Dedicated tooling gets down to business

Dedicated tooling gets down to business

With aluminum milling on the rise, jobshops are improving machine productivity, saving money, and maintaining good finishes with tooling made just for aluminum.

With aluminum milling on the rise, jobshops are improving machine productivity, saving money, and maintaining good finishes with tooling made just for aluminum.

The CoroMill 245 45° face mill is the first Sandvik milling cutter that uses dedicated-for-aluminum inserts. Together, they can improve throughput by 30% and edge life more than 50%.

The Sandvik H10 dedicated-for-aluminum milling insert (right) is shown with a carbide insert optimized for cast iron. The chipbreaking geometry on the top face of the H10 is what helps increase productivity.

The pitch of a milling cutter is the distance between the point of one edge to the same point on the next edge. The closer the pitch, the more teeth per cutter, and the more inserts engaged in the cut — thus, the potential for higher feeds.

Off-center advantages in facemilling
With on-centerline milling, the radial cutting forces will fluctuate as the inserts enter and exit the cut, which can cause vibration. Moving the cutter slightly to either side of centerline preloads the spindle in one direction and eliminates this condition. Cutting forces are directed to the centerline of the workpiece, providing optimum average chip thickness.


Aluminum milling is big righ tnow, fueled by increased use in the aerospace, automotive, and computer indus-tries. As a result, milling cutters and inserts are being optimized just for aluminum. These tools remove material faster — without trading off precision and surface finish — than tools that have not been optimized. Optimizing tools for aluminum also betters cutting edge security, tool life predictability, and overall reliability. Shops using optimized tools report that they can machine up to 20,000 rpm, in-crease spindle uptime 25 to 50%, and improve accuracy.

Dedicated-for-aluminum inserts, for example, provide the sharp edges, high positive rake an-gles, and optimized chipbreaking geometries needed for high production and clean, burr-free cuts. Besides these benefits, they cost the same as comparable carbide milling inserts for other materials.

When combined with a dedicated milling cutter, inserts such as Sandvik’s CoroMill 245/H10 let operators run high speeds and feeds on large machining centers, small taper machines, and transfer lines — even at shallow depths of cut. Power require-ments are also lower than with conventional milling tools, and a dedicated-foraluminum insert performs well on magnesium and other lightweight materials, as well as on titanium alloys.

Aluminum machinability
Most aluminum workpieces are wrought or cast, heat or non-heat treatable, and strain-hardenable. Wrought and cast alloys machine better in a tempered condition rather than an annealed one. Their Brinell hardness fluctuates between BNH 60 to 130.

The main alloying elements of these materials are copper, manganese, silicon, magnesium, zinc, and iron. Copper increases strength and improves machinability, while manganese improves ductility and formability for castings. Silicon promotes both corrosion resistance and formability, and magnesium provides strength and also corrosion resistance. Zinc brings strength and castability; iron adds to strength and hardness.

Most aluminum alloys are machine-friendly, generating moderate cutting pressure and low machining temperatures. Milling aluminum requires relatively less horsepower than steel; however, the horsepower needed for high speed machining of soft metals is much greater than currently available in conventional machines.

Up to now, the limiting factors to cutting at high speeds, assuming a machine has adequate horsepower, were the risks of built-up edges (BUE), flank wear, poor surface finish, and loss of chip control. Fortunately, dedicated-for-aluminum inserts minimize those risks.

Insert geometry
In some aluminum alloys, BUE can happen even at relatively high cutting speeds, while flank wear is more prevalent with some silicon-content alloys. Both of these conditions result in poor surface texture and shorter tool life.

Dedicated-foraluminum inserts have a 15° higher rake angle than those of cast iron inserts, which were used previously for aluminum. The sharp, positive rake cutting edge ensures the correct shearing action — thus no buildup on edges — and the tool runs longer.

Chip thickness control is also important in aluminum milling. When running at high speeds, slow feedrates lead to excessive rubbing instead of cutting. This creates thick chips, which can cause overheating, discoloration, and poor tool life.

Typically, chip thickness depends on how a cutter is presented to a workpiece. A 45° lead angle generates a thinner, longer chip, which puts less load on the edge for higher feeds per tooth. The geometry pressed into the optimized-for-aluminum insert's top face then breaks these chips into uniform shapes and sizes. In addition, the insert's more open rake angle provides extra clearance for easier chip evacuation.

Matching the milling cutter
Fitting the dedicated-for-aluminum insert into a positive geometry cutter, such as Sandvik's CoroMill 245, 45° face mill, optimizes the presentation geometry at the cutting edge. Taken together, matched cutter and insert can improve throughput by 30% or more and insert edge life in excess of 50%.

The CoroMill 245 accommodates three separate insert geometries. With the same cutter, applications can range from light cutting for a mirror finish <25 rms to heavy cutting at >50 in. 3 /min. A mere switch of inserts on the same cutter transforms it from an aluminum roughing to a steel finishing tool.

As for accuracy, a self-locating pocket consistently maintains cutting edge position, so users don't have to preset edges after indexing. Indexing repeatability of ±0.0005 in. and cutter repeatability of ±0.0001 in. are now routine.

Edge replacement time is also decreased. Changeouts that once took 10 min or more are now done in seconds — without removing a cutter from a machine. Another timesaver is that the insert mounting screw doesn't need to be removed; rather, it is indexed by turning just two-thirds of the way.

