Speeds and Feeds addendum

Here are some empirical speeds and feed for the M3 using carbide 2 flute on 5052o 1/4" milling f 34 1x speed (0-6 so its on 1) 1/8" milling f 27 4.5x 1/16" milling f 12 full speed Using 0.0165" depth for milling (4.5x)

for drilling using the 118 self centered carbide drill dropping 0.4mm per pass for 3 settings First drill divots Etch contours and folds rough pass mill with tabs smoothing pass with 1/8" smoothing pass with 1/16

Carbide End Mills : Harvey Tool's Speeds and Feeds

see also:

Note I believe the SFM values are incorrect on the tables listed On this link... ignore them, I cross checked them against other sites and forums, but the calculator on it is great feed rate calculator

for plastics:

Notes: We use the DeWalt DWP611 Router which can range from 16,000 - 27,000 rpm So Dial=(RPM-16000)/(5500/3) (since dial is 0-6)

Carbide End Mills - Non-Ferrous

MATERIAL SFM 1/8" 3/16" 1/4" 3/8" 1/2" 5/8" 3/4" 1"
Aluminum 1 500-1000 .001 .002 .002 .003 .004 .005 .006 .007
Aluminum 2 800-1500 .001 .002 .002 .003 .004 .005 .006 .007
Copper 3 600-1000 .001 .001 .002 .0025 .003 .004 .004 .005
Copper 4 800-1500 .001 .001 .002 .0025 .003 .004 .004 .005
Copper 5 700-1000 .001 .001 .002 .0025 .003 .004 .004 .005
Copper 6 800-1000 .001 .001 .002 .0025 .003 .004 .004 .005
Magnesium 7 1000 min .001 .002 .002 .003 .004 .006 .008 .009
Plastics 8 200-500 .001 .002 .003 .004 .006 .008 .010 .015
Plastics 9 200-600 .001 .002 .003 .004 .006 .008 .010 .015
Carbon 10 500-1000 .004 .004 .006 .008 .010 .010 .015 .020

GRADE

  1. 440, 356, 380, C61300
  2. 2024-T4/T6, 2014, 6061-T6/T651, 7075-T6
  3. Navel Brass, High Silicon Bronze, A-17, C-17200
  4. Yellow Brass, High Lead Brass, Red Brass
  5. Alloys Nickel Silver, Beryllium Copper, Oxygen-Free Copper
  6. Alloys Alum/Bronze, Low Silicon Bronze
  7. Die-Cast, Extruded
  8. Polycarbonate
  9. Acrylics, Phenolics, Polysulfone
  10. Carbon, Graphites

When milling or drilling, or creating a tool path for a CNC machine the feed rate must be determined. Materials have rated surface speeds for a given type of cutter. The harder the material the slower the speed (for feed rate). Given the diameter of the tool and the surface speed, the RPMs of the spindle can be calculated. Then if the tooth load for the cutter is known, and the number of teeth, the feed rate can be determined.

Milling Formulas & Glossary

FORMULAS

  1. RPM = (3.82 x SFM) / D
  2. IPM = RPM x IPR
  3. IPM = RPM x IPT x T
  4. SFM = D * RPM / 3.82 (rearranged equation of RPM, useful to see where the SFM is when RPM is known)
  5. Chipload in inches = Feedrate in Inches Per Minute / (Cutting RPM x Number of Flutes) (reaaranged from 3)
  6. RPM = (3.82 x Surface Feet per Minute) / tool diameter (written from 1)
  7. Feed Rate = RPM x Number of Flutes x Desired Chip Load. (written from 3)
  8. RPM = (12 Surface_Speed) / (PI Cutter_Diameter) (More accurate definition of 1) Note 12 is the feet to inches
  9. RPM= 3.82*Surface_Speed/Cutter_Diameter (rewritten from 1)
  10. Fm = Ft x Num_Teeth x RPM, where Ft is feed/tooth, and Fm feed rate. (equation 3)
  11. N = 1000 x V / pi x D (see 8.. this is the metric version)
  12. IPT=IPM / (RPM * T) (rearranged from 3)

GLOSSARY 1

SFM - Surface Feet per Minute RPM - Revolutions per Minute (Speed) IPT - Inches Per Tooth (Chip Load) IPR - Inches Per Revolution IPM = Inches Per Minute (Feed) D - Cutter Diameter T - Number of Teeth

