 2600mm/min.
 * Plunge rate: 500mm/min.
 * Cut Depth: 3mm
 * Spindle: Kress 1050

Baltic Birch
1/16" 2 flute up-cut in BB last weekend, 55ipm .05doc

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

1mm endmill --- 0.6mm cutting depth with 600mm/min feed rate at 16000 rpm.

https://www.reddit.com/r/CNC/comments/8s1s4g/looking_for_optimal_speed_when_cutting_baltic/

Lauan
Relatively cheap, fibers are long in it, so splintering is an issue. Use climb cutting for roughing, (chops the fibers without tearing out as much as conventional) cutting".

Oak
Surfacing w/ an SO3: ¼" flat mill, 85 IPM, Dewalt611 at speed 4, stepover 0.2". Single pass, 0.080" depth

Carbide 3D Shapeoko 3 (Plywood)

 * DOC: 6.35 mm
 * RPM: 19700 (Dial setting: Dewalt: 3, Makita: 3)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 2540 mm/min
 * Plunge: 1270 mm/min

Bamboo
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

Typical dimensions:


 * flooring --- 14mm less ~0.45mm grooves

Following is from an article on Easel:
 * Speed: 762mm/min (30 inches per minute)
 * Depth per pass: 0.7112mm (0.028")

"better edge with a climb cut as the finish pass"

Carbide 3D (Bamboo)
First numbers are from Carbide 3D chart for a Nomad, second numbers are from Carbide Create for a Shapeoko


 * DOC: 1.016mm (0.04") (Carbide Create: 0.7 mm)
 * RPM: 9000 (Carbide Create: 6250)
 * Tool: 1/8" #102 square
 * Feed: 1397 mm/min. (55") (Carbide Create: 424 mm/min)
 * Plunge: 584.2 mm/min. (23") (Carbide Create: 106 mm/min)

Carbide Create settings cut well with a Shapeoko 3 XL using a long reach endmill w/ a Makita set to 3.25

Carbide 3D Shapeoko 3 (Bamboo)

 * DOC: 5.59 mm
 * RPM: 19000 (Dial setting: Dewalt: 2.5, Makita: 3.25)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1651 mm/min
 * Plunge: 762 mm/min

Red Oak

 * DW660
 * Speed: 1,000 mm/min
 * Depth per pass:1.5 mm

Pocketing 800mm/min. 1/4" step down w/ 1/4" 4 flute carbide up cutting.


 * Shapeoko 3: .1875 two flute,50 ipm %45 step over .1875 depth, full depth passes, border was .1" passes at 30ipm

Walnut
Shapeoko 3 - Walnut Carbide Logo


 * Stock Material - Walnut (11-1/2" x 5-1/2" x 7/8")
 * Cutting Bit - 3 Flute, 1/4" Square Endmill
 * Total Cutting Depth - 1/4" (0.25")
 * Depth Per Pass - 1/8" (0.125")
 * Feed Rate - 60 inches Per Minute
 * Plunge Rate - 30 inches Per Minute

Fine details in delicate parts: https://community.carbide3d.com/t/stabilized-walnut-inlay-for-a-watch-case/13901

Downcut endmill: ramp pass 2mm max doc, 10,000 rpm and 1500mm a min. I left a 0.5mm of stock then did a finishing pass at 500mm a min

Multiple Passes in Walnut
from: https://www.facebook.com/groups/unofficialshapeoko/permalink/386992208375411/?comment_id=387217465019552&comment_tracking=%7B%22tn%22%3A%22R%22%7D

This is the protocol I use for walnut stool seats, about 18 x 16 ovals (I have to orient them 45 degrees to get an 18 wide oval). The wood is 12/4 walnut sawn from the log and then air dried for 4+ years. The CAM is from Fusion 360.


 * First pass - to clean the surface, get a flat reference face, to check final adjustments on position, etc - 1/2" 2 flute Bosch bit, 50 ipm, stepover 0.350", stepdown 0.100"


 * Second pass - This is the one where I remove the bulk of the wood - Pocket cutting strategy - 1/2" 2 flute Bosch bit, 35 ipm, max stepover 0.180", max stepdown 0.080"


 * Third pass - Since I am going so deep (taking almost a full 2.5" in the center) I have to reset the bit - same strategy, bit and feeds and speeds


 * Fourth pass - So now I have a terraced surface - it's time to make it pretty - spiral facing strategy - 0.75" ball end, 35 ipm, stepover, 0.080", max stepdown 0.075"


 * Fifth pass - This pass is optional - I am just removing the cusp left between the spiral passes - parallel strategy, two directions - 0.75" ball mill, 60 ipm, stepover 0.080", max stepdown 0.010"

Yeah, the fifth pass is basically to exchange machine time for hand sanding time.

