FANUC CNC Manual

1 Contents

OVERVIEW OF CNC TRAINING IN DFAB ------------------------------------------------------------------------ 3

2.1

PREREQUISITES------------------------------------------------------------------------------------------------------------------ 3

2.2

READ FANUC OPERATORS MANUAL -------------------------------------------------------------------------------------- 3

2.3

CNC LEVEL 1-------------------------------------------------------------------------------------------------------------------- 3

2.4

CNC LEVEL 2-------------------------------------------------------------------------------------------------------------------- 4

2.5

CNC LEVEL 3-------------------------------------------------------------------------------------------------------------------- 5

SAFETY ----------------------------------------------------------------------------------------------------------------------- 6

3.1

GENERAL FANUC CNC MACHINE SAFETY------------------------------------------------------------------------------- 6

3.2

MACHINE CRASH / ACCIDENT REPORTING ------------------------------------------------------------------------------- 6

FUNDAMENTAL CONCEPTS ----------------------------------------------------------------------------------------- 7

4.1

AXIS OF MOTION --------------------------------------------------------------------------------------------------------------- 7

4.2

G CODE PROGRAMING WORDS AND SYNTAX----------------------------------------------------------------------------- 7

4.3

OFFSETS ------------------------------------------------------------------------------------------------------------------------ 11

CNC TOOLING FOR WOOD, PRIMARILY ------------------------------------------------------------------------14

5.1

DRILL VS. MILL ---------------------------------------------------------------------------------------------------------------- 14

5.2

TOOL LOAD-------------------------------------------------------------------------------------------------------------------- 14

5.3

FLUTE TYPE-------------------------------------------------------------------------------------------------------------------- 15

5.4

TOOL PROFILE ---------------------------------------------------------------------------------------------------------------- 16

5.5

TOOL HOLDERS --------------------------------------------------------------------------------------------------------------- 16

5.6

FEEDS AND SPEEDS ---------------------------------------------------------------------------------------------------------- 17

5.7

WORK HOLDING-------------------------------------------------------------------------------------------------------------- 18

CREATE A CAM FILE ---------------------------------------------------------------------------------------------------19

6.1

DRAWING ---------------------------------------------------------------------------------------------------------------------- 19

6.2

RESERVED WORK OFFSETS FOR FANUC IN DFAB--------------------------------------------------------------------- 19

6.3

TOOLPATH BASICS ------------------------------------------------------------------------------------------------------------ 20

6.4

SIMULATION ------------------------------------------------------------------------------------------------------------------- 21

6.5

CHECKING GCODE ----------------------------------------------------------------------------------------------------------- 21

6.6

SAVE A PROGRAM ON THE NETWORK DRIVE --------------------------------------------------------------------------- 23

ALL THOSE BUTTONS! ----------------------------------------------------------------------------------------------- 24

7.1

CONTROL PANEL ------------------------------------------------------------------------------------------------------------- 25

7.2

MACHINE PANEL ------------------------------------------------------------------------------------------------------------- 26

MACHINE OPERATION ---------------------------------------------------------------------------------------------- 29

8.1

POWER UP---------------------------------------------------------------------------------------------------------------------- 29

8.2

QUICK REVIEW OF NOMENCLATURE ------------------------------------------------------------------------------------- 29

8.3

LOAD AND RUN A FILE ------------------------------------------------------------------------------------------------------ 29

8.4

SPINDLE WARMUP ------------------------------------------------------------------------------------------------------------ 32

8.5

STORE A WORK OFFSET (M402) ------------------------------------------------------------------------------------------- 32

8.6

JOG MODE --------------------------------------------------------------------------------------------------------------------- 33

8.7

SOME COMMON MISTAKES ------------------------------------------------------------------------------------------------- 33

8.8

CLEAN UP ---------------------------------------------------------------------------------------------------------------------- 33

ADVANCED MACHINE OPERATION ---------------------------------------------------------------------------- 34

9.1

STOP AND JOG AWAY, RETURN AND CONTINUE CUTTING ----------------------------------------------------------- 34

9.2

MAKE A RELATIVE MEASUREMENT --------------------------------------------------------------------------------------- 34

9.3

STORE A TOOL LENGTH OFFSET ------------------------------------------------------------------------------------------ 35

9.4

VIEW OR MODIFY THE VALUES STORED IN A WORK OFFSET-------------------------------------------------------- 36

ALARMS AND RECOVERY ------------------------------------------------------------------------------------------- 37

10.1

SOFT OVER-TRAVEL ALARM------------------------------------------------------------------------------------------------ 37

10.2

HARD OVER-TRAVEL ALARM ---------------------------------------------------------------------------------------------- 37

10.3

PAUSED IN THE MIDDLE OF A TOOL CHANGE------------------------------------------------------------------------- 37

REFERENCE-------------------------------------------------------------------------------------------------------------- 39

11.1

I/O CHANNELS --------------------------------------------------------------------------------------------------------------- 39

11.2

COMMON PARAMETERS------------------------------------------------------------------------------------------------------ 39

11.3

G CODES (UNABRIDGED) --------------------------------------------------------------------------------------------------- 40

11.4

M CODES (UNABRIDGED) --------------------------------------------------------------------------------------------------- 42

11.5

TOOL SIZE SHAPE AND SPEED FOR HSD SPINDLE --------------------------------------------------------------------- 43

2 Overview of CNC Training in dFab

We all learn at various speeds and all have diverse existing skill sets. Take your time and have fun!

2.1 Prerequisites

• Understanding of CAD software used in dFab is fundamental in using this equipment. You must have a

foundation in Rhino3d, Fusion360 or Inventor. Approximately 6 months to a year of heavy use in the

software is sufficient.

• Understanding of why you want to use a CNC machine and what it does.

• Other rapid prototyping experience such as laser cutting and 3d printing

• Understanding of Windows file structure and how to access a server

2.2 Read FANUC Operators Manual

Estimated Time: 1-3 Hours independent work

Please read, take notes and comment on this document. A printed copy is available in dFab or upon request

for current MICA students. This is a working document and we would like to make it better, your input

matters!

2.3 CNC Level 1

Learn Through Coursework

Students are only permitted to use the CNC under direct supervision of their training faculty in Level 1.

Training faculty (Level 3) or Level 3 Tech scheduled for that purpose must be present at the machine while

any student in Level 1 is using the CNC.

2.3.1 Hands on Introduction

Prior to taking any tests or even performing any reading, you may be introduced to the CNC on a superficial

level so that the concepts and procedures in training are more meaningful. The files are carefully prepared by

your faculty member, and they will guide you through responsible and safe machine operation as well as

discus any safety risks associated with this specific task. Students are not permitted to generate their own files

at this time. Tasks students may perform after this instruction and under direct faculty supervision include:

Jogging the machine, loading the file, punching into the MDI. Faculty will demonstrate operator position and

run the file.

2.3.2 Introduction to CAM and Toolpaths

In this coursework you will learn about:

• Setting Stock in your file

•

2d operations including profiling, pocketing and engraving

•

Tooling, tool offsets, climb cutting

•

Work zero, fixtures, work holding

•

Simulations and checking for collisions

•

Axial and Radial tool load

•

Entry and Exit/Linking parameters

Take notes in your coursework. To work independently you will be expected to know all of the above

concepts.

2.3.3 Written Test

After reading this manual, take the CNC Test 1. You must complete the test with a 100% score to operate the

machine. The test is not graded on your transcript and you may take the test as many times as you would like

to achieve a perfect score. You will be emailed a response with a copy of your test. Click “VIEW SCORE” to

see how you did, and click “Edit response” to change your answers. Successfully achieving a perfect score on

the written test is mandatory before students can operate the machine in class.

2.3.4 First Operation

We will review the manual, cover safety and have time for questions. After a demonstration, each student will

operate the machine under direct supervision of their training faculty during class or CNC Level 3 tech

scheduled for that purpose to cut a file prepared by the student. We will review jogging the machine, then

cover how to perform a tool change with the MDI and finally run a job on the machine.

Topics Covered: Jog Mode, MDI, Feed Override, Emergency Stop, Reset, Loading Files, Work Offsets, Tool

Offsets, Control Navigation, Work Holding/Fixtures.

2.3.5 Practice

Estimated Time: 2-10 jobs

Create your own files including a design file and all CAM work. Stay within your existing skill set! Work with

your instructor and have them review your work before each cut. Your faculty will supervise cuts in this stage.

Please wait to buy material until after a consultation with your instructor after you believe you have

completed a good set of toolpaths to cut your part, often considerable changes are desired by the student in

this initial meeting.

Try to do as much as possible. If your instructor shows you how to set something up or how to create a

toolpath, break it down and re-do it right after your meeting so you can really grasp the concept.

Be patient and try to learn one thing at a time. Learning this content can be overwhelming due to all the

seemingly minute details. The best practice for overcoming this learning curve is to make multiple small or

short cuts on consecutive days. Focus on learning the workflow, then apply it to your work.

2.4 CNC Level 2

Use of CNC after taking CNC Coursework

Complete the below requirements to use CNC outside of class time or after the course covering CNC ends.

