1. 3.0 - CNC tools

2. Lesson overview 3.1 End Mills 3.2 Face Mill 3.3 Corner Radius Tool
3.4 Slot Mill/Slotting Saw
3.5 Hole Making Tools
3.6 Cutting Tool Fundamentals
3.7 Cutting Speeds & Feeds Formulas
3.8 Speed/Feed Examples
3.9 Cutting Data & Best Practice Parameters

3. objectives List most commonly used CNC tools.
Determine spindle rotational direction.
Interpret a chip formation diagram.
Define chip load.
Distinguish between Climb and Conventional milling.
Compute cutting speeds and feeds for a specified tool, material and operation.

4. Overview Many cutting tool types/shapes/sizes.
Tools Used in this Course
End Mill
Face Mill
Corner Round
Slot Mill
Spot/Center Drill
Twist Drill
Tap
Reamer
Many cutting tool types/shapes/sizes.
Few types needed for most CNC parts.
Most often used listed to right.
Tip: If possible acquire a tool catalog from a supplier.
Other good sources:
Company
Web Address
McMaster-Carr
MSC Industrial Supply
Sandvik
Valenite

5. 3.1 - End mills
End Mills are the primary cutting tool used in CNC milling.
Many different:
Shapes
Sizes
Geometric configurations
Materials
Convex
Radius
Corner
Rounding
End Mill
Tapered
End Mill
Roughing
End Mill
Ball Nose
End Mill
Chamfer
Mill
Concave
Radius
Lollipop
Carbide Insert
Face Mill

6. 3.1 - End mills: Nose types

7. End mills: Nose Types/applications
Flat Nose:
2D contours and pockets.
Bull Nose:
Fillets and 3D roughing.
Ball Nose:
3D rough and finishing.
Chamfer
De-burr or chamfer edges.

8. End mill: number of cutting flutes
Four flutes.
Rigid.
Higher feed rates than 2 or 3 flute (see Feed Formula).
Two flutes.
More chip clearance (room for chip to be ejected).
Three flutes.
Less common, but good compromise.

9. End mills: center cutting
Center cutting: Cutting edges extend across center of tool (see cutting end view below).
Non-center cutting: Relief hole in center.

10. End mills: center cutting
Only center cutting end mills can plunge straight down through material.
Non-center cutting must be ramp, spiral, or drop through existing hole.

11. 3.2 - Face mill Very high material removal rate.
High initial cost (tool body).
Carbide inserts can be replaced when worn.
Do not use coolant:
Environmental. Cleaner. Lower maintenance.

12. 3.3 - Corner round
Use to machine fillet on outside corners of part.

13. 3.4 - Slot mill Includes: Side milling cutters. Slitting saws.
Woodruff keyset cutters.

14. 3.5 Hole making Tools Center drills Countersink Drills
Drill Point Countersink
Twist Drills (Jobber Length)
Stub-Length Drill
Taps-Spiral Point (Gun Tap)
Taps-Bottoming
Reamer
Counterbore
Center
Drill
Drill Point
Countersink
Countersink
Drill
Twist Drill
(Jobber Length)
Reamer
Stub Length
Drill
Spiral Point Tap
(Gun Tap)
Bottoming
Tap

15. 3.5 - Center & Countersink Drills
Center drills:
Short, very rigid.
Used to put conic on part.
Prevents subsequent twist drill wobble.
Ensures hole will be located precisely.
Countersink drills:
Create conical face for flush machine screws.
Drill Point Countersink (Combined Spotting + Countersink):
Create both screw clearance hole and C’sink.

16. Center & Countersink Drills
Many different sizes and tip angles:
C’sink tip angle = machine screw tip angle (60, 82, 100, 110, 120 degrees).
C’sink body diameter > screw head diameter.

17. Twist drill Tip angle usually 118 degrees.
Long drills will wobble before piercing part surface.
Spot drill first to create conic.

18. Taps Cutting: Form tap: Bottoming: Spiral Point.
Create thread by removing material.
Form tap:
Create thread by displacing material.
Preferred, especially for plastics and aluminum.
Bottoming:
For blind (not through) holes.
Spiral Point.
Best for through holes.

19. Rigid Tapping Rigid tapping:
CNC Machine can grip tap in rigid (not floating) holder.
Spindle reverses to retract tap.

