Millport SmartLathez 1740 CNC Lathe

Millport SmartLathez 1740 CNC Lathe
Millport SmartLathez 1740
General Info
Make	Millport
Model	SmartLathez 1740
Serial	622005
Specs	SmartLathEZ1740Manual
Manual	822LatheManual
Asylum Info
Location	Machine Shop
Rubric	HSMworks turning step by step
Training	Tool classes
Testing	Tool testing
Restrictions	red

Link to: Machine Shop Main Page

		Eye protection required!

Manuals

SmartLathEZ1740Manual

822LatheManual

HSMworks turning step by step . You will need a STEP file to work with this manual.

HSMworks use for CNC Lathe

CNC Lathe Notes

Centroid controller

G-code with some extra M-codes

lathe motor is 10-HP, but, with VFD speed control %age of top speed corresponds to roughly the mount of HP availabe.

Uses Tri-Cool for coolant

Chk oil level on back, way oil

Turn on

Set home: Green button at lower right of controller will cause it to run through its homing procedure.

The tailstock will trip the furthest Z-limit switch, so move tailstock towards chuck. If it is not appearing to move switch from ‘Inc’ to ‘Cont.

MPG: Mean Pulse Generator

Part Design Considerations:

• Inside corners should have radii greater than that of the tool insert tip.
• Outside corners should be set to 0.005-0.010” radii to avoid burrs.
• Stock to leave for finish passes: 0.015” axial & 0.030” radial
• Can cut 0.1” off of radius with Aluminum

Define tools in HSMWorks
Define Tool Positions & Angles
Define Tool Feeds & Speeds

Parting in hard alloys should be 300SFM for carbide cutters

Parting defaults to 0.040”/rev., which leads to DESTRUCTION! Better to set at 0.0035”/rev.

Make sure that your tools have different numbers in the tool library for a single job

Inserts with a negative rake are mounted at an angle on the toolholder, so cannot cut away from the chuck as the rake is actually negative in that direction.

Set max spindle speed when changing gears and ranges. This is a global var?

Post-processing: Use FANUC

G53:  Retract
G54:  Work Offset

Keep in mind that G53 & G54 go to coords (0,0) which will be the face of the stock.

Tool changes are done explicitly by:

• Rapid Traverse  -  G53, G54, etc.
• Tool Offset
  • Home machine
  • Set 0s on stock
  • The set tool offsets

In graph mode we can get range to see only those moves due to those lines of code.

VS-Codes is good for editing G=code. Use G-code add-in

Use locknut on toolholder to avoid changing height when handling toolholder.

F1/Set-up

F2/Tools

• Offset Library
• Tool: may set to 0, or set offset to a Var

MPG: Can turn off to avoid changing values if you accidentally bump into the hand wheels during operation

F2/Measure

• Sets the offset

Set Z-Ref: 2” when using indicator

Move manually to where you expect (0,0) to be and look at the numbers on the screen as a check.

Run Menu

Set part count to 1

Re-set spindle speed and coolant back to Auto CTRL

For the big chuck, the max speed is 700RPM

For the Medium chuck, the max speed is 900RPM

For the collet closer, the max speed is 2-2,400RPM

Lathe Tool Codes

Profiling and boring insert codes are 4 letters and 3 numbers (single digit is ANSI/inches, double digit is ISO/mm).  Formatted ABCD123 (ANSI)  or ABCD010203 (ISO)

Example code is D C M T 3 2.5 1

- Letters define shape of insert, numbers define size (not all TCMT inserts the same size)

- http://www.carbidedepot.com/formulas-insert-d.htm for more information

• A Shape code: T for triangular, R for round, many others
• B relief angle: N=0 degree, up to G=30 degree (lookup chart)
• C tolerance: when in doubt use "M" (loosest tolerance inserts)
• D cross section: is mounting hole countersunk?  chipbreaker?  one or both sides?
• 1 size: english - diameter of inscribed circle in 1/8" (1/32" for IC less than 1/4")
  •             metric - diameter of inscribed circle in mm
• 2 thickness: english - thickness in 1/16" (1/32" if IC is less than ¼") decimals allowed
  • metric - approximate thickness in mm (look up exact values)
• - 3 nose radius: english - radius in 1/64" (0 = "sharp" = max radius 0.005")
  • metric - radius in 1/10 mm

2. Tool holders have a nomenclature too.  5 letters, 2 numbers, letter (S D J C R 10 3 A)

- http://www.carbidedepot.com/formulas-th-d.htm for more information

- first letter (A) is how the insert is locked to the holder

- second letter is insert shape (redundant if you know insert code)

- third letter (C) is insert angle relative to holder (-5 degree, +3 degree, etc...) Note that a 0

  degree tool has leading edge perpendicular to rotation axis.  (Not a “neutral” tool)

  For Right hand tool: positive rotation is CW, negative CCW from perpendicular.

  For Left hand tool: positive rotation is CCW, negative CW from perpendicular.

- fourth letter is relief angle of insert (again redundant)

- fifth letter (E) is direction (Left, Neutral or Right handed)

- first number is square shank in 1/16” (10 = 5/8” = 10/16”, etc...)

- second number is insert IC size (redundant)

- last letter is overall length (look up or just measure)