Wait! There’s an even better approach!
For the latest article on this topic and some new tools in G-Wizard to help solve the problem, please check out our new article and videos on Calculating Cut Depth and Cut Width.
I got a note from a G-Wizard Calculator user recently wondering about the trade-offs for Cut Depth and Cut Width and Tool Life. As he put it, you can go deep and not very wide or wide and not very deep, so what’s better? Like so many things, the answer is, “It depends,” which is not very satisfying. So let’s talk about what it depends on.
The Duty Cycle of the Flutes
Let’s start with one of the biggest factors for tool life when you’re pushing hard, and that is heat. Too much heat kills tool life quickly because it softens the cutting edge which allows it to dull faster. Having the correct feeds and speeds is one way to minimize the heat, because well-formed chips carry away most of the heat in the chip. You get well-formed chips from the proper feeds and speeds, that’s what “proper” means in this case. Using coolant is another way to control heat, although sometimes flood coolant is too much of a good thing because it can shock cool carbide and cause microcracks which accelerate tool wear. A very safe way to reduce heat is to change the Duty Cycle of the flutes.
What do I mean by “Duty Cycle?” It’s a pretty simple concept: If the flute is actively cutting, it is doing “Duty”. If it is spinning through air until it comes back around to the material, it is not doing “Duty”. For example, if we have a width of cut equal to half the diameter, we have a 25% duty cycle. Each flute spends 25% of its time in the cut and 75% in air. On a full slot, it is half air, half cutting time. It is the time in air that gives it a break and a chance to cool off a little bit. The Duty Cycle also facilitates chip clearing. The chip is trapped and moving along in the gap between flutes until the flute is exposed to air at which point it can be ejected. A flute that only spends 10% of its time in the cut has a very easy job conveying chips out of the cut, whereas a full slot has a difficult time. Both this tendency to allow more cooling and to allow better chip evacuation lead to much longer tool life.
So, in general, we want to minimize the width of cut. HSM (High Speed Machining) toolpaths are the masters of this because they keep the Duty Cycle (which is directly proportional to the tool engagement angle) constant and typically fairly low. You’d try for cutter engagement in the range of 15% cut width, for example. This is a big reason why the HSM tool paths can be so much faster. The other reason is that since they don’t slam into corners, you don’t get the shock loads of cornering.
Spreading Wear Along the Length of a Flute
Wherever possible, take the cutter as deep as possible on a pass because it spreads the wear along the length of a flute instead of concentrating it all near the tip of the endmill. This depth will tend to put more of the cutter into the cut instead of air, but the heat doesn’t conduct fast enough through the cutter anyway, so it’s okay if we’ve kept the Duty Cycle low by not cutting very wide.
Deflection Kills Endmills
Too much length is bad, because of tool deflection. It’s not good for the tool to be heavily deflected in a cut. Imagine a bent tool like the one in the photo above thrashing around. Chiploads go up, part accuracy suffers, and you’re beating the tool against the side of the cut with a hammering motion. Therefore, we want to get as much tool length as possible without having too much deflection. There are allowable deflection limits as recommended by tooling manufacturers. For example, on endmills larger than about 1/8″ diameter, you really shouldn’t exceed 0.001″ of deflection. If you do, you’re going to start fatiguing the tool and you also invite chatter.
Using G-Wizard Calculator to Optimize the Cut
Let’s put all this together and show how to use the G-Wizard Speeds and Feeds Calculator to set up some ideal Cut Widths and Depths. We’ll take it step-by-step: 1. First, let’s dial in some specifics about our tooling and material. Let’s say we’re cutting some Low Carbon Steel (1020 or some such) and we’ll use a 4 Flute Carbide Endmill. We need to cut a pocket that is 3/4″ deep, and it has some internal radiused corners that have a 1/8″ radius. So, we have to stick to a cutter no larger than 1/4″ to be able to make the corner radii. Here’s what that looks like worst case:
I say worst case because I have specified full width of cut (slot all the way) and full depth. This has caused G-Wizard to slow the cut way down, and we’re still showing almost 0.004″ of deflection on the tool. That’s way too much deflection so GWC has called that out in orange. The MRR for this cut is 0.5944, but with that kind of deflection on a fully shrouded cutter we’re unlikely to see those MRR’s because we’ll be too busy breaking cutters.
