This document provides an extensive overview of CNC (Computer Numerical Control) manufacturing technologies, including historical development, programming basics, and machine control concepts. It discusses the advantages and disadvantages of CNC systems, various machine types, and reference systems for programming and operation. Furthermore, it covers ISO programming techniques and includes exercises for practical application.

1. MANUFACTURING TECHNOLOGIES
CNC
by Endika Gandarias
BACHELOR OF ENGINEERING

2. 2by Endika Gandarias
Dr. ENDIKA GANDARIAS MINTEGI
Mechanical and Manufacturing department
Mondragon Unibertsitatea - www.mondragon.edu
(Basque Country)
www.linkedin.com/in/endika-gandarias-mintegi-91174653
Further presentations: www.symbaloo.com/mix/manufacturingtechnology

3. 3
CONTENTS
 BIBLIOGRAPHY
 INTRODUCTION
 REFERENCE SYSTEMS
 BASIC ISO PROGRAMMING
 FIXED CANNED CYCLES
 EXERCISES
 FAGOR SIMULATOR
 GLOSSARY
by Endika Gandarias

4. 4
BIBLIOGRAPHY
BIBLIOGRAPHY
by Endika Gandarias

5. 5
The author would like to thank all the bibliographic references and videos that
have contributed to the elaboration of these presentations.
For bibliographic references, please refer to:
• http://www.slideshare.net/endika55/bibliography-71763364 (PDF file)
• http://www.slideshare.net/endika55/bibliography-71763366 (PPT file)
For videos, please refer to:
• www.symbaloo.com/mix/manufacturingtechnology
BIBLIOGRAPHY
by Endika Gandarias

6. 6
INTRODUCTION
INTRODUCTION
by Endika Gandarias

7. 7
1942 Bendix Corporation, a USA helicopter blade manufacturing company,
needs three-dimensional cam parts.
 Coordination of movements is necessary.
1947 John Parson (a Bendix corporation worker) using punched tapes
is able to control simultaneously axes movements of a machine
 MIT collaborates
1953 Numerical Control (NC) term appears at M.I.T.
1960 Adaptative Control term appears at M.I.T.
1970 Computer Numerical Control (CNC) is created
 Microprocessors origin.
1980 Direct Numerical Control (DNC) is possible.
A large number of machines are controlled by a computer.
INTRODUCTION
by Endika Gandarias
Brief history
Definition
 CNC (Computer Numerical Control (CNC) refers to the method of controlling a machine tool or
the machining process by means of a computer.
 Coded numerical instructions are inserted into the CNC  PROGRAMMING LANGUAGE
NC Punched Tape

8. 8
Machine control feedback: position & velocity
CNC block diagram
INTRODUCTION
by Endika Gandarias
Velocity
Feedback
Position
Feedback
VIDEO
VIDEO
CNC machine tool description Loop control types
OPEN LOOP
CLOSED LOOP

9. 9
 Every position of an absolute device is unique.
 The disk has many circular tracks, the higher the
number of tracks the higher the resolution.
 These devices do not lose position when power
is removed (homing sequence not needed on
startup).
 They do not accumulate errors (not affected by
noise signal).
 They are more complex and expensive.
INTRODUCTION
by Endika Gandarias
CNC machine tool description
Feedback devices
ABSOLUTE ROTARY ENCODER INCREMENTAL ROTARY ENCODER
 The feedback signal is always referenced to a start
or home position. They need an external processing
of signals.
 In the event of a power failure, it must be
reinitialized.
 They are susceptible to noise, thus, errors.
 They are simpler and cheaper.
An encoder is a sensor for converting rotary
motion or position to analog/digital signal.
VIDEO VIDEO
VIDEO

10. 10
 It measures directly the position of linear axes.
 High positioning accuracy.
 High permissible traversing speed.
 It can correct next errors:
 Positioning error due to thermal behavior of the recirculating ball screw.
 Reversal error.
 Kinematics error through ball-screw pitch error.
INTRODUCTION
by Endika Gandarias
CNC machine tool description
Feedback devices
LINEAR GLASS SCALE ENCODER
VIDEO
VIDEO
Absolute glass scale
Incremental glass scale
VIDEO

11. 11
INTRODUCTION
Advantages
 High Repeatability + High Trueness = High Accuracy.
 More complex 3-dimensional geometries.
 Better quality.
 Higher productivity.
 Greater safety and lower operator qualification.
 Greater flexibility to part changes.
 Minimizes human errors.
Disadvantages
 Higher investment cost.
 Higher maintenance cost.
 Time consuming set-up.
 Training is needed for CNC programming.
Increasing Repeatability
IncreasingTrueness
by Endika Gandarias
CNC FAGOR - USER MANUAL
www.fagorautomation.com/download/

12. 12
Type of machines
 Turning Centers
 Milling Centers
 Machining Centers
 Drilling Machines
CNC manufacturers
INTRODUCTION
by Endika Gandarias
 Grinding Machines
 EDM Machines
 Laser-Cutting Machines
 …

