QuickGuideforLatheFlipBook

torbjornbergstrom

QUICK

GUIDE

FOR

HAAS LATHES

HAAS LATHES

TORBJORN BERGSTROM


CNC Quick Guide

for Haas Lathes

Torbjorn Bergstrom

Flip Book Edition

Copyright Engineering Media Productions LLC.

2018 Worcester, Massachusetts, USA

Page i


Foreword

This guide is intended to assist AUTHORIZED USERS in machining

facilities equipped with Haas CNC machine tools.

This document does not replace supervised training.

The photographs (and supplemental videos) used in this guide are taken

from a variety of vintages of the Haas Controller some may be from

controllers newer than the one you are using, and some from an older

version. One of the beauties of the Haas controller is that it has been a

stable platform from its inception. If you know how to use one vintage

controller you can use any of them with little or no additional training.

As indicated by the title this book is intended as a quick reference guide

and is not a replacement for the operators manual or other training

materials available from Haas Automation, available at:

http://haascnc.com/

Table of Contents

Page ii


Acknowledgements and Authors

This guide has been compiled over a period of several years of teaching.

The guide has grown and evolved over these years and I hesitate greatly to

claim authorship. The first revision of this document was distributed in the

spring of 2006; it was 14 pages long and I was the sole author.

Since this first version there have been dozens of WPI students and staff

who have contributed in one way or another. It would be impossible for

me to list all of them here but I will try to list some of the most significant

contributors below. If you are reading this and think your name should be

on this list you are probably correct. Please contact me and I will make the

correction.

Contributing Authors:

Wei Tian

James Loiselle

Adam Sears

David Ephraim

Aaron Cornelius

Kevin Arruda

Mikhail Tan

Table of Contents

Page iii


Table of Contents

Foreword

ii

Acknowledgements and Authors

iii

Table of Contents

iv

Safety 1

Operations Checklist 3

Startup Procedures 4

Program Selection 8

Machine Operation Basics 14

Setting Tool Offsets 30

Setting Work Offsets 46

Program Operation 51

Clean Work Area 56

Page iv


Safety

The safe operation of any manufacturing facility is the responsibility of

everyone involved from the CEO to the person sweeping the floors.

In 1968, the bloodiest year of the Vietnam War, more Americans were

killed in industrial accidents than died in combat. In 1971, OSHA was

founded.

The owners and managers of your facility are responsible for establishing

safe operating procedures. They are responsible with providing all

personnel and equipment with functional safety systems and appropriate

personal protective equipment (PPE.) If they fail to do this they will be

subject to substantial fines, penalties, and criminal prosecution.

No judge has ever been able to award an injured worker a new hand

or orphaned children a new mother or father.

Table of Contents

Page 1


Before operating any piece of equipment or using any tool:

• Review the Operator’s Manual: particularly the section on safety

• Inspect the tool for obvious signs of misuse or damage

• Make sure you have someone within sightline to assist you

• When in doubt, ask for help

Whenever you are in a manufacturing facility:

• Follow all safety policies

• Pay attention to what is going on around you.

• Stop any activity you think is unsafe

• Clean up spills and debris immediately

• Always use the appropriate PPE

• Report damaged machines, guarding, or other unsafe situations to

your supervisor

Table of Contents

Page 2


Operations Checklist

Operator

Signature

Start Time

End Time

ID#

Machine Tool

Date

Date

All users must complete this checklist

anytime they operate a machine tool.

All of the steps must be repeated under

any of the following circumstances:

1. the program has been modified,

2. the user has altered the setup

in the machine tool since

the program was last run,

3. the user has been away from

the machine for someone else

to have altered the setup.

Notes

☐ Check here if you are completing

a non-standard operation that

precludes completing one

or more of the steps below.

The current lab monitor

must initial and approve.

☐ Set Tool Offsets

This tells the machine about the

tools that are installed and must be

done before a program can be run.

☐ Set Work Offsets

This tells the machine about the

location of the workpiece and must be

done before a program can be run.

☐ Simulate in CAM Software

This ensures that you know what

the program is intended to do.

☐ Simulate on Controller

This ensures that you know

what the machine tool thinks

the program should do.

☐ Reduce Rapid Rate

This gives you a chance to stop the

machine tool before something

bad happens if you have made a

mistake in the previous steps.

☐ Check Distance to Go for Each Tool

This is your last chance to catch

setup and possible programming

mistakes. Almost every crash that

happens can be stopped if we pay

attention and complete this step.

Table of Contents

Page 3


Startup Procedures

Before you start the machine tool it is a good idea to check a few things:

1. Check the coolant level

2. Check the way oil level

3. Check that the power switch at the rear of the machine tool is turned

on (shown below)

After this, follow these instructions to turn the machine on and prepare it

for use.

