How to make cutting speed calculations

Recently a reader asked a great question about how to calculate speeds and feeds. 

Speeds and feeds are at the heart of all machining. Learning the CNC codes or using a conversational control can be achieved in a relatively short period of time. Selecting the right speeds and feeds is almost as much art as it is science.

 In this article, I will be discussing how to calculate cutting speeds, but before we get into details, here are a few things to keep in mind. (at the bottom are calculations for speeds and feeds)

1. Safety – always an important consideration – don’t jeopardize your or another operators safety for the sake of speed.
    
2. Rigidity – if your setup is not rigid, you can toss a part or tool out of the machine, experience excessive chatter, fail to achieve acceptable surface finish, fail to maintain dimensions and so on.
    
3. Machinability – all materials have unique machinability characteristics. You’ve no doubt observed aluminum machines easier than steel.
    
4. Cutting Toom Material - high speed steel, carbide, ceramic, etc.
    
5. Available Horsepower – Machinability determines the horsepower requirements to cut the material. If you don’t have the horsepower, you will have to lighten your cuts to avoid stalling the spindle.
    
6. Tool geometry- Tools that have positive cutting geometry cut more freely than do tools with negative geometry, but are limited in the amount of shock and interrupted cuts they can take. Some materials cut much better with negative geometry, others with neutral or positive geometry.
    
7. Heat – machining creates a lot of heat and it is going to go into the tool, the material, the chips that are removed and so on.  Too much heat will quickly break down your tool. Too much heat can cause the material to expand and make it difficult to control part size.
    
8. Chip control – your ability to control the chips made during the machining process is an indication of having chosen the correct speeds, feeds and tool geometry.
    
9. Surface Finish – there is a direct relationship between cutting feeds and tool radius to surface finish.

All of the above factors (and many more) affect or are directly affected by speeds and feeds.

With respect to machinability, there are numerous websites that outline the machinability of various materials. Many tool manufacturing websites like Kennametal.com have great resources for determining the optimum cutting speeds and feeds for their tools and a wide variety of materials.

Cutting speed, in the US, is generally expressed in terms of Surface Feet Per Minute often expressed as (SFM) or (SFPM). SFM is the speed at which tool tip is cutting through the material. Imagine you are dragging a stick behind a car that is traveling at 60 miles per hour. In one minute your stick has traveled 5,280 feet across the ground. That would be expressed as 5,280 SFM.

Unless you are running a shaper or other linear cutting machine, your surface feet per minute is based upon the rotational speed of either the part or the cutting tool. Obviously, on a lathe it is the chuck speed that matters. On a milling machine it is the spindle speed that matters.

The other major factor in calculating SFM is the diameter of the diameter you are cutting on a lathe or the diameter of the tool you are using on the milling machine. So here are the steps to calculating SFM.

For SFM / RPM calculations you need to know the following:

D = the diameter of the milling tool or the diameter you are cutting on a lathe
Pi / π = 3.1416 (approximately but close enough)
SFM = The surface feet per minute you want to use for a cutting speed
RPM = The RPM required to achieve the desired SFM based on the diameter of the tool/part
K = Constant use for SFM calculations (3.8197)
    = 1 / [(D*π) /12]
    = 1/( 3.1416 /12)
     = 3.8197

RPM Calculations when you know the SFM you want to achieve.

RPM = SFM * 3.8197
                            D
Example: You are cutting a 2.5 diameter on a part (or using a 2.5 dia milling cutter)

• Material is free machining steel
• Cutting tool is coated carbide
• Carbide manufacturer recommends 500 SFM

Your cutting RPM would be:
             = (500 * 3.8197) / 2.5= 1909.85 / 2.5
             = 763.94
             = 764 RPM (rounded to the nearest RPM

SFM calculations when you know the tool diameter and RPM

But what do you do if you know the diameter of the part or cutter diameter and the RPM but you need to know the SFM so you can verify if it is appropriate.

              SFM = RPM * Diameter
                                    3.8197

Example:

• You know the milling cutter is 6” in diameter
• You know the RPM is 1000
• You need to know is the SFM appropriate for cutting aluminum

          SFM= (1000 * 6) / 3.8197
                   = 6000 / 3.8197
                   = 1570.80

Since cutting speeds for aluminum using carbide can range from 800-2000 SFM  1570.8 SFM  may or may not be a good speed. It will depend on all the factors listed at the beginning.

Watch my next article that will discuss how to calculate feed rates for mills, drills and lathes.

About these ads