2.4.1 Written Test

You must complete the Level 2 Test with a 100% score to operate the machine after taking coursework that

covers this content. The test is not graded on your transcript and you may take the test as many times as you

would like to achieve a perfect score. You will be emailed a response with a copy of your test. Click “VIEW

SCORE” to see how you did, and click “Edit response” to change your answers.

2.4.2 Practical Test

After successfully achieving a perfect score on the CNC Level 2 written test, you may take the Level 2

Practical Test, certifying that you are capable of creating a basic CAM file, checking that file and safely

running that file.

2.4.3 Getting Help

You may reach out to your faculty or the studio manager directly to schedule a time to review your file. The

expectation is that you will have specific questions prepared for the discussion and that you will have your file

available on the server for review. Expect to take notes on what is covered in your meeting.

2.4.4 Scheduling the Machine

Each time you want to use the CNC, schedule a meeting to review your file with the Studio Manager. After

reviewing your file we will schedule a cut time.

Prepare to run your file by reviewing the training manual. On the day of Cut Time, arrive 10-15 min before

you are scheduled to prepare yourself, review the toolpaths, get material ready, consider your

fixture/spoilboard etc. If no one is on the machine, go ahead and start setting up even if you arrive early.

2.5 CNC Level 3

Independent Use

Complete the below requirements to use CNC when Studio Manager is not present.

2.5.1 Written Test

After you become proficient with the CNC machines there is no better way to continue to progress then to

help others learn this process! Initiate this stage by taking the CNC level 3 written test then reach out to the

Studio Manager. A perfect score on the test is the first step, followed by a practical discussion with the Studio

Manager. You will begin to help students individually while maintaining close communication with the Studio

Manager.

2.5.2 Practical Test

You will be provided with an example file containing common student errors. Fix the errors, post the code,

check the code and successfully run the program to pass. No mistakes are permitted. One week must elapse

before taking the practical test for a second time.

3 Safety

3.1 General FANUC CNC Machine Safety

• Never step inside the painted line while the machine is in operation.

• Wear safety glasses when performing setup operations (spindle off) and whenever the spindle is on

• During setup, only the operator may reach inside the yellow line to make measurements.

• Hearing protection is advised for everyone in the machine shop while the CNC spindle is on

• Always firmly check the fixture (vacuum table hold down or other fixture devices) prior to running a

job

• Warped plywood or any material that is not completely flat will not be held securely by the vacuum.

If you can move the part at all, you will need to devise another method to hold the part down

• Verify work offsets, tool offsets and your program prior to execution

• Check your gCode for breakthrough amounts, work offsets and correct post processor.

• UNDERSTAND WHAT YOU ARE DOING! NOT UNDERSTANDING = SEVERE

DANGER!!!

• The first time you run the machine, practice stopping the program with your instructor. Be sure to

discuss cycle stop, reset, spindle stop and the E-Stop.

• Ensure that E-stop is depressed prior to powering on or off the machine. Do not press any keys or

switches on the control until the position display or alarm screen appears. Some keys are dedicated to

maintenance or other special operations. Pressing any of these keys may place the CNC in other than

its normal state, starting the machine in this state could cause it to behave unexpectedly.

3.2 Machine Crash / Accident Reporting

Do not move anything, we will need the tool, material and files

Ensure the safety of yourself and others, contact Campus Safety if medical attention is needed.

DO NOT MOVE THE SPINDLE. An attempt to recover the machine incorrectly will damage the machine

further. FAR MORE DAMAGE CAN OCCUR AFTER THE CRASH BY JOGGING THE SPINDLE.

Collect the following materials and information:

1. Student Name and contact information (remind them that they are not in trouble)

2. CAM file - Rhino file with RhinoCAM used for project or Fusion 360 file

3. The actual *.nc file (gCode) that was running at the time of crash

4. The material being cut, leave this in place on the machine. The student may get it back if they desire,

but we will need it until we are able to fully understand what happened.

5. The time of incident

6. Your account of what happened, your assessment of what procedure was not followed leading to the

mistake.

7. Store the files and information collected on the server under

\\picasso\Courses\_Student Resources\dFab\Shared\__FANUC__\Crash Log

8. Have the student reach out to McKibbin to find a time the next day when they can discuss what

happened

9. Lock out the machine

4 Fundamental Concepts

4.1 Axis of Motion

There are 6 axis of motion for any one rigid body, 3 rotational axis and 3 linear axis. The linear axis are

termed X Y and Z, while the rotational axis are termed A, B and C. The A axis rotates with the X as its

center, B with the Y axis and C with the Z axis.

4.2 G Code Programing Words and Syntax

A CNC (Computer Numeric Control) machine uses gCode as a list of sequential instructions. This is a text

file that contains a series of axial and sometimes rotational moves. A document containing gCode is typically

created with a CAM (Computer Aided Manufacturing) program. It may be viewed and edited in a text editor

and is stored as an *.nc file. The axis is specified with a letter, XY or Z for linear axis and a number which

tells the machine how far to travel on the corresponding axis. To change the machine state, such as turn on

or off the spindle, M and G codes are used.

4.2.1 Building Blocks: Blocks, EOB ,G01, Decimal, Comment, Sections

Each line in a program is called a block. Each block ends with a semicolon ; called and end of block

character [EOB]. The control will execute one block of code at a time. It will consider all information on that

line and interpret that entire line as one. For example

G01 X62.0 Y99.0 Z-1.0 F100.0;

The control will simultaneously move in all three axis at once arriving at the XYZ location (62,99,-1) at the

end of the line. This is to say that the machine will not first go to X62.0, then to Y99.0, then to Z-1.0. All

motion will happen synchronously. The machine is put in this state of synchronous linear interpolation

(simultaneous straight line motion between the current location and the location specified by the current

block) through the use of the code G01. This is pronounced gee zero one, or gee one. It’s a really common

code, probably the most used gCode in machining. The line is followed by an F word. By the way, for some

reason letters are called words in CNC programming… I don’t know, it’s a convention that’s used so you

may see it pop up from time to time. The number following the F is the feed rate, the units are inches per

minute or ipm.

Notice that each number specified includes a decimal point. On most CNC machines if we forget the decimal

point, the measurement is assumed to be in the minimum units on that control. So saying X1 is equivalent to

saying X0.0001 on our FANUC. Get in the habit of always specifying a decimal.

Another important concept in all programing languages is a comment. Comments are easy for a human to

read, and understand what is going on in the code. In gCode, comments are contained with parentheses.

(this is a comment)

Comments can follow code too

G01 X62.0 Y99.0 Z-1.0 F100.0; (like this)

Finally all programs start and end with a percent sign.

Now that you have an understanding of the basic syntax, we need to briefly discuss program structure.

Programs, like essays, can be thought of as divided into sections. Programs can be broken down into three

sections, safe startup, actions, and reset. Below is a short example program showing what this looks like. You

may notice that the EOB (;) has been omitted. On most modern controls EOB is only needed for programs

run out of the MDI (manual data input mode, a method of punching in code directly on a control rather than

editing in a text editor or CAM software)

(My First Program)

(Safe Startup)

G00 G90 G17 (Rapid, Absolute, XY plane for circles)

G80 (Cancel Canned Cycles... drilling cycles)

G20 (Inches)

G54 (work offset)

(Actions)

M6T9 (tool change tool 9)

G00 X0 Y0 (rapid move to work offset)

G00 G43 H9 Z3.0 (instate the tool length offset and move the tool tip to 3 inches

above the work offset)

G01 Z-0.25 F30.0 (plunge down into the cut at a slow feed rate)

G01 X20.0 Y20.0 F100.0 (make our diagonal cut at ¼ inch)

G00 Z1.0 (return to a safe height above the material)

(Reset)

G53 Z0.0 (raise the tool to machine coordinate Z0)

G53 Y99.0 (move the tool as far away as possible)

M5 (turn off the spindle)

M6 T0 (put the tool away)

G53 X62.0 (park the spindle off to the side of the machine)

M30 (end the program, reset the control, return to program top)

4.2.2 Tool Change (M6)

M6 Tnn;

The M6 is a function, a tool change function, which calls a sub program to perform the tool change. That sub

program needs to be passed a variable, the tool number, to know what tool to use. The ‘nn” stands for

number, in this case up to two digits.

So for example to put the tool away you would use

M6 T0;

To pick up tool 6 you would type

M6 T6;

4.2.3 Park the Machine, Machine Coordinates (G53)

The G53 allows us to temporarily access the machine coordinate system. The code below would park the

spindle where it’s left over night. Doing so communicates to anyone in the shop that the machine is working

correctly and available for use.

G53 z0;

G53 X62. Y99.;

Notice that we first make the Z move up to Machine Zero, then the X Y move. Most times this is the safest

way to move, first move away in Z then in X and Y. It’s really important to think about the order in which

the commands will be executed, do this with the X Y first then Z and you could really easily crash.

We are using Machine Coordinate System (G53) which is a non-modal code, meaning it only is active for that

block. For example, check out the following code:

G54;

G00 X0. Y0.;

G53 X0.Y0.;

Y20.;

First the machine would move to the G54 work offset, then it would move to machine home, then it would

move to Y20 relitive to G54.