Contents

Power On 5

Clear Alarms 6

Power Up/Restart 7

Table of Contents

Page 4


Power On

1. Press the green button (POWER ON) located

on the upper left side of the controller

If the machine fails to start it may indicate

that it has been locked out, that a room level

emergency stop has been activated, or electrical

issuse with the machine.

If this has happened, check with your

supervisor before continuing.

2. Reset the EMERGENCY STOP

Twist it to the right and it will pop out (Pulling

the button out may cause it to fail prematurely!)

Startup Procedures

Table of Contents

Page 5


Clear Alarms

When you power on the machine tool there will be at least one alarm

message (two if the emergency stop was activated before the machine was

shut down)

1. Press the ALARM button to enter the alarms display, and check the

displayed alarms to make sure that there’s nothing critical. Use the

ARROW Keys to scroll between them

2. Press the RESET button for each alarm displayed to clear it

3. On machines with servo auto doors, you will need to open and close

the door to check the sensor

Startup Procedures

Table of Contents

Page 6


Power Up/Restart

Because of the construction of Haas

machine tools it is necessary to reference

(home) all of the axes before you run a

program.

The process of referencing the axes

involves the controller moving each axis

over a limit switch at one end of its travel in

turn.

1. Verify there are no obstructions blocking the travel of the axes from

their present location to the home position

If tools will cause a collision during the POWER UP/RESTART

operation, STOP and complete Single Axis Return. This may happen

if the machine was turned off with

a tool in the part. See your Haas

manual for details.

2. Close the door, press the

POWER UP/RESTART button,

and wait for the machine to

complete operation

Startup Procedures

Table of Contents

Page 7


Program Selection

It’s important to make sure the machine has the right program selected.

This section will cover basic methods of selecting and loading programs

onto the controller.

Contents

Select Program From Memory 9

Load from Floppy Disk 10

Load from USB 11

Load with RS232 12

Drip Feed from Hard Drive or USB 13

Table of Contents

Page 8


Select Program From Memory

1. Press LIST PROGRAM

2. On newer controls, press WRITE/

ENTER to enter the MEMORY

tab. On older controls, this won’t be

necessary

3. Use the arrow keys to highlight your

program

4. Or type in the program number

eg “O02021”

5. Press SELECT

PROGRAM to select

that program

6. Press MEM, and

check that the

correct program has

been selected.

Program Selection

Table of Contents

Page 9


Load from Floppy Disk

1. Insert the floppy disk with the program into the

controller

2. Press EDIT, then F1 to activate the menus

3. Use the ARROW KEYS and WRITE/ENTER

to select the I/O tab

4. Select Disk Directory and press WRITE/

ENTER

5. Use the ARROW KEYS

or JOG HANDLE to

highlight the desired

file, then press WRITE/

ENTER to start loading

the program

New files are listed at the

bottom

6. If there’s already a program

with that number, you’ll be

prompted to overwrite it.

Press Y for Yes and N for

No

7. Press MEM, and check that

the correct program has

been selected

Program Selection

Table of Contents

Page 10


Load from USB

1. Insert the USB drive with the program into the controller. Wait a few

seconds for the drive to

load properly.

2. Press LIST PROGRAM

3. Use the cursor arrows

to select USB DEVICE

and press WRITE/

ENTER to enter the

tab. If the list of devices

isn’t active, press

CANCEL

4. Locate the program you

are trying to load and

press WRITE/ENTER

5. Press F2

6. Use the cursor arrows to

select MEMORY from

the list

7. If there’s already a

program with that

number, you’ll be

prompted to overwrite

it. Press Y for Yes and N

for No

8. Press MEM, and check that the correct

program has been loaded

Program Selection

Table of Contents

Page 11


Load with RS232

1. Select LIST PROG to

view listed programs

2. Press END to make sure

ALL is highlighted

3. Press RECV RS232.

The controller is

now waiting to

receive data. Check

to make sure it says

“waiting...” on the

screen

4. Send the program

from your DNC

software. It will

automatically be

loaded and selected

on the controller

5. Press MEM, and

check that the

program has been

loaded correctly.

Scroll down to the bottom and make sure the whole program has been

loaded

Note that this option requires additional configuration to run

correctly.

