Speeds and Feeds
Wisc-Online Learning Material:
Drill Feed & Speed Video: Calculating cutting speed for twist drills Video gives an overview of calculating cutting speed for twist drills and some quiz questions.
Feed and Speed Drills, Reams, Counter Sink Charts: Speed & Feed Charts & example calcs Gives an overview of speeds and feeds for various drilling operations along with charts.
Charts for speed for turning: Speed for Turning Gives a speeds chart along with some examples.
A Discussion on Speeds and Feeds
Learning Outcome: Outcome #4 Process Parameters and Production Efficiencies
Upon completion of this Learning Module, students should be able to:
· describe the meaning of cutting speeds and feeds.
· use charts to find recommended cutting speeds and feeds
· calculate spindle RPM.
· Calculate fipm and cut time
Speed and feed (or sometimes called feeds and speeds) describe machine tool inputs that, together, determine the material removal machining process. Speed refers to the rate of contact between the tool and work surface while feed refers to the relative motion of the tool to the part.
Speed, or more correctly called cutting speed or surface speed, quantifies the rate of contact a tool makes with a part surface. The units for Speed (V) are surface feet per minute (SFPM or FPM) or surface meters per minute (SMPM or MPM). Speed values are looked up in a reference chart and depend on tool type, material, and process.
This table shows a small sample of recommended Cutting Speeds in Surface Feet Per Minute (FPM) and Surface Meters Per Minute (MPM). For more detail, search online for cutting speed charts or calculators. Most charts will show ranges of suggested cutting speed values.
High Speed Steel (HSS) Tool
Free Machining Plain Carbon Steel
200 FPM; 50 MPM
950 FPM; 200 MPM
55 FPM; 30 MPM
200 FPM; 180 MPM
40 FPM; 25 MPM
900 FPM; 200 MPM
400 FPM; 100 MPM
1000 FPM; 500 MPM
When determining input parameters to a machining process, start by looking up the recommended cutting speed (V). Cutting speed is used to determine N (RPM of the spindle). N is an input value to a machining process.
Example resource for speeds an feeds: https://www.rockrivertool.com/speeds-and-feeds.php
The equation that describes cutting speed is: V = (π * D * N)/12
where D is the diameter in inches of the thing that is turning, and N is the RPM. In milling and drilling, D refers to the tool, and in turning, D refers to the part diameter. In the equation above, if V is in surface meters per minute, then D is in mm and 12 is replaced by 1000.
Note that π * D is the circumference of the tool and N is the rate of rotation of the tool. As such, V reflects the rate that the circumference of the tool contacts the part surface.
Now use V to determine N: N= (12*V)/(π * D)
Since 12/π =3.82, then N=3.82*(V/D) or simply 4*(V/D).
Feed is the other part of Speeds and Feeds. Recommended values of Feed are also looked-up in a chart. Detailed charts are available online.
Feed is an input parameter to a machining process. Values of feed depend on the type of material, tooling type, depth of cut, surface finish required, horsepower available at the spindle, fixture and tooling rigidity, and material strength characteristics.
There are three types of Feed and they are all interrelated.
1. Feed in Inches per Revolution (or MM per Revolution). This feed is abbreviated fipr
This value is looked up in a chart and is common in drilling and turning. Values of fipr are small, such as .003 ipr to .090 ipr
2. Feed in Inches per Tooth (or MM per Tooth). This feed is abbreviated fipt. This value is looked up in a chart and is used in multi-teeth processes such as milling. It is not used in turning. Values of fipt are small, such as .001 ipt to .020 ipt
3. Feed in Inches per Minute (or MM per Minute). This feed is abbreviated fipm and is determined using the looked-up values for fipt or fipr.
fipm values are generally whole numbers, such as 5 ipm up to 50 ipm.
fipm is related to the other two as follows:
fipm = fipr * N where N is spindle RPM.
fipr = fipt * n where n = the number of teeth (or flutes).
fipm is used to determine cut time as follows:
cut time = fipm * L where L is the length of cut.
Here is an example: Assume a process sheet calls for milling a slot .100” deep across a 2” wide aluminum part, using a .500” diameter, 4-flute, HSS, flat end mill.
Look-up charts suggest a cutting speed of 40 fpm at fipt=.005”
The recommended spindle RPM (N)
The recommended cutting feed in fipr and fipm
Also, assume the total Length of cut is 2.500”. What is the cut time?
Refer to a Machinery Handbook, tool manufacturer’s web site, or an internet search to compare recommended cutting speeds (V) when using HHS tools vs carbide tools. Notice the significantly larger values of recommended cutting speeds when using carbide.
Suggested lab activity:
Setup a manual turning operation to machine the OD of a piece of aluminum .100” deep along a distance of 1” in one pass. Use the information from above to determine the recommended spindle RPM. First make the cut using a HSS steel tool. Repeat the process using a carbide tool.
Note: Since you are turning the Z axis feed manually, there will not be a controlled feedrate.
What RPM did you use for the HHS tool? What RPM did you use for the carbide tool?
Which operation resulted in the better finish?
Which operation required greater force to feed the tool through the material?
https://www.wisc-online.com/learn/manufacturing-engineering/man-eng-machine (search cutting speeds)
Material Removal Processes (Turning, Milling, and Drilling)
Turning (Power Point)
Milling (Power Point)
Drilling (Power Point)