Feeds and Speeds
This is one of the most confusing aspects for beginners. When you first start out using these machines at MICA, your instructor will typically provide you with a tool library that already has feeds and speeds programmed into the tool. But what if you want to use a different tool or cut a different material? You gotta learn about how to calculate feeds and speeds!
There are two key factors in determining a starting spindle speed and feed rate to use with your material and cutting tool. While the spindle speed and feed rate are what we actually use in the CNC program, they are determined from a recommended cutting speed, in surface feet per minute (SFM) and chip load, then tweaked and perfected through experimentation and experience. There are numerous factors that could influence your feed rate and spindle speed and much more information can be found on this subject in Machinery’s Handbook. We have two copies in dFab, one is behind the Haas controller, and the other is in Ryan’s office (you can borrow it for the day if you ask nicely)
Determining Spindle Speed:
The cutting speed, in combination with the tool diameter are used to determine spindle speed. The cutting speed (SFM) is the linear velocity with which a cutting tooth of your tool moves through the material to be cut. It is important to note that cutting speed is different than feed rate. In the case of a milling machine or CNC router, cutting speed is the speed at the cutting edge of a tool in relation to the material, whereas the feed rate is the speed of the entire cutter in relation to the material. Cutting speed, sometimes called surface speed, will allow us to determine spindle speed. Then we will move on to feed rate.
To understand the relationship between cutting speed (SFM) and spindle speed (RPM), think about a lathe. On that lathe there is a round piece with a radius of 1 foot. The distance that part would travel per revolution would be 2*pi*r or about 6 feet. If that part were rotating once per second (a spindle speed of 60 rpm), the cutting speed at the perimeter would be 6feet/rev *60rev/min = 360feet/min or 360 SFM. Notice how the units work too. The circumference of the circle is in feet per revolution or (feet/rev) and we are multiplying that by revolutions per min (rev/min), the revolutions cancel and we end up with (feet/min). We typically measure cutting tools in inches so the formula becomes:
V = (pi * D * S) / 12
Where V is the cutting speed in feet per min (SFM), D is the diameter of the cutting tool in inches and S is the spindle speed in revolutions per minute. It’s helpful to solve for spindle speed because the cutting speed and tool diameter are known.
S = (12 * V)/(pi * D)
Cutting speed can be lowered to meet your needs, but you don’t want to exceed the given high end limit for your tool material and part material. You can look these up in Machinery’s Handbook, or poke around on the web. Experimentally I have found that 1200 feet/min is a good cutting speed limit for hardwoods and plywood using a carbide tool, and have seen recommended speeds ranging from 900 SFM to 1600 SFM. A High Speed Steel (HSS) tool should be slower (maybe half?), but I’ve only used them on metals.
Determining Feed Rate:
Chip load in combination with the spindle speed, calculated above, and the number of teeth on your cutting tool will determine your feed rate. Chip load, also called feed per tooth, is the thickness in inches of a little shaving or chip generated by your cutting tool while making a cut. This could also be described as inches per revolution in the case of a single flute tool, or the feed per tooth if there are more than one flute. Chips can be measured if you are cutting plastic or metal, but wood chips tend to break when cut and are unreliable indicators of chip load. The formula for chip load is below:
f = F / (S * n)
Where f is chip load (inches), F is the feed rate in (inches/min), S is spindle speed (rev/min) and n is number of teeth. If we solve this for feed rate we get:
F = f * n * S
Step Over/Step Down:
It’s almost always going to be most efficient to step down as much as possible. This is the change in Z per pass. Here we are talking about end milling where the tool is cutting a dado or channel through the material and is effectively stepping over 100% of the tool diameter as in the case of cutting contours with a profiling pass.
A recommended starting step down is about 25% of the tool diameter. We’ll want to adjust that a tad for smaller tools in hard metals for example a 1/4 inch HSS tool cutting steel will break if the z step is more than about 0.05 inches (20%) but a 3/4 inch tool can step down up to half the diameter in steel with the correct feed and speed. This is not the case for wood.
When working with wood, you should step down a minimum of the diameter with tools larger than and including 1/4 inch unless you are using a down spiral tool. With a 1/4 inch compression tool, it is advisable to cut through a 3/4 inch piece of plywood in two or three passes. In this case, 2 cutting passes are taken at roughly 3/8 inch and, if you have small parts, one onion skin pass at about 1/16 is completed after all of the parts have been cut to that level. The chip load must be adjusted to 75% if you step down more than the diameter, and if you are stepping more than 2 times the diameter it should be adjusted to 50%.
I want to cut plywood with a 1/4 inch 2 flute cutting tool. For a carbide tool cutting plywood the recommended chip load is 0.004, so I’ll use a chip load of 0.003 in (75% for a 3/8 step down) and a cutting speed of about 1200 feet/min. Using the formulas above, first we will calculate spindle speed.
S = (12 * V)/(pi * D)
S = (12 * 1200)/(3 * .25)
S = 19,200 rpm
That maxes out our spindle on the MultiCAM, which has a range of 6,000rpm to 18,000 rpm, so I would lower the spindle speed to its maximum and use that number for the next calculation. Go back to the formula and think it through, all we did there is lower the cutting speed to lower the spindle speed, which is totally ok. To get feed rate we need the chip load (0.003), number of teeth (2) and spindle speed (18,000)
F = f * n * S
F = 0.003 * 2 * 18000
F = 108 ipm
Dialing It In:
The above calculations are a great way to get started, but realistically cutting conditions vary extensively and should be dialed in for your exact purposes. Start out with the recommendation or your best guess, Increase Feed Rate until the part finish starts to decrease, then decrease the Feed Rate by 10%. Second, decrease the Spindle Speed until surface finish starts to decrease, then increase it until it’s acceptable again.