13. 13by Endika Gandarias
The axes are named
according to DIN 66217.
Axis nomenclature
VIDEO
Three-axes milling machine
Six-axis milling machine
Turning machine
VIDEO
A+
C+
B+
INTRODUCTION

14. 14
Reference systems
by Endika Gandarias
INTRODUCTION
VIDEO

15. 15
 M  Machine Zero or home: This is set by the manufacturer as the origin of the coordinate
system of the machine.
 W  Part zero or point of origin of the part: This is the origin point that is set for
programming the measurements of the part. It can be freely selected by the programmer.
 R  Machine Reference point. This is a point on the machine established by the
manufacturer around which the synchronization of the system is done. The control positions
the axis on this point.
by Endika Gandarias
INTRODUCTION
Reference systems

16. 16
Pre-Start
Power ON
Find Machine Zero or Home (M)
Load Tools
Set Machine Reference (R)
Set Part zero (W)
Load CNC program
Run Program
Power OFF
 Define Tool Length & Radius Offsets
 Check coolant and air supply levels,
ensure work area is clean, …
INTRODUCTION
CNC machine setup and operation
 Fill the tool carousel.
 Once he workholding device is properly
installed and aligned, set part X,Y&Z zero
datum.
by Endika Gandarias
1
2
3
4
5
6
7
8
9

17. 17
REFERENCE SYSTEMS
REFERENCE SYSTEMS
by Endika Gandarias

18. 18
Machine Reference (R) setting
TOOL LENGTH
COMPENSATION OFF
G44
TOOL LENGTH
COMPENSATION ON
G43
REFERENCE SYSTEMS
by Endika Gandarias
RRRR
T1
L1 L2 L3 L4
RRRR
T2 T3 T4
TOOL
TOOL
OFFSET
RADIUS LENGTH
T1 D1 55.234
T2 D1 72.345
T3 D1 61.098
T4 D1 66.683
… … ... …
OFFSET TABLE

19. 19
Tool presetting machine
REFERENCE SYSTEMS
Machine Reference (R) setting
1
by Endika Gandarias
 High accuracy.
 Based on camera images (contact methods were used in
the past).
 Tool length (L) and radius (R) values are measured.
 Minimizes tool setting times.
 Used at high production runs.
TOOL LENGTH MEASUREMENT
TOOL RADIUS MEASUREMENT
X
Z
VIDEO

20. 20
Tool on the workpiece
REFERENCE SYSTEMS
Machine Reference (R) setting
2
by Endika Gandarias
 Low accuracy.
 Time consuming method.
 Only tool length (L) values are measured.
 Tool is rotating and thus, part or referencing block gets marked.
TOOL LENGTH MEASUREMENT
W
T1 T2 T3 T4
L4 = 0L3 < 0
L2 > 0
L1 < 0
W
RRRR

21. 21
3
REFERENCE SYSTEMS
Machine Reference (R) setting
by Endika Gandarias
Using a tool length setter gauge
TOOL LENGTH MEASUREMENT
 Good accuracy.
 Time consuming method.
 Only tool length (L) values are measured.
 Part or referencing block does not get marked.
W
L2<0L1=0
RR
L1
M
50
z1
z2
L2
50
L1= z1-50 L2= z2-50
R
R
BASEDONAREF.TOOLBASEDONMACHINEDATUM
VIDEO

22. 22
REFERENCE SYSTEMS
Machine Reference (R) setting
Using a touch probe4
by Endika Gandarias
 High accuracy.
 Fast method.
 Tool length (L) and radius (R) values are measured.
 Tool rotates counterclockwise not to mark the probe at low RPM.
Additional applications
Low RPM
TOOL LENGTH MEASUREMENT
TOOL RADIUS MEASUREMENT
VIDEO

23. 23
REFERENCE SYSTEMS
Machine Reference (R) setting
Using a laser beam5 Additional applications
 Highest accuracy.
 Fast method.
 Tool length (L) and radius (R) values are measured.
 Tool rotates at working conditions. TOOL LENGTH MEASUREMENT
TOOL RADIUS MEASUREMENT
by Endika Gandarias
VIDEOVIDEO

24. 24
Part zero (W) setting
 Prior to defining part zero, procedure should be:
1. Study how the drawing is dimensioned.
2. Decide on the workholding device type and part zero (W) definition.
 Machine operator defines part zero (W) position anywhere.
 Most common positions:
o Left lower side of the part (all data position values are positive).
o Part symmetry axis.
o CLAMP CASE  Centering pins side.
o VISE CASE  Stationary chuck & vise stop side.
REFERENCE SYSTEMS
by Endika Gandarias
Clamps (with or without centering pins) Vise (with or without vise stop)
Movable chuck
Stationary chuck
Vise stop
Centering pinsClamps

25. 25
X
Z
Y
Symmetry
X
Y
Z
Y
Part zero (W) setting
X
Z
Y
X
Y
Z
Y
Stationary chuck & Y axis part symmetryX-Y axis part symmetry
REFERENCE SYSTEMS
by Endika Gandarias
VISE VISE