For Lexan (Polycarbonate) boedeker plastics recommends (see link above) for 1/4" tool 270-450 for 0.25 depth cut... and 300-500 for a shallow 0.05 cut. chip load 0.002 and 0.001 respectively Drilling 1/4 or less is 0.007-0.015 feed load in revolutions Face Milling is 0.15 depth 1300-1500... with chip load of 0.02 for a 0.05 depth its 1500-2000 with a chipload of 0.005

More on Lexan (this may work, but the math suggests it can be done better) Yeah, polycarbonate likes to melt. You can get pretty high feedrates with a high speed spindle by using multiple passes with small step downs. Blowing compressed air on the bit(very carefully keeping body parts away from the bit) can help too.

Edit in: I usually cut .093" polycarbonate at about 1000mm/min with a 0.5mm step down per pass, using a 3mm end mill( lil' bit smaller than a 1/8"). Haven't messed with the spindle speed, I always run my dwp611 at full speed when cutting acrylic or polycarbonate.

Translating this to english measurements: 1000mm/min = 39.37 0.5mm step down is surprisingly small... about 0.002 of an inch 3mm end mill is 0.118 which is pretty much the same as 1/8 which is .125 But running the dwp611 at 27000 rpm... wow

doing the math

SFM = 834 Chip load is really small 0.000729 Millright Calculator

The depths and feeds are tailored more to this level of machine in order to derate the chiploads a some from what is recommended in charts for heavy duty machines, but it should give people a good base line

Provides chip tooth load and depth but not SFM per bit (and takes flute count into consideration) Aluminum 6061 1/8 0.0229 0.4572mm-0.6094 <--lighter chip load 0.0009 and depth 0.018-0.024 1/4 0.0279 0.4445mm-0.5925 <-- 0.00109 light depth 0.0175-0.0233 Hard Plastic 1/16 0.0381 1.27-1.6929mm <--0.0015 1/8 0.0508 1.65-2.2008mm <--0.002 slightly heavier (depth 0.065-0.08664) <--2 passes on 1/8" 1/4 0.0686 1.90-2.5394mm <--0.0027

Trying to find ideal router setting for 5052o Aluminum: Material spec for harder aluminum from harvey tool: Aluminum 800-1500

Let's try the midpoint of 1100 (3.82 * 1150) / 0.25 = 17572.0 <--rpm

The router has dial range of 0-6, Dial=(RPM-16000)/(5500/3) since we have a flexible SFM lets figure out where 17572 is (17572-16000)/(5500/3) = 0.857 and round it up so that I can just adjust to a number... in this case where is 1x solve([2 =(x-16000)/(5500/3)], [x]) = 19666.666; Ok we'll use RPM 19666... just curious what is this SFM solve([19666 = (3.82 * x ) / 0.25], [x])=SFM 1287

Ok so using 1x setting on the router with 19666, now onto the calculator: But I'll do it by hand here since I have the table already.

I want to do a rough cut using 1/4 end bit. the table on this is as follows: 1/4 chipload=0.0279mm depth cut=0.4445mm-0.5925

I need to convert this to inches Chipload=0.0010984

With chipload and RPM I can now compute the feed

IPM = RPM x IPT x T

GLOSSARY 2

SFM - Surface Feet per Minute RPM - Revolutions per Minute (Speed) IPT - Inches Per Tooth (Chip Load) IPR - Inches Per Revolution IPM = Inches Per Minute (Feed) D - Cutter Diameter T - Number of Teeth

Feed=43.2 Router=1x depth=0.02 (will manually slow down feed and attempt an aggressive deeper cut)

Testing 1/8" bit RPM = (3.82 * 800) / 0.125 = 24448 (using 800 as SFM) Dial = (24448-16000)/(5500/3) = 4.608 use 4.5 just a bit slower 793.5 SFM IPM = 24250 0.0009 2 = 43.65 Apparently the feed rate remains the same because the chip load is the same and the difference in size is compensated by increasing the speed of the router. However, since my SFM is lower I could slow it down in regards to temperature, as long as it can handle the chip load its fine... the depth is about the same as well.

Motor frequency f43 F# 91.1 f43.5 92 f52 A5 110.1

F26 A 441.1 F25.97 A4 440.5

F13 A3 220.4 F6.5 A2 110.1 F3.25 A1 55.1

F6.5 D#2 77.7 (when x and y are at 45 degree angle)