It is often necessary for CNC people to determine how long machining operations will take to perform. You may be trying to determine which of two or more processes will be used to machine a workpiece - or you may just be wondering how long a machining operation will require to complete.
Frankly speaking, the formulae related to calculating machining time are pretty simple to understand and use. Indeed, many manufacturing people have incorporated them into spreadsheets (like Microsoft Excel) - or they have programmed their calculators to include the related formulae. Here is the most important formula:
Time (minutes) = length of motion in inches divided by motion rate in inches per minute
That's it - no problem, right? You simply divide the length of the motion required for machining in inches by the inches per minute feedrate. The metric equivalent is:
Time (minutes) = length of motion in millimeters divided by motion rate in millimeters per minute
We'll be using the inch mode for the rest of the discussions in this article.
Say you must drill a 1.0 inch diameter hole. The hole depth is 0.75 and you intend to use an approach distance of 0.1 inch. The intended feedrate is 7.0 inches per minute. When we divide the motion distance (0.85) by the feedrate (7.0), we find that the time needed to drill this hole is 0.12143 minutes.
How many seconds is this? We obviously need to be able to convert decimal minutes (0.12143) into seconds. Here's the formulae:
1 second = 0.01666 minutes
Time in seconds = time in minutes divided by 0.01666
When we divide 0.12143 by 0.01666, the result is 7.2887 seconds (just over 7-1/4 seconds). So we now know how long it will take to drill the hole.
In order to use the formula, of course, you must be able to determine the feedrate in inches per minute (ipm). Most machining data handbooks, however, provide feedrate in inches per revolution (ipr), meaning you must first calculate the spindle rpm and then calculate the inches per minute feedrate. But speed recommendations are usually given in surface feet per minute (sfm). This speed is how much workpiece material will pass by each cutting edge during one minute. Here are two more formulae, based on speed being recommended 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 recommendation for feedrate will be in "per tooth" fashion, meaning you need to know the number of cutting edges (inserts, flutes, or teeth) there are on the cutting tool. This is commonly the case for milling operations. So we need to add yet one more formula:
ipr = ipt times number of cutting edges
Say you need to determine how long it will take to rough mill a 3.0 inch long slot with a 0.75 diameter, four flute, cobalt end mill. The three inch motion distance is the total motion length, including feed-on and feed-off distances. Based upon the material you are machining and the kind of machining operation you are going to perform (rough milling), the end mill's manufacture recommends a speed of 90 sfm and a feedrate of 0.002 ipt.
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 determine the number of seconds, divide 0.8187 by 0.01666 - this comes out to 49.141 seconds.
Fixed diameter machining versus changing-diameter machining
Note that it is quite easy to apply these formulae to machining center machining operations since the cutting tool diameter does not change during the machining operation. This is the case for the vast majority of cutting operations, including milling cutters, drills, taps, reamers, and just about any tool you use in a milling machine or CNC machining center. Again, the diameter being machined does not change during machining.
But do note that there are some operations during which the diameter being machined will change during the machining operation. Consider, for example, a rough turning operation on a CNC turning center that requires multiple passes to be made. The feature called constant surface speed will cause the spindle speed in rpm to change based upon the diameter being machined. For rough turning, this means you must calculate a new rpm and inches per minute feedrate for each rough turning pass.
Say you need to rough turn a 4.0 inch long diameter down from 1.0 inch to 0.75 inches, taking two passes (0.125 inch each). One of the passes will be at 0.875 and the other will be at 0.75. And each pass will be 4.1 inches long, including the approach. For the material being machined and the machining operation being performed, the cutting tool manufacturer recommends a speed of 400 sfm and a feedrate of 0.011 ipr.
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 no more difficult to make - there are just more of them. One per roughing pass.
Calculating time for finish turning and boring operations done on a CNC turning center are also more complicated. To do it perfectly, you must treat each segment being machined separately. For this reason, many quoting people will try to come up with an "average" diameter on which to base the rpm calculation. This allows the to more quickly come up with a pretty accurate machining time.
Diameter changes while machining
There are even CNC turning center operations that require the diameter to change even while the cutting tool in engaged with the workpiece. The two most common are facing and necking operations (including cut-off operations). If constant surface speed is used (as it should be), the speed in rpm will accelerate as a facing tool moves toward the center of the workpiece. Again, most estimators will try to come up with an average diameter in order to quickly determine approximate machining time.