9.9 Spindle Speed, Feed Rate, Depth Of Cut And Finish Allowances
9.9 Spindle Speed, Feed Rate, Depth Of Cut And Finish Allowances
Micky R. Jennings
Spindle Speed
Milling machines have the same spindle speedcalculation as the rest of the rotational tools in the shop. Based on surface feet per minute (SFPM) of a tool and the cutting conditions, the operator can calculate the appropriate RPM.
RPM = SFPM × 4 / Diameter
Milling machines are machine tools that can utilize carbide tooling. In these instances, it is always a good idea to consult the manufacturer for the correct surface feet per minute for the tool in a specific material. If there is no technical data on the tool to be usedavailable, a conservative starting point would be 4x the SFPM of HSS.
For example, the calculation for cutting mild steel with a 1/4 carbide end mill would be:
RPM = SFPM × 4 / Diameter
RPM = 400 × 4 / .25
RPM = 1600 / .25
RPM = 6400
Another example is the calculation for cutting aluminum with a 3/4 HSS end mill.
RPM = SFPM × 4 / Diameter
RPM = 200 × 4 / .75
RPM = 800 / .75
RPM = 1066
Feed Rate
Manual milling machines have a side cutting feed ratethat is expressed in Inches Per Minute (IPM). This feed rate is completely independent of the rotation of the spindle. The formula to calculate the feed rate is:
IPM = RPM × number of flutes × Chip Load Per Tooth (CPT)
The chip load per tooth (CPT) is another area where the manufacturer will have some helpful information about their product. If that information isn’t available, the following generalized conservative estimate can be used to get the operator started.
CPT = Diameter / 1/8 × .0005 to .001
As the tool size gets larger and stronger, more CPT can be taken with the tool without damaging it.
For example, let’s calculate roughing out aluminum with a 2 flute 1/2″ carbide end mill.
First, the RPM:
RPM = SFPM × 4 / Diameter
RPM = 400 × 4 / .5
RPM = 1600 / .5
RPM = 3200
Now the CPT:
CPT = Diameter / 1/8 × .001
CPT = 1/2 / 1/8 × .001
CPT = 4 × .001
CPT = .004
Now the feed rate formula can be calculated:
IPM = RPM × FLTS × CPT
IPM = 3200 × 2 × .004
IPM = 25.6
Author’s Tip
Whenever I am calculating spindle speed in RPM or feed rate in IPM, I take my answer and round it to the nearest 50 RPMs or nearest whole IPM. This makes sense for manual equipment because the machine isn’t accurate to single RPMs or decimal points of IPM, but it will also make sense later on if you utilize a CAM system to aid you in writing technical programs for CNC machines. This rounding generally won’t hurt the tool or the part.
Depth of Cut
Depth of cut is the amount of the tool engaged in the work while making a cut. On a milling machine, the depth of cut can be axially or radially measured. Depth cuts axially use the tip of the tool more heavily and have a tendency to wear the tool out prematurely. Radial depth cuts use a larger portion of the cutting edges and are generally preferable as the tool will last longer.
On manual milling machines, heavy depth cuts in steel are best performed with roughing end mills. In