HSMworks use for CNC Lathe

1) Tool setup

• HSMworks uses Geometry codes for tools
• Indexable lathe tools usually specify the insert code (ie TPGH32.51)
• if you know the insert code, just set geometry parameters to match
• if you DON'T know, or want to use custom tools, you have to guess closest insert to use

A) 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

B) Threading inserts have a different coding system.  Typical threading insert code looks like “16 E R M AG 60”.

• in order, threading insert codes are:
  • diameter of IC (usually 11=1/4”, 16=3/8”, 22=1/2” or 27=5/8”)
  • (E)xternal or (I)nternal threading
  • (R)ight or (L)left hand thread
  • M = chip breaker groove.  Blank = no chip breaker
  • Thread pitch (numbers = TPI, letters = range of thread pitches).
    • Number thread pitch is“full profile” - will round crests, so only for specific TPI.
    • Letter thread pitch is “partial profile” - more like standard lathe threading tool
  • thread standard (ISO=metric, UN=english, others, number=partial profile pitch angle)
  • HSMworks only really needs to know the thread pitch (coarsest pitch for partial)  

C) grooving inserts are less complicated (in HSMworks) – fewer options

• parting blade is a “grooving” tool for HSMworks
• do not use a real parting blade for grooving operations other than parting (Z moves)
• be sure to set width correctly – HSMworks accounts for blade width in parting
• depth and height of grooving tool helps prevents crashes
• corner radius less important for parting.  More for grooving operations

D) 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)
• HSMworks doesn't use holder codes for size – just for shape.  Measure shank and enter length and size numerically.  3^rd and 5^th letter most important info

2) Feeds and Speeds

• lathe supports two speed modes:  RPM and SFM
• SFM mode adjusts RPM as tool moves in toward center - maintain SFM across tool nose
• max RPM limit must be used in HSMworks, based on gear choice (see below)
• also two feed modes.  IPM and IPR (aka Spindle Synchronous Feed)
• Inches Per Revolution syncs feed rate to spindle rotation
• IPR is primarily for threading operations

3) HSMworks Turning Operation types:

• profiling: most common - cut outside shape.  Includes boring - cut inside shape
• threading: next most common - add threads to flat model
• grooving: grooves and other features too small for normal lathe tools
• parting: grooving all the way through the part
• facing: normally done by hand.  Used only rarely for multi-part runs w/work stop collet
• drilling: don't do CNC drilling.  Use tailstock and drill by hand.  HOWEVER, sometimes you
• can add a “fake” drilling operation when working on tube stock.

4) Turning / Exterior Profiling Operations

• relatively straight forward, select tool, set speed & feed, similar to mill ops
• be sure to select correct direction for left hand tools (back to front)
• check tool engagement on left hand side at end of cut (right side for LH tools)
• if leading edge of insert extends past nose (positive angle), can get very heavy cuts at end
• one solution: do a partial parting operation.  Set bottom high to prevent parting off
• partial parting reduces diameter, so greater risk of snapping off part

5) Boring / Interior Profiling Operations

• same as profiling, but everything is “inside out” because all tool paths must be “top-down”.
• be sure to check “Machine Inside” on tool setup tab
• later versions of HSMworks; TOP = OD, BOTTOM = ID.
• retract and clearance heights should be from BOTTOM of model
• bottom should be from model TOP
• top should be from stock BOTTOM
• may also need to set clearance to a negative value "above" retract height
• very confusing at first, but easy once you figure it out
• check tool engagement at end of bore, same as exterior profile

6) Grooving / Parting Operations

• used for features with steep edges, grooves for o-rings, etc...
• similar to profiling.  Used for deep recesses.
• parting is a special purpose grooving operation.  Always at the end of modeHSMworks knows to cut on the BACK side of parting tool, so set correct thickness

7) Threading Operations

• Thread pitch specified by crest spacing (ie inverse of TPI)
• Be sure to use synchronous feed rate, set to thread pitch (in inch per thread)
• HSMworks understands fractions (i.e. enter 1/13 in, rather than decimal value)
• Also need to manually set thread depth
• select a flat (not tapered) surface to thread – may not be true in later HSMworks versions
• Be sure to leave clearance for threading tool at end of cut
• Infeed modes: constant, reduced, alternating flank
  • constant infeed can place a lot of stress on the tool, especially for coarse thread pitches
  • infeed reduction reduces cutting load on insert by reducing stepdown each pass
  • alternating flank cuts on both sides of the insert (one side then the other)
• Use “Spring” passes to clean off burrs – no increase in thread depth
• can do single (normal) or multiple start threads

8) HSMworks post processing

• Experimental customized post processor available for HSMworks, otherwise
• use 'Generic Fanuc Turning' post processor, with some output tweaks as follows
• remove all G17, G18 and G19 references from code (curve plane – lathe has only one)
• gear codes: manually insert after speed changes.  Add M01 to pause for gear shifting
  • make sure spindle OFF for gear changes (M05 stop, M03 forward, M04 reverse)
  • M41 low gear: speeds 10 to 84 RPM (36:1 ?)
  • M42 medium gear: speeds 45 to 380 RPM (8:1 ?)
  • M43 high gear: speeds 240 to 2000 RPM (3:2 gear ratio?)
  • Program will STOP if you are in a gear that can't support selected speed!
  • RPM mode easy: select gear that supports RPM desired
  • if you have a choice: high end of lower gear is usually best (higher torque & Max HP)
  • SFM mode harder: have to know starting OD and OD at deepest cut
  • 3.82 * SFM  / OD = RPM (3.82 = 12/Pi)
  • find minimum and maxiumum RPM and select gear that covers both speeds
  • be sure to set RPM cap in HSMworks, based on gear selection, when using SFM
  • can use top/bottom to split a cut in to two passes, one at lower gear than the other
• check insertion path after tool change, especially when switching from vertical (exterior) to horizontal (interior) tools!  May have to split positioning move into two steps.
  • HSMworks does not check tool length changes after a tool swap
  • insert M05 before tool change to stop spindle (if you want – not required)
  • look for first rapid after tool swap (N...... G0 X... Z...) or (N.... G28 U0. W0.)
  • having X and Z on same line causes a “dog-leg” tool move – 45 degree path
  • cut out X word and paste on to next line (line numbers optional – control ignores)
    • N..... G0 Z........
    • X.......
  • this will cause a box move – move all the way on Z, then move on X
  • when switching from interior to exterior tool, do X move first (put Z on next line)
  • may have to do this at the lathe, after looking at tool path (more later)

