IMTS 2024
Published

CNC Machining: Programming the Appropriate Rates for Your Tool

A bit of math is involved in programming the appropriate rates for a particular tool.

Share

Machining center programmers specify spindle speed in revolutions per minute (rpm). Many also specify feed rate in per-minute fashion, either inches per minute (ipm) or millimeters per minute (mmpm). With cutting tools used on machining centers, tool diameter does not vary during the machining operation, so for most machining operations, this means one speed (in rpm) and one feed rate (in ipm or mmpm) is determined and used per cutting tool. 

An exception may be a milling cutter that can both plunge and side mill. In such a case, one feed rate is commonly required for plunging and another for side milling. Even so, compared to varying diameters machined on turning centers, which require the use of constant surface speed, cutting-condition variation internal to a given cutting tool is relatively minimal in machining center applications.

Consider a 0.5-inch-diameter carbide drill. Based on the material to be machined, the cutting tool manufacturer may recommend a speed of 250 surface feet per minute (sfm) and a feed rate of 0.004 inch per revolution (ipr). Using these recommendations, the programmer will apply this formula:
rpm = 3.82 * sfm / cutting tool diameter

The speed result, 1,910 rpm (3.82 * 250 / 0.5), will be programmed as S1910.

After determining spindle speed, feed rate in ipm is calculated with this formula:
ipm = rpm * ipr

Using a speed of 1,910 rpm and a feed rate of 0.004 ipr, the feed rate will be 7.64 ipm. Again, only one speed word (S1910) and one feed rate word (F7.64) will be required in the program for this drill, regardless of how many holes must be drilled.

Everything stated here so far is pretty conventional for machining center programming. The only exception may be that feed rate is often programmed directly in per-revolution fashion, which eliminates the feed rate calculation. 

Now consider the feature cutter radius compensation. It allows a range of cutter sizes (diameters) to be used. A programmer may plan on using a 1.0-inch-diameter cutter, but in reality—at the machine—a 0.75- or 1.25-inch-diameter cutter is actually used. If the programmer specifies spindle speed and feed rate based on the planned cutter size, actual cutting conditions used in the program will be incorrect if a different cutter is used. Machining will either be too slow or overly aggressive.

This problem can be easily overcome with a custom macro since it is possible to access the value stored in the cutter radius compensation offset register from within a CNC program. We can determine the actual cutter size (diameter) being used as the program is run and then calculate, right in the program, the exact rpm and ipm values.

There are two ways to use cutter radius compensation: 1) program the work-surface path, which requires the cutter size to be placed in the offset register, or 2) program the cutter’s center-line path, which requires the deviation from a planned cutter size to be place in the offset register. Additionally, the value placed in the cutter radius compensation offset register could be a radial or diameter value, so you must, of course, know what the offset register value represents if you want to use this technique.

For our example, we’ll say the programmer specifies the work-surface path and the value in the offset register is the cutter’s actual radius (a very common method).

For current-model FANUC CNCs, system variables starting with #2401 commonly provide access to geometry registers for cutter radius compensation (you must confirm this in the documentation that came with your machine). In this case, system variable #2403 provides access to offset number 3’s cutter radius compensation geometry register value, which in our example, will be the milling cutter’s radius.

Consider these commands that specify the speed and feed rate for a milling cutter running at 240 sfm and 0.005 ipr:
N340 T03 M06 (1.0 carbide end mill)
#1 = 3.82 * 240 / [#2403*2] (Store appropriate rpm in local variable #1)
N345 G54 G94 G90 S#1 M03 (Work offset, feed rate mode, absolute mode, start spindle)
N350 G00 X-0.75 Y-0.75 (First XY move)
N355 G43 H03 Z-0.6 M08 (Instate tool-length compensation, first Z move, coolant)
N360 G42 D03 Y0.125 (Instate cutter radius compensation)
N365 G01 X2.5 F[#1*0.005] (Begin milling, use appropriate feed rate)

With this program segment, the speed and feed rate will be based on the cutter size that is currently being used. If the setup person stores a value of 0.4375 in geometry offset register number 3 for cutter radius compensation (again, the cutter radius), speed and feed rate will be based on using a 0.875-inch-diameter cutter.

Note that feed rate is also a function of cutter diameter. The bigger the cutter, the more aggressive the feed rate should be. If you have a large range of potential cutter sizes, you can easily incorporate feed-rate-calculating logic statements into the program segment as well:
N360 G42 D03 Y0.125 (Instate cutter radius compensation)
IF[#2403 GT 1.0] THEN #2=0.006
IF[#2404 LE 1.0] THEN #2=0.005
N365 G01 X2.5 F[#1*#2] (Begin milling, use appropriate feed rate)

NTMA
MMS Online Apr-2021
Become a NTMA member today!
IMTS 2024
VERISURF
OASIS Inspection Systems
MMS Made in the USA
Gardner Business Intelligence
Paperless Parts
Universal Homepage Package W4900 Indicator
DNS Financial Services America
Gravotech

Related Content

Turning Tools

Buying a Lathe: The Basics

Lathes represent some of the oldest machining technology, but it’s still helpful to remember the basics when considering the purchase of a new turning machine. 

Read More
Basics

How To Calibrate Your Calipers

If you’re interested in calibrating your own digital, dial or Vernier calipers, here are some steps to take to make sure it goes off without a hitch.

Read More

Understanding Errors In Hand-Held Measuring Instruments

Different instruments (and different operators) are prone to different errors.

Read More
Basics

A New Milling 101: Milling Forces and Formulas

The forces involved in the milling process can be quantified, thus allowing mathematical tools to predict and control these forces. Formulas for calculating these forces accurately make it possible to optimize the quality of milling operations.

Read More

Read Next

Encountering Surface Finishes in the Everyday World

Surface measurement is becoming increasingly important to ensure proper performance of a manufactured product. Advanced surface measurement tools are not only beneficial in the manufacturing industry but also have unconventional applications.

Read More
Basics

Obscure CNC Features That Can Help (or Hurt) You

You cannot begin to take advantage of an available feature if you do not know it exists. Conversely, you will not know how to avoid CNC features that may be detrimental to your process.

Read More
Turning Machines

A History of Precision: The Invention and Evolution of Swiss-Style Machining

In the late 1800s, a new technology — Swiss-type machines — emerged to serve Switzerland’s growing watchmaking industry. Today, Swiss-machined parts are ubiquitous, and there’s a good reason for that: No other machining technology can produce tiny, complex components more efficiently or at higher quality.

Read More
MMS ad