Program Selection

Table of Contents

Page 12


Drip Feed from Hard Drive or USB

1. Load the program

onto a USB drive or

the machine’s hard

drive

Only newer model

machines will have

built-in hard drives

2. Press LIST

PROGRAM

3. Use the cursor

arrows to select USB

DEVICE or HARD DRIVE and press WRITE/ENTER to enter the

tab. If the list of devices isn’t active, press CANCEL

4. Highlight the desired program, and press SELECT PROGRAM

Program Selection

Table of Contents

Page 13


Machine Operation Basics

In order to operate the machine tool and to complete machine tool setup

steps there are a few basic operations you should know how to do. In this

section we show you how to:

Contents

Tool Change 15

Handle Jog 16

Install Tools 17

Change Inserts 22

Fixturing Methods 23

Clamp the Chuck 24

Change Chuck Jaws 25

Turn Soft Jaws 26

Install Collets 27

Start and Stop the Spindle 28

Face the Part 29

Table of Contents

Page 14


Tool Change

1. Check to ensure the tool

changer can rotate without

any of the tools impacting

fixturing or parts (Handle Jog

the turret as necessary to clear

the tool change area)

2. Select MDI mode

3. Type “T” followed by the

desired Tool Number. Do not

press WRITE/ENTER

Example: For Tool Number 10,

enter “T10”

4. Press TURRET FWD or

TURRET REV

If you press Turret FWD or

Turret REV with no number

entered it will toolchange one

spot in the indicated direction

Machine Operation Basics

Table of Contents

Page 15


Handle Jog

Handle Jog Mode is used to manually position the axis of the machine tool.

You can use either the Jog Handle or the Jog Buttons

1. Select the HANDLE JOG mode

2. Select an Increment / Speed

The top number indicates the distance the selected axis will move for

each “click” of the Jog Handle, here in inches.

The bottom number indicates the speed the axis will move (here in

inches/min) if the Jog Buttons are held in, or JOG LOCK is used

3. Select the axis to jog (X, Z) with the Jog Buttons

4. Either turn the Jog Handle or press and hold the the appropriate Jog

Button to handle jog

Machine Operation Basics

Table of Contents

Page 16


Install Tools

There are many different ways of holding tools in the machine. This section

will cover some of the most common methods, but methods may vary

depending on your specific machine and tools.

1. Tool change so you have clear access to the tool holder

2. Proceed to the appropriate section below

OD Turning Tools 18

Boring Bars 19

Drills 20

VDI Tools 21

Machine Operation Basics

Table of Contents

Page 17


OD Turning Tools

OD turning tools are held in place with a

clamping wedge.

1. Loosen the two bolts. Use a mallet to tap the

tool out

2. Clean out any chip or debris from the holder

and turret

3. Put the new tool in place. Make

sure it’s butted firmly up against the

turret, and that you have the tool in

the correct cutting orientation

4. Tighten the two fastening bolts to

secure it in place

Machine Operation Basics

Table of Contents

Page 18


Boring Bars

1. If you’re using a bushing to

adapt the tool, slide the boring

bar into the bushing. Line the

flat up with the opening in the

bushing

2. Tighten the bushing’s set screw

onto the flat, wiggling the bar

back and forth to make sure it

seats properly. If there’s another

setscrew, get it snug, but not tight

3. Slide the boring bar into the

tooling block

Make sure it’s sticking out far

enough to avoid crashes.

4. Rotate the boring bar so the flat

lines up with the setscrews that

will hold it. Remember that the

insert needs to be facing down, on

the positive X side

5. Slowly tighten the set screw, wiggling the boring bar back and forth as

you do to make sure that it seats properly

6. Tighten the set screws onto the flat of the bar. Get the other set screws

on the opposite side lightly snug, but not tight

Machine Operation Basics

Table of Contents

Page 19


Drills

Drills are generally held in

collet or drill chucks.

1. Loosen the chuck

using a spanner

wrench or chuck key,

and remove the drill.

2. If necessary, change

the collet to the

correct size. Make

sure there are no

chips or other debris inside the

chuck that will prevent it from

clamping properly.

3. Put the new drill bit in and

tighten the chuck. Make sure

you are only clamping on the

straight shank of the tool, not

the flutes.

Machine Operation Basics

Table of Contents

Page 20


VDI Tools

VDI tools are used for quick change

tools, as well as axial and radial live

tooling. They use a serrated clamping

wedge to repeatably locate the tool in

place.

1. Loosen the clamping wedge

from the turret and pull the

previous tool holder out

2. Clean the tool’s shank and face,

as well as the turret’s bore and

clamping wedge.

3. Place the new tool in,

making sure the serrations

are aligned properly

4. Tighten the clamping

wedge to hold it in place

For radial live tooling you

will now need to tram

the tool in. See your Haas

manual for details.

Machine Operation Basics

Table of Contents

Page 21


Change Inserts

Note that there are many different insert

clamping methods. The exact steps may

vary.

