Show Me How to Improve Speeds and Feeds For

Deciding on Best Depth and Width of Cut When Milling

I got a note recently from a G-Wizard user who wanted to know how to decide on best depth and width of cut when milling. It’s a great question. Most machinists, I suspect, use rules of thumb and habit more than anything else unless the situation dictates something in particular based on the dimensions of the feature being machined. They’re used to using some fraction of the cutter’s diameter or some figure that they got to some other way through habit (40 thousandths or some such is what they’ve always used). Perhaps their CAM program has a hardwired default that is a percentage of the cutter’s diameter.

But these values, while they have worked over time, are not necessarily optimal figures with respect to material removal rates, tool deflection allowances, or a host of other variables we might choose to consider. What’s a more systematic way to approach the problem?

First thing is we have two variables (width and depth of cut), so it’s hard to make progress unless we can nail one of the two variables down and focus on the relationship of the other. It’s usually pretty easy to nail down one of the variables based on the situation. Let’s divide our work into two categories:

– Slotting: I’ll generalize this to be any situation where the material to be removed is very close to the cutter’s diameter. It may be a slot, or it may involve interpolating a hole or pocket that’s only a little bit larger than the endmill’s diameter.

– Pocketing: Here again, I will generalize this to be any situation where the cutter’s diameter is quite a bit smaller than the dimensions of the material to be removed. That doesn’t mean there isn’t some inside radius or other feature that isn’t more like the slotting example, but for the most part, we have some room to work in. Note that profiling will be considered to be the same as pocketing for this discussion.

Okay, so now we have to take the task before us and decide whether it is closer to slotting or pocketing. The reason I’ve defined these two the way I have is that it informs our choice of which variable to work on first. If we are slotting, the cutting width is the first variable. If we are pocketing, the cutting depth is the first variable. Why?

When slotting, the feature is very close to the cutter’s diameter in size. We can’t take a 1/2″ endmill and use it to make a 1/4″ slot. In general, we want to use the largest diameter endmill that fits the feature, and then we pretty much have to make at least one cut that is full width. Once we’re cleared that cut, anything remaining is handled the way we would under pocketing. So, when slotting, we focus first on cut width and make that the cutter’s width to get started.

When pocketing, our limitation will be the smallest inside radius we have to deal with as well as the depth of the pocket. Remember, it may be advantageous to make two passes. The first with a cutter that has a diameter too large for the smallest inside radii we have to deal with. That’s a roughing pass that uses a larger cutter just to get done faster. The second pass is a finishing pass, and must use a cutter whose diameter is less than or equal to that required to reach into the smallest internal radius the pocket holds. Note that we can go around an outside radius (a boss) with any diameter cutter, it is the inside radius that limits us.

So, we pick a cutter that is either as big as the smallest radius, or we choose to go two passes and go with a larger cutter. Let’s leave the two pass issue aside for the moment, because figuring out when that is optimal can take a bit of trial and error. Its similar to think of one pass. Given that the cutter is chosen, we can choose just about any width of cut we want. So how do we nail down a variable when pocketing? On the slotting case, I like to nail down cut width. On the pocketing case, I prefer to nail down cut depth.

In general, we get a nicer finish if we cut the pocket in as few layers as possible. CAM programs are good at layering down into the pocket, so we can pick arbitrary depths of cut. If I can, I like to do it in one layer for a pocket that isn’t two deep. If not, I prefer the depths of the layers to be equal. In other words, I wouldn’t go down 1/4″, 1/4″, and then 0.19″ on the third layer. So pick a layer depth that satisfies that criterion.

Now, in both cases we have locked one of the two variables–slotting locks width, pocketing locks depth. We need to determine the best value for the variable we left floating based on the value of the one we locked. This is where the G-Wizard Cut Optimizer makes it easy. Enter the values you know for the cut and let the Optimizer figure the value for the floating variable.

For example, let’s suppose we need to cut a pocket that is 3/4″ deep in 6061 aluminum. The smallest internal radius is 1/4″, so we’ve decided to use a 1/4″ 3 flute carbide endmill. Here is the problem set up in G-Wizard:

Material, Tool, Tool Diameter, Flutes, and 3/4″ Cut Depth Entered…

Now we can invoke the Cut Optimizer just by pressing the “Rough” button:

As you can see from the red arrows I added, for a 3/4″ depth of cut, this endmill can handle no more than 0.1799″ width of cut when roughing. Let’s round that down and go with 0.170″

Press the finish button to see what sort of finish allowance we should have the CAM leave for our finish path and we get 0.0052″. That’s a pretty light pass, but 3/4″ is deep for this 1/4″ endmill. Here’s an interesting thought: if we reduce tool holder to tip length to 0.9″ instead of 1″, we can increase that cut to 0.0095″. That gives you an idea of how important it is to keep the tool stick out as little as possible. I’d be inclined to go with choking up on the tool and a finish width of cut of 0.009″ were this my job. The other thing to consider is two levels of finish pass. If we don’t mind taking two levels and still choke up on the tool, we can get 0.015″ width of cut for the finish. That’s about as much as I like to take on a finish pass.

The problem with this cut is its a little bit deep for our 1/4″ endmill. That’s a 3:1 ratio of diameter to depth. We can tell its straining because the max recommended widths of cut are so light. If I had a CAM program that made it easy to make the roughing pass with a bigger cutter, I would be tempted to jump in with a 1/2″ endmill (or maybe even larger) for the roughing pass and then go to the 1/4″ for finishing, but you get the idea.

The slotting case is pretty similar, except for that case, instead of trying to compute the width of cut, we want to use the optimizer to figure out the depth. For example, if we continue with our 1/4″ 3 flute, let’s say we need to cut a slot 0.300″ wide to a depth of 3/4″. Our plan is to cut a full slot 0.250″ wide down the middle, and then finish it up by cutting the remainder on each side. How deep can we make our full slot passes? Once again, dial up the initial parameters, and this time, hit the “Slot” button. For roughing, the Cut Optimizer tells us we can cut to a depth of 0.3466″ before we get too much deflection. Two passes at that depth will get us to 0.6932″ deep. That leaves 0.0568″ on the bottom for us to finish and 0.0259″ on either side for the finish pass. Remember, we’re not cutting a full slot for the finish pass, so we treat it just like we did our pocket to figure out the width and depth of cut.

That’s all there is to it. To summarize:

1. Decide whether you are slotting or pocketing.

2. When slotting, pick a value for width, and use Cut Optimizer to decide depth.

3. When pocketing, pick a value for depth, and use Cut Optimizer to decide the width.

If you approach the problem this way, you’ll maximize your MRR’s while minimizing your tool deflection as appropriate for either roughing or finishing. That’s a much more optimal approach than the old wet finger in the wind!

For more thoughts on cutting parameters when milling, check out the Milling Surface Finish page.

 

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:

Full Name
Email *
100% Privacy: We will never Spam you!

Rate this post