26. 26
Part zero (W) setting
Stationary chuck & left lower part
REFERENCE SYSTEMS
by Endika Gandarias
X
Y
Z
X
X
Z
Y
VISE CLAMP
Stationary chuck & Y axis part symmetry
X
Y
Z
X

27. 27
Part zero (W) setting
VIDEO
Using the tool
 Low accuracy.
 Tool is rotating and thus, part gets
marked.
REFERENCE SYSTEMS
by Endika Gandarias
Using a mechanical edge finder1 2
 Low accuracy.
X
Y
DATUM SETTING
X
Y
Z
DATUM SETTING
Optical edge finder  similar
VIDEO

28. 28
3
Part zero (W) setting
VIDEO
REFERENCE SYSTEMS
by Endika Gandarias
Using a touch probe
 High accuracy.
X
Y
Z
DATUM SETTING
VIDEO

29. 29by Endika Gandarias
VIDEO
2 types:
1. Touch-trigger probes
2. Scanning probes (continuous measuring)
PRO & CON:
Almost any machined geometry may be measured in-situ.
Reduced machine downtime.
Part unclamping for measuring is avoided.
It cannot consider possible machine axes errors.
Touch probe stylus tips
3
Part zero (W) setting
REFERENCE SYSTEMS
Using a touch probe

30. 30
BASIC ISO PROGRAMMING
FAGOR 8055-M
by Endika Gandarias
BASIC ISO PROGRAMMING

31. 31
BASIC ISO PROGRAMMING
by Endika Gandarias
Block identification
Identifies the block of information.
/ N**** G** X****.*** Y****.*** Z****.*** A****.*** B****.*** C****.*** F****.** S****.**
Preparatory
functions
or G-codes
Linear and angular
positioning data Feed function
Speed function
Block structure
T** D** M** N** ;*****
Tool number
Tool offset number
Miscellaneous or auxiliary functions
Block skip condition
Number of block repetitions
Block comment
Not ISO,
corresponds to
FAGOR 8055M
=

32. 32by Endika Gandarias
Feed function (F) Speed function (S)
 The feed function F is the speed at which the tool
center point moves.
 The programmed F is effective working in linear
(G01) or circular (G02, G03).
 The maximum F value is limited by the machine
parameters.
 The speed function S is the speed at which the
tool (in milling) or part (in turning) rotates.
 The maximum S value is limited by the machine
parameters.
BASIC ISO PROGRAMMING

33. 33by Endika Gandarias
Tool number (T)
The "T" code identifies the tool position in the tool magazine.
Tool offset number (D)
The tool offset contains the tool dimensions.
Each tool may have several offsets associated with it.
TOOL
TOOL
OFFSET
RADIUS LENGTH …
T1
D1 8.002 55.234 …
D2 7.502 55.234 …
D3 8.002 55.026 …
… … … …
TOOL
TOOL
OFFSET
RADIUS LENGTH …
T2
D1 4.000 72.345 …
D2 11.990 60.036 …
D3 7.500 33.110 …
… … … …
…
BASIC ISO PROGRAMMING

34. 34
M functions DESCRIPTION
M00 Program STOP / Spindle STOP / Coolant OFF
M03 Spindle ON clockwise
M04 Spindle ON counterclockwise
M05 Spindle STOP
M06 Tool change
M08 Coolant ON
M09 Coolant OFF
M30 End of program
BASIC ISO PROGRAMMING
Auxiliary or Miscellaneous (M) functions
by Endika Gandarias

35. 35
M functions MODAL DESCRIPTION
G00 * Rapid traverse
G01 * Linear interpolation
G02 * Clockwise circular interpolation
G03 * Counterclockwise circular interpolation
G05 * Controlled corner rounding
G07 * Square corner
G36 Automatic radius blend
G39 Chamfer
G37 Tangential entry
G38 Tangential exit
G40 * Cancellation of tool radius compensation
G41 * Left-hand tool radius compensation
G42 * Right-hand tool radius compensation
G43 * Tool length compensation
G44 * Cancellation of tool length compensation
G90 * Absolute programming
G91 * Incremental programming
… … …
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
by Endika Gandarias
MODAL = Once programmed, it remains active until
another incompatible G function is
programmed or until M30 / EMERGENCY
or RESET.

