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)