Janka Hardness
Janka Hardness is the standard technique for measuring the hardness of wood. See Guesstimating Feed Rates for a technique for using these numbers to derive a first approximation for cutting a softer or harder wood which one has numbers for.

http://woodgears.ca/hardness_test/

https://www.precisebits.com/reference/relative_hardness_table.htm

Stone
Safety considerations:


 * http://www.sculpture.net/community/showthread.php?t=3287
 * http://www.who.int/occupational_health/publications/en/oehairbornedust3.pdf

Only softer stones are suitable for cutting on a stock machine.

https://www.reddit.com/r/CNC/comments/alnjt0/question_best_bits_for_cutting_stone/

Engraving: 130mm/min, 0.2 mm/pass, with a 1mm diamond bit.

Carbide 3D Shapeoko 3 (Limestone)

 * DOC: 2.54 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1016 mm/min
 * Plunge: 305 mm/min

Soapstone
Abrasive and dusty. Potentially hazardous.

http://www.soapstonecompany.com/soapstone-diy/

Marble
May contain quartz which will dull bits.

Slate
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

Granite
Very hard, requires diamond tooling and active cooling and a very rigid machine.

http://community.carbide3d.com/t/engraving-a-picture-in-granite/11197

PCB
Discussion of safety implications for dust: http://community.carbide3d.com/t/1-8-carbon-fiber/626/3

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

Great results milling PCBs from Eagle with the Nomad

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)

PCB


 * Bit: 30 deg bit
 * Feed: 100 mm/min
 * Cut Depth: 0.3mm inch

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

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:
 * 3) 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
 * 4) 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.
 * 5) 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.

Height/Depth Probing
See Grbl: Height/Depth Probing

Cork
(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

Carbide 3D Shapeoko 3 (Cork)

 * DOC: 7.62 mm
 * RPM: 24000 (Dial setting: Dewalt: 5, Makita: 4.5)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1524 mm/min
 * Plunge: 762 mm/min

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.

Glass
http://hackaday.com/2014/12/04/cutting-glass-with-cnc/

http://community.carbide3d.com/t/machining-glass/4584

https://www.reddit.com/r/CNC/comments/cijwu8/milling_a_1x1_cm_glass_square/

Graphite
Used in making glass molds. Dust is conductive and potentially hazardous. Some work setups will put dust collection underneath the workpiece and add bristles projecting up to collect and contain it.


 * Roughing pass: 60 inches/minute
 * Step down: 1/16"
 * 1/4" end mill


 * Finishing pass: 30 inches/minute
 * 1/8" ball nose

Carbide 3D Shapeoko 3 (Graphite)

 * DOC: 2.54 mm
 * RPM: 19800 (Dial setting: Dewalt: 3, Makita: 3.5)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 508 mm/min
 * Plunge: 381 mm/min

Linoleum
https://plus.google.com/u/0/+DanaSpisak/posts/hzHNShVwWnD

https://www.youtube.com/watch?v=7R7PsCu5TZM

Carbide 3D Shapeoko 3 (Linoleum)

 * DOC: 0.76 mm
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1905 mm/min
 * Plunge: 889 mm/min

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


 * 1.5 mm endmill
 * 500 mm/min feedrate
 * 1 mm depth increment

One option for parts which can be cut quickly is to freeze the rubber (with dry ice or even colder temperatures) before cutting.

https://m.youtube.com/watch?v=-xhfiS_Q1aw&feature=youtu.be

https://www.youtube.com/watch?v=0Yvcizt83DA

Settings used for wax work, but adjust depth of cut to be less.

Available as gag erasers: https://www.amazon.com/Toysmith-4801-Really-Big-Eraser/dp/B00KSGSOB8

Foam
https://youtu.be/_FRc8q-3b5M

https://www.reddit.com/r/CNC/comments/44xlrt/best_foam_for_cnc_milling/

http://www.surfscience.com/topics/surfboard-anatomy/materials/know-your-foam/

May be helpful to wipe the machine down w/ an anti-cling dryer sheet before cutting to help reduce static sticking chips everywhere.

High density polyurethane foams are often used in sign-making, as well as for props. Density ranges from 10--30 pounds per cubic foot. Creates a gritty dust which is hard to clean up. See Tooling Board below.

https://www.reddit.com/r/CNC/comments/7k4gh2/cutting_and_bonding_closed_cell_polyethylene_foam/

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

 * Bit: 6, 8 or 12mm wood end mill (such as these http://www.bois.com/media/192315/360x300-fraises.jpg)
 * Feed: 1200 mm/min (can probably go higher, but I'm in no rush)
 * Speed: ?
 * Cut Depth: 5 to 10 mm
 * Stepover: 50% of bit diameter

One brand name is Plastazote. Use dual-colour for tool drawers, top : 5mm (less than 1/4"), then for the color below, adjust to match drawer thickness (leave a reasonable amount of space above). mill fast speed with low rotation speed.


 * ~6000 rpm (Bosch Colt lowest speed)
 * feed rate 1400 mm/min (~55 in/min)
 * 1/2" straight bit (a router bit with 2 flutes)
 * step down of 3--4mm (0.11 in)

“leave about 5mm (1/4") minimum between 2 pockets so you have enough material to maintain some strength.”