36. 36
 It is a positioning linear movement at maximum
F value defined in the machine parameters.
 Not valid for cutting.
 It can be programmed as G00, G0 or G.
by Endika Gandarias
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
Rapid traverse (G00) Linear interpolation (G01)
 It is a working linear movement at the
programmed F value.
 It can be programmed as G01 or G1.
…
N80 G00 X500 Y300
…
…
N120 G01 X500 Y300 F400
…
(TP)
(SP)
(TP)
(SP)
G00 X___ Y___
TP
G01 X___ Y___
TP

37. 37by Endika Gandarias
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
Rapid traverse (G00) Linear interpolation (G01)
EXERCISE 1
w
= SP

38. 38
I
J
SP
TP
CC
I
J
SP
TP
CC
 It is a working circular movement at the programmed F value.
 It can be programmed as G02 or G2 / G03 or G3.
by Endika Gandarias
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
Clockwise circular interpolation (G02)
Counterclockwise circular interpolation (G03)
…
N60 G02 X300 Y300 I200 J0
…
CARTESIANCOORDINATES
WITHARCCENTER
G02 X___ Y___ I___ J___
Distance from the SP to
the Circle Center (CC).
TP
…
N60 G03 X300 Y300 I0 J200
…
G03 X___ Y___ I___ J___
Distance from the SP to
the Circle Center (CC).
TP

39. 39
SP
TP
SP
TP
by Endika Gandarias
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
…
N40 G02 X400 Y150 R150
…
Clockwise circular interpolation (G02)
Counterclockwise circular interpolation (G03)
CARTESIANCOORDINATES
WITHARCRADIUS
G02 X___ Y___ R___
R + : Arc < 180º
R ˗̶ : Arc > 180º
TP
 A complete circle cannot be programmed.
…
N40 G02 X400 Y150 R-150
…
R+
R ˗̶
…
N40 G03 X400 Y300 R150
…
…
N40 G03 X400 Y300 R-150
…
R+
R ˗̶
G03 X___ Y___ R___
R + : Arc < 180º
R ˗̶ : Arc > 180º
TP

40. 40by Endika Gandarias
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
Clockwise circular interpolation (G02)
Counterclockwise circular interpolation (G03)
EXERCISE 2 EXERCISE 3
EXERCISE 4 EXERCISE 5
w w
w w
SP SP
SP SP

41. 41by Endika Gandarias
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
Clockwise circular interpolation (G02)
Counterclockwise circular interpolation (G03)
EXERCISE 6
w
SP

42. 42
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Absolute programming (G90)
Incremental programming (G91)
G90: The positioning data refers to the part zero (default).
G91: The positioning data corresponds to the distance to be travelled from the point
where the tool is situated.
w
…
N70 G01 G90 X70 Y15 F350 ; P2
N80 G01 X70 Y30 ; P3
N90 G01 X45 Y45 ; P4
N100 G01 X20 Y45 ; P5
N110 G01 X20 Y15 ; P6
…
Absolute programming (G90)
…
N70 G01 G91 X50 Y0 F350; P2
N80 G01 X0 Y15 ; P3
N90 G01 X-25 Y15 ; P4
N100 G01 X-25 Y0 ; P5
N110 G01 X0 Y-30 ; P6
…
Incremental programming (G91)
= SP

43. 43
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Absolute programming (G90)
Incremental programming (G91)
EXERCISE 7
w
EXERCISE 8
SP
SP

44. 44
BASIC ISO PROGRAMMING
by Endika Gandarias
Other functions
REPEAT
(RPT N___ ,N___)N___
Number of
repetitions
From
block
To
block
EXERCISE 9
100 275 450 600 775 950 1100 1275 1450
SP

45. 45
Pocket Milling
Engraving
by Endika Gandarias
Profile Milling
Face Milling Slot Milling
BASIC ISO PROGRAMMING
Pecking / Drilling /
Threading / Reaming

46. 46
Face milling
by Endika Gandarias
N00 T1 D1 ; Ø28mm end-mill, assign tool 1 value D1
N10 M06 ; Tool change action
N20 G00 G43 X14 Y40 Z100 F400 S1500 M03
N30 G00 Z58
N40 G01 X116 Y40
N50 G00 X116 Y54
N60 G01 X14 Y54
N70 G00 X14 Y68
N80 G01 X116 Y68
N90 G00 X116 Y82
N100 G01 X14 Y82
N110 G00 X14 Y96
N120 G01 X116 Y96
N130 G00 Z100
N130 M30 ; End of program
SP
60
70
20 40 60 80 100
100
80
60
40
20 Security
distance ~ 2 mm
For exercises consider:
ae = 50% of tool Ø
BASIC ISO PROGRAMMING

47. 47by Endika Gandarias
Face milling
EXERCISE 10
Tool: Ø50mm HSS end-mill, z=4
Material: Aluminium
• CASE A  apTOTAL=5mm; ap=5mm
• CASE B  apTOTAL=5mm; ap=2.5mm  RPT
• CASE C  apTOTAL=5mm; ap=1mm  RPT & G91
BASIC ISO PROGRAMMING

48. 48
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Square corner (G07) Round corner (G05)
 The CNC starts executing the following block as
soon as the position programmed in the current
block has reached the dead band (default) 
Sharp edges, Machining time ↑, Shocks ↑.
 To be used with G00: face milling, canned
cycles, …
 The CNC starts executing the following block as
soon as deceleration of the currently executing
axes start (“?” distance depends on the feedrate
F value)  Rounded edges, Machining time ↓
 NOT to be used with G00: slot milling,
engraving, contouring,…
…
N60 G01 G07 X50 Y100 F400
N70 G01 X140 Y100 F300
…
…
N60 G01 G05 X50 Y100 F400
N70 G01 X140 Y100 F300
…
w
t
Fy
t
Fx
w
DEAD BAND: The range
through which an input can be
varied without initiating response
t
Fy
t
Fx
Acceleration
Constant feed
Deceleration

