CNCCookbook: Software and Information for Macihnists

Free CNC Software

G-Wizard G-Wizard G-Code Editor

 

 

The Smart Machinist's Ultimate Feeds and Speeds Tool

 

Get a Second Opinion on Your G-Code

 

{PageNav}

G-Wizard Machinist's Calculator

Feeds and Speeds Cookbook

Chip Thinning, Lead Angles, and Ballnose Compensation

Getting the right feeds and speeds is essential to producing good results efficiently with machine tools, but it's not particularly easy to optimize feeds and speeds. There are basic formulas and rules of thumb that the majority of machinist's go by. For any material and cutter combination, you can look up the recommended Surface Speed (SFM, or Surface Feet per Minute and SMM or Surface Meters per Minute) and Chipload (inches of cut per tooth of the cutter). Various simple formulas then yield a recommended spindle rpm so as not to exceed the recommended SFM and a recommended feedrate to deliver the chipload to the cutter teeth. Easy, right?

Not so fast!

Would you believe that especially for light cuts, the basic math combined with SFM and chipload tables often gives results that are wrong and radically increase the wear on your tools?

The reason is that there is more going on here than meets the eye. For example, if I poke around various endmill manufacturer's literature in search of speeds and feeds for steel, I can get to a page like this one from Niagara cutter. First thing to note is that the recommended chiploads and SFM vary depending on the exact operation being performed, and in particular, the depths of cuts. If you're just using the basic shop math around SFM and chipload, no such compensation is available. I have built compensation like this into my G-Wizard Machinist's Calculator, but trust me, it isn't so easy just to do it by hand. You'll be constantly referring to pages like this.

OK, so let's say we're going to do some peripheral (edge) milling to profile a part made out of mild steel using a 1/2" uncoated HSS 4 flute endmill. We plan to take fairly shallow finishing quality cuts of 5% of the cutter diameter. Further, let's do a pretty deep cut axially, a full cutter diameter of 1/2". So if I am profiling a 1" high part, I can make a full pass by going around twice and cutting 1/2" each time.

What feeds and speeds should we use?

The Niagara page says for cuts less than 1/16 of a diameter (5% is 1/20), we want 210 SFM and a chipload of 0.0035. If I plug all that into G-Wizard, but ignore the chip thinning, I get the following results:

Radial Depth Ratio of 5% = 0.015" depth of cut

210 SFM and 0.0035 chipload gives us 22.46 IPM feedrate and a 1600 rpm spindle speed.

Is that the right speeds and feeds?

Yes and no. It's certainly what the majority of folks would use. In fact, they might even be less aggressive than that.

Let's see what G-Wizard would suggest by default and why:

For the same depth of cut and cutter, G-Wizard wants a little slower SFM of 160, and a little less aggressive chipload at 0.003.

The spindle speed works out to be 1200 rpm due to the lower SFM, but the feedrate is now 84.69 IPM!

How can we go so fast?!??

The answer lies in chip thinning. Because we're taking such a shallow cut, you have to speed up the feedrate just to get to the same chipload as on a much heavier cut. In fact, any time you cut less than half the tool's diameter radially (i.e. when viewed looking straight down the spindle axis), your chips will be thinner than expected.

It's easy to understand the geometry that leads to chip thinning:

The blue chip is a shallower cut. Note how thin it is at its widest compared to the red chip from a deeper cut...

The blue chip represents a very shallow cut, and the red chip a deeper cut. Note how thin the blue chip is at its widest compared to the red chip from a deeper cut. You can see that the chip gets thicker all the way up to the point where we've buried the cutter to 1/2 its diameter. That's the thickest point.

Chip thinning simply answers the question, "How much faster do we have to go so the maximum width of the blue chip is the recommended chipload?"

The differences in required feedrate can be quite substantial. In this case, we needed to be going almost 85 IPM instead of 22.5 IPM, over 3x as fast. And remember, this isn't some hot rod feedrate that is guaranteed to wear out your cutters before the even finish the first pass. This is the speed you need to reach to get the chipload you thought you had already chosen.

Here is my IH Mill running at 35 IPM in steel due to chip thinning:

Note how quiet the cut is--the gearhead on the mill makes more noise than this cut. I could go quite a bit faster too, this isn't the full rate specified by G-Wizard, but it is quite a bit more than what the basic Niagara numbers would have called for. The finish came out extremely nice, with no visible burrs or other blemishes. A little buffer time and I could have had a mirror finish if I'd liked.

You can see where this kind of circular geometry affects a lot of different cutter combinations. We talked about peripheral (edge) milling first. But it's a function of surfacing too, which is mostly about edge cutting down at the tip of the mill. There is no impact on plunge cutting where we move straight down. Surfacing with a big face mill or a fly cutter is impacted, however.

How about button cutters, or as they are sometimes called toroidal cutters? These are indexable face mills and endmills that use round inserts. The diagram above shows the same effect, its just that instead of the spindle axis coming right out of the screen, it goes straight up. So we want to run chip thinning calculations for them too. Running one without chip thinning may account for why so many people find them to be gentle cutters--they're taking a lot less cut than they expect.

How about lead angles? Some facemills cut a 90 degree shoulder, others may cut a 45 degree or other angle. Similar geometric effects apply, and there is compensation needed for lead angle that G-Wizard also builds in.