4.2.4 Check Tool Length, Work Offset (G54), Tool Offset (G43)

The below code would allow you to check if the tool length and work offset are correct. It presumes that

your work offset is at the top of the material. Typically in dFab we set the work zero to the bottom of the

material, but that makes this code a little more complicated… understand this first.

G54; (Work Offset)

G00; (Rapid Move)

M6 T5; (Tool 5)

G43 H5 Z3.0; (Use tool length compensation, move tool tip to 3” above work offset)

4.2.5 Essential G and M Codes

Knowing some of these code is essential to understanding and using CNC machines. There are about 200

common G and M codes, you do not need to know all of them! Let’s start with some basics. Below are lists

of essential G and M codes for our FANUC. G codes (G standing for General) are standardized across

machines, they will work with any machine. Once you learn these for one machine, they are the same codes

used on any other CNC machine, and almost identical to the gCodes for 3d printers. M codes (M standing for

Miscellaneous or Machine) on the other hand are machine specific. Many are standard such as M6 for tool

change or M30 for end of program, but how the machine performs that tool change is likely quite different.

A block must not contain multiple G codes from a single group (you can’t put G00 and G01 on one line) and

can only contain one M code.

Take 2 minutes to read over this abridged list of codes and try to memorize just 4 of them for now: G00,

G01, M6 and M00.

4.2.5.1

G Codes

G00 Rapid Move

G01 Linear Interpolation

G02 CW circle

G03 CCW circle

G04 Dwell (G4 Xnnn.nnnn)

G43 Instate Tool Length Compensation (G43 Hnn Z3.0)

G53 Machine Coordinate System (G53 X62. Y99.)

G54-G59 Work Offsets

G81 Drill

G90 Absolute Coordinates (almost always use this)

G91 Relative Coordinates (rarely use this)

4.2.5.2 M Codes

M00 Program Stop, Non Optional

M01 Optional Stop

M03 Spindle on CW (M3 Snnnnn)

M05 Spindle Off

M06 Tool Change (M6 Tnn)

M30 End of Program

M48 Dust Hood Up

M49 Dust Hood Down

M402 Store Work Offset (M402 Wnn)

4.2.6 Modal or Non-Modal

It’s worth noting here that all of these codes fall into two categories modal or non-modal. With the non-

modal commands in bold above.

Modal commands stay active until they are turned off with another command. Examples of modal

commands would be G54-59 or G01. Once this word has been said, it is always active. It’s perfectly OK to

state a modal word redundantly, and sometimes we do for clarity. For example, G00 is turned off by G01, so

after it is stated at the top of the code, we wouldn’t need the G00 on any other lines until after the G01, but

many programmers prefer to have G00, G01 G02 or G03 etc. at the start of each line.

Some examples of non-modal commands would be G53 or M00. These are only active for that single line,

then are no longer considered by the control. If I wanted to make two sequential moves that are relative to

the machine coordinate system on different lines, I need to use a G53 word on each line as in the example

“my first program” above, otherwise the second move, Y99 in this case, will be relative to the active work

offset (G54).

4.2.7 Variables

Our control is equipped with Custom Macro B which allows for conditional statements and variables to

appear in the gCode. This is used extensively behind the scenes, in the tool change script. Custom Macro is

beyond the scope of this document, however we do use one local variable in the gCode. It’s #1 and will look

something like

#1=0.70;

This code stores the value (0.70) into #1 and can be called in the program by saying #1

4.3 Offsets

Offsets make your program more flexible, and easier to write. When we write gCode for a CNC we are

programming for the center of the tool tip, and we want the point X 0.0 Y0.0 Z 0.0 in the program to be in a

convenient location that is easy to find on the machine and on the computer.

4.3.1 Definitions

Origin: An agreed upon fixed point of reference for the geometry of the surrounding space. World zero in

the CAD model, machine home in the physical world.

Work Zero: Similar to an origin, all points in the toolpath and subsequent gCode of a programmed part are

relative to a work zero. Unlike an origin, a work zero may be moved within the referenced geometry and there

may be multiple work zero locations within one CAM file. When setting a work zero, there is the option to

choose which work offset (G54-G59) will be output. If no work offset is chosen, G54 will be used.

Work Offset (Work Coordinates): Similar to an origin, this is a physical location stored on the machine

control. It is relative to the Machine Coordinate System (G53) and may be referenced in the gCode with the

following range of words G54-G59.

In practice the terms origin, work zero, work offset, work coordinates and G54 are all used

interchangeably.

Double and triple check that your work zero correlates with your work offset. The most common mistake is to

set your work zero to the top near left corner of your stock in the model but set the work offset to the

bottom near left corner of your part on the machine. This will result in a pretty scary crash!

4.3.2 Work Offsets

On any CNC machine (including lasers, plasma, router, mill, 3d printer etc.) all coordinates are relative to a

home position (or G53 X0.0 Y0.0 Z0.0). This is the location where all axes touch some sort of switch to

let the control know they are zeroed or home. On simple machines like 3d printers, all moves are relative to

the machine home position. On the Prusai3MK3 that’s the near left hand corner of the bed, about where it

makes that first purge and wipe move before printing.

On more sophisticated equipment such as a CNC Mill you will want to move that coordinate system around

for a variety of reasons. For example, you may want hold a part in a vice for its first operation, but then move

it to the 4th axis for the second operation. You may want to have two setups side by side so that you can do a

production run cutting both sides of a part. Imagine how annoying it would be to have to measure locate the

fixture in your file! What if it moved even the slightest amount?

It’s so common to move the coordinate system around that you must specify a work offset before you can

make any cuts on a CNC Mill. Let’s say that the vice is G54 and the 4th axis is G55. To use the vice you

would put G54 at the top of your program and everything that follows would be relative to the position you

stored for G54, to move to the 4th axis you would put a G55 in the program, every move following the G55

would be relative to the 4th axis.

To store the location of the work offset on the machine we need to record it relative to Machine Home.

Machine home is 0,0,0 so if we want to have G54 away 3” and to the right 2” we would have to tell the

machine that G54 is located at Y3.0 and X 2.0. Specifics on how to do this are addressed in the Machine

Operation section. See Reserved Work Offsets for FANUC in Create a CAM File for more on how we use them.

4.3.3 Tool Length Offsets

If we were working with only one tool, there would be no need for tool length offsets. We could easily

include them in the Z component of the work offset and start making chips. Because the tools will vary in

length, if we are wanting to use multiple tools in one file, tool offsets become necessary. Think of them as a

variable Z component for a work offset. Like work offsets, tool offsets are modal and will remain active until

they are canceled or replaced with another offset.

There are two main schools of thought with work offsets, we’ll call them the FANUC method and the HAAS

method. In both methods a value is stored in a tool height registry. There is a spot for each tool number and

they are called from the program with an H value like in the Check Tool Length, Work Offset, Tool Offset example

above. Specifics on how to do this are addressed in the Machine Operation section, below we will cover the

concepts.

4.3.3.1 FANUC Method

The work offset is stored as the distance in

XYZ from Machine Home (G53) to the

spindle nose, centered on the offset

location.

The Tool Length Offset (Hnn) is stored as

the distance from the spindle nose to the

tool tip. We use a height gauge to measure

this length of each tool on a surface plate

and manually input it to the control.

Using this method you never actually need

to drive the spindle nose to the location to

find a work offset. It’s possible to find any

new work offset by driving the tool tip

down, then subtracting the tool length

from the measurement.

The Z component of the work offset will

be a rather large negative number, and the

tool length will be a positive number.

When the two are added together we get a

negative number that is closer to zero than

the Z work offset alone.

4.3.3.2 HAAS Method

Each Tool Offset is stored as the

distance from Machine Home (G53) to a

known location. In dFab we use the 3 in

side of a 123 block off the table.

To find the work offset, we make a

relative measurement with any tool from

the 123 block to the work offset and

enter that for the Z component in the

work offset.

If the tool is long we will have a smaller

negative number and if the tool is short

we will have a larger negative number as

the tool offset.

The work offset will always be the

distance in Z from the top of the 123

block to wherever your Work Zero is

located on your material.

4.3.4 Offset Safety

When we make measurements on the machine, we NEVER actually move the machine to touch our stock.

We always drive the machine close and use a 123 block, a precision ground piece of steel that has the

dimensions 1”x2”x3”, to gauge the distance.

When adjusting the tool height, move the 123 block off to the side, then once the adjustment has been made

slide the block to check. Do not force the block under the tool, move it slowly and feel for any contact. If

there is contact, raise the tool by 0.001” and try again. This is a very fast and safe method of verifying the Z

components of our work and tool offset. The control is capable of addition and subtraction so we can just

subtract 1” from our measurement and move right along.

5 CNC Tooling for Wood, Primarily

Because it is so much more affordable and forgiving, our conversation about tooling will be focused on wood

cutting tools. Where applicable there are some parameters and information below that applies to metal cutting

tooling as well.

5.1 Drill vs. Mill

Drill bits intended to cut along the axis of rotation (axial engagement) as when plunging, or stepping down

into the material. The flutes are not sharpened and are intended only to remove chips. Drills are not effective

at cutting when moved sideways in the cut.