49. 49
Pocket Milling
Engraving
by Endika Gandarias
Profile Milling
Face Milling Slot Milling
BASIC ISO PROGRAMMING
Pecking / Drilling /
Threading / Reaming

50. 50
Slot milling
by Endika Gandarias
SP
20 60 85
20 Security
distance
~ 2 mm
70
95
45
N00 T7 D1 ; Ø10mm end-mill
N10 M06
N20 G00 G43 X85 Y13 Z100 F400 S3500 M03
N30 G00 Z20
N40 G00 G91 Z-2
N50 G01 G90 G05 X85 Y45
N60 G01 X60 Y70
N70 G01 X60 Y95
N80 G01 G07 X3 Y95
N90 G00 G91 Z10
N100 G00 G90 X85 Y13
N110 G00 G91 Z-10
N120 (RPT N40,N110)N1 ; Repeat
N130 (RPT N40,N80)N1 ; Repeat
N140 G00 Z100
N150 M30
20 40 60 80 100
60
40
20 6
+Z
•
•
•
•
Tool: Ø10mm H.S.S. end-mill
ap TOTAL = 6mm ; ap = 2mm
BASIC ISO PROGRAMMING

51. 51
35
100
40
SP
85
65
6555
•
••
•
•
85
Slot milling
by Endika Gandarias
EXERCISE 11
60
40
20
5
+Z
Tool: Ø16mm H.M. end-mill, z=3
Material: Steel
ap TOTAL = 5mm ; ap = 2.5mm
BASIC ISO PROGRAMMING

52. 52
Engraving
by Endika Gandarias
EXERCISE 12 Tool: Ø12mm HSS engraving tool, z=1
Material: Steel
ap TOTAL = 2mm ; ap = 2mm
H.S.S.
engraving tool
H.M.
engraving tool
60
40
20 2
+Z
20 40 60 80 100
100
20
20
45
60
70
35 45 55 70 85 100
52.5
BASIC ISO PROGRAMMING

53. 53
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Cancellation of tool radius compensation (G40)
Left-hand tool radius compensation (G41)
Right-hand tool radius compensation (G42)
 The CNC automatically calculates the path the tool should follow based on the contour of the part
and the tool radius value stored in the tool offset table.
G41 - CLIMB CUTTING G42 - CONVENTIONAL CUTTING

54. 54
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Cancellation of tool radius compensation (G40)
Left-hand tool radius compensation (G41)
Right-hand tool radius compensation (G42)
…
N50 G01 G41 G05 X77.5 Y70 F400
N60 G01 X100 Y70
N70 G01 X100 Y60
N80 G03 X85 Y45 I0 J-15
N90 G02 X70 Y30 I-15 J0
N100 G01 X50 Y30
N110 G01 X20 Y20
N120 G01 X25 Y70
N130 G03 X55 Y70 I15 J0
N140 G01 X77.5 Y70
N150 G01 G40 G07 X77.5 Y100
…
G41
 Tool entry & exit should always be perpendicular to the workpiece contour.
 Tool entry & exit should be avoided to be from a workpiece edge  may produce burr.
20 25 50 55 70 85 100
20
45
60
70
30
SP
•
22.5
30

55. 55
Pocket Milling
Engraving
by Endika Gandarias
Profile Milling
Face Milling Slot Milling
BASIC ISO PROGRAMMING
Pecking / Drilling /
Threading / Reaming

56. 56
BASIC ISO PROGRAMMING
by Endika Gandarias
Roughing operation
Tool: Ø8mm H.M. end-mill, z=3
Material: Aluminium
ap TOTAL = 10mm ; ap = 2.5mm
+Z
30 60 90 120 150
30
60
30 60 90 120 150
30
60
90
25
SP
•
Profile milling
EXERCISE 13

57. 57
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Automatic radius blend (G36) Chamfer (G39)
 It rounds a corner with a determined radius,
without having to calculate the center nor the
start and end points of the arc.
 Function G36 is not modal.
…
N60 G01 G36 R5 X250 Y450 F400
N70 G01 X400 Y0
…
…
N60 G01 G39 R15 X350 Y600 F400
N70 G01 X500 Y0
…
G36 R___
 It chamfers corners between two straight lines,
without having to calculate intersection points.
 Function G39 is not modal.
G39 R___