1. Tool Change so that you have clear access

to the insert

2. Loosen the top clamp holding the insert

in place. After you loosen it enough it will

swing out of the way, so you don’t have to

remove it entirely

3. Loosen the lock pin at the center of the

insert and pull the insert off. You may

need to loosen it several revolutions

before the insert will come out

4. Clean any debris off of the insert pocket

and clamp

5. Put the new insert on, and tighten the lock

pin. This doesn’t need to be very tight

6. Swing the top clamp back into place and

tighten it down to secure the insert

Machine Operation Basics

Table of Contents

Page 22


Fixturing Methods

All fixtures must serve the following two purposes in CNC turning:

1. Locating the workpiece within the machine tool’s work envelope

2. Counteracting machining forces applied during the machining

operations.

A third function that is common to many fixtures, especially in a

production environment, is:

3. Relocating subsequent workpieces at the same location.

Entire text books have been written on the topic of fixturing.

Following are some examples of common fixturing methods and uses.

Follow the links in the table for information on the methods, or here

to clamp your part.

Fixture Types:

Hard chuck jaws

Soft chuck jaws

Collet chucks

Common Uses:

Round parts with common diameters

Round parts with odd diameters or

shapes

Round, square, and hex parts with

common sizes, high spindle speeds

Machine Operation Basics

Table of Contents

Page 23


Clamp the Chuck

Most fixturing will use a hydraulically

actuated chuck to clamp the part.

1. Set the clamping pressure with

the hydraulic pressure regulator.

Consult the clamping force chart on

the machine for reference

Generally 200-250 psi is a good

starting point

2. Press MDI

3. Make sure the inside of your chuck and

clamping surfaces are clean, and insert

your part into the bore

4. While holding the part, press the chuck

foot pedal to clamp it

Be careful not to press the tailstock

foot pedal.

5. Try to pull out the part to ensure it’s

clamped in place

6. Spin the part by hand to make sure it’s

spinning true

7. When your operation is done, press

the pedal again to unclamp the part

You must be in MDI or CURRENT

COMMANDS mode to clamp or

unclamp the part

Machine Operation Basics

Table of Contents

Page 24


Change Chuck Jaws

1. Use a wrench to grab a jaw and keep

the chuck from turning

2. Loosen the bolts holding the jaws

on, and slide the jaws off

3. Remove the bolts fully to remove the

wedge from the back, and move it to

the new chuck jaws

4. Slide the new jaws into place and

lightly fasten the bolts. Make sure

they’re lined up on the correct

serrations for grabbing your stock

The wedges can’t extend outside

the chuck. It is very important that

they are all on the same serration,

otherwise it won’t clamp properly.

5. Use a torque wrench to tighten the

bolts to spec. Check your chuck’s

manual for the correct torque spec

If you are using soft jaws, go here for

instructions on turning them to size.

6. Clamp your part and spin slowly to ensure that

you are on the correct serration and don’t have

excessive runout

Machine Operation Basics

Table of Contents

Page 25


Turn Soft Jaws

Soft jaws are commonly used to hold parts

with odd sizes or shapes. They are turned

to fit the shape of the part. When turning

soft jaws, the chuck needs to be clamped

partway through its travel, using a boring

ring or plug in the back of the jaws.

1. Change the jaws to soft aluminum or

steel jaws, if necessary

2. Clamp the jaws on a boring ring or

plug. Make sure that it’s clamped

partway through its travel

If you are using a plug, remember

that you can’t go all the way through

the jaws.

3. Toolchange to a boring bar

4. Start the spindle, and use handle jog

to turn the jaws to the appropriate

diameter

You can also use a program to make

jaws for contoured parts.

Machine Operation Basics

Table of Contents

Page 26


Install Collets

1. Loosen the setscrew holding the

current collet in and make sure the

chuck is unclamped

2. Use the collet wrench to remove the

collet

3. Spread grease on the threads of the

collet

4. Note which section of the collet has

the keyway

5. Thread the collet into the chuck

using the wrench until the tapers just

touch

6. Back the collet out until the setscrew

lines up with the keyway

7. Snug the setscrew down while

turning the collet back and forth

slightly to make sure it lines up

8. Clamp a part in the chuck and try to

turn it by hand to make sure it’s held

securely

Do not clamp the collet without a

part. It will bend and break the collet.

Machine Operation Basics

Table of Contents

Page 27


Start and Stop the Spindle

1. Go into MDI mode

2. Press ERASE PROGRAM to clear

any code that’s in there.

3. Type in S, followed by the spindle

speed you want, eg “S1000”. Press

WRITE/ENTER

With the door open the machine will

cap spindle speed at 750 RPM

4. Press CYCLE START.

This will set the spindle speed, but

won’t start the spindle motor.

5. Press FWD in the Overrides panel

to start the spindle

6. After the spindle has been started

this way and the speed is set, you

can start it again just by pressing

CW

7. To stop the spindle, press STOP or

RESET.