Mills are most effective at cutting when stepping over along the radius as the tool rotates (radial engagement),

some mills cannot plunge, and can only cut when the side of the tool is engaged with the material.

5.2 Tool Load

When we engage the tool with the material it moves along its radius as it cuts. Here we are imagining a

section cut of side view of the tool as it cuts through the material.

5.2.1 Peripheral

Whenever possible, axial depth of cut is maximized, this maximizes usage of the sharpened flutes. We need to

leave space for the chips to go, and don’t want to overstress the tool causing breakage, so radial engagement

is low. This strategy is used for finishing operations in pockets, or when removing a small amount of material

around the perimeter of a shape to achieve final dimension. Tools cannot cut deeper than their flute length

when peripheral milling, this is sometimes referred to as CEL or cutting edge length.

5.2.2 Slotting

When cutting parts that are nested on a plywood sheet in dFab we must engage 100% of the tool diameter

radially. As we get deeper into the slot, it becomes more difficult to get the chips out. In wood, all of our

feeds and speeds are calculated so that slots 2x diameter of the tool can be cut in a single pass. In other

words, 100% Radial Depth of cut and 200% Axial Depth of cut are standard in dFab for the tools in the

FANUC library.

5.2.3 Step Over/Step Down:

Step down is the vertical change in Z per pass also known as axial engagement.

Step over is the amount the tool engages in X and Y per pass also known as radial engagement.

5.3 Flute Type

Below are the most common flute types available for router bits along with reasons for selecting a specific

flute type.

5.3.1 Straight Flute

Inexpensive tool with decent finish. Most commonly used with hand held

routers, or on router tables (not CNC). Disadvantages are lower chip loads

(longer cut times). Advantages are low cost and minimal tear out. These

tools are often made from high speed steel with brazed carbide tips. They

are intermittently in contact with the part, whacking it each time a flute

comes around.

5.3.2 Up Spiral

Because of the excellent upward chip evacuation and low cost, these tools

are used for roughing operations where high removal rates are prioritized

over a perfect finish on top of the part. These tools are capable of cutting

deeper and faster than their straight flute counterparts, however they often

tear out on the top of the cut due to the upward sheering motion. Because

of the spiral, the flutes are in constant contact with the part.

5.3.3 Down Spiral

These tools have a sheering spiral that rotates in the opposite direction

from the up spiral, pressing the chips down. The advantage is a clean finish

on the top of your part, no tear out! The disadvantage is terrible chip

evacuation which translates to shallow depth of cut, using many passes to

reach the desired depth. Use in shallow pockets less than ~0.200 inches.

5.3.4 Compression

Most expensive grind on a solid carbide tool, these combine both up and

down spiral into one tool. There is up spiral on the bottom ~0.200 inches

and down spiral on the rest of the tool. These are great for achieving high

feed rates and perfect surface finish on top and bottom plywood, melamine,

particle board, and other engineered woods- producing a good finish on

solid woods too.

5.4 Tool Profile

Descriptions and uses of common tool profiles used when machining 2.5d features in wood on a CNC

router.

5.4.1 End Mill

This is the most common and versatile tool profile. All of the examples so

far have been end mills. These are capable of machining a flat floor and

vertical walls. They have a negligible corner radius, leaving a sharp inside

corner on a pocket when viewed as a section from the front or side. We

use these tools primarily for joinery and cutting parts from a nested sheet.

Due to sharp corners, these tools do not have as long of a lifespan as a

tool with a small radius. These are sometimes offered with 0.005”-0.05”

radius for longer tool life, we use these radius end mills for steel on the

Haas.

5.4.2 Ball Mill

The radius of this style mill when viewed from the side is equal to the

radius of the tool from the top. These are primarily used for 3D machining

operations because they will produce less error in matching an undulating

surface as they follow the toolpath than an end mill. They are also good

for use in pockets when strength is prioritized such as when making

enclosures. The radius edge eliminates tear out when the tool is engaged

axially less than the radius.

5.4.3 V - Mill

These come in a variety of angles, measured as the included angle, so a 45

degree chamfer would be a 90 degree V-Mill. Primary uses include

chamfering edges, engraving, and lettering.

5.5 Tool Holders

Tool Holders allow for the use of an automatic tool changer, tools can be pre-loaded with offsets stored on

the control. This makes for easy and accurate use of a variety of tools in one file. These are held into the

spindle taper with a draw bar which pulls on either a pull stud or on a race inside the cone of the holder.

5.5.1 Tool Holder Types

In dFab we use CAT 40 tool holders on the HAAS and HSK63-F holders on the FANUC.

5.5.2 ER Collet System and How to Assemble

The collet holds the tool into the tool holder, and it is tightened with a collet nut. The first step after selecting

the correct size collet is to snap the nut onto the collet. Next insert that assembly into the tool holder and

finally put the tool into the holder. Be sure not to insert the tool such that the flutes go inside the collet. Also

be sure that the shank of the tool is held by at least ¾ of the length of the collet.

5.6 Feeds and Speeds

These attributes are associated with each tool in the tool library and will be automatically selected. These are

essential concepts, and should you begin to use tooling outside of the tool library or want to work with the

Haas you will need to know this content.

There are two key factors in determining a starting Spindle Speed and Feed Rate for your material and cutting

tool. While the Spindle Speed and Feed Rate are what we actually use in the CNC program, they are

determined from a recommended Cutting Speed in Surface Feet per Minute (SFM) and Chip Load and then

tweaked and perfected through experimentation and experience. There are numerous factors that could

influence your Feed Rate and Spindle Speed and much more information can be found on this subject in

Machinery’s Handbook.

5.6.1.1

Determining Spindle Speed:

The cutting speed, in combination with the tool diameter are used to determine spindle speed. The

cutting speed (SFM) is the linear velocity with which the cutting edge or tooth of your tool moves through

the material to be cut. It is important to note that cutting speed is different than feed rate. In the case of a

milling machine or CNC router, cutting speed is the speed at the cutting edge of a tool in relation to the

material, whereas the feed rate is the speed of the entire cutter in relation to the material. Cutting speed will

allow us to determine spindle speed.

To understand the relationship between cutting speed (SFM) and spindle speed (RPM), imagine a lathe where

the part spins and the cutting tool is stationary. On that lathe there is a round piece with a radius of 1 foot.

The distance that part would travel per revolution would be 2*pi*r or about 6 feet. If that part were rotating

once per min (a spindle speed of 1 rpm), the Cutting Speed at the perimeter would be 6 feet per min or 6

SFM. Notice how the units work too. The circumference of the circle is in feet per revolution or (feet/rev)

and we are multiplying that by revolutions per min (rev/min), the revolutions cancel and we end up with

(feet/min). We typically measure cutting tools in inches so the formula becomes:

V = (pi * D * S) / 12

Where V is the cutting speed in feet per min (SFM), D is the diameter of the cutting tool in inches and S

is the spindle speed in revolutions per minute. It’s helpful to solve for spindle speed because the cutting

speed and tool diameter are known.

S = (12 * V)/(pi * D)

Cutting speed can be lowered to meet your needs, but exceed the given limits for your tool material and part

material and you will damage tooling and have poor part finish.

5.6.1.2

Determining Feed Rate:

Chip load in combination with the spindle speed, calculated above, and the number of teeth on your cutting

tool will determine your feed rate. Chip load, also called feed per tooth, is the thickness in inches of a little

shaving or chip generated by your cutting tool while making a cut. This could also be described as inches per

revolution in the case of a single flute tool, or the advancement per tooth if there are more than one flute.

Chips can be measured if you are cutting plastic or metal, but wood chips tend to break when cut and are

unreliable indicators of chip load. The formula for chip load is below:

f = F / (S * n)

Where f is chip load (inches), F is the feed rate in (inches/min), S is spindle speed (rev/min) and n is

number of teeth. If we solve this for feed rate we get:

F = f * n * S

5.6.1.3

Dialing It In:

The above calculations are a great way to get started, but realistically cutting conditions vary extensively and

can be dialed in for your exact purposes. This can be time consuming for prototyping, so use safe speeds and

feeds to get your part done slowly successfully the first try.

If you are making a long cut or doing a small production run, you’ll want to really dial it in. Start out with the

low end recommendations or your best guess, increase your surface speed within the recommended range for

your tool and material until the part finish starts to decrease. Back off a little bit, then increase your chip load

until part finish starts to decrease.

Tools are designed to handle a specific chip load, and you’ll want to keep them at that chip load if possible.

Reducing the chip load within reason can be good for your cut quality and easier on your setup, however

going too far can make the tool perform very poorly, causing a ton of heat to damage the tool. ¼ inch and

larger tools need 0.001” feed per tooth at minimum.