58. 58
BASIC ISO PROGRAMMING
by Endika Gandarias
Preparatory functions or G-codes
Tangential entry (G37 RENTRY) Tangential exit (G38 REXIT)
 It is used to create a tangential entry in Finishing
operations so tool entry mark can be unnoticeable
(not necessary for roughing).
 It is used to create a tangential entry in Finishing
operations so tool exit mark can be unnoticeable
(not necessary for roughing).
…
N60 G01 G05 G41 G37 R12 X25 Y30 ; Tool Ø 22mm
N70 G01 X10 Y30
…
…
N60 G01 G38 R12 X25 Y30 ; Tool Ø 22mm
N70 G01 G07 G40 X25 Y5
…
RENTRY > RTOOL-OFFSET
LENTRY ≥ 2 * RENTRY
RENTRY
LENTRY
REXIT > RTOOL-OFFSET
LEXIT ≥ 2 * REXIT
12 ≥ 11
25 ≥ 2 * 12
12 ≥ 11
25 ≥ 2 * 12
REXIT
LEXIT
NOT MODAL FUNCTION NOT MODAL FUNCTION
G38 REXIT
G37RENTRY

59. 59
G01
G05
G41
G37 RENTRY
G00
G43
G01
G07
G40
RENTRY = REXIT
G38 REXIT
1
2
3 4
5
0
WORKPIECE
LENTRY = LEXIT
TOOL
BASIC ISO PROGRAMMING
Preparatory functions or G-codes
Summary for profile milling operations
by Endika Gandarias
NOTE:
- G37 & G38 only for finishing operations.
RENTRY > RTOOL-OFFSET
LENTRY ≥ 2 * RENTRY

60. 60
Pocket Milling
Engraving
by Endika Gandarias
Profile Milling
Face Milling Slot Milling
BASIC ISO PROGRAMMING
Pecking / Drilling /
Threading / Reaming

61. 61
SP
Profile milling
by Endika Gandarias
Roughing operation:
Tool: Ø20mm H.M. end-mill, z=3
Stock: 0.4mm
Finishing operation:
Tool: Ø20mm H.M. end-mill, z=3
Stock: 0mm
Material: Steel
ap TOTAL = 5mm ; ap = 2.5mm
(Use G36 R__ and G39 R__)
BASIC ISO PROGRAMMING
+X
+Y
+X
+Z
•
EXERCISE 14
• CASE A  Same tool
• CASE B  Different tool

62. 62
 Cycles are referred to repetitive program sequences commonly used In machining operations
that makes easier programming.
 Canned cycles or Fixed cycles: They are an inbuilt feature of the CNC usually
permanently stored as a pre-program and cannot be altered by the user (G80-G89)
 User-defined cycles or Sub-routines: They are created when the necessary fixed
cycle is not available.
FIXED CYCLES OR CANNED CYCLES
by Endika Gandarias
CANNED
CYCLE
NUMBER
DESCRIPTION
G80 Canned cycle cancellation
G81 Drilling cycle
G69 Deep hole drilling cycle with variable peck
G84 Tapping cycle
G85 Reaming cycle
G87 Rectangular pocket cycle
G88 Circular pocket cycle

63. 63
G81 G98/G99 X___ Y___ Z___ I___ K___
G81: Drilling cycle
FIXED CYCLES OR CANNED CYCLES
by Endika Gandarias
 Valid for drilling depth
≤ 3*Ø
 Valid for pecking cycle
N0 T1 D1 ; Ø8mm drill
N10 M06
N20 G00 G43 X30 Y20 Z100 F300 S1400 M03
N30 G81 G98 X30 Y20 Z2 I-15 K100 ; P1
N40 G80
N50 M30
Only one drill machining
N0 T1 D1 ; Ø8mm drill
N10 M06
N20 G00 G43 X30 Y20 Z100 F300 S1400 M03
N30 G81 G99 X30 Y20 Z2 I-15 K100 ; P1
N40 G00 X80 Y20 ; P2
N50 G00 X80 Y50 ; P3
N60 G00 G98 X30 Y50 ; P4
N70 G80
N80 M30
Four drills machining
Dwell time
(1/100s)
I.P. R.P.
Distance from
w to the
drilling depth
Distance from
w to the R.P.
Machining
coordinates
Withdrawal
planes
Z
I
Reference Plane (R.P.) - G99
Initial Plane (I.P.) - G98
W
15
8
4 3
1 2

64. 64
G81 G98/G99 X___ Y___ Z___ I___ K___
G81: Drilling cycle
FIXED CYCLES OR CANNED CYCLES
by Endika Gandarias
 Valid for drilling depth
≤ 3*Ø
 Valid for pecking cycle
N0 T1 D1 ; Ø8mm drill
N10 M06
N20 G00 G43 X30 Y20 Z100 F300 S1400 M03 ; Z100
N30 G81 G99 X30 Y20 Z2 I-15 K100 ; Z2
N40 G00 G98 X30 Y50 ; Z100
N50 G81 G99 X80 Y50 Z27 I10 K100 ; Z27
N60 G00 G98 X80 Y20 ; Z100
N70 G80
N80 M30
Dwell time
(1/100s)
I.P. R.P.
Distance from
w to the
drilling depth
Distance from
w to the R.P.
Machining
coordinates
Withdrawal
planes
Z
Z’R.P. - G99
Initial Plane (I.P.) - G98
W
15
Ref. Plane’ (R.P.) - G99’
I’
I
25
10
8
2 3
1 4
Four drills machining

