**Feeds and Speeds**

*//Your instructor or Staff can advise you on Feeds and speeds for many different tools, however for some tools, it may take some calculation to determine the proper settings for your tool and material. Remember that there these settings are not uniform and can change based on material, tooling or machine. often Finding the correct settings is a process of trial and error, so save pieces of material to run tests on.//*

Feeds generally refers to the Federate at which the machine tool is moving through space in terms of x,y and z coordinates.

Speeds refers to the speed at which the spindle is spinning for the tool. In some cases this may be a constant value- i.e. a Router which only has off and on as speed settings,

While the spindle speed and feed rate are what we actually use in the CNC program, they are related to one another and affected by recommended cutting speed, in surface feet per minute (SFM) and chip load, which are assigned by tool and material. These settings also can be adjusted to accommodate differences in material or numerous other factors through experimentation and testing.

**Cutting Speed**– Refers to the speed at which the tooth of a cutter moves through material. this is both rotational movement and directional. This number is generally calculated from the diameter of the bit and the speed of rotation in RPM This is also referred to as surface speed.

**Feed rate**– is the speed of the entire cutter in relation to the material in terms of xyz coordinates.

**Spindle Speed**– the speed in RPM which the tool is spinning. It can be calculated by the following formula-

V is the cutting speed in feet per min (Often this is known,)

D is the diameter of the cutting tool in inches (also known or easily determined)

S is the spindle speed in revolutions per minute.

**S = (12 * V)/(pi * D)**

Often you solve for spindle speed because the cutting speed and tool diameter are known.

1200 feet/min is a good Cutting speed (V) limit for hardwoods and plywood using a carbide tool, you can adjust the Cutting speed (V) between 900 SFM to 1600 SFM to find a sweet spot for your given material.

**Chip Load**– Refers to the size and volume of chips produced by a cutting tool. Too big of chips are caused by aggressive cutting, which puts stress on material and driver motors, and dulls tooling. Too Small causes dust, burning of material or overheating bits because of friction.

Chip Load is calculated in the following manner.

f = F / (S * n)

f is chip load (inches)

F is the feed rate in (inches/min),

S is spindle speed (rev/min)

n is number of teeth

This formula can also determine federate F = f * n * S

**Step Over**– The amount of surface area which a tool is overlapping a previous cut at the same depth level- so a 1/4” Bit with a 50% Stopover cuts 1/8 in of new material with each pass. If the tool is cutting a dado or channel through the material It is effectively stepping over 100% of the tool diameter for examples profile cutting contours or engraving.

**Step Down**– The amount of depth (change in Z per pass) that a tool makes as it cuts in each pass at each level.

It’s almost always going to be most efficient to step down as much as possible with a given tool. higher step-down means fewer cuts and shorter time on table, as well as extended tool life.

When working with wood, you should step down a minimum of the diameter with tools larger than and including 1/4 inch unless you are using a down spiral tool. The chip load must be adjusted to 75% if you step down more than the diameter, and if you are stepping more than 2 times the diameter it should be adjusted to 50%.

To understand the relationship between cutting speed (SFM) and spindle speed (RPM), think about a lathe. On that lathe there is a round piece with a radius of 1 foot. The distance that part would travel per revolution would be 2*pi*r or about 6 feet. If that part were rotating once per second (a spindle speed of 60 rpm), the cutting speed at the perimeter would be 6feet/rev *60rev/min = 360feet/min or 360 SFM. Notice how the units work too. The circumference of the circle is in feet per revolution or (feet/rev) and we are multiplying that by revolutions per min (rev/min), the revolutions cancel and we end up with (feet/min).

Example:

Material- plywood

Tool- 1/4 inch 2 flute cutting tool.

For a carbide tool cutting plywood the recommended chip load is 0.004

More info here- https://www.onsrud.com/xdoc/feedspeeds

Chip load Calc- 3/8 in Step down = .75 *.0004 = 0.0003 (75% for a 3/8 step down)

Cutting speed of about 1200 feet/min. (adjustable)

S = (12 * V)/(pi * D)

S = (12 * 1200)/(3 * .25

S = 19,200 rpm

The spindle on our Shopbot has a range of 6,000rpm to 18,000 rpm, so we need to lower the spindle speed to its maximum and use that number for the next calculation. We can lower the cutting speed to lower the spindle speed without changing anything significant, as long as we stay in range for material and machine. To get feed rate we need the chip load (0.003), number of teeth (2) and spindle speed (18,000)

F = f * n * S

F = 0.003 * 2 * 18000

F = 108 ipm

Fine adjustment:

Start out with the recommendation or calculation, Increase Feed Rate until decrease (tearout), then decrease the Feed Rate by 10%. then, decrease the Spindle Speed until surface finish starts to decrease, then increase it until it’s acceptable again. Once you have Ideal numbers be sure to save them to your tool library for future use!