Keep in mind that even if you have theoretically perfect feeds and speeds, you can still have terrible part

finish or break tools if you are not able to get the chips out of the cut or if your part is not securely held or if

your machine is not rigid enough to take the cut. If your part is moving around, or if you are suspicious that

your part is moving, try reducing the axial load, or try reducing the chip load (feed per tooth), or try

increasing the spindle speed. If you have no idea what to use for some random no-name brand carbide tool,

start here: Chipload: 0.001 to 0.003” SFM: 1000 (wood or plastic), 600 (rigid insulation foam), 80 (steel), 500

(aluminum)

5.7 Work Holding

The part to be machined can be held by various means. Two common methods a vice, or by vacuum. When

using a vacuum, a large vacuum pump is connected to the machine that is gated with valves at the front of the

machine which can be opened or closed to direct the vacuum under your part. The vacuum can be further

directed by use of rubber plugs. Gasket is used to prevent air from leaking in around the sides. To provide a

sacrificial surface so we can cut through our part, we typically use MDF as a spoilboard. This piece of

material holds the vacuum and transfers that holding force to our part. Our vacuum pulls 13” of mercury,

which is under power for a production setting, but still pretty awesome. Using vacuum we can hold parts

around 12” by 12”, smaller parts will require tabs to hold them to the larger sheet, or screws. If you use

screws, you must model them into your stock and be sure not to hit one with the tool.

6 Create a CAM File

CAM (Computer Aided Manufacturing) software is used to create toolpaths from CAD (Computer Aided

Design) geometry. In dFab, our workflow is Rhinoceros 3d (CAD) to RhinoCAM (CAM) or Fusion 360 to

HSMworks which is built into Fusion360 in the “Manufacture” workspace.

This software is beyond the scope of this manual and is only taught through coursework. Your faculty will

review your file with you before they oversee your operation of any dFab CNC equipment. After you and

your faculty are confident with the file, you may schedule time on the machine with the dFab studio manager.

Do not purchase material prior to the review with your faculty, often design changes are made at this time

that result in a change of material thickness or type.

A good overview of this process has been created by Autodesk and can be found under

https://help.autodesk.com/view/fusion360/ENU

Choose manufacture on the left under the Learning header.

Below are important steps in creating a good CAM file.

6.1 Drawing

Your model is the foundation on which everything else is built. You will want to be sure that it is precise.

Often you will need to model in fixtures or stock. These will help the software determine areas to avoid or to

cut.

You do not need to be great at 3d modeling to use CNC, but you do need to be precise and you absolutely

need to be able to think through what the machine will do when cutting your file.

If you just need a couple simple shapes cut out and you can draw them in 2d but do all the 3d planning by

other physical means, go right ahead and do it that way. Too often students let this stuff get way more

complicated than it needs to be. It’s perfectly ok and often advisable to plan your project using methods that

are familiar to you, then draw only the shapes you need before planning your CAM file.

Use the laser cutter or 3d printer to prove concepts or prove your drawing. These methods are incredibly fast

and inexpensive. You will save so much time learning about some small flaw in your file by prototyping with

either of these tools first, and you’ll have some cool models or prototypes to hang on the wall!

6.2 Reserved Work Offsets for FANUC in dFab

We have reserved work zeros in dFab. They are listed here as a reference.

G54 - The top, near, left corner of the spoilboard when it is pressed against the popup pins. This would be

the near left corner of your stock at the bottom. When setting your work zero you must place it at the

corner of your stock that has the lowest value for XY and Z. Maximum depth when cutting on the

spoilboard is G54 Z-0.010, this would be a break through amount of 0.010 inches.

G55 - The near, left top corner of the table. This is used often when cutting solid wood stock to get better

vacuum. Maximum depth when cutting directly on the table is G55 Z0.100, do not ever cut through.

G56 - The near, left, top corner of the 30” by 60” spoilboard when it is centered on the mark on the table.

This would be the near left corner of your stock at the bottom. When setting your work zero you must

place it at the corner of your stock that has the lowest value for XY and Z. Maximum depth when

cutting on the spoilboard is G54 Z-0.010.

G57 -May be reserved on whiteboard check with studio manager, erase when you’re done

G58 -May be reserved on whiteboard check with studio manager, erase when you’re done

G59 -May be reserved on whiteboard check with studio manager, erase when you’re done

6.3 Toolpath Basics

Do not include any extra geometry in the file, it can make setting the stock and clearance plane difficult.

Input geometry is critical. Simple mistakes such as drawing your input curve at the wrong z height will

crash machine. Always use the shortest tool with largest diameter possible.

6.3.1 Stock Setup

Measure your actual stock after you have purchased it with a ruler to the nearest 1/8 inch for X and Y

dimensions, and nearest 0.005 to 0.01” for the Z dimension. Take measurements from all 4 corners for Z

measurement. Don’t forget to adjust your stock in your file and double check the work zero location after the

adjustment.

Extruded Stock: stored in file as “Regions Stock” (RhinoCAM)

Disadvantage - Only extrusions can be defined

Advantage - No separate layer needed, very easy to use,

Recommended to primarily use this form of stock definition whenever possible

From Selection: stored in file as “Regions Stock” (RhinoCAM)

Disadvantage - when hidden then shown after programming, your toolpaths will be affected because

rhino will think you have added new control geometry.

Advantage - Any stock shape can be defined

When using Stock from Selection, put it on a separate layer

6.3.2 Toolpath Types

Do not cut deeper than the CEL (cutting edge length or flute length) and do not break through (cut into the

spoilboard) more than 0.010 inches.

Profile: Intended for cutting shapes from a larger sheet, or carefully finishing a shape to final dimensions.

The cutting tool follows the edge of your control curve or input curve, the centerline of the cut will

be offset by the radius of the tool.

The feeds and speeds used in dFab are such that any tool can cut two times its diameter in wood, and

foam, up to 1x in plastic and ½ its diameter in aluminum or steel in a profiling pass (full width cut)

Pocket: Intended for rough clearing of all material inside of, and up to a control curve or input curve and

down to a single depth. Pockets may go partially through or all the way through your material.

Pockets can be set up to include a finish pass where the tool will cut the walls to size, though best

practice is to follow a pocket with a profiling pass to cut walls to specification. Pockets are used in

place of profiles when small scraps would be sucked off the table and into the dust collection system.

The feeds and speeds used in dFab are such that any tool can cut two times its diameter in wood, and

plastic aluminum or steel with appropriate step over being 10-25% of the tool diameter. Careful

attention must be paid to entry and exit. 1-2 degree helical entry on metals, plastics are 2-5 degrees

and woods or foam is 10 degrees. Watch out for areas where the tool would be slot cutting (not

actually stepping over at the prescribed 10-25%).

Facing: Intended to remove material from the top of stock to bring it to dimension in the Z axis. The center

of the tool cuts up to the line ensuring that the entire part has been cut to the depth specified. Step

over is 25% to 95% with step down being 0.005 to 0.100 inches.

Drill: Intended to engage a tool along its axis to make a round hole. Drills can only go three times their

diameter before we must back the drill out of the hole to clear chips. This process is called pecking.

6.3.3 Entry and Exit

Because end mills are designed to cut radially and not axially (move laterally but not plunge) one of the most

important considerations are how the tool enters the material. RhinoCAM has funny names for these, which

are listed in parentheses below.

Plunge (None) - Tool moves straight down at the programmed plunge feed rate. Plunging implies that there

was no hole drilled prior to engaging the tool with the material, it’s functioning like a drill. This is the

least desirable way to enter a cut.

Ramp (Along Path) - Tool moves along the Z axis while also moving in X and Y to “ramp” down to the

cutting depth. This is the easiest to program and much easier on the tooling than plunging. Use this

for nested sheet cutting or when entering pockets. The path angle must be less than 10 degrees for

wood, and in plastics or aluminum between 2-5 degrees. For steel 1 degree to 3 degrees. The height

of a ramp must be the depth of cut or a little more or the tool will still be plunging.

Pre-defined positions (None) - if prior to plunging a drilling operation is used, the tool can start in that

hole created by the drill. This is the most efficient way to go, but tedious. Generally this would be

used for a production situation in a machine with extra tool holders.

Leads (Lines and Arcs)- These are arc or straight line moves that start off the side of the part or in

previously cut material then engage the uncut material radially. They are used on finishing passes for

pockets, or when access to the outside of the part is easy. These leave a better surface finish than a

ramp.

6.4 Simulation

Both RhinoCAM and Fusion360/Inventor HSM have robust simulation capabilities. You must use the

simulation to check for and verify that there are no collisions.

Both softwares will display red for collisions in the solid simulation model and have the capability alert the

operator of any collisions.

Ask your instructor to show you how to check for collisions, this is especially true when cutting deeper than 1

an inch or when doing any 3d machining.

6.5 Checking gCode

After posting your gcode, review the text file to ensure that you got what you expected.

Notepad++ is the recommended software for this procedure. You can set up a user defined language which

will make viewing gCode much easier.

Go to Language=> Define Your Language… choose Import… and navigate to this folder on the server

\\picasso\Courses\_Student Resources\dFab\Resources\Notepad++ Language

Choose the gCode.xml file. Save and restart Notepad++

You will now see gCode as a language choice at the bottom of the Language Menu

6.5.1 File Name and Post Processor

Your file name will be posted as the first comment in the file, double check that this is on line 3

Directly below the file name, the next comment is which post processor you used. Double check that it is the

dFab FANUC post, or the post for the machine that you are using. All dFab posts will say dFab and the

name of the machine, also below this will be the name of the last person to edit the post and the date it was

last edited.