65. 65
G69: Deep hole drilling cycle
with variable peck
FIXED CYCLES OR CANNED CYCLES
by Endika Gandarias
 General drilling
cycle (≥ 3*Ø)
G69 G98/G99 X___ Y___ Z___ I___ B___ C___
Drilling
peck
I.P. R.P.
Distance from
w to the R.P.
Machining
coordinates
Withdrawal
planes
Distance from
w to the
drilling depth
D___ H___ J___ K___ L___ R___
Reduction factor
for drilling peck
Dwell time
(1/100s)
Minimum
drilling peck
Approach
to the
previous
drilling
Distance between R.P.
and working surface
(absolute value)
Withdrawal
after drilling
Num. pecks
before total
withdrawal
N0 T3 D3 ; Ø10mm drill
N10 M06
N20 G00 G43 X30 Y20 Z100 F300 S1400 M03
N30 G69 G99 X30 Y20 Z2 I-60 B4 C1 D2 H10 J5 K100 L2 R0.8 ; Z2
N40 G00 G98 X30 Y50 ; Z100
N50 G69 G99 X80 Y50 Z27 I-20 B4 C1 D2 H10 J5 K100 L2 R0.8 ; Z27
N60 G98 X80 Y20 ; Z100
N40 G80
N50 M30
8
2 3
1 4
Z
Z’R.P. - G99
Initial Plane (I.P.) - G98
W
60
Ref. Plane’ (R.P.) - G99’
I’
I
25
20
B
D
D’

66. 66
G84: Tapping cycle
N0 T7 D7 ; M-10 tap
N10 M06
N20 G00 G43 X50 Y20 Z100 F600 S600 M03
N30 G84 G98 X50 Y20 Z2 I-60 R0
N40 G80
N50 M30
Z
I
Ref. Plane (R.P.) - G99
Initial Plane (I.P.) - G98
W
60
G84 G98/G99 X___ Y___ Z___ I___ K___ R___
Dwell time
(1/100s)
I.P. R.P.
Distance from
w to the thread
depth
Distance from
w to the R.P.
Machining
coordinates
Withdrawal
planes
FIXED CYCLES OR CANNED CYCLES
by Endika Gandarias
Type of tapping
R=0 Normal tapping
R=1 Rigid tapping

67. 67
N0 T4 D4 ; Ø12H6 reamer
N10 M06
N20 G00 G43 X30 Y20 Z100 F500 S2500 M03
N30 G85 G99 X30 Y20 Z2 I-35 K100
N40 G00 G98 X30 Y50
N50 G85 G99 X80 Y50 Z22 I-15 K100
N60 G00 X80 Y20
N70 G80
N80 M30
G85 G98/G99 X___ Y___ Z___ I___ K___
Dwell time
(1/100s)
I.P. R.P.
Distance from
w to the
reaming depth
Distance from
w to the R.P.
Machining
coordinates
Withdrawal
planes
FIXED CYCLES OR CANNED CYCLES
by Endika Gandarias
G85: Reaming cycle
12
2 3
1 4
Z
Z’R.P. - G99
Initial Plane (I.P.) - G98
W
35
Ref. Plane’ (R.P.) - G99’
I’
I
20
15

68. 68
Pocket MillingPecking / Drilling /
Tapping / Reaming
Engraving
by Endika Gandarias
Profile Milling
Face Milling Slot Milling
FIXED CYCLES OR CANNED CYCLES

69. 69by Endika Gandarias
FIXED CYCLES OR CANNED CYCLES
Pecking / Drilling / Tapping / Reaming
EXERCISE 15
Tool:
 Ø12mm H.M. spot drill, z=2
 Ø7.75mm H.S.S. drill, z=2
 Ø8H7 H.M. reamer, z=5
Material: Steel

70. 70by Endika Gandarias
FIXED CYCLES OR CANNED CYCLES
Pecking / Drilling / Tapping / Reaming
EXERCISE 16
Tool:
 Ø12mm H.M. spot drill, z=2
 Ø5mm H.S.S. drill, z=2
 M-6x1 H.M. tap
Material: Aluminium

71. 71by Endika Gandarias
FIXED CYCLES OR CANNED CYCLES
Pecking / Drilling / Tapping / Reaming
EXERCISE 17
Tool:
 Ø16mm H.S.S. spot drill, z=2
 Ø5mm H.S.S. drill, z=2
 M-6x1 H.M. tap
Material: Steel

72. 72
EXERCISES
EXERCISES
by Endika Gandarias

73. 73by Endika Gandarias
EXERCISES
Face milling / Profile milling
EXERCISE 18
Material: Steel

74. 74by Endika Gandarias
EXERCISES
Face milling / Profile milling
EXERCISE 19
Material: Aluminium

75. 75
EXERCISES
by Endika Gandarias
Face milling / Grooving / Pecking / Drilling / Tapping / Reaming
EXERCISE 20
Material: Aluminium

