Tool Parameters for Slot Drills on aluminium

Tool Dia. Spindle speed Horizontal feed rate [cut_feed] Vertical feed rate Step depth Maximum [total] depth of cut
2.5 6000 100 60 1 2.5
3 6000 200 60 1 6
6 5000 250 60 1 12
8 4000 300 60 1 14
10 3000 300 60 1 16
5.8 drill 2500 – 60 – 10
0.5mm engraving tool 6000 200 100 0.2 0.2

Remember to set a vertical feed rate – all tools must feed more slowly into materials than horizontally through material. This is the RAMP_FEED parameter in the volume roughing sequence and the PLUNGE_FEED parameter in the volume rough and trajectory sequence.

Diameters between those stated are also available in 1mm increments.

All feed rates are in mm per minute.

Ball Nosed cutters – decrease feedrates by 20%

Tools above 10mm dia. can be used but are restricted by machine power and the clamping system used – seek appropriate advice.

 

Maximum Depth of Cut

Whether it’s a slot drill or ball nosed cutter, our standard tool range has either a 6mm or 10mm shank diameter.  The cutter diameter will be equal to or less than this dimension – see below image. The maximum depth of cut is restricted by the length of the cutting edge, therefore if you want a 1.5mm radius in the corner of a pocket, that pocket can be no greater than 6mm deep – the cutting edge length of a 3mm dia. tool.

Engraving Tool

This tool will produce a line on a surface 0.5mm wide with a depth of cut of 0.2mm.  This will show as a raised line on your widget and can be used for lettering and logos.  Use with an Engraving sequence. Watch out for clearance from side walls in cavities – see below.

 

 

Tool Spindle Speeds and Feedrates

 

Surface Speed

A particular cutting tool material has an optimum speed at which it should travel through a particular material.

Example: The tip of a High Speed Steel (HSS) cutting tool should travel through aluminium at 150m/min.

Therefore we need to control the tip speed of the milling cutter at the radius of the tool – its circumference [in metres] multiplied by its revolutions per minute.

 

Spindle Speed

Spindle Speed = Surface Speed / Circumference

For a 10mm [0.01m] dia. cutter:

circum. = Pi x Dia = 3.14 x 0.01 = .0314m

For a cutting speed of 150m/min:   150m/.0314m = 4777rpm

Free cutting mild steel 38 m/min
Low carbon steel 32 m/min
Brass or bronze 55 m/min
Aluminium alloys 150 m/min
Plastics 250 m/min
Woods 500 m/min

 

Feedrate

Feed rate is the distance a cutting tool moves through the material per minute. This rate dictates how much material each tooth of the cutting tool removes per revolution.

Feedrate is dependent on the:

  • Surface finish desired
  • Power available at the spindle (to prevent stalling of the cutter or workpiece)
  • Rigidity of the machine and tooling setup (ability to withstand vibration or chatter)
  • Strength of the workpiece (high feed rates could damage thin walls)
  • Characteristics of the material being cut, chip flow depends on material type and feed rate
  • The ideal chip shape is small and breaks free early, carrying heat away from the tool and work

Feed rate (mm/min) = Tooth Load (mm). X Number of teeth. X Spindle Speed in RPM.

 

Denford: http://website.denford.ltd.uk/support/89-tutorials/101-speedfeed

Wiki: http://en.wikipedia.org/wiki/Cutting_speed

 

Parameters used in these pages

 

CLEAR_DIST – the default 2 will be OK but must be greater than 0

CUT_FEED – horizontal feedrate – variable

CUT_TYPE > ZIG_ZAG

GROOVE_DEPTH

HELICAL_DIAMETER

LACE_OPTION to LINE_CONNECT

MAX_STEP_DEPTH – generally 1mm

NUMBER_CUTS

OPEN_AREA_SCAN or CLOSED_AREA_SCAN set to FOLLOW_CONTOUR

PLUNGE_FEED

RAMP_FEED

RAMP_FEED (in the ALL parameters list) – vertical feedrate – generally 60mm/min

RAMP_ANGLE  [try approx 5 deg]

scallop height

SPINDLE_SPEED – variable

STEP_DEPTH > set slice increment

STEP_OVER – must be less than the tool radius

TRIM_TO_WORKPIECE