CNC Lathe Specs and Control

Millport SmartLathez Model 1740

• Bed swing-over: 17-5/16” (maximum diameter stock w/o hitting bed)
• Height of center: 8-5/8”
• Cross slide swing-over: 7-1/2” (maximum diameter stock w/o hitting cross slide)
• Cross slide travel: 11”
• Distance between centers: 40” (headstock to tailstock)
• manual tailstock travel: 6-5/16”
• tailstock taper: Morse Taper #5
• Spindle: D1-8 Camlock mount
• headstock bore: 3-3/8” diameter
• headstock taper: Morse Taper #7
• Spindle motor: 10HP (7.4kW) Max (VFD control reduces HP output at lower speeds)

1) Startup procedure

• load G-code file onto 2GB or smaller USB drive
• insert USB drive into control head USB port
• check fluids (way oil, coolant)
• power on lathe
• release E-stops if necessary
• home machine (press CYCLE START)
• load program (F2 Load, F3 Remote to access the USB drive)
• evaluate toolpath (F8 Graph).  X origin is center of graph.
• press F1 (Setup) then F2 (Tool) then F1 (Offsets) to start measuring tool offsets

2) Setup tool and work offsets

• X tool offsets using “skim cut” method
  • turn down a piece of scrap round bar stock (inside tube stock for boring bar)
  • measure diameter after cut (again measure bore for boring bar measurement)
  • select correct tool number X offset and set X Diameter (F1)
  • Measure Tool (F2)
  • repeat for each tool (change diameter for each tool based on cut)
  • save changes (F10) when finished!  Otherwise you start over from beginning.
• Z tool offsets
  • face end of stock to get flat surface (use right hand tool that can face for reference)
  • select correct tool number Z offset and Set Z reference (F1)
  • Measure Tool (F2)
  • if necessary, apply an Incremental offset (F4) to measured value.  -Z is toward head
  • repeat last two steps for each tool.  DO NOT RESET Z REFERENCE!!!
  • left hand tools, either touch off on a parallel or touch off on back and apply offset
  • shallow and neutral angle tools (ie threading) are tough to measure  
  • save changes (F10) when done
• Nose Radius and Nose Vector
  • ignore these for HSMworks generated programs (you did this in HSMworks)
  • necessary for conversational programming
  • +X vector tools are pointing toward center (exterior), -X away from center (interior)
• Tool details setting
  • optional for HSMworks programming, used by conversational programming
  • also used for live graphing of program while running
  • F1 (Setup), F2 (Tool), F2(Tool Details) to access
• Z work offset
  • F1 (Setup), then F1 (Part)
  • F6 and F7 select work offset (Usually G54 but check your code)
  • use the reference tool you had above to skim face the stock
  • Do not move tool on Z axis.  Enter tool number and press F10 (set)
  • If you use multiple work offsets (why?) repeat for each offset
• X work offset
  • you should NOT have to do this step!  X zero NEVER changes (spindle center)
  • to check, skim cut and check diameter against DRO.  X should be measured diameter
  • if it is NOT the same, double check all your X tool measurements!
  • if X tool offsets are correct and X work offset is STILL wrong, press F8 (Set X)
  • skim cut with a tool, and measure diameter
  • select Set all WCS and press spacebar to say Yes
• double check all tool and work offsets (measure twice, cut once)
  • load a tool on the toolpost
  • press F3 (MDI), and type TXYXY where XY is the 2 digit tool number
  • press CYCLE START to execute the G code.  DRO should update
  • ESC to back out of DRO move
  • move tool to end of stock and check Z offset, move in and check X offset
  • repeat for each tool

3) G-code editor

• If you forget to remove G17/18/19 or add M41/42/43 codes, use the on board text editor
• F6 (Edit) to edit the currently loaded program
• Pretty self explanatory.  Use F keys as listed at the bottom of the screen.  
• F2 will over-write the file on the USB drive.  F10 aborts w/o saving

4) Running a program

• F4 (Run) to start your program
• Set part count to 1 (we have no stock feeder)
• to stop a program, press the red CYCLE STOP or yellow TOOL CHECK button
• TOOL CHECK allows you to jog clear of the work, 2^nd press returns tool to home position
• to resume, press F4 (Run) then F1(Resume) to resume last program
• you can resume from an E-stop as well
• avoid F2 (Search) unless you know EXACTLY what you are doing!

5) Power feed

• used to manually turn down stock
• same as using G code MDI commands
• power feed seems to bug the MPGs – have to park machine to regain MPG control

6) InterCon (Conversational Interface)

• Press F5 (CAM) to access conversational programming
• read manual for details on specific operations (not covered in class)

CNC Lathe Notes on Operation

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