20. Reamer Used to finish holes that require precise size.
Examples: ground pins and bushings (+/ typical).
Machining parameters must be correct to achieve high precision, including:
Cutting speed.
Cutting feed.
Material to remove (Stock allowance).
See Cutting Data and Best Practices, Chapter 4.

21. Reamer
Chamfer on end of reamer helps it get started and centered in hole.

22. Counterbore (About) Looks like an end mill with “pilot” in center.
Used to spot face holes for cap screws.
Centers spot face on hole.
Not often used on CNC machines.
Use End Mill and either Drill or Circular Pocket instead.

23. 3.6 Cutting Tool fundamentals
Rotational direction.
Chip formation diagram.
Chip load.
Climb vs. Conventional Milling.

24. Rotational direction
Most CNC Tools cut when rotating Clockwise (view looking down from machine spindle).

25. Chip formation Tools cut using a shearing action.
Cutting flute produces a chip that is ejected away from part.

26. Chip load
The (max) thickness of material removed by each sweep of each cutting flute across the part (typically: in).

27. Climb vs. conventional milling
Climb Milling: Tool begins at max chip thickness and ends with minimum.
Conventional Milling: Tool begins at min chip thickness and ends with max.

28. conventional milling Creates excessive heat increasing tool wear.
Rakes chips across surface leaving poor finish.
Not used often on CNC (mostly on Manual mills).

29. Climb milling Reduces heat and tool wear. Reduces horsepower used.
Better surface finish.
Use unless material requires otherwise.

30. Tips
Never use a cutting tool to machine plastic that has cut any metal.
Machining metal compromises the sharp edge of the tool and will produce poor results in plastic.
A good practice is to keep 2 sets of tools, one for plastic and the other for metal.
High speed steel cutter work best for plastic.
Carbide cutters work best for metals.

31. 3.7 cutting speeds and Feeds
Speeds and feed definition.
Resources.
Speed formula.
Feed formula.
Tapping feed rate calculation.

32. Speeds and feeds definitions
Speed = Rotational velocity of tool.
Revolutions per minute (RPM).
Feed = How fast tool moves through material.
Inches per minute (IPM) or
Millimeters per minute (mm/min)
Selection based primarily on tool, material, and machining operation.

33. Speeds and feeds resources
Tool supplier/salesman.
Tool maker web site.
Tooling catalogs.
CAD/CAM software.

34. Speeds and feeds resources
Based on many variables including:
Setup rigidity.
Quality of CNC machine.
Capabilities of CNC machine.
Material variation.
Even the best speeds and feeds data is a “scientific guess”.
Often adjusted at machine based on actual conditions (chip formation, sound, etc).

35. Speed formula–where it comes from
Derived from a formula that relates rotational velocity of tool with flute speed for a given tool diameter.
Do not memorize this formula. It is there so you can see how the simpler formula is derived. The complete step-by-step derivation is in the reading assignment.

36. Speed formula – derived version
Dia = Tool Diameter (in)
3.82 = Constant
SFM = Speed (ft/min) at which material moves past cutting edge
Get from reference tables, CAD/CAM or other resources.

37. Feed formula Feed (in/min) = rate tool advances through material.
CL (in) = Chip Load: Amount of material removed by each pass of a cutting flute.
NumFlutes = Number of cutting flutes of tool (for drill, use 1).

38. Tap feed formula Feed = Linear (plunge) feed rate of tap.
Based on cutting speed and Threads Per Inch (TPI) of tap.
Example: ¼-20 tap = 20 TPI
Feed = Linear (plunge) feed rate of tap.
Speed = Cutting speed (from Speed formula).
TPI = Threads Per Inch

39. 3.8 Milling speed/feed examples
Calculate the cutting speed and feed for a milling operation given the following parameters.
Parameter
Value
Tool Diameter
.500in
NumFlutes 4
SFM
600ft/min
IPR
.005in

40. Milling speed/feed example – step 1
Calculate Speed (RPM).
Where:
Speed (rev/min)
SFM (ft/min) = 600
3.82 = Constant
Dia (in) = .500
Solution:
a. Speed = [(SFM x 3.82) / Dia]
b. Speed (rev/min) = [(600 x 3.82) / .500]
c. Speed (rev/min) = 4584 RPM
Note: Always round off Speeds to the nearest integer.

