Using G-Wizard to Calculate Feeds and Speeds for Fly Cutters and other Manual Machining Conundrums

Jan 15, 2012 // by Bob Warfield // Blog, Manual, Software, Techniques // No Comments

This article is the newest chapter from our Feeds and Speeds Cookbook. The original is in the Cookbook here.

I got an email from a customer the other day who wondered if there wasn’t some way to make G-Wizard more focused to the needs of manual machinists. He felt that it was overly “CNC specific”, and wanted some sort of “CNC versus Manual” switch to make it easier. I need to cogitate more on the idea of a switch, but it is certainly true that if you start dialing up modern tooling in G-Wizard and cutting softer materials, you will end up with feeds and speeds that are impossible–the manual machinist just can’t crank the handwheel fast enough.

Let’s back up just for a second and realize a key thing:

The physics are the same for the cutter, whether it’s a manual machine or a CNC machine.

I’m tempted to respond as one famous Starship Chief Engineer did with, “I canna change the laws of physics, Captain!” But, that’s just telling us we need to think about the problem differently: we don’t have to change the laws of physics, we just have to apply them properly.

Take the issue of trying to madly crank the handwheel to hit 100 inches per minute or some other similarly silly thing that G-Wizard may recommend to the manual machinist. First question is, “Why did it recommend that?” And the answer is, unless you keep chipload up, you run the risk of rubbing the cutter. You’ll learn all of this and more in our Feeds and Speeds Cookbook, but let me explain that particular issue.

Consider this diagram:

Too little chipload produces rubbing

Cutter at the top has large chipload relative to radius of cutting edge, so it cleanly slices off chips. Cutter at the bottom has a large cutting edge radius relative to the chipload. It can hardly get under the chip to slice, so it plows, scrapes, and rubs. It may produce a fine finish, but it does so by burnishing. This creates a lot of heat and is very hard on your cutting tools. When G-Wizard asks for a particular feedrate, and it seems too fast, it’s only because it’s trying to get the picture at the top where the cutter slices cleanly.

Okay, so how do we manage feedrate on machines that can’t feed fast enough? Here are some thoughts:

Be sure you tell G-Wizard what your maximum feedrate is–it will limit itself automatically. Let’s try an example. Take a 1/2″ TiAlN 3 flute in 6061, 1/2″ depth of cut, 1/8″ width of cut. Let’s say our spindle will do a maximum of 5500 rpm. We get back a feedrate of 78 IPM and a chipload of 0.0041″. If the spindle would do 10,000 rpm, it jumps up to 142 IPM to maintain the same chipload.

Now let’s say a manual machinist decides they can turn a handwheel twice a second and still be smooth, but that’s the limit on hand cranking. If each turn moves the table 0.100″, we’re moving at 2 * 60 * 0.1 = 12 inches per minute. That’s well short of our goal. If we override G-Wizard’s feedrate on the 5500 rpm spindle to be 12 IPM, we have a chipload of 0.0007″. I try not to let chipload fall below 0.001″ on carbide and maybe 0.0005″ on HSS if I am overriding G-Wizard. Those are just estimates of how low I can go and not get into that edge radius rubbing issue. So this cut is iffy for me.

How can G-Wizard help?

Well, let’s go to the Setup page and create a machine profile better suited to our manual machine:

Setting up a manual mill for G-Wizard

Here’s a Machine Profile suited to a Manual Mill…

I just went in and customized some of the fields to be better suited to a manual mill. I didn’t bother with a lot of it–a manual mill has no toolchanger and we don’t care how fast it accelerates the spindle or which CNC Controller it uses (LOL), those are fields used by the G-Wizard Editor / Simulator. Here are the important points:

- Manual mills usually have a slower spindle rpm, so be sure to set that up. I used 5500 rpm.

- They have lower horsepower and use a spindle taper like R8

- No TSC (through spindle coolant), PCN (programmable coolant nozzle), and if they have flood, it is not strong and might as well be mist.

- Perhaps most important: set the feedrate based on how fast you can crank or how fast your power feed will allow! I used 12 IPM, which is 2 turns a second on a handwheel where 10 turns is an inch.

If we go back to the Feeds and Speeds calculator with that profile, we’ll see that G-Wizard has adjusted to the machine’s capabilities. Our 5500 rpm / 78 IPM cut is now a 3800 rpm / 12 IPM cut. That’s manageable! And, you’ll note the chipload will be 0.0011″. What G-Wizard has done is to try to balance all the factors and get the required feedrate down by slowing the spindle (good for tool life too!) and allowing the recommended 0.004″ chipload to fall as low as 0.0011″.

Fly Cutter Feeds and Speeds

Fly cutters

Fly cutters on a manual mill…

Let’s talk Fly Cutter Feeds and Speeds as long as we’re talking G-Wizard for manual machinists. I get asked about Fly Cutters a lot, there is a lot of traffic to my site on those keywords, and Fly Cutters are very commonly used by manual machinists. While the CNC crowd will more often prefer facemills, even many CNC machinists realize that a very fine surface finish may be better done by fly cutting. Remove all but one insert from your facemill, and finish improves. The exception are those most expensive facemills where you can individually adjust the cutting height of each insert to 0.0001″, because that’s what it takes, and that’s why fly cutters can leave a better finish. Many say their secret weapon for fine aluminum finishing is a fly cutter with a PCD (diamond) insert. But we digress.

How do we set up G-Wizard for a fly cutter?

The writer that prompted me to write this post had the right idea–just tell G-Wizard you’ve got a Facemill with only 1 insert. That’s exactly right. If your fly cutter has a lead angle, the ones pictured both do–the edge is angled, try using the lead angle feature on the Facemill type. If I do all that on G-Wizard, the result is: 1834 rpm @ 12 ipm for a 0.100″ DOC and 1.8″ cut width. That’s not too bad for hogging a surface flat, it’s a half horsepower cut, but there’s way too much chipload for a fine finish. It’s showing 0.0065″ chipload. That’s because it thinks you’ve got a nice facemill with some chunky carbide inserts that can take it. Surface speed is 1440 IPM.

A good manual machinist who wants a great finish on aluminum will grind themselves a razor sharp HSS tool and stick that into the fly cutter. It’ll look something like this:

HSS Fly Cutter Grind

Note the large radius, sharp edge, and steep positive rake on this HSS Fly Cutter tool…

A tool like that will put a beautiful finish on aluminum, but its edge is too delicate for tougher materials or for the carbide feeds and speeds G-Wizard wants to dish up. Let’s adjust for that with the following steps:

1. Bring up an HSS endmill and check out the chipload and surface speed. Chose something about the same scale as the flycutter’s tool. A 1/2″ endmill is fine. I see 400 SFM and maybe 0.003″ chipload.

2. Go back to your Facemill feeds and speeds and try using those figures for SFM and chipload.

3. If finishing, take the chipload down to 0.001″, or even less if you have a razor edge on that tool. The one pictured is knife sharp and I’d be comfortable as low as 0.0006″ or 0.0005″.

With those settings, G-Wizard gives 500 rpm @ 0.36 IPM. To convert that to seconds per handwheel rotation, multiply by 50 and we get one handwheel turn every 18 seconds. That will produce a fine finish indeed with such a cutter.

The 50 is just a rule of thumb that’s close, but a little fast. The real number is 16.67 seconds a turn, but its easier to remember 50. In fact, you can use the field arithmetic in G-Wizard to do the calculation. Just go to the feedrate and type “*50<enter>” and you’ll be looking at the number.

I hope this gives a good idea of how manual machinists can use G-Wizard to good effect!