Face Milling Basics
What is Face Milling? Think of milling with the side of an end mill. The general term for that is “peripheral milling”. Now, what if we cut strictly with the bottom? Technically, that’s face milling, though we typically only refer to it as face milling when we are using special milling cutters called “Face Mills” or “Shell Mills”. Note that there is literally no difference between face mills and shell mills. You may also hear “Face Milling” referred to as “Surfacing”.
If you’re on a CNC Router, a very common operation is “Spoilboard Surfacing“, and while the router crowd likes to call the milling cutters used for Spoilboard Surfacing “Spoilboard Cutters”, they’re just another form of Face Mill.
Let’s start by choosing the best type of Face Milling Cutter for your Face Milling needs. The biggest differences between Face Milling Cutters are:
- Cutter Diameter: Face Mills are available in large and small Cutter Diameter sizes. Determine cutter diameter so that cutting speed (feed rate) and spindle speed lie within your machine’s capabilities as does the horsepower requirement of the cut. You’ll get the best finish if your cutter’s maximum cutting diameter is larger than the area you are Facing. But, larger cutters require more powerful spindles and don’t always fit into tighter places.
- Number of Inserts: The more inserts, the more cutting edges, and the faster you can feed a Face Mill. Higher cutting speed means the job gets done sooner. A Face Mill with only one insert is called a Fly Cutter. But faster isn’t always better. Unless you can adjust the individual height of all the inserts, your multiple cutting edges Face Milling Tool won’t have as smooth a finish as a single insert Fly Cutter. In general, the number of inserts will be higher for larger cutter diameters.
- Geometry: This is determined by the shape of the insert as well as how it is held in the Face Mill.
Let’s look at that geometry issue more closely.
Choose the Best Face Mill: 45 or 90 Degree?
45 or 90 Degree Face Mill – Which gives better results for face milling operations?
First, what are we talking about when we say 45 or 90 degrees? The answer is fairly obvious from the photo above comparing two Glacern cutters. Take a look at the angle of the cutting edge on the inserts.
Yes! The angle is the angle of that cutting edge–45 degrees for the cutter on the left and 90 degrees for the one on the right. That angle is also called the lead angle of the cutter.
And here are the optimal operating ranges for different shell mill geometries:
By the way, round insert cutters are also called “Button Cutters”. We have an entire article about Button Cutters if you’re interested.
So which one will give better results for face milling operations?
Of course if you can afford it, it’s great to have both 45 and 90 degree face milling tools, but what are the pros and cons for each?
Pros and Cons
- Cutting forces are better balanced so that axial and radial forces are about even. Lowering the radial forces so they’re more balanced with axial can not only enhance the surface finish, it’s also kinder to your spindle bearings.
- Cut entry and exit are better behaved–less shock, less tendency to break out.
- The 45 degree cutting edge is better for demanding cuts.
- Better surface finish–the 45’s leave a noticeably nicer finish. Lower vibration, balanced forces, and better entry geometry are three reasons.
- The chip thinning effect is at work and leads to higher feed rates. A higher cutting speed means higher material removal rates and the job gets done sooner.
- The 45’s tend to have less tendency to chatter as well.
There are also some disadvantages to 45 degree face mills:
- Reduced max depth of cut due to lead angle.
- Larger body diameter can cause clearance problems.
- No 90-degree corner or shoulder milling
- Can cause chipping or burring on the exit side of the cutter rotation.
- The 90 degree version exerts less sideways (axial) force, about half as much. This can give it an advantage where thin walls are concerned because transferring too much force into the wall can lead to material chatter and other problems. It can also be an advantage when it is hard to impossible to hold the part securely in a fixture.
And lest we forget button cutters, they combine some of the advantages of each plus they are also the strongest. So if you have to deal with nasty materials, a button cutter might be your best choice.
If you’re primarily after a great finish, then you probably want a fly cutter. The lowly fly cutter gives the best finish in most cases. BTW, you can easily convert any face milling tool to a fine fly cutter by simply removing all but one cutting edge.
Face Mill Speeds and Feeds
It’s easy to compute Feeds and Speeds to compare these two face milling solutions using our G-Wizard Calculator software (click the link for a free 30-day trial if you’ve never played with G-Wizard).
Here’s a typical cut set up for 90 degree Face Mills / Shell Mills:
G-Wizard set up for a 90 degree face mill…
I selected my machine, workpiece material, and indexable tool type. I’m modeling a smallish 2″ diameter face mill with 4 inserts, and I have set the Lead Angle to be 90 degrees. My Cut Depth is 1/8″.