41. Milling speed/feed example – step 2
Use Speed from previous formula to help calculate Feed.
Where:
Speed = 4584 (rev/min)
Chip Load = .005in
NumFlutes = 4
Solution:
a. Feed = Speed x Chip Load x NumFlutes
b. Feed = 4584 x .005 x 4
c. Feed = 91 in/min
Note: Round off milling feeds to nearest integer value.

42. Drilling speed/feed example
Calculate the cutting speed and feed for a drilling operation given the following parameters.
Parameter
Value
Tool Diameter
.201in
SFM
250ft/min
IPR
.002in

43. Drilling speed/feed example – step 1
Calculate Speed (RPM).
Same formula as mill but different data.
Where:
SFM = 250 (ft/min)
3.82 = Constant
Dia = .201 (#7 Drill)
Solution:
a. Speed = [(SFM x 3.82) / Dia]
b. Speed (rev/min) = [(250 x 3.82) / .201]
c. Speed (rev/min) = 4751 RPM

44. Drilling speed/feed example – step 2
Use Speed from previous formula to help calculate Feed.
Where:
Speed = 4751 (rev/min)
Chip Load = .002in/rev
NumFlutes = 9.5
Solution:
a. Feed = Speed x Chip Load x NumFlutes
b. Feed = 4751 x .002 x 1
c. Feed = 9.5 in/min
Note: Round off milling feeds to first decimal point.

45. Tap speed/feed example
Calculate the cutting speed and feed for a tapping operation given the following parameters (1/4 – 20 tap).
Parameter
Value
Tool Diameter
.25in
SFM
100ft/min
TPI (Threads per Inch) 24

46. Tap speed/feed example – step 1
Calculate Speed (RPM).
Where:
SFM = 100 (ft/min)
3.82 = Constant
Dia = .250 )
Solution:
a. Speed = [(SFM x 3.82) / Dia]
b. Speed (rev/min) = [(100 x 3.82) / .250]
c. Speed (rev/min) = 1528 RPM

47. Tap speed/feed example – step 2
Calculate Feed (IPM.
Where:
Speed = 1528 (rev/min)
TPI = 24 (threads/in)
Solution:
a. Feed = Speed / TPI
b. Feed = 1528 / 24
c. Feed = in/min
Note: Round off tapping feeds to three decimal points.

48. What if speed exceeds max spindle rpm?
In cases were the calculated RPM exceeds the maximum spindle speed capability of the machine:
Substitute max spindle speed for Speed value.
Use max spindle speed in Feed calculation.

49. 3.9 Cutting data Mill Cutting Speeds (SFM) surface ft/min Material HSS
Carbide
Aluminum
600
800
Brass
175
Delrin
400
Polycarbonate
300
500
Stainless Steel 303) 80
Steel (4140) 70
350
Cutting Feeds (IPR) in/rev
Operation
Tool Diameter Range (in)
<.125
.25-.5
.5-1.
>1.
Milling
Aluminum
.002
.005
.006
.007
Brass
.001
.004
Delrin
Polycarbonate
.003
.008
.009
Stainless Steel (303)
.0005
Steel (4140)
Drilling
.010
.015
Reaming
.012
Drill Cutting Speeds (SFM) surface ft/min
Material
Drilling
C-Sink
Reamer
Tap
Aluminum
300
200
150
100
Brass
120 90 66
Delrin 75
Polycarbonate
240
160
Stainless Steel 303) 50 35 25
Steel (4140) 60 45

50. Cutting data – parameters/allowances
Recommended Machining Parameters
Operation
Parameter
Value
All
Clearance Height
1.0 inches
Feed Height
.1 inches
Rapid Height
As needed to clear clamps and fixtures
Mill (Roughing)
Stepover (XY)
50-80% of tool dia.
Stepdown (Z)
25-50% of tool dia.
Drill
Peck Increment
.05 inches
Spot Drill
Dwell
.5 seconds
Stock Finish Allowances (Inches)
Operation
Tool Diameter Range (in)
<.125
.25-.5
.5-1.
>1.
Milling (XY)
.001
.005
.015
.020
Milling (Z)
.002
Reaming
.010
.012
.030

51. Troubleshooting speeds/feeds
Be methodical.
Analyze what is happening and draw on resources.
Don’t make the mistake of thinking the best solution is always to reduce cutting speeds and feeds: sometimes increasing is better.
Machinery’s Handbook has detailed troubleshooting information.