2. Now let’s start using GWC to optimize the cut. I want to go through a couple of scenarios just so you can see some tradeoffs. We’ll start by doing the opposite of what we’ve recommended–we’ll keep full width on the cut and use the Cut Optimizer to decide how much depth of cut we can use within reasonable (0.001″) deflection limits. Here is that scenario:
Optimizing Cut Depth to be as much as it can be within deflection limits is easy. Just click the little “Cut” speedometer to the right of Cut Depth. You’ll get the Cut Optimizer popup with the values already calculated, and I just accepted them and closed the popup. As we can see, we can’t cut very deep–only about 0.070″. That’s probably a lot less than most would have guessed. But, despite having to make lots of little 0.070″ deep stepdown passes, our MRR (Material Removal Rate), wasn’t penalized all that much–it’s 0.4556 cubic inches a minute versus 0.5944. The different is that this cut is not going to be breaking cutters constantly.
We can simulate this cut with G-Wizard Editor’s Conversational CNC Wizards. Here’s the parameters to generate g-code for this cut:
If we look at GW Editor’s Info Tab after simulating the g-code, we see it says this particular pocket will require about 1 minute 30 seconds and almost 1400 lines of g-code. With the individual passes being so shallow (0.070″), there’s a lot of too’ing and fro’ing the poor machine has to do.
3. Now let’s try it with some more recommended parameters. Let’s see what’s needed for a cut width that is 15% of diameter. If you have GW Calculator up and the full slot cut width, just click to the right of the last digit of the width and type “*15%<enter>”. GW will do the math for you and you’ll have a 0.0375″ cut width. I optimized the Cut Depth again based on that Cut Width and I see I can go full depth. So I can cut the pocket in a single pass. GW Calculator is going to be a little timid doing the cut in one pass–it slows the cut way down to 1600 rpm and about 5 IPM. Clearly it’s worried about having the cutter 3 diameters deep. You’d have to experiment a bit to see how to make GW happier by doing more step down passes and thereby having less Cut Depth.
The problem is GW has to stay conservative in the corners, even though this is very slow for the straightaways. Since we have cornering problems, let’s activate the HSM mode and see what it’ll do with a high speed tool path. Just click “Const TEA” and then check the “Show HSM Feeds and Speeds”. I got radically higher feeds and speeds and a deflection warning cutting a single pass. Still too much deflection. So, I went for three passes (0.25″ cut depth) and since there was still slightly too much deflection, I took the feedrate down by hand until I had 0.001″ deflection exactly. Here’s the result:
And now we see how the HSM toolpaths earn their keep. RPM’s are way up to 8100 rpm and feedrate is at 80 IPM. The RPM’s are up because of that Duty Cycle concept. With a 15% cut width, the flutes are getting a lot of air cooling time. Feedrate can be upped because the Duty Cycle ensures adequate chip clearing. Feedrate is largely a chip load issue and chip load is largely a function of how fast we can get the chips out of the way. If they pack the flutes, the cutter breaks.
MRR is now 0.75, much better than the 0.45 of the full slot method. If we simulate, we’ve gone from circa 1:30 to 1:10. In addition, tool life should be much improved.
Many more scenarios could be evaluated. For example, if I don’t have HSM tool paths, I could do this cut in 4 passes with conventional tool paths and run 4575RPM at 28IPM, which helps us past our long tool limitation on feeds and speeds. Four passes with HSM and I can run 8100 rpm at 105 IPM. These are coming in pretty close in MRR terms, so I think I’d be sticking with the 3 pass, 8100 rpm at 80 ipm scenario.
In general, when I want to do a quick pocket, I’ll choose 15% cut width (or stepover if you prefer that term) and as few stepdown passes as possible. There will be cases where it is worth looking at different numbers of passes either 1 more or 1 less usually to see if it gets you better MRR’s.
Like what you read on CNCCookbook?
Join 100,000+ CNC'ers! Get our latest blog posts delivered straight to your email inbox once a week for free. Plus, we’ll give you access to some great CNC reference materials including:
- Our Big List of over 200 CNC Tips and Techniques
- Our Free GCode Programming Basics Course
- And more!
Just enter your name and email address below:
100% Privacy: We will never Spam you!