6.5.2 Work Offset

The default work offset, G54, from RhinoCAM appears on line 13, just before the tool list. If you used

another work offset, look for it after the tool list.

In Fusion the first toolpath will be commented with whatever its name was in your setup. The work offset

will be the first line below that comment probably on line 19. Our post is set up to use the actual offset

number, so do not follow directions from Autodesk on this one, if for example you use 1, it will not post

G54, it would post G1.

6.5.3 Stock Length Z

This line will look something like #1=0.7000 for 0.70 inch plywood. It will be located on line 21 or 22 and

must be the distance in Z from your work zero to the top of your stock.

The machine will stop and prompt the user to check the tool length. The number stored in #1 will be added

to 3” on a line that looks like this:

/ G43 H11 Z[#1+3.0]

This code makes it possible to have the work zero set to the bottom of the stock and check your work offset,

tool offset and stock thickness in one step.

If you are using offsets G57-G59 and your work zero is set to the top of your stock, then change this to

#1=0.00

6.5.4 Max Tool Depth and Break Through

Our standard work offsets (G54 and G55) are at the bottom of your stock (the top of the spoil board) and

the standard break through amount is 0.010” so the max tool depth is usually Z-0.0100 inches

In code posted from RhinoCAM use ctrl+F to find all negative z moves. This would be done by searching

for “z-.” Searching for this will allow you to find each instance where the tool goes negative, it’s far safer than

searching for z-0.010 because in this second case the tool could be cutting to z-0.100 and you would not see

that in your results.

All the keys can be a little overwhelming at first. Let’s take a tour of the Control Panel followed by the

Machine Panel. You will find that it’s not as complicated as one may think after looking closely at each set of

keys and identifying their function.

7.1 Control Panel

We will go from top to bottom, left to right.

7.1.1 Soft Keys

The row of keys at the top are labeled on the screen, you activate them by pressing the button below the

label. In the image below the (CHECK) screen is active.

Notice the two arrow keys on either side? The one on the right is the (CONTINUOUS MENU) key, when a

little + sign is displayed above it the Control is telling you that there are more options available which will be

displayed above the soft keys after pressing it. This will loop around to the beginning after all the options are

displayed.

There is also an arrow on the left, this is the (RETURN MENU) key. Some soft keys, such as (OPRT),

pronounced “operate,” above will have a sub menu of soft keys associated with that choice which will be

displayed. If you want to return to the previous menu, you would press this key. It is available when a little <

character is displayed on the bottom left of the screen.

Throughout this manual we use different nomenclature for [HARD KEYS] and (SOFT KEYS). A [HARD

KEY] is a button which does not change; these keys have labels printed on them.

7.1.2 Reset

This little key is quite important. When pressed it will stop the spindle and stop motion. It will

also return the program to the top and re-set the machine to its power on state. Try not to press

this during a tool change, it will mess up some settings leaving you to wait for help.

7.1.3 ONG - Text Editing Keys

These keys are used to input information first to the input

buffer, an editing line at the bottom of the screen. The

[INPUT] key is used to copy the text from the input

buffer into the control. The most commonly used letters

are available, with the less common ones available by first

pressing the [SHIFT] key. You do not need to hold down

shift, a ^ will be displayed in the input buffer meaning

shift is active. [SHIFT] [Z] would put a W in the buffer.

[CAN] or cancel is backspace, and [DELETE] will clear the input buffer. [EOB] is a semicolon. [ALTER]

will overwrite whatever is selected and [INSERT] will put the code after the word selected by the curser.

7.1.4 Display Modes

[POS] Stands for position, pressing this will display on the screen the

current position with the soft keys offering different coordinate systems.

Relative, Absolute, Machine, or Distance To Go.

[PROG] stands for program. This will display the active program. We always

run from the (CHECK) screen within program which also displays all

coordinate systems as well as the active G and M codes.

[OFS/SET] This key is referred to as offsets. It is where you can store work offsets and tool length offsets.

[MESSAGE] is the key which will display the alarm screen or the operator message screen. Some dFab code

activates this screen to display a message. To return the screen to display the program you are running you

would need to hit the program key.

7.1.5 Navigation

This functions as a regular old “d-pad” up down left right used to navigate

fields on the control. Don’t discount the [PAGE UP] / [PAGE DOWN]

buttons. They are quite efficient.

7.2 Machine Panel

We will go from top to bottom, left to right.

7.2.1 Emergency Stop (E-Stop)

This is a standard twist lock switch. It tells the control to immediately stop all

motion, including the spindle and all axis. Always depress this switch prior to

turning the main power switch on or off as a safety measure.

On the machines we have in dFab, it is always OK to press the E-Stop in the event

of emergency. However, on some machines the E-Stop will disconnect power to

the entire machine which can cause axis to drift while the spindle is winding down

before breaks are activated causing severe damage to the machine.

7.2.2 Spindle Speed Override

This knob will modify the programmed spindle speed

M3 Snnnn (spindle on clockwise, spindle speed is nnnn)

Ranging from 0.5 to 1.2 times the programed speed above, this will change the

actual spindle speed during operation. It’s really useful for dialing in speeds and

feeds for a new tool or cutting condition.

7.2.3 Feed Rate Override

This knob will modify the programmed feed rate

G01 X2.5 Y28. F200. (Make a cutting move at 200 ipm)

Ranging from 0 to 1.2 times the programmed feed above, this will change the

actual feed rate during operation. Notice that this goes all the way to 0 which is a

convenient way of stopping motion in certain circumstances. This is also quite

useful in dialing in feeds and speeds for a new tool or cutting condition.

7.2.4 Operation Modes

Similar to the display modes, however these

change which input will control machine

motion. Only one switch can be active at any

time and they must be chosen correctly for the

desired function to be performed both by the

machine and on the control panel display. A light appears above the switch to show that it is active.

We only use three of these modes in dFab.

[MDI] Manual Data Input allows for gCode to be input using the Text Editing Keys to write simple programs

on the fly. This is used extensively in setup to load tools, check offsets, or drive to a specific location, it’s

faster than jogging the machine… but you’ve got to know a little gCode.

[REMOTE] mode tells the control that you want to run a file from the server. This is the mode that allows

you to run a large program like the ones you created in RhinoCAM, Fusion 360 or InventorHSM. Files are

stored centrally and are drip fed, and buffered in local memory. This process is called DNC or direct

numerical control.

[JOG] mode allows you to press and hold the marked keys below to continuously

jog in those axes. You will jog at 100ipm by pressing the key alone, and 600ipm by

holding down the directional axis key then also depressing the [RAPID] key.

When you are closer than 3 inches from the part in any direction it’s time to use the

Manual Pulse Generator (MPG) also called the Hand Wheel. This will give you

much more control.

Not pictured here, there are two selector knobs at the top, one for axis and one for

step speed with a large wheel labeled + in one direction and - in the other. Axes are

X, Y, Z and 4. Use 4 to lock off the hand wheel when passing it off or hanging it up,

that axis it is not connected. The other selector knob chooses step amount. The x10

label is 0.001” per click and x100 is 0.01” per click. There is also a x1 label, though

that level of precision is not often needed when woodworking and can be ignored.

8 Machine Operation

8.1 Power Up

Ensure that the E-Stop is depressed

Turn the switch on the machine side of the control cabinet

Wait for the display screen to show the position page,

Do not hit any buttons until you see that position screen.

Gently depress the E-stop and twist the outer ring to disengage it

8.2 Quick Review of Nomenclature

Throughout this manual we use different nomenclature for [HARD KEYS] and (SOFT KEYS). A [HARD

KEY] is a button which does not change; these keys have labels printed on them.

The CONTROL PANEL is up top with the LCD display, the MACHINE PANEL is down below with the

E-stop button.

Check out the All Those Buttons! section for a more detailed review.

8.3 Load and Run a File

You have already posted your gCode the CAM software. You verified the toolpaths through the simulation

screen, checked for collisions and reviewed both your posted gCode and toolpaths in the CAM software with

your faculty member.

8.3.1 Ensure that the control is in Embedded Ethernet Mode

MACHINE PANEL: [REMOTE]

CONTROL PANEL: [PROG] (FOLDER) (OPRT) (DEVICECHANGE) (EMBETH)

8.3.2 Load a Program from the Network Drive (Set Your File to DNC)

MACHINE PANEL: [REMOTE]

CONTROL PANEL: [PROG] (FOLDER)

Use the directional keys to navigate the folder tree to your file.

Press [INPUT] to navigate to a sub folder, use the RETURN TO UPPER FOLDER to go up a folder.

Select the file with the directional keys, files have a file extension, folders do not.

Press (DNC SET) you will see the path appear in the DNC FILE field at the top of the screen.

If you do not see (DNC SET) in the middle of the screen as a soft key, choose (OPRT) on the right, then you

will see (DNC SET).

Press [PROGRAM] (CHECK). You will now see a screen that displays position, active G and M codes, as

well as the current feed rate and your gCode (once it’s loaded, nothing will display in this field at this time)

8.3.3 Operator Position

While running a job, the operator will have their index and middle fingers of their right hand covering

[CYCLE START] and [CYCLE STOP] on the MACHINE PANEL.

