How to Calculate the CNC Machining Time?
You may be trying to decide which of two or more processes will be used to machine a workpiece, or you may simply want to know how to calculate the CNC machining time.
To be honest, the formulae for calculating machining time are fairly simple to grasp and apply. Indeed, many manufacturers have incorporated them into spreadsheets (such as Microsoft Excel) or programmed their calculators to include the related formulae. The most important formula is as follows:
Time (minutes) = length of motion in inches divided by motion rate in inches per minute
That’s all there is to it, right? Simply divide the length of the machining motion in inches by the feedrate in inches per minute. The metric equivalent is as follows:
Time (minutes) = length of motion in millimeters divided by motion rate in millimeters per minute
The inch mode will be used for the remainder of this article’s discussions.
Assume you need to drill a 1.0-inch-diameter hole. The hole depth is 0.75 inches, and the approach distance is 0.1 inch. The feedrate is set to 7.0 inches per minute. When we divide the motion distance (0.85) by the feedrate (7.0), we get 0.12143 minutes to drill this hole.
How much time is this? We must, of course, be able to convert decimal minutes (0.12143) into seconds. Here are the formulas:
- 1 second = 0.01666 minutes
- Time in seconds = time in minutes divided by 0.01666
7.2887 seconds (just over 7-1/4 seconds) is the result of dividing 0.12143 by 0.01666. So we now know how long the hole will take to drill.
To use the formula, you must first be able to calculate the feedrate in inches per minute (ipm). However, most machining data handbooks provide feedrate in inches per revolution (ipr), which means you must first calculate the spindle rpm and then the inches per minute feedrate. However, most speed recommendations are given in surface feet per minute (sfm). This is the amount of workpiece material that will pass by each cutting edge in one minute. Here are two more formulas based on the recommended speed in sfm and feedrate in ipr.
- rpm = 3.82 times sfm divided by diameter (the tool diameter in our case)
- ipm = rpm times ipr
Note that for some tools, the feedrate recommendation will be in “per tooth” fashion, which means you must know the number of cutting edges (inserts, flutes, or teeth) on the cutting tool. This is frequently the case with milling operations. As a result, we must add another formula:
ipr = ipt times number of cutting edges
Assume you need to calculate the time required to rough mill a 3.0 inch long slot with a 0.75 diameter, four flute cobalt end mill. The total motion length, including feed-on and feed-off distances, is three inches. The end mill’s manufacturer recommends a speed of 90 sfm and a feedrate of 0.002 ipt based on the material you’re machining and the type of machining operation you’ll be performing (rough milling).First, determine the speed in rpm: 3.82 times 90 divided by 0.75 is 458 rpm.
- Next determine the inches per revolution feedrate: 4 times 0.002 is 0.008 ipr.
- Next, determine the inches per minute feedrate: 458 times 0.008 is 3.664 ipm.
- Finally, determine the time required in minutes: 3 inches of motion divided by 3.664 ipm is 0.8187 minutes.
To calculate the number of seconds, divide 0.8187 by 0.01666, which equals 49.141 seconds.
- Fixed diameter machining versus changing-diameter machining
Because the cutting tool diameter does not change during the machining operation, these formulae are quite simple to apply to machining center machining operations. This is true for the vast majority of cutting operations, such as milling cutters, drills, taps, reamers, and nearly any tool used in a milling machine or CNC machining center. Again, the diameter being machined remains constant during the process.
However, there are some operations in which the diameter being machined changes during the machining process. Consider a rough turning operation on a CNC turning center that necessitates multiple passes. The constant surface speed feature changes the spindle speed in rpm based on the diameter being machined. This means that for each rough turning pass, you must calculate a new rpm and inches per minute feedrate.
Assume you need to rough turn a 4.0-inch-long diameter from 1.0-inch to 0.75-inch in two passes (0.125 inch each). One pass will be at 0.875, while the other will be at 0.75. And each pass, including the approach, will be 4.1 inches long. The cutting tool manufacturer recommends a speed of 400 sfm and a feedrate of 0.011 ipr for the material being machined and the machining operation being performed.
Again each pass must be calculated separately. For the first pass:
- rpm = 3.82 times 400 divided by 0.875, or 1,746 rpm
- ipm = 0.011 times 1,746, or, 19.206 ipm
- time = 4.1 divided by 19.206, or 0.213 minutes (12.785 seconds)
For the second pass
- rpm = 3.82 times 400 divided by 0.75, or 2,037 rpm
- ipm = 0.011 times 2,037, or 22.407 ipm
- time = 4.1 divided by 22.407, or 0.182 minutes (10.924 seconds)
As you can see, the calculations are not any more difficult to perform; they are simply more numerous. One for each roughing pass.
Time calculations for finish turning and boring operations performed on a CNC turning center are also more complex. To do it correctly, you must machine each segment separately. As a result, many people who quote will try to come up with a “average” diameter to base the rpm calculation on. This allows them to produce a more accurate machining time more quickly.
Diameter changes while machining
There are even CNC turning center operations that necessitate changing the diameter of the workpiece while the cutting tool is engaged with it. Faceting and necking operations are the two most common (including cut-off operations). If a constant surface speed is used (as it should be), the speed in rpm increases as a facing tool moves toward the workpiece’s center. Again, most estimators will attempt to calculate an average diameter in order to quickly calculate an approximate machining time.
According to above samples, I hope you have much learned how to calculate the CNC machining time.
If you want to learn our delivery time for your projects, please send the details including drawings and quantity to us!