Also, cutters themselves are more dynamically balanced by design. This means high surface cutting speeds, fast material removal, and, generally, no chatter or part distortion.

Tips for machining
The following rules-of-thumb can help users increase productivity and lower part cost. In addition, they can improve tool life, workpiece dimensional accuracy, and surface finish.

First, select the correct cutter body size. Use a cutter diameter 25 to 40% larger than the workpiece width. Doing so will provide the proper entry/exit angle for the cutting edges, longer tool life, and the best dimensional accuracy.

Secondly, equip the cutter with dedicated inserts with high positive rake angles and sharp cutting edges. This optimizes machine settings and the horsepower available to the machine.

Third, select the correct cutter pitch for engaging just the right amount of inserts in a cut. The closer the pitch, the more teeth per cutter, and the faster the feed.

In addition to these tips, one should always program with average chip thickness in mind. This is suggested for ensuring maximum productivity and tool utilization and eliminating problems with finish, vibration, deflection, and noise.

Another important factor is to make sure that the machine and the toolholding are stable. Otherwise, the resulting deflection or vibration can lead to chatter marks on the workpiece. One should also flood a workpiece with plentiful coolant for good chip evacuation.

A way to prolong insert, cutter, and spindle life is by positioning the cutter slightly off-center. This strategy directs cutting forces to the centerline of the workpiece for optimum chip thickness. Additionally, it doesn't expose the spindle to unnecessary loads.

Finally, most tooling suppliers recommend conservative machine settings. Once comfortable with the tooling, a user can increase machining data 20 to 30%. Run each edge approximately 15 min — no more, no less.

Putting tools optimized for aluminum up to the test

A Southern California machine shop needed to increase its aluminum milling productivity. The company evaluated three different milling tools on a 6061 wrought aluminum workpiece.

Originally, the firm used a 3-in.-diameter square-shoulder mill with flat wiper inserts on a Mazak 40-taper milling center. Comparison tests were conducted using a 3-in.-diameter Sandvik CoroMill 245 face mill with H13A carbide inserts optimized for cast iron. The feedrate was set at 220 ipm and 96% load. Next, the procedure was repeated with the CoroMill 245/H10 dedicated-for-aluminum inserts at 320 ipm and 94% load. The results were as follows:

H10 insert CoroMill 245
H13A insert CoroMill 245
Flat wiper insert Square shoulder mill
Cutting speed (sfm)
7,860
7,860
4,000
Machine speed (rpm)
10,008
10,008
5,093
Feed (ipm)
320
220
150
Feed/tooth (in.)
0.0106
0.0055
0.0074
Axial depth of cut (in.)
0.200
0.200
0.200
Radial depth of cut (in.)
2.2500
2.2500
2.2500
Cutting time/component (min)
0.15
0.20
0.32
Total machining cost/component
$0.34
$0.38
$0.57
Total cost/component
$0.14
$0.13
$0.20
No. of edges/insert
4
4
3
No. of inserts/cutter
4
4
4
Insert consumption/year
100
100
133.33

This machine shop increased productivity 29.41% and saved 8.33 hr/shift along with $0.0458/component. The same test (CoroMill 245/H10 insert) at another company showed comparable improvements with less vibration, better surface finish, and longer tool life than the previous non-dedicated tool — despite unstable and weak fixturing.

Aluminum machinability

Aluminum alloy types
Tensile strength/specific
cutting force (k
c) lb/in.
Brinell hardness
Wrought, wrought and coldworked
72,500
60
Wrought, wrought and aged
116,000
100
Cast, non-aging
108,700
75
Cast, cast and aged
130,500
90
Non heat-treatable
108,700
75
Heat treatable
130,500
90
Cast, 13-15% Si
137,700
130
Cast, 16-22% Si
137,700
130
Chip thickness and feed per tooth
Fz (in.)
Ac
0.0016
0.0032
0.004
0.006
0.008
0.012
0.016
0.020
0.024
0.031
0.040
Hm (in.)
1/50
0.0011
0.0015
0.0024
0.0028
0.0031
0.0043
0.0055
1/40
0.0011
0.0011
0.0019
0.0024
0.0031
0.0035
0.0051
0.0062
1/25
0.0011
0.0015
0.0024
0.0031
0.0039
0.0047
0.0062
0.0078
1/20
0.0011
0.0015
0.0028
0.0035
0.0043
0.0051
0.0070
0.0086
1/10
0.0011
0.0019
0.0024
0.0035
0.0047
0.0062
0.0074
0.0098
2/10
0.0011
0.0015
0.0028
0.0035
0.0051
0.0066
0.0086
0.0102
3/10
0.0015
0.0019
0.0031
0.0039
0.0062
0.0082
0.0102
4/10
0.0019
0.0024
0.0035
0.0047
0.0070
0.0090
Hm = Average chip thickness
Fz = Feed per tooth
Ac = Radial depth of cut
diameter of cutter
5/10
0.0011
0.0019
0.0024
0.0039
0.0051
0.0074
0.0098

In face milling, it is often accurate enough to let the feed per tooth (Fz) equal the value of the average chip thickness (Hm). An exception may be when there is a large lead angle. The table shows average chip thickness for a given feed per tooth.

Hide comments

Comments

  • Allowed HTML tags: <em> <strong> <blockquote> <br> <p>

Plain text

  • No HTML tags allowed.
  • Web page addresses and e-mail addresses turn into links automatically.
  • Lines and paragraphs break automatically.
Publish