Their left hand will be holding the FEED OVERRIDE KNOB with thumb down when the knob is at 100%.

Practice turning that knob from 100% to zero twice at this time ensuring you are able to turn that knob

quickly to zero.

Pressing [CYCLE STOP] will stop motion similar to turning the FEED OVERRIDE KNOB to zero

percent.

8.3.4 Starting Your Program

Refer to the Spindle Warmup section below if you want to warmup the spindle before running your file. The

machine will automatically run a warmup if needed when you run your file.

On the MACHINE PANEL:

Ensure that [BLOCK SKIP] is DISABLED and the light above it is NOT lit

Turn the FEED OVERRIDE KNOB to 0% and press [CYCLE START].

Your gCode will be displayed on the right side of the screen. Verify that this is the correct file by checking the

file name in the first comment.

The next two steps verify offsets and are narrated through comments in the gCode on screen. You

will be able to follow along by reading the comments highlighted in blue on the CHECK screen

when actually running your file.

8.3.5 Verify Your Work Offset in X and Y

Press [CYCLE START] and slowly turn the FEED OVERRIDE KNOB to 100%.

While the machine is moving, watch the machine in motion. Always stop motion before looking away from

the spindle.

The machine will move to the tool change position and pick up the first tool (if different than the tool in the

spindle).

The next move will be to X0 Y0 relative to your work offset (G54-59). Practice controlling the [FEED

OVERRIDE] during this move. Visualize a target location on the path of motion and practice stopping the

machine. Motion will automatically stop before any Z motion occurs at the line that says /M00 (unless

[BLOCK SKIP] is depressed).

The tool in the spindle should still be quite high above your part, but close to the Work Zero you chose in

RhinoCAM. If this looks close in X and Y, it’s safe to proceed. If not, stop and figure out where things went

wrong.

8.3.6 Verify the Z Location of Your Work Offset

Set FEED OVERRIDE KNOB to 0%

Ensure that the vacuum is on

Press [CYCLE START], look at the DIST TO GO values. X and Y should read 0.0000; Z should read a

negative number which is the distance between the top of your part and the tool tip plus 3 inches.

Slowly increase the FEED OVERRIDE KNOB while watching the spindle plunge toward your work piece.

Stop motion approximately 4 inches above the surface of your material. DISTANCE TO GO should read

close to -1.000 when you stop, implying that the Z axis has another 1 inch of motion left in the current move.

If you stopped 4 inches above your material and DISTANCE TO GO reads a number that is not close to

1inch, leave the FEED OVERRIDE KNOB at 0% and press [RESET] on the MACHINE PANEL, then

figure out what went wrong.

If all looks correct, you may turn the feed override back up until we complete this block of code. Motion will

stop after this block because the next block is /M00.

Follow the on screen directions to check offsets with the 123 block. The tool should be exactly 3” off the

surface of your material, and centered on the corner of your work offset. If this is the case, Congratulations!!!

You are ready to run your file. Don’t forget to remove the 123 block and turn on the dust collection.

8.3.7 Run Your File

After verifying that your work offset is correct we are ready to execute the rest of your file.

It is imperative that you carefully checked each toolpath for collisions in your CAM software’s

simulation and have not programmed any tools to cut deeper than their cutting edge length, which

is saved with each tool in our library.

Turn the FEED OVERRIDE KNOB to 100%.

With your hand ready to crank FEED OVERRIDE KNOB back to zero, press [CYCLE START] make

some chips! At the next tool change you will be prompted to check the tool length again. Follow instructions

and then press [CYCLE START] to continue.

Each time you run a new file, you must watch the entire program run and check all offsets. Stand in front of

the control, with your hand ready to stop the feed override. This is one of the best opportunities to learn

about how to program a machine, by carefully watching what you have programmed and thinking about how

you could do it better.

If anything happens which is unexpected, such as a tool cutting too deep. Turn the FEED OVERRIDE

KNOB back to 0% and press [SPINDLE STOP] or press the [RESET] button. If there is an emergency,

press the E-stop.

8.4 Spindle Warmup

There are bearings inside the spindle that are so precise they need to be run under no load so that they can

expand. If this step is skipped the spindle bearings will be damaged, it’s a quick 5 min cycle that runs the

spindle at 10,000 rpm, 18,000 rpm then 24,000 rpm. This is performed automatically on a tool change if the

spindle has not been used for an hour or more. Running the spindle without a tool loaded will

catastrophically damage the draw bar, which holds the tools in the spindle.

Some tools, such as T16 (Vortex 4” plainer) cannot be used for spindle warmup because it is not safe

to spin them that fast. The control checks for tool number, certain tools have been flagged as not able to run

a spindle warmup and will warn the operator. If this happens use the MDI to run a spindle warmup before

running your file by picking up tool 2. Follow the procedure below.

MACHINE PANEL: [MDI]

CONTROL PANEL:[PROG](PROGRAM) [M] [6] [T] [2] [EOB]

Verify that the input buffer looks like this:

A) M6T2;

Press [INPUT]

At the top of the screen you should now see

O0000 M6 T2;

Using the directional pad on the CONTROL PANEL press the up arrow to ensure that there is no code

above the displayed information.

MACHINE PANEL: press [CYCLE START]. If the compressed air is on, you will pick up tool 2 and be

prompted to run the spindle warmup. Press [CYCLE START] to continue.

You may walk away from the control while the warmup cycle runs. There is an M00 in the code at the end of

the spindle warmup to stop motion even if the warmup happens while running a file.

8.5 Store a Work Offset (M402)

Use the MDI to type in the following code

M402 Wnn; (nn is the work offset number you want to overwrite)

When you press [CYCLE START] the machine will drive to Z Home, then to X6. Y6. relative to the

currently stored offset.

It will prompt you to set the Z first. Follow the instructions in [JOG] mode, then press [CYCLE START] in

[MDI] mode to store the Z value and continue. This will store the correct Z value for Work Offset no matter

what tool you have loaded, so long as the correct tool length offset has been stored in the machine.

The machine will again drive to Z home, then to X0 and Y0. If you would like to make modifications move

the machine in [JOG] mode. Press [CYCLE START] and the XY values will be stored.

8.6 Jog Mode

Jog mode allows the operator to manually position the spindle. This is the simplest way to move the machine.

8.6.1 Continuous Jog

On the CONTROL PANEL press

[POS] (ALL AXIS).

On the MACHINE PANEL press [JOG].

Press and hold any of the directional keys [X] [Y] or [Z].

It is possible to jog multiple axis at one time by holding more than one key.

To jog faster hold down the [RAPID] key after depressing the directional key.

On this machine X+ and X- behave backward of what you would expect by the locations of the buttons on

the panel.

8.6.2 Handle Jog

On the CONTROL PANEL press

[POS] (ALL AXIS).

On the MACHINE PANEL press [JOG].

Pick up the MPG or Handle Jog wheel.

Using the selector knobs choose the axis and step amount. x10 is 0.001” per click and x100 is 0.01” per click

Use the wheel to jog around with more control

Set the Axis Selector back to “4” before hanging up or handing off to prevent accidental motion.

8.7 Some Common Mistakes

While possible to fix some common mistakes by editing the gCode directly, please do not do so. Often you

will need to make another change in the file later on and can easily forget that you edited the gCode. The

preferred procedure is to change the RhinoCAM file each time you make a change and re-post.

8.7.1 Forgot the Vacuum

If the 123 block does not fit between the tool and your part, it’s likely you forgot the vacuum, turn it on and

try again

8.7.2 Measured Incorrectly

Its probably not the tool offset or the work offset, double check your material thickness with calipers.

8.7.3 Set work zero to top of stock, set work offset to bottom of stock

Be meticulous and avoid distractions when setting your work zero in your CAM file and your work offset on

the machine. Be sure it’s correct, this is the most common mistake for beginners and experts alike. It’s really

easy to screw this up. Always double check these when you set them, luckily while you are at MICA the code

will prompt you to check this.

8.8 Clean Up

After the file completes running, you will get out the vacuum and clean up all the dust after removing your

part from the vacuum table. On a short production run, don’t bother to clean anything else until you’re done.

After you’re completely done, use handle jog or the MDI to move the machine around and vacuum up any

areas you can’t reach including the floor. If you had [BLOCK SKIP] active the tool will be left in the spindle.

Please do not leave any tools in the spindle overnight.

M6T0;

Never use compressed air near the spindle!!! You will damage or destroy the spindle.

Be careful not to press the green tool release button while vacuuming!

9 Advanced Machine Operation

9.1 Stop and Jog Away, Return and Continue Cutting

9.1.1 Stop Motion and Spindle

MACHINE PANEL: [CYCLE STOP] [SPINDLE STOP]

You can walk away from the machine at this time.

9.1.2 Jog Away

CONTROL PANEL: [POS] (RELITIVE) or [POS] (ALL)

AXIS LETTER [X Y OR Z],

You will see that letter in the input buffer and the correlating axis letter start to blink.

(ORIGIN) (EXEC).

The RELITIVE display will read 0.000

MACHINE PANEL: [JOG]

Go ahead and jog around, before starting your file again, jog back to where the RELATIVE display reads 0

on all axes.