Machine Operation Basics

Table of Contents

Page 28


Face the Part

Facing the front of the part will create

a flat surface that can be used as a

reference for tool or work offsets.

1. Toolchange to a tool that’s

appropriate for facing.

2. Handle jog the tool in front of the

part in Z, as shown in the photo.

3. Start the spindle at an appropriate

speed.

4. Jog towards the part in Z 0.001”

increments until you see the tool

cut a chip.

5. Jog slowly and smoothly to the

center of the part in X, then back

off the part in X.

6. Stop the spindle by pressing the

stop BUTTON.

7. If the face isn’t totally flat, start the

spindle, jog a few thousandths of an inch

further in in Z, and face it off again.

Machine Operation Basics

Table of Contents

Page 29


Setting Tool Offsets

Lathes have two tool offsets that need

to be set. Tool offsets tell the machine

how to compensate for the size of the

tool, either in X or Z. Offsets can be set

manually or using the machine’s tool

probe.

Contents

Set Z Tool Offsets On a Reference Gauge and Surface31

Choosing a Reference Gauge and Surface 32

Positioning the Tool Using a Reference Gauge 33

Record the Z Tool Offset 34

Z Compensation for Neutral-hand and Cutoff Tools 35

Verifying Tool Offsets 36

Setting X Offsets Manually Using a Skim Cut 37

Setting X Offsets With a Skim Cut for OD Tools 38

Setting X Offsets With a Skim Cut for ID Tools 39

Set the X Offset with a Measured Diameter 40

Setting X Offset for Drills 41

Set Tool Offsets Using the Tool Presetter 42

Determining Probing Direction 43

Deploying the Presetter 44

Touching Off of the Presetter 45

Table of Contents

Page 30


Set Z Tool Offsets On a Reference Gauge and Surface

The Z tool offset is the position of the turret in machine coordinates when

the tool tip is at the reference surface. Every tool must be set at the same

reference surface, you can’t mix and match.

If you use the front of your part as the reference surface, the work

offset is zero

When you manually set your offset Z, there are three main steps.

1. Select a reference gauge and surface

2. Position the tool relative to the reference surface using the reference

gauge

3. Record the tool offset

Set Tool Offsets

Table of Contents

Page 31


Choosing a Reference Gauge and Surface

Reference gauges should be dimensionally accurate, consistent, and easy to

handle. There are three main choices for gauges: cigarette paper, gauge

blocks, dowel pins

Dowel pins are optimal as gauges. They have the following advantages:

1. Greater dimensional accuracy and safety than paper

2. Lower cost and longer life than gauge blocks

Reference surfaces need to be flat, durable, large enough to gauge off of,

and ideally fixed. Common surfaces include: top of the part, back of the

vise/fixture, machine table. All have advantages and disadvantages.

Reference Surface

Front of the part (requires turning

the front face)

Back of the chuck (not always

possible)

Advantages

No need to set Z work offset, good

for fast setups

Consistent between parts. Flatter

and more stable than the part top

Once you’ve chosen your references, use them to position the tool.

Set Tool Offsets

Table of Contents

Page 32


Positioning the Tool Using a Reference Gauge

If you are using the front of the part, face off

the part.

1. Handle jog the tool towards the reference

surface so the gauge does NOT fit

2. Jog the tool away in 0.001” increment, one

click at a time, until the gauge just fits

Don’t jog forward while the gauge is

in place.

3. Remove your gauge, jog forward

one step so the gauge doesn’t fit, and

switch to 0.0001” increment. Repeat

the process until the gauge fits.

4. With your tool accurately

positioned, next record your offset

Set Tool Offsets

Table of Contents

Page 33


Record the Z Tool Offset

1. Press the OFFSET button until the Tool Offset screen is selected

2. Highlight the Z Geometry offset

for the tool you’re setting

3. Press Z FACE MEASURE

This sets the offset at the

machine’s current location. Now

accommodate for the thickness of

your gauge.

4. With the offset still highlighted, type a

negative sign, and then the thickness

of your gauge. Your control may give a

warning, “Error in setting tool offsets too

great”. Press Y to confirm

5. Press WRITE/ENTER to subtract from the

offset

6. If the offset for the tool is not set at the

front of the tool, compensate for the tool

thickness

7. Verify that your offset is set correctly

Set Tool Offsets

Table of Contents

Page 34


Z Compensation for Neutral-hand and Cutoff Tools

If the tool offset is not set at the front of the tool, you need to compensate

for the tool thickness. This is usually true for cutoff/grooving tools, set on

the right side, and neutral-hand tools, set at the center.