I did do a couple of jazzy things. First, I’m doing a 60 percent width pass. This will give a better finish and go easier on the inserts in tough materials than a full width pass. Second, I have specified this as an HSM cut. That’s HSM for “High Speed Machining.”
I can do that since I will use a toolpath that arcs gently into the cut and I will arc the end of each pass to avoid a sharp corner and also to avoid completely leaving the cut. Those are CAM toolpath tricks that can really help you out on tool life, surface finish, and in this case, they let you opt for a big increase in feeds and speeds too. If your CAM won’t do those things the Conversational CNC Face Milling Wizard in G-Wizard Editor will do them very easily.
Now, we can check out the 45 degree face mill / shell mill just by changing the lead angle to 45. Let’s assume every thing else stays the same, here are the results:
G-Wizard for a similar 45 degree face mill…
Wow! Check out that Material Removal Rate:
- 57 cubic inches a minute for the 90 degree
- 80 cubic inches a minute for the 45 degree
Now we see why the 45 degree models are so popular–that’s more than 40% more material removed. That’s definitely going to pay for the new face mill pretty quickly if you’re using it for very many parts.
Note that it’s all down to the increased cutting speed (feed rate) possible with the 45 degree lead angle.
Alternatives to 45 Degree Face Mills: Octagonal, 75 Degree, and Button Cutters
At one time, octagonal face mills were at war with the 45 degree face mills for supremacy. The octagonal inserts have more edges, so you can rotate the insert if one gets chipped. But, tooling costs are usually only about 3 percent of the manufacturing cost, so the greater efficiency of the 45’s eventually won out.
Lately, you can get some face mills that use a 45 degree insert that’s double sided, so we have the best of both worlds since these inserts now have 8 edges like the octagonal inserts.
Other alternatives include 75 Degree Face Mills and Button Cutters (Round Insert Indexable Mills). The 75 Degree Face Mill’s primary purpose seems to be providing just a bit more clearance than the 45 degree can. It might be your 3rd or 4th choice if you already have a 45 and 90 and want more options for difficult cases.
The Button Cutter (also called a Copy Mill or Toroidal Cutter) uses a round insert and has many advantages of its own. Tough to call a winner with a Button Cutter versus these other Face mills, so click through and see about Button Cutters in their own right.
More Face Milling Tips and Techniques
Here’s a 45 degree lead facemill slogging right through a weld–they are a little tougher than 90 degree face mills!
If there’s a slot or other recessed feature in the surface you’re Face Milling, you’re going to be doing some interrupted cuts. This is hard on the inserts, so if you’re dealing with a tough material, you may want to reduce the feedrate up to 50%.
Try to roll into the cut with an arc. It will improve your finish as well as your insert life. More toolpath ideas here.
Use of Wiper Inserts can greatly improve the surface finish when Face Milling. High feed rates and low depth of cut (0.8mm or less) will facilitate this. PVD (diamond) inserts with very sharp edges can also improve your surface finish.
You can get a face miling cutter in a wide range of cutter diameter. What you want to do is balance 2 factors. First, the bigger the better. It will take fewer passes, and ideally maybe even a single pass, which is best for surface finish. Number two is the counter point to number one. You must respect the horsepower and rpm limits of your machine. The bigger the cutter diameter, the more power it takes. I will also add that spindle speed can be a limiting factor. In general, larger cutter diameter cutters have to spin at lower rpms, while smaller cutter diameters can spin at higher rpms.
Can I Use An End Mill for Surfacing?
Of course you can use end mills for surfacing, but it is seldom optimal to use an end mill. There are two major problems using end mills. First, end mills are generally smaller in diameter. This means it will take many more passes to do the job and all those passes will leave that many more marks on the work. The end result is end mills will take longer and they will have a much less fine surface finish. Second, solid end mills are more expensive than indexable tooling.
I keep a 2″ diameter 90 degree facemill in my shop as well as a 3″ Glacern FM45 45 degree face mill. The FM45 sees a lot more use for sure.
One last thought about face mills–they’re horsepower hogs. Don’t try to use too large a face mill on your machine. I’ve stalled the 3 horsepower spindle of my mill running my 3″ pretty easily. Granted, it’s a smaller mill, but you need to keep in mind even if you have plenty of spindle power that the face mill is going to transfer a whole lot of it into your workpiece. Make sure it’s clamped down tight!
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!
Recently updated on November 16th, 2023 at 03:40 pm
Bob is responsible for the development and implementation of the popular G-Wizard CNC Software. Bob is also the founder of CNCCookbook, the largest CNC-related blog on the Internet.