Ballnosed cutters are another problem child when you try to use the most basic speed and feed calculations. In this case, it isn't just the feedrates that have to be considered, it's also the spindle rpm. If we are running a 1/2" ballnosed endmill, and we are profiling, with a depth of cut of 0.040", the cutter is only 0.040" down into the cut. The effective diameter of the cutter is no longer 1/2". The diameter of the ball at the top of the cut is actually 0.2713", so we need to spin the cutter faster--about 1800 rpm instead of the 1200 rpm we had been using with a regular cylindrical endmill.

These are all forms of compensation that affect the feeds and speeds of your cutters quite a lot. I've built all of them into G-Wizard so I can quit worrying about it. The math to do it is available on the web if you Google for it, or you can just use a calculator like G-Wizard to figure it out for you. There are several of them out there. Some CAM programs do this kind of compensation as well.

How Much Feed is Too Little Feed?

Now here is the dark side of chip thinning and similar compensation: it isn't just about going faster, it's about tool life. Amazingly, just when you think you're really babying your cutters by reducing the feedrate and taking light cuts, you're actually giving them the worst possible treatment. Surface finish may improve (because the tool is essentially burnishing the workpiece), but tool life will go way down. Consider a magnified view of your cutting edge versus the material:

Cutter edge radius centerline travels along the yellow lines. If the radius is too large relative to the depth of cut (bottom), all the force goes to pushing the chip under the edge. This is the "rubbing" effect you'll hear talked about when feedrate and hence chipload are too low. Use a calculator like G-Wizard that has radial chip thinning to avoid this problem.

Tool manufacturers will tell you that too little feed is just as bad for tool life as too much feed (or too much spindle rpm). But how little is too little? That part is seemingly hard to find out. I went fishing around with Google to try to find what speeds and feeds result in a "burnishing" effect with tools. Here is what I found:

- Article on hard milling: 0.0008" per tooth is definitely burnishing because it is "less than the edge hone typically applied to the insert."

- De-Classified 1961 Batelle Institute report on aerospacing machining of super-alloys says an IPR greater than 0.0035 will result in burnishing and likely work hardening of these alloys. Interesting how well this number agrees with the one above for a 4 flute cutter. 8 tenths times four would be 32 tenths.

- Kennametal says the "highest possible feed per tooth will usually provide longer tool life. However, excessive feeds may overload the tool and cause the cutting edges to chip or break." So feed as fast as you can until you start to chip or break edges. They reiterate this under work hardening. One wonders whether rubbing leading to work hardening isn't the principal risk of cutting with too-low chiploads with respect to tool life in susceptible materials.

- Another reference, like the first, to keeping chiploads higher than tool edge radius. In this case, IPT should be greater than 0.001". This is once again an article on hard machining where work hardening may be a factor.

- Minimum chip thickness is 5-20% of the cutting edge radius. Below that level, chips will not form and the cutter will "plow" across the workpiece causing plastic deformation and considerable heat.

- Ingersoll says that as a general rule carbide chiploads should not be less than 0.004" or you run the risk of rubbing which reduces tool life and causes chatter.

I take away two things:

1. If you cut too little, you run the risk of work hardening if your material is susceptible to it. That will wreck your tool life if you are over-stimulating work hardening.

2. If chip thinning and other effects leave you cutting much less than the cutting edge radius, you're rubbing and not making clean chips. That will heat the tool and material and drastically reduce tool life.

Figuring out the work hardening part is easy. If your material is susceptible, keep the chipload up. Figuring out the whole cutting radius issue is harder. Most of the time we don't know what the cutting radius is. I'm not talking about tip radius on a lathe tool, for example. I'm talking about the actual radius of the sharp edge. In other words, the smaller the radius, the sharper the tool. A lot of carbide inserts are pretty blunt. A chipload of less than 0.001" may very well be too little. Modern tools for aluminum are often much sharper, and can take less chipload. In general, indexable tools are usually less sharp than endmills, so they need higher chiploads.

It's ironic that just when you think you are taking it easy on a cutter with a very light cut, you may be doing the most damage of all due to rubbing.

Why chance it though? Use a calculator like G-Wizard to figure out how to deliver the manufacturer's recommended chipload by increasing the feedrates. Not only will the job go faster but your tooling will last longer.

 

 

 

 

 

 

Home      

 

Software

  GW Calculator

  GW Editor

  Gearotic

  Conversational     

  Deals and Steals

Blog

  Software

  Techniques

  Beginner

  Cool

  Projects

  Webinars

 

 

Cookbooks

     Feeds and Speeds

     G-Code Tutorial

     CNC Machining & Manufacturing

     Lean Manufacturing

     Cost Estimating Software

     DIY CNC Cookbook

     CNC Dictionary

 

CNC Projects

Machines

     CNC Mill Retrofit

     Plasma Table

     Welding

      3D Printers

     

Resources

     Machinist's Search

     Videos

     Online Groups

     Individuals

     Reference Data

     Books

     Suppliers

     Tool Brands

Workshop

     Hall of Fame

 

About

     Support

     Customers

     Partners

     Our History

     Cheapskate Page

     Privacy Policy

 
All material © 2010-2014, CNCCookbook, Inc.