1. Look at the program or setup sheet to determine where on the tool

the offset is set

2. If the tool is a cutoff or grooving tool with the offset on the right side,

subtract the thickness of the tool from the offset

3. If the tool is a neutral-hand tool, subtract half the thickness of the tool

from the offset. It may be useful to set the offset off the tool holder

instead, then subtract half the thickness of the holder

Your control may give an error, “Error in setting tool offsets too

great”. Press Y to confirm that you mean to set it.

Set Tool Offsets

Table of Contents

Page 35


Verifying Tool Offsets

After setting the offsets for a tool, you should verify the offset to make sure

it is correct.

1. Go into the tool offset page, and press

HANDLE JOG

2. Carefully jog the tool in X until the machine

coordinates match the offset. Make sure you

don’t run into anything

3. Visually verify that the cutting edge is at the

spindle centerline. If it isn’t reset your tool

offset

4. Jog the tool clear in X, and then carefully jog

it to the Z position in the Z tool offset

5. The cutting edge should be at the reference

surface you set your tool at. If it isn’t reset

your tool offset. Remember that all of your

tools must be set to the same reference

surface

6. When you’re done, jog the tool clear and

then home the machine

This method won’t detect small problems with your offsets, but it will

ensure that it is set closely enough to avoid breaking anything.

Set Tool Offsets

Table of Contents

Page 36


Setting X Offsets Manually Using a Skim Cut

The X tool offset is the position in machine coordinates when the cutting

tip of the tool is positioned at the spindle centerline. It can be turning the

diameter of the part, measuring it, and using that to calculate the centerline

position.

This can be used for OD and ID tools, but not for drill bits. See this

page for information.

There are two basic steps to this process.

1. Take a skim pass off the outside of the part. See the steps for OD tools

here and ID tools here

2. Set the offset

Set Tool Offsets

Table of Contents

Page 37


Setting X Offsets With a Skim Cut for OD Tools

1. Put a piece of stock in the spindle. It doesn’t have

to be your final part

2. Tool change to the tool you want to set

3. Jog the tool just outside the diameter of the part

in X

4. Start the spindle at an appropriate speed

5. Jog the tool slowly towards the part in 0.001”

increments until it forms a chip

Make sure you turn a large enough area

to measure

6. Jog the tool slowly out in Z, turning

the OD of the part

Don’t jog the turret in X. It uses

the current position in X for the

calculations

7. Stop the spindle. If the whole OD isn’t

turned, take a deeper cut

8. Set the X offset

Set Tool Offsets

Table of Contents

Page 38


Setting X Offsets With a Skim Cut for ID Tools

1. Put a piece of stock in the spindle. It

doesn’t have to be your final part

2. Use a drill to make a hole big enough

that you can fit your boring tool

through it.

3. Tool change to the tool you want to

set

4. Jog the tool just in front of the bore

5. Start the spindle at an appropriate

speed

6. Jog the tool slowly towards the part

in 0.001” increments until it forms

a chip

7. Jog the tool slowly in and out in

Z, making a bore deep enough to

measure

Don’t jog the turret in X. It uses

the current position in X for the

calculations

8. Stop the spindle. If the whole ID

isn’t turned, take a deeper cut

9. Set the X offset

Set Tool Offsets

Table of Contents

Page 39


Set the X Offset with a Measured Diameter

Before you do this step, you need to

have taken a skim pass off the diameter

of the part.

Make sure you haven’t moved the X

axis since you took the skim pass

1. Press OFFSET until the Tool

Geometry Offsets screen is shown

2. Highlight the X offset for the tool

that you want to set

3. Press X DIAMETER MEASURE

4. Press CANCEL until the input area is

empty

5. Measure the diameter that you just cut

using calipers or micrometers

6. Type in that measured number, and then

press WRITE/ENTER

7. Your control may give an error,

“Error in setting tool offsets too

great”. Press Y to confirm that you

mean to set it

8. Verify the offset to ensure it’s set

correctly

Set Tool Offsets

Table of Contents

Page 40


Setting X Offset for Drills

The holders for center-cutting tools like drill bits are standardized. This

allows their offsets to be set very easily when the machine is properly

calibrated.

1. Press HANDLE JOG

2. Press OFFSET until the tool geometry

page is shown

3. Highlight the offset you want to set

4. Press F2. Watch the number to make

sure it changes

5. If it didn’t change, then either

something went wrong or it

was already set correctly. Make

sure you’re in Handle Jog

mode. Press 0 and then F1 to

zero the offset, and then press

F2 again

6. Verify the offset to ensure it’s set correctly

Combination VDI/BOT turrets are calibrated off the VDI bores.

Look in your manual for the offset from the VDI bores to the BOT

bores.

Set Tool Offsets

Table of Contents

Page 41


Set Tool Offsets Using the Tool Presetter

The tool probe can be used to set your X and Z tool offsets. The operator

jogs the tool near the probe, then slowly feeds the tool into the probe. It

will automatically stop and set the offset when it triggers.