9.1.3 Continue File after Stopping Spindle

MACHINE PANEL: [JOG] [SPDL CW] [REMOTE]

Wait for spindle to get to speed

[CYCLE START]

9.2 Make a Relative Measurement

From time to time, you may need to make a measurement with the machine. This is possible by first zeroing

the desired axis in the RELITIVE position screen (on some machines called OPPERATOR), then by driving

to the other location and reading that same RELITIVE position.

CONTROL PANEL: [POS] (RELITIVE)

MACHINE PANEL: [JOG] then jog to first position. Do this carefully, always use a 123 block or some other

method to keep the tool and spindle away from your workpiece.

CONTROL PANEL: AXIS LETTER [X Y OR Z], you will see that letter in the input buffer and the

correlating axis letter start to blink. (ORIGIN) (EXEC). The RELITIVE display will read 0.000

MACHINE PANEL: [JOG] then move to the second position and read the distance.

9.4 View or Modify the Values Stored in a Work Offset

Modify these only after instruction on the process. Modifying a work offset or tool length could cause a crash

leading to severe injury and/or damage to the machine.

MACHINE PANEL: [MDI] or [JOG]

CONTROL PANEL: [OFS/SET] (WORK)

Use the d-pad to navigate to the desired work offset

Make the necessary edits (+INPUT) will add to the stored value, (INPUT) will overwrite the value

9.4.1 Store a Work Offset X and Y (Edge Finder)

• Load the edge finder using the MDI and jog it close to your part

• Use the MDI to turn the spindle on at 1000rpm

• Using the x10 step on the MPG jog the edge finder until it splits at the X edge of your part.

• Stop the spindle and jog up in Z

• Zero the X axis in the relative position screen

• With the edge finder above your part, drive the spindle over 0.1” so that the center of the edge finder is

on the edge of your part, zero the relative position screen again.

• Repeat for Y axis

• Drive the X and Y axis to zero on the relative position screen, double check that the tool is centered on

the desired work zero.

• CONTROL PANEL: [OFS/SET] (WORK)

• Use the d-pad to navigate to the desired work offset

•

[X][0](MEASUR) [Y][0](MEASUR)

•

Use d-pad to highlight Y1, type the value stored for Y into the input buffer and press [INSERT]

9.4.2 Store a work Offset Z (With Tool)

• Load a tool and drive it to 1” off the top of your work zero location using the 123 block

• Don’t drive up or down with the block under the tool. Ever. Seriously don’t do it.

• CONTROL PANEL: [OFS/SET] (WORK)[Z][1.](MEASUR)

•

(OFFSET) copy the tool length stored for the tool in the spindle to the whiteboard

•

(WORK) type in the copied value with the Z field selected

•

(+INPUT) verify the math and press (EXEC)

•

Use the MDI to check your work offset and tool offset with the following code

G5n;

G00 X0Y0;

M00; (Turn feed override down, stop if the tool gets closer than 3” to material)

G43 Hnn Z(3.0+n);

10 Alarms and Recovery

10.1 Soft Over-Travel Alarm

Soft over-travel alarms occur when an axis has traveled beyond a coordinate limit. To clear the alarm, jog the

offending axis away (remember that the X axis jog buttons are transposed on the controller)

10.2 Hard Over-Travel Alarm

Any axis that creates a hard over-travel alarm will cause all axes to be in alarm state. This is more common

when jogging the X axis, but can happen on either end of any axis. The display will automatically go to the

ALARM screen and display an entire page of red error messages for all axes at once.

You must jog the offending axis off the switch before the alarm can be cleared.

Bypass the alarm state by pressing [RESET] while holding down the left bottom [UNLABELED] button

(under [+X] and to the left of the [-Y]).

Continue holding the [UNLABELED] button and jog the over-traveled axis off the limit switch.

10.3 Paused In The Middle Of a Tool Change

WAIT - high risk of crash/causing damage or further damage GET HELP from McKibbin

10.3.1 Check that machine knows what tool is in spindle.

Check macro 510 (current tool) - McK Tool Change

[System] (PMCMNT) (DATA) - Laguna Tool Change

Highlight D0400

Press (OPRT)(ZOOM) to see data in D0400.

Verify that D0402 is set to 0 if there is no tool in spindle, or the tool number for the tool in spindle.

10.3.2 Check that the machine knows the current tool changer carousel position.

[System] (PMCMNT) (COUNTER)

Check that C0000 is set to the current tool changer position in the “current” column.

10.3.3 Check that the Rapid Traverse Rate is correct.

Parameter #1420 should read as labeled in Common Parameters section. If not it will need to be changed back

before moving forward. This would only be performed by McKibbin. Turn off the machine and lock it out

you’re done for the day.

11.3 G Codes (Unabridged)

G00

Rapid Positioning

G01

Linear Interpolation

G02

Circle/Helical Interp CW

G03

Circle/Helical Interp CCW

G04

Dwell

G09

Exact Stop

G10

Programmable Data Input

G11

Programmable Data Input Cancel

G12

N/A

G13

N/A

G14

N/A

G15

Polar Coordinates Command Cancel

G16

Polar Coordinates Command

G17

XY plane

G18

XZ plane

G19

YZ plane

G20

Inches (G70)

G21

Metric (G71)

G22

Stored Stroke Check On (2 ONLY)

G23

Stored Stroke Check Off (2 ONLY)

G24

N/A

G25

N/A

G26

N/A

G27

Reference Position Return Check

G28

Automatic Return to Reference Position

G29

Movement from Reference Position

G30

2nd, 3rd and 4th reference pos return

G31

Skip Function

G32

N/A

G33

N/A

G34

N/A

G35

N/A

G36

N/A

G37

Automatic Tool Length Measurement

G40

Tool Radius Comp Cancel

G41

Tool Radius Comp Left

G42

Tool Radius Com Right

G43

Tool Length Comp +

G44

Tool Length Comp -

G45

Tool Offset: Increase

G46

Tool Offset: Decrease

G47

Tool Offset: Double Increase

G48

Tool Offset: Double Decrease

G49

Tool Length Comp Cancel

G50

Scaling Cancel

G51

Scaling

G50.1

Programmable Mirror Image Cancel

G51.1

Programmable Mirror Image

G52

Local Coordinate System Setting

G53

Machine Coordinate System Setting

G54

Work Offset

G54.1 Extra work offsets (P01 through P48)

G55

Work Offset

G56

Work Offset

G57

Work Offset

G58

Work Offset

G59

Work Offset

G60

Single Direction Positioning

G61

Exact Stop Mode

G62

Automatic Override for Inner Corners

G63

N/A Tapping Mode

G64

Cutting Mode (Normally Active)

G65

Macro Call

G66

Modal Macro Call A

G66.1

Modal Macro Call B

G67

Modal Macro Call A/B Cancel

G70

Inches (G20)

G71

Metric (G21)

G73

Peck Drilling Cycle - High Speed

G74

N/A - LH Tapping

G75

N/A Plunge Grinding

G76

N/A Fine Boring Cycle

G77

N/A Grinding Cycle

G78

N/A Grinding Cycle

G79

N/A Grinding Cycle

G80

Canned Cycle Cancel

G81

Drill / Spot Drill Cycle

G82

Drill with Dwell

G83

Peck Drilling Cycle - Return to feed plane

G84

N/A Tapping

G85

N/A Boring Cycle

G86

N/A Boring Cycle

G87

N/A Boring Cycle

G88

N/A Boring Cycle

G89

N/A Boring Cycle

G90

Absolute

G91

Incremental

G92

Setting a Workpiece Coordinate System

G93

Inverse Time Feed

G94

Feed per Minute

G95

Feed per Revolution

G96

Constant Surface Speed Control

G97

Constant Surface Speed Control Cancel

G98

Canned Cycle: Return to Initial Level

G99

Canned Cycle: Return to R point Level

11.4 M Codes (Unabridged)

M00

Program Stop

M01

Optional Stop

M02

End of program, superseded by M30, M2 does not rewind tape (used to make

physical loops of tape)

M03

Spindle on CW

M04

Spindle on CCW

M05

Stop Spindle

M06

Tool Change

M13

Drill Block (not dFab)

M15

Drill Block off (not dFab)

M16

Start ATC

M17

index magazine to new tool #

M18

Update tool # in spindle, copies #405 to #402

M19

Index magazine to match tool # in spindle

M20

main spindle tool grip

M21

main spindle tool release

M25

Servo Tuning

M27

Extend magazine

M28

Retract magazine

M30

End of Program

M35

Attach 4th axis (not dFab)

M36

Detach 4th axis (not dFab)

M48

Dust Hood Up

M49

Dust Hood Down

M50

SPINDLE WARMUP

M52

Spindle Piston Up (not currently dFab... Can I use?)

M53

Spindle Piston Down (not currently dFab... Can I use?)

M60

pass a T code, stores current pos into tool stand location for tool change

macro

M98

Sub Program Call

M99

return from sub program

M401

DO NOT USE

M402

STORE WORK OFFSET; W-WORK OFFSET NO., Z-HEIGHT OF TOUCH OFF TOOL