Presentation

1. 03/30/15
Manufacturing Automation
Computer Numerical Control (CNC)*
Dr. L. K. Gaafar

2. 03/30/15
Numerical Control
Numerical Control is the operation of a
machine using coded instructions which
consists of letters, numbers, punctuation
marks, and other symbols. This coded
information is known as the Part Program
These types of systems are referred to as
“hardwire controls” and were popular from
the 1950’s to 1970’s.

3. 03/30/15
Components of Numerical Control
Machine
Part Program
Machine Control Unit (MCU)

4. 03/30/15
Engineering design of a part
Develop manufacturing plan for the
part
Program numerical control
instructions to allow the part to be
manufactured according to the plan
Process the program to develop
cutter location data set
Post Process for a specific machine
tool
The basic NC
Process
From Bedworth et
al. 1991

5. 03/30/15
Computer Numerical Control
CNC
NC machine with a microprocessor as an
integral part of the MCU. Data handling, control
sequences, and response to input is determined
by the integrated microprocessor.
Started in the 1970s

6. 03/30/15
CNC Advantages
Increased Program storage capability at the machine
Program editing at the machine
Control systems upgrades possible
Option -resident CAM system at machine tool
Tool path verification

7. 03/30/15
Part Programming
APT (Automatically Programmed Tool) is a
software compiler for simplifying numerical
control Programming.
Developed by MIT in 1959
APT is the most widely used processor

8. 03/30/15
APT
APT (Automatically Programmed Tool) is a
software compiler for simplifying numerical
control Programming.
Developed by MIT in 1959
APT is the most widely used processor

9. 03/30/15
APT Characteristics
•Three-dimensional unbounded surfaces and
points are defined to represent the part to be made
•Surfaces are defined in a X-Y-Z coordinate
system
•In Programming, the tool does all the moving; the
part is stationary.

10. 03/30/15
APT Statement Types (5)
•Identification
•Geometry
•Motion
•Postprocessor (feed, speed, coolant, … etc.)
•Auxiliary (tool, tolerance, part, … etc.)

11. 03/30/15
APT NC Words (Codes)
N Code - Sequence Number
G Code - Control Functions
F Code - Feed Rate
S Code - Spindle Speed
T Code - Tool Selection
M Code - Miscellaneous functions
X, Y, Z Code - Coordinate position

12. 03/30/15
APT Programming Example
Cylindrical Part
Φ25
Φ22.5
Φ17.5
20
Raw Material
Finished Part
70

13. 03/30/15
APT Programming Example
Cylindrical Part
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
N0090 G00 X26.0 Z2.0 S500
N0100 G84 X17.5 Z-20.0 D0=200 D2=200 D3=650
N0110 G00 Z2.0
N0120 X50.0 Z50.0 T00
N0130 M30
Please sign up to the lab demo and watch this program running

14. 03/30/15
APT Program Interpretation
O0013
Program identification number

15. 03/30/15
APT Program Interpretation
O0013
N0010 T0404
N0010 Sequence number
T0404 Select tool number 404

16. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.0 Z0.0 S500 M04
G57 PS0
G00 Rapid movement (no cutting)
X26.0 X location (as a diameter; 13 form zero)
Z0.0 Z location
S500 Spindle speed is 500 rpm
M04 Rotate spindle counterclockwise
APT Program Interpretation
x
z
(0,0) +ve
+ve

17. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
G01 Linear interpolation (cutting)
X-0.20 Move only in x direction until you pass
the center by 0.1 mm (facing)
F100 Set feed rate to 100 mm/min.
APT Program Interpretation

18. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
G00 Move rapidly away from workpiece (no cutting)
Z2.0 the movement is 2 mm away from the face.
APT Program Interpretation

19. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
Go to a safe location away from the
workpiece [x = 50 (25 from zero), z = 50] to
change the tool.
APT Program Interpretation

20. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
T0404 Select tool number 404
Since we are using the same tool (404)for
both turning and facing, N0050, N0060 are
not needed
APT Program Interpretation

21. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
G57 PS0
G00 Rapid movement (no cutting)
X25.0 X location (as a diameter; 12.5 form zero)
Z2.0 Z location
S500 Spindle speed is 500 rpm
M04 Rotate spindle counterclockwise
APT Program Interpretation

22. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
G01 Linear interpolation (cutting)
Z-70 Move only in z direction (external turning)
F100 Set feed rate to 100 mm/min.
APT Program Interpretation

23. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
N0090 G00 X26.0 Z2.0 S500
G00 Move rapidly away from workpiece (no cutting) to
location x= 26.0 (13.0 from zero) and z = 2.0.
APT Program Interpretation

24. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
N0090 G00 X26.0 Z2.0 S500
N0100 G84 X17.5 Z-20.0 D0=200 D2=200 D3=650
G84 Turning cycle for machining the step
X17.5 final diameter
Z-20 length of step is 20 mm
D0=200 Finish allowance in X direction (0.2 mm)
D2=200 Finish allowance in Z direction (0.2 mm)
D3=650 Depth of cut in each pass (0.65 mm)
APT Program Interpretation

25. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
N0090 G00 X26.0 Z2.0 S500
N0100 G84 X17.5 Z-20.0 D0=200 D2=200 D3=650
N0110 G00 Z2.0
G00 Move rapidly away from workpiece (no cutting)
Z2.0 the movement is 2 mm away from the face.
APT Program Interpretation

26. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
N0090 G00 X26.0 Z2.0 S500
N0100 G84 X17.5 Z-20.0 D0=200 D2=200 D3=650
N0110 G00 Z2.0
N0120 X50.0 Z50.0 T00
X50.0 Z50.0 Move to the tool changing location
T00 cancel tool selection
APT Program Interpretation

27. 03/30/15
O0013
N0010 T0404
N0020 G57 G00 X26.00 Z0.0 S500 M04
N0030 G01 X-0.20 F100
N0040 G00 Z2.0
N0050 X50.0 Z50.0
N0060 T0404
N0070 G57 G00 X25.00 Z2.0 S500 M04
N0080 G01 X22.5 Z-70.0 F100
N0090 G00 X26.0 Z2.0 S500
N0100 G84 X17.5 Z-20.0 D0=200 D2=200 D3=650
N0110 G00 Z2.0
N0120 X50.0 Z50.0 T00
N0130 M30
M30 Program End
APT Program Interpretation

28. 03/30/15
Sample Geometry Statements
APT Vocabulary
POINT
LINE
PLANE
CIRCLE
PATERN
CYLNDR

29. 03/30/15
Programming Example
Raw Material Finished Part

30. 03/30/15
Programming Example
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
N008 G01 X0 Y40 Z-0.5 XYFeed 75
N009 G01 X0 Y0 Z-0.5 XYFeed 75
N010 G81 R3 E9 N7 Z-0.5
N011 M05
N012 M02
x
y

31. 03/30/15
Programming Example
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
N010 G01 X50 Y45 Z10 ZFeed 150
N011 G01 X50 Y45 Z-10 ZFeed 75
N012 G01 X50 Y45 Z10 ZFeed 150
N013 M05
N014 M02
x
y

32. 03/30/15
Program Interpretation
G55 X200 Y80
Setting the datum to the lower left corner of the work piece

33. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
Program Identification Number

34. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N001 Sequence Number
M06 Tool Change (End Mill with
Diameter=12mm
T1 Tool Number

35. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
Start rotating the spindle clockwise with 400
rpm

36. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
Go to Safe Position with feed 150mm/min

37. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
Lower the end mill to determine the depth of
cut

38. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
Move from the lower left corner
of the work piece to the right
lower one cutting with
feed=75mm/min

39. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
Move from the lower left corner
of the work piece to the right
lower one cutting with
feed=75mm/min

40. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
Cutting the horizontally up to
X=30

41. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
N008 G01 X0 Y40 Z-0.5 XYFeed 75
Cutting to X=0 & Y=40

42. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
N008 G01 X0 Y40 Z-0.5 XYFeed 75
N009 G01 X0 Y0 Z-0.5 XYFeed 75
Complete the countering

43. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
N008 G01 X0 Y40 Z-0.5 XYFeed 75
N009 G01 X0 Y0 Z-0.5 XYFeed 75
N010 G81 R3 E9 N7 Z-0.5
Repeat 7 times blocks from N003 to N009
with incremental offset of Z=-0.5

44. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
N008 G01 X0 Y40 Z-0.5 XYFeed 75
N009 G01 X0 Y0 Z-0.5 XYFeed 75
N010 G81 R3 E9 N7 Z-0.5
N011 M05
Spindle Off

45. 03/30/15
Program Interpretation
G55 X200 Y80
Program 1
N001 M06 T1
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X-8 Y0 Z-0.5 ZFeed 150
N005 G01 X70 Y0 Z-0.5 XYFeed 75
N006 G01 X70 Y60 Z-0.5 XYFeed 75
N007 G01 X30 Y60 Z-0.5 XYFeed 75
N008 G01 X0 Y40 Z-0.5 XYFeed 75
N009 G01 X0 Y0 Z-0.5 XYFeed 75
N010 G81 R3 E9 N7 Z-0.5
N011 M05
N012 M02
End Program

46. 03/30/15
Program Interpretation
Tool Change
Changing the tool

47. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Setting the datum to the lower left corner of the work piece

48. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
Program Identification Number

49. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N001 Sequence Number
M06 Tool Change (Drill with
Diameter=6mm
T2 Tool Number

50. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
Start rotating the spindle clockwise with 400
rpm

51. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
Go to Safe Position with feed 150mm/min

52. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
Stop above the center of the first hole

53. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
Start Drill the first hole

54. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
Retract to a position above the hole

55. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
Stop above the center of the second hole

56. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
Drill the second hole

57. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
Retract to a position above the second hole

58. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
N010 G01 X50 Y45 Z10 ZFeed 150
Stop above the center of the third hole

59. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
N010 G01 X50 Y45 Z10 ZFeed 150
N011 G01 X50 Y45 Z-10 ZFeed 75
Drill the third hole

60. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
N010 G01 X50 Y45 Z10 ZFeed 150
N011 G01 X50 Y45 Z-10 ZFeed 75
N012 G01 X50 Y45 Z10 ZFeed 150
Retract to a position above the third hole

61. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
N010 G01 X50 Y45 Z10 ZFeed 150
N011 G01 X50 Y45 Z-10 ZFeed 75
N012 G01 X50 Y45 Z10 ZFeed 150
N013 M05
Spindle off

62. 03/30/15
Program Interpretation
Tool Change
G55 X200 Y80
Program 2
N001 M06 T2
N002 M03 rpm 400
N003 G01 X-8 Y0 Z0 XYFeed 150
N004 G01 X20 Y15 Z10 XYFeed 150 ZFeed 150
N005 G01 X20 Y15 Z-10 ZFeed 75
N006 G01 X20 Y15 Z10 ZFeed 150
N007 G01 X50 Y15 Z10 ZFeed 150
N008 G01 X50 Y15 Z-10 ZFeed 75
N009 G01 X50 Y15 Z10 ZFeed 150
N010 G01 X50 Y45 Z10 ZFeed 150
N011 G01 X50 Y45 Z-10 ZFeed 75
N012 G01 X50 Y45 Z10 ZFeed 150
N013 M05
N014 M02
End Program

63. 03/30/15
Sample Point Statements
PTA = POINT/3,4,5
PTB LIN1
LIN2
PTB = POINT/ INTOF, LIN1,LIN2
PTC
PTD
C1
LIN3
PTC = POINT/YLARGE, INTOF, LIN3,C1
PTC = POINT/XLARGE, INTOF, LIN3,C1
PTD = POINT/YSMALL, INTOF, LIN3,C1
PTD = POINT/XSMALLE, INTOF, LIN3,C1
x
y

64. 03/30/15
Sample Point Statements
PTE
PTF
C1
PTE = POINT/YLARGE, INTOF, C1,C2
PTE = POINT/XLARGE, INTOF,C1, C2
PTF = POINT/YSMALL, INTOF, C1, C2
PTF = POINT/XSMALLE, INTOF,C1, C2
C2
x
y