1. Change to the correct tool

2. Determine which direction you need to probe for your tool

3. Deploy the tool presetter

4. Touch the tool off against the presetter

5. Repeat with any other tools

Set Tool Offsets

Table of Contents

Page 42


Determining Probing Direction

To set the offset at the cutting tip

of the tool, you’ll need to touch

off the correct side of the presetter

tip. Refer to the diagram and

chart to determine your probing

strategy. Certain tools may have

links to more information about

their probing strategy.

Tool

Orientation

Examples

Z Probing

Direction

1 Rear boring or ID Z+ X+

grooving tools

2 ID boring tools Z- X+

3 OD turning tools Z- X-

4 OD grooving or cutoff Z+ X-

tools

5 Drill bits for sub Z+ See here

spindle

6 Neutral hand or Z-, then compensate for X+

threading ID tools tool thickness

7 Drill bits Z- See here

8 Neutral hand or

threading OD tools

Z-, then compensate for

tool thickness

X-

X Probing Direction

Once you have determined which direction you need to probe, deploy the

presetter

Set Tool Offsets

Table of Contents

Page 43


Deploying the Presetter

For safety, the presetter is stored outside the

machining zone when not in use. Newer presetter

are deployed differently than older ones

1. Make sure that the arm won’t hit the part or

turret when it comes down. Home the turret

and remove any long stock

2. If your presetter arm looks like the first

picture on the side, carefully pull the arm out

and lower it by hand. Make sure it sits all the

way down. To retract it, carefully

pull it up and back into the storage

position. Make sure the limit

switch is depressed when your raise

it

3. Newer presetters (the second

picture) are deployed by the

controller pneumatically. Go into

MDI, press PROGRAM. Scroll over

to the PROBE tab, and press WRITE/

ENTER to go into it. Now press F1 to

deploy the presetter. Pressing F1 again

while in the same menu will retract

it again. Make sure the turret is clear

before retracting it

Do not try to lower the new presetters

by hand, you will damage it

4. Now that the presetter is deployed, touch the tool off of it

Set Tool Offsets

Table of Contents

Page 44


Touching Off of the Presetter

Now that the presetter is down, use it to set

your offsets.

1. Press HANDLE JOG

2. Press OFFSET until the Tool

Geometry Offsets page is displayed

3. Jog the tool in front of the face of the

probe you want to touch

4. Press the 0.001” handle jog increment

5. Press and hold the jog direction arrow

to jog the tool towards the part

6. Watch the offset. When the machine

beeps, it will stop the tool and set the

offset

7. Jog the tool away from the presetter.

Set the other direction with the tool, if

necessary

8. Verify that the tool offsets were set

correctly

9. Handle jog the tool back to home

position, and repeat with any other tools

Do not use the home button, it may jog

through the probe.

Set Tool Offsets

Table of Contents

Page 45


Setting Work Offsets

On a two axis lathe, the Z axis offset is

generally the only work offset that needs to

be set. The X offset should always be set to

zero.

The Z offset is the distance between the tool

reference plane and the part origin. If you

set your tools off the front of the part, zero

the Z offset in the same way as the X offset.

Contents

Zero the X Offset 47

Set Z Work Offset on a Lathe with a Gauge 48

Set Z Work Offset on a Lathe with a Test Cut 49

Verify Z Work Offset 50

Table of

Contents

Page 46


Zero the X Offset

The X axis offset should always be set

to zero on lathes. Failure to do so can

break drills and taps since they’ll cut off

centerline.

1. Press OFFSET until the Work

Offsets screen is active

2. Highlight the X offset you need to zero

3. Press the 0 button, then F1 to overwrite the existing number

4. Double check to make sure that the X offset is zero

Page 47


Set Z Work Offset on a Lathe with a Gauge

1. Set your tool offsets with a gauge

If you set your offsets from the front of the

part your Z work offset should be zero

2. Handle jog a tool that has its

offsets set to the front of the

part

3. Use the reference gauge to

touch the tool off the front

of your part

Set the offset off a low point

on the surface if it hasn’t been faced

off.

4. Press OFFSET until you’re at the

Work Offsets screen

5. Highlight the Z offset you want to

set, and press Z FACE MEASURE

Watch the offset carefully to make

sure it updates.

6. Subtract the width of your

reference gauge

7. Verify the offset

Setting Work Offsets

Table of Contents

Page 48


Set Z Work Offset on a Lathe with a Test Cut

1. Face off the front of your part

using a tool whose offsets are set.

Don’t move your tool in Z after

you finish the cut.

2. Press OFFSET until you’re at the

Work Offsets screen.