76. 76
FAGOR SIMULATOR
FAGOR SIMULATOR
by Endika Gandarias

77. 77
FAGOR SIMULATOR
by Endika Gandarias
CNC FAGOR 8060/65 SIMULATOR
www.fagorautomation.com/download/
CHANGE LANGUAGE: https://www.youtube.com/watch?v=rFTlmvQJdk8 VIDEO
VIDEOVIDEO

78. 78
GLOSSARY
GLOSSARY
by Endika Gandarias

79. 79
GLOSSARY
by Endika Gandarias
ENGLISH SPANISH BASQUE
Accuracy Exactitud Zehaztasun
Adaptative control Control adaptativo Kontrol moldagarri
Blade Hélice Helize
Burr Rebaba Bizar
Cam Leva Espeka
Carousel Carrusel Karrusel
Chamfer Chaflán Alaka
Clamp Brida Brida
Climb cutting Corte en concordancia Konkordantzia ebaketa
Clockwise Sentido horario Erlojuaren norantza
Closed loop Lazo cerrado Lotura itxia
Conventional cutting Corte en contraposición Kontraposizio ebaketa
Coolant Regfrigerante Hozkarri
Counterclockwise Sentido anti-horario Erlojuaren aurkako norantza
Dead band Banda muerta Tarte hila
Deep hole drilling Taladrado profundo Zulaketa sakona
Downtime Tiempo de inactividad Aktibitate gabeko denbora
Drill Broca Barauts
Drilling Taladrado Zulaketa
Driving system Sistema de regulación Erregulazio sistema
Dwell time Tiempo de espera Itxaron denbora
Edge finder Centrador Zentratzaile
EDM Electroerosión Elektrohigadura
Encoder Encoder Encoder
End mill Fresa plana Fresa planua
Engraving Grabado Grabaketa
Face milling Planeado Planeaketa
Feed Avance por minuto Aitzinamendua minutuko

80. 80
GLOSSARY
by Endika Gandarias
ENGLISH SPANISH BASQUE
Finishing Acabado Akabera
Fixed canned cycle Ciclo fijo Ziklo fijoa
Glass scale Regla óptica Erregela optiko
Grinding Rectificado Artezketa
Grooving Ranurado Artekaketa
Homing Búsqueda de cero máquina Zero makina bilatzea
HSS Acero rápido Altzairu laster
Investment Inversión Inbertsio
Left-hand tool Herramienta a izquierdas Ezkerretarako erraminta
Load Cargar Kargatu
Loop Lazo Lotura
Machine zero Cero máquina Zero makina bilatzea
Machining centre Centro de mecanizado Mekanizatu zentru
Modal Modal Modal
Noise Ruido Zarata
Offset Corrector Zuzentzaile
Offset table Tabla de correctores Taula zuzentzaile
Open loop Lazo abierto Lotura irekia
Part zero Cero pieza Zero pieza
Peck Picada Ziztada
Pecking Punteado Punteaketa
Pin Pasador Ziri
Pocket Cajera Kajera
Power failure Fallo de alimentación eléctrica Elikadura elektriko gabezia
Profiling Perfilado / Contorneado Perfilaketa / Kontorneaketa
Punched tape Tarjeta perforada Tarjeta perforatu
Rapid traverse Recorrido rápido Ibilbide azkar
Reamer Escariador Otxabu

81. 81
GLOSSARY
by Endika Gandarias
ENGLISH SPANISH BASQUE
Reaming Escariado Otxabuketa
Reference system Sistema de referencias Erreferentzi sistema
Referencing block Bloque de referencia Erreferentzi bloke
Repeatability Repetibilidad Errepikagarritasun
Rigth-hand tool Herramienta a derechas Eskuinetarako erraminta
Roughing Desbaste Arbastaketa
Round corner Arista matada Ertz hila
Setter gauge Calibre de alturas Altuera kalibratzailea
Set-up Puesta a punto Prestaketa
Skip Salto Jauzi
Slot Ranura Arteka
Speed Velocidad de giro Biraketa abiadura
Spot drill Broca de puntear Punteatzaile
Square corner Arista viva Ertz bizia
Stationary chuck Parte no movil Atal ez higikor
Stylus Estilete Estilete
Tap Macho de roscar Hariztatze ardatz
Tapping Roscado (con macho de roscar) Hariztaketa (hariztatze ardatzarekin)
Target position Posición objetivo Jomuga posizio
Thermal growth Alargamiento térmico Luzapen termikoa
Threading Roscado Hariztaketa
Tip Punta Punta
Tool magazine Cambiador de herramienta Erraminta aldatzaile
Tool presetting machine Máquina de pre-reglaje Doikuntza makina
Touch probe Palpador Haztagailu
Track Pista Pista
Trueness Veracidad Egiatasun
Unnoticeable Imperceptible Hauteman ezin

82. 82
GLOSSARY
by Endika Gandarias
ENGLISH SPANISH BASQUE
Vise Mordaza Baraila
Wear Desgaste Higadura
Withdrawal planes Planos de salida Irteera planu
Workholding Sistema de amarre de pieza Pieza lotze sistema