Craft Foam
1/32" four flute end mill

Insulation Board
650 for the speed and 5mm depth per pass though. I had my dw611 set around 3 for the speed

Owens-Corning “Foamular” project boards: 125 iPM and 0.35 doc. 1/4" 2-flute straight bit

https://www.reddit.com/r/CNC/comments/791h9z/speeds_and_feeds_for_milling_pink_insulation_foam/

Recommended Bits
http://www.toolstoday.com/p-6221-solid-carbide-spiral-foam-cutting-up-cut-router-bits.aspx

Tooling Board
Polyurethane tooling board machines very well, and lacking grain, holds excellent surface detail. Density ranges from 20--50 pounds per cubic foot. Popular for pattern-making, product mockups and toolpath testing (hence the name).

RenShape 440 --- http://www.freemansupply.com/RenShape440Styling.htm --- formula for a DIY alternative: http://community.carbide3d.com/t/machining-materials-questions/482

Corian
Cutting Corian

https://community.carbide3d.com/t/milling-wilsonart-solid-surface/14041/13

"Corian is mostly Acrylic/Acrylate-based resins, with fillers depending on what the ‘look’ is the designer was going for"

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.


 * Bit: 1/8" end mill
 * Feed: 900 mm/min
 * Speed: 20,000 r.p.m.
 * Cut Depth: 0.5--1 mm

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

0.0625" DOC, 1/4" end mill, and 60 IPM on a heavily modified SO2 ~7lb of cutting force

Dust is fine and potentially dangerous, if cutting for extended periods of time, released / generated gases are a potential hazard.

http://www.shapeoko.com/forum/viewtopic.php?f=30&t=6215&p=48324

A horizontal roughing cut was done at 80IPM with a 0.25in, 0.060 corner radius end mill from lakeshore carbide (where I buy all my tools). The DNP611 was set to 3.5 on the speed controller. Stepover was 50% with a 0.055" step down, and stock remaining set to 0.02". Finishing was done at 120IPM with a 0.125in ball nose mill, 15% stepover. A leading edge curve following cleanup path was run with the same 1/8" ball mill and an 8% stepover.

Carbide 3D Shapeoko 3 (Resin)

 * DOC: 2.29 mm
 * RPM: 17500 (Dial setting: Dewalt: 1.25, Makita: 2.8)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 1524 mm/min
 * Plunge: 1270 mm/min

Leather
Best cut w/ a drag knife or laser.

Engraving leather

I have a small endmill 1/32” that I use. I lay down a layer of masking tape on the spoil board, then a layer of tape on the back side of the leather and use spray adhesive to stick the backs of the tape together. It does a pretty good job, but you will have to do some sanding and burnishing on the edges of the leather to smooth it out since the endmill leaves a rough edge on the leather



https://old.reddit.com/r/CNC/comments/b3z8hx/any_suggestions/

Bone
https://www.practicalmachinist.com/vb/general-archive/machining-deer-bone-73823-post17765/#post17765

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.

http://www.precisebits.com/materials/ivory_shell/natural_shell.htm

https://www.precisebits.com/products/carbidebits/shell.asp

Plaster
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. Static may be an issue.

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

https://www.reddit.com/r/CNC/comments/45sol1/anyone_ever_try_and_mill_plaster/

Polymer Clay
http://www.kronosrobotics.com/polymer

Machinable Wax
Often used for quickly testing toolpaths which will be run in expensive materials or which require inordinate amounts of machine time. It may also be used to make molds for casting, esp. by jewelers.

Best results when chips are well cleared (fewer flutes / deep gullets) --- small endmills will benefit from compressed air or a vacuum or coolant to clear chips and keep the stock cool.

It is easily made:


 * http://madmodder.net/index.php/topic,2729.0.html
 * http://www.instructables.com/id/Machinable-Wax/?ALLSTEPS
 * http://community.carbide3d.com/uploads/default/original/2X/2/2e3c9d6977a1fb9722b95424e054f90fc95d7fb9.pdf http://community.carbide3d.com/t/home-made-machinable-wax/1209

Various tools may be used to heat it:


 * http://www.walmart.com/ip/Presto-Kitchen-Kettle-Multi-Cooker-Steamer/14321003

CNCzone thread: http://www.cnczone.com/forums/hobby-discussion/26351-cnc-post210273.html#post210273

One notable potential supply for wax is companies doing investment casting.

http://www.machinablewax.com/technical.php

Roughing: Spindle speed 3,000 rpm at ~ 100 inches per minute Finishing: Spindle speed 8,000 to 10,000 rpm at ~ 40-100 inches per minute

Carbide 3D Shapeoko 3 (HD Wax)

 * DOC: 7.62
 * RPM: 17000 (Dial setting: Dewalt: 1, Makita: 2.75)
 * Tool: 1/4" #201 square or #202 ball
 * Feed: 2540 mm/min
 * Plunge: 1270 mm/min

Ceramic Tile
Engraving: 1/4" 30 degree carbide vbit, 10ipm of cutting speed and .020" deep cut

Other Materials to Consider
Polyurethane (notes on this on the Nomad Trello)