3. Highlight the Z offset you want to

set

4. Press Z FACE MEASURE

5. Verify the work offset

Watch the offset carefully to make

sure it updates.

Setting Work Offsets

Table of Contents

Page 49


Verify Z Work Offset

The Z work offset is the distance between

the reference plane where your tools are

set and the work origin of your part. It’s

important to verify this to make sure that it’s

set correctly to prevent crashes.

1. Handle jog your tool to the Z tool

offset position, like when you verified

the tool offsets

2. Look at the active Z work offset, and

jog your tool that distance relative to

the current location of the tool

Be careful to keep track

of signs. Going towards

the chuck is negative,

away is positive.

3. Check that the current

position of the tool is at

the origin of your part.

If it isn’t, reset your

offset

Page 50


Program Operation

When you are running the program, there are some basic steps you can

take to ensure that your program won’t fail. This section describes how to

perform some of the steps on the operator checklist.

Contents

Simulate in CAM 52

Simulate on the Controller 53

Reduce the Rapid Rate 54

Check the Distance to Go 55

Table of Contents

Page 51


Simulate in CAM

The instructions given here are for ESPRIT. However, the process will

be similar for any CAM software

1. Open your CAM file.

2. Enter the simulation mode

3. Enter Simulation Parameters and enable collision detection to Full

4. Run the simulation and watch for crashes

Program Operation

Table of Contents

Page 52


Simulate on the Controller

1. Ensure the desired program is selected. Press the MEM button

2. Press SETNG GRAPH twice above the arrow keys to enter the

graphics display

3. Press F3 and F4 to show the code and machine position

4. Press CYCLE START to start the simulation

5. Look at the display to check if there are alarm messages or whether

the tool path is as expected

6. If the tool path isn’t on the screen, press F2. Use the arrow keys to

move the window around. PAGE UP and PAGE DOWN will zoom

the display in and out. WRITE/ENTER will confirm the movement,

then press CYCLE START to run the simulation again

Pay attention to the small preview display below the main display.

You can see where the window will end up

Program Operation

Table of Contents

Page 53


Reduce the Rapid Rate

Rapid rape on CNC machines

is generally very fast, over 500

inches per minute. In order to

give time for the operator to

react, you should reduce the

rapid rate during setup.

1. Determine what rapid

rate you’re comfortable

with

2. Hit the appropriate rapid

rate override in the override section

3. Check the display to make sure that the rapid rate has actually been

reduced

Program Operation

Table of Contents

Page 54


Check the Distance to Go

1. In the CURRENT COMMANDS

display, pull up the DISTANCE TO GO

coordinate display:

a. On older controllers, press the DOWN ARROW until DIST TO GO

appears in the top right of the screen

b. On newer controllers, press

PAGE DOWN until the

coordinates display appears

2. Run your program. As each

tool approaches the part, press

feedhold about 0.5-1” away

from the part

3. Check which X and Z position

it’s going to by reading the

program

4. Compare the distances in the

DIST TO GO coordinate to

how far the machine physically

has to go

This measurement is an

eyeball measurement, just a rough check. Also note that the X

distance to go is in diameter, not radius.

If you can’t see the tool clearly, stop the spindle and open the door.

5. If the DIST TO GO matches up with the physical distance, continue the

program. Otherwise, stop and fix your offsets

Program Operation

Table of Contents

Page 55


Clean Work Area

It is important to clean the work

area every time you use the

machine.

1. Remove your part safely

and brush chips off the

chuck

2. Use a chip brush to move

all the chips down into the

chip augur/conveyor

3. Close the door

4. Press CHIP FWD to start

the conveyor or augur.

Wait until the chips are

dumped in the bin

5. Press CHIP STOP

6. Wipe down the outside of the

machine tool and the controller as

necessary

Table of Contents

Page 56


ABOUT THE AUTHOR

Professor Torbjorn Bergstrom has been researching and

teaching advanced manufacturing topics since 1998. The

contents of this Quick Guide were developed over a period of

over 10 years spent teaching over 10,000 students the basics

of CNC Machining. Users of these materials have ranged in age

from 12 to 66 and have successfully used the materials to learn

the basics of CNC Setup.

In addition to CNC Training Professor Bergstrom has been

active in the areas of Surface Metrology and Additive

Manufacturing. As a Member of the Haas Technical Education

Center Council he has served as 4 Year University

Representative and Vice President and President.

For more information or to contact Professor Bergstrom please

visit his professional website.

http://profBergstrom.com

HAAS LATHES

updated content and video instructions please visit us at

For

http://CNCQuickGuide.com

Printable PDF Edition ISBN: 978-0-9971886-0-8

Copyright Engineering Media Productions 2015

More magazines by this user