In Stores

Categories
Subscribe to Blog

Everything related to numerical metal cutting theory
Pages:(1) [1]

## General Speeds and Feeds Formulas

December 24, 2010, 2:10 pm by Eldar Gerfanov

## What are Machining Speeds and Feeds

One of the basic tasks a machinists must learn to perform is calculation of speeds and feeds required for milling, drilling and turning.

It starts from knowing your workpiece materiel and tooling you are going to use in order to cut it.
The combination of these two factors determines your initial Cutting Speed and Chip Load that you can put into the speed and feed formulas to calculate the cutting tool RPM and feed rate.

Cutting Speed is the speed at which the tip of the tool travels through material. It is commonly expressed in Surface Feet per Minute (SFM) or Surface Meters per Minute (SMM).

Chip Load is the advancement of each tooth per revolution of the tool.

In other words Chip Load is the thickness of the material that each tooth removes per each revolution.

## So how do you find the Cutting Speed and Chip Load for your tool?

Tool manufacturers often post Cutting Speeds and Feeds for their tools for various materials and cutting conditions.

Most experienced machinists simply remember cutting speeds and chip loads for materials they machine most often.

Here are commonly recommended cutting speeds and chip loads for carbide tools for a couple of materials:

• Aluminum: 300SFM, 0.7% of the diameter (for example fz = 0.5"dia x 0.007 = 0.0035in/tooth)

• Annealed Tool steel: 150SFM, 0.4% of the diameter (for example fz = 0.5" x 0.004 = 0.002in/tooth)

When you have manufacturers data simply find your tool in the catalogue and cross-reference the cutting speed and chip load against the tool diameter:

Since cutting speeds can be in either Imperial (SFM) or Metric (SMM or m/min) units, you have to use two formulas to calculate the RPM.

## Imperial Speed and Feed Calculation

Code

 RPM= 12 x SFM = Please enter Speed and Diameter 3.14 x in

Feed Rate = RPM x x in = Please enter RPM, number of teeth and chip load (in/min)

## Metric Speed and Feed Calculation

Code

 RPM= 1000 x m/min = Please enter Speed and Diameter 3.14 x mm

Feed Rate = RPM x x mm = Please enter RPM, number of teeth and chip load (mm/min)

Want something better?

### More about formulas needed to calculate turning, drilling, and of course milling speeds and feeds

Here are a few basic formulas with term explanations to get you going:

## Calculating Spindle Speed (RPM) Using Imperial Cutting Speed:

Code

 RPM= 12 x SFM 3.14 x Diameter

Simplified imperial formula:

 RPM= 3.8 x SFM Diameter

## Calculating Spindle Speed (RPM) using Metric Cutting Speed:

Code

 RPM= 1000 x SMM 3.14 x Diameter

Simplified metric formula:

 RPM= 318 x SMM Diameter

## Calculating Feed Rate :

Feed_Rate=RPM x N(teeth) x CL(chip load)

## Numbers Behind High Speed Machining (HSM)

May 28, 2013, 7:01 am by Eldar Gerfanov

HSM or High Speed Machining is becoming more and more popular each day.
Many of us have seen those youtube videos where endmlls remove large amounts of material at high speeds/feeds.

While definitions of HSM may vary between tool manufacturers and even individual shops, the physics behind it remain the same.

## What is HSM?

HSM is a complex of programming, machining and tooling techniques aimed at radical increase of productivity.

## Programming

The cornerstone of HSM is low radial and high axial engagement of an endmill with the workpiece.

There are many CAD/CAM systems that allow you to create HSM tool-paths. Mastercam's Dynamic milling and SurfCAM's Truemill are some of them.

When radial cutter engagement with the material is smaller than the radius of the tool an interesting thing happens.
Chip load- the distance the tool advances per cutter revolution per tooth- does not equal the actual chip thickness anymore.
Chip thinning mainly happens at radial engagements below 30% of the diameter.

 100% 1 50% 1 30% 1.091 25% 1.212 20% 1.641 15% 2.1 10% 4.375 5% 6.882

In order to get compensated chipload you need to multiply recommended by manufacturer chipload by the chip thinning factor.

Usual Radial Engagement for HSM toolpaths however is between 5 and 15%.

Axial depth of cut varies depending on geometry, but

## Plunging and Ramping Recomendations and Techniques

February 12, 2013, 1:03 pm by Eldar Gerfanov

Quite often in order to start cutting in x-y direction you need to first plunge into the material.

Here is a compliled list of recommendations for different kinds of plunging that works in most if not all cases.

### Plunge with center cutting endmill:

• Regular Chipload/Number of flutes , half the cutting speed. (for 3 flute endmill divide normal chipload by 3)

### Ramp:

• Ramp Angle: Indexed/non center cutting endmills: 1-2.5 degree; Center cutting endmills- Up to 45 deg

### Ramp chipload ajustment for 4 flute Center cutting endmills:

• 0-2.5deg=100% of normal feedrate
• 2.5-5deg=75% of normal feedrate
• 5-15deg=50% of normal feedrate
• 15-30deg=25% of normal feedrate
• 30-45deg=5% of normal feedrate

Dont forget to reduce cutting speed for ramping above 5deg by half!

## Calculating Tool Engagement Angle, Radial Depth of Cut

August 18, 2012, 11:14 am by Eldar Gerfanov

Here i will show you how to calculate Tool Engagement Angle using tool diameter and Width Of Cut (radial deopth of cut)

Lets first draw a pretty image that shows us everything we need.

Where:

• r: Radius of the cutter = Diamater /2
• a: TEA - Enagagement angle we are trying to find here
• WOC: Width of cut or RADIAL Depth of Cut
• r2: The difference between r and WOC, r=r2+WOC

Below we develop 2 formulas that allow us to find TEA and WOC