# Feet and Inches Per Minute: A Basic Primer in Machining Speeds and Feeds

0

This document will help explain how to achieve maximum tool life and productivity by allowing the reader to better understand SFM, IPM and how to calculate them.

Surface feet per minute (SFM) is the concept of what speed the very tip of a cutting tool is travelling in comparison to the material it is cutting, Inches per minute (IPM) is the how fast to feed your tool.

Using the correct SFM and IPM will provide a good balance between production speed and tool life. Excessively high SFM can result in the cutting edge of a tool degrading almost instantly, as the materiel that makes up the cutting edge overheats and becomes softer than the material it is cutting. Tooling with wide cutting angles such as negative rake inserts can handle higher SFM/IPM than tooling with narrow cutting angles like positive rake inserts as there is more material to support the tip, and to absorb heat away.

SFM is RPM * PI * Diameter / 12″, Where diameter is the diameter of the work in a lathe, of the drill when drilling, and of the end mill/face mill when milling. The / 12″ is because SFM is in feet, And typically one measures the work or tool in inches.

You can calculate what RPM you need with:

RPM = Desired SFM * 12″ / PI / Diameter

this can be simplified to

RPM = Desired SFM * 3.82 / Diameter.

Using 4 instead of 3.82 makes math much easier in your head, and results in only a 5% higher SFM result.

As far as what SFM to use, this depends on what material you are cutting, and what material you are cutting it with.

Recommended SFM is what the industry has found to be the most productive for good tool life. Using lower SFM is acceptable, Using higher SFM will often burn out tools rapidly unless the cut is very shallow. Increasing SFM past these recommendations for a finishing cut of less than 0.005″ depth of cut is often used on mills and lathes.

Mild steel being cut with HSS has a recommended SFM of 100. It is recommended to aim for steel chips that turn a light golden colour a few seconds after cutting. If they turn darker or blue, your SFM and/or feed rate is too high. Carbide can handle chips that turn blue, however these chips are much more of a burning hazard to the operator.

Stainless steel being cut with HSS has a recommended SFM of only 50 to 80, depending on alloy. Some harden alloys as low as 30 to 50 SFM. Carbide can handle the toughness and abrasive nature of stainless much better than HSS and is highly recommended for stainless steel.

Most Aluminium alloys are very soft and absorb heat well. They however need sharp tools, and with negative rake carbide tools, high SFM can be needed to achieve a good surface finish.

Aluminium being cut with HSS has a recommended SFM of 200, Sometimes much more depending on what chart you consult, up to 600SFM on some.

Plastics being cut with HSS can be cut with exceptional high SFM, However melting of the plastic, not the tool will limit SFM in practice.

Typically with carbide you can double the SFM of HSS, However during interrupted cuts, it is recommended to use lower SFM to reduce the impact stress on the easier to fracture carbide and is best to use a more durable grade of carbide. In the C# series of carbide, C1 through C4 are used for cast iron, non ferrous and non metallic materials, while C5 through C8 are for steel alloys as they resist wear and pitting better, But do not deal with impact stresses as well.

Generally, the higher the C number, the more wear resistant and brittle carbide will be, In the C1 to C8 range. Grades C9 and above are for totally different tasks and may or may not be more brittle than C1 through C8.

Ideal feed rates and depth of cut and different from material to material. You should calculate feed rates from a desired tooth load. Feed rates are measured in Inches per minute (IPM), And tooth load is measured in inches.

Tooth load = IPM / (RPM * cutting edges). This applies to mills. drills and lathes however use chip load (CL). That is just:

Chip Load = IPM / RPM

Desired chip or Tooth load, depends on the finish you desire and material and tool size. Larger tools can handle larger loads. To calculate what tooth load for drills and end mills, You can use:

Tooth load = Diameter * 0.017

Smaller tooth loads are typically used for finishing passes when milling. For turning, Inserts will often have recommendations on depth of cut and feed rate, with custom ground HSS experimentation will be required to find the ideal feed rates, as chip color is the main indication in such a case.

To calculate a feed rate, you would use:

IPM = Tooth load * Cutting Edges * RPM Generally, one should use the manufacturers recommendations for tooth load for milling and turning.

Excessive tooth/chip load can chip cutting edges or even snap tools. A proper balance between SFM and IPM will give you the highest tool life and productivity.

Some common feed and speed mistakes to avoid:

Using too high a RPM for a drilling steel, with too little pressure. 100 SFM * 4 / 1/2″ = 800 rpm, meaning not only is the typical 1800 rpm portable drill way too fast, but with only 1HP of a typical small drill press or portable drill, you can only feed at about 5IPM in steel before stalling at 1/2″ drill size.

This results in 0.0062″ CL (5IPM / 800rpm), A little low for a 1/2″ drill (Recommended 0.0085), But it will overload 1hp drill press to achieve that, and would quickly damage a 1800rpm drill to run at high power levels at lower speeds. a 1/2 inch drill will easily withstand that much feed pressure as long as it is straight down. It is better to run even slower, and produce larger chips that will easily clear the drill flutes without snapping, And you cut more with less linear feet of material cut, hence better tool life. a 500rpm portable drill is highly recommended for drilling 3/8″ to 1″ in steel and will operate much better at full RPM a higher speed drill with electric speed reduction, And will still drill smaller holes fine, just slower.

Using low depth of cut and feed rate, thinking it saves tool life and machine wear. The extra passes cutting will cause extra tool and machine wear. If you want to save on tool life, reduce the RPM until you are able to cut at the ideal chip load for the tool. Use high depth of cut and chip load, as fewer deep cuts is more efficient than many small cuts, If you have a gearbox or multiple pulley speed reduction, You can get high torque at lower RPM’s and cut amazingly efficiently at low speeds, If you have electronic variable speed only, Using higher speeds only if HP limited.

Using high SFM when deep drilling plastic, The friction of the drill flutes heat up and melt the plastic. The drill bit itself may also heat up and melt the plastic if the time between holes is short. Some plastics do not respond well to high feed rates, So high production rates may require coolant/lubricant to prevent melting, or allowing the tool to cool down while other operations or tools are preformed.

Allowing a tool to dwell or rub on work hardening stainless steel alloys. The alloy will quickly harden and it may take a carbide tool to be able to cut through the hardened skin. Always use low enough RPM that you can achieve an aggressive feed with stainless steel and never stop feeding until the tool is clear of the work.

Using too low a feed rate on a lathe. Using higher feed rates can greatly improve chip control by causing the chip to fracture into smaller chips. Depth of cut and feed rate are critical to proper chip control and one should pay attention to manufacturer recommendations on chip load and depth of cut for proper chip breaking. Low feed rates and depth of cut do not extend tool life and the extra cycles needed to complete a job will wear out a machine more than the extra stress of deeper cuts.