Numerical Control Programming

1 / 56

# Numerical Control Programming - PowerPoint PPT Presentation

Numerical Control Programming. 6.1 NC PART PROGRAMMING. Introduction Coordinate Systems NC Words. 6.1.1 Coordinate System. Z // rotating spindle. Z AXIS workpiece-rotating machine : Z is parallel to the spindle tool-rotating machine : Z is parallel to the tool axis. Z. Z.

I am the owner, or an agent authorized to act on behalf of the owner, of the copyrighted work described.

## PowerPoint Slideshow about 'Numerical Control Programming' - helki

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -
Presentation Transcript

### Numerical Control Programming

6.1 NC PART PROGRAMMING
• Introduction
• Coordinate Systems
• NC Words
6.1.1 Coordinate System

Z // rotating spindle

Z AXIS

• workpiece-rotating machine:

Z is parallel to the spindle

• tool-rotating machine:

Z is parallel to the tool axis

Z

Z

Z

6.1.1 Coordinate System

X // table

X AXIS

• workpiece-rotating machine:

X is the direction of tool movement

• horizontal milling machine:

X axis is parallel to the table

• vertical machine:

+X axis points to the right

when the programmer

is facing the machine.

X

Z

X

Z

Z

X

6.1.5 NC Words
• N, G, X, Y Z, A, B, C, I, J, K, F, S, T, R, M
• N: specify the sequence number
• G: preparatory word

to prepare for control functions (the motion of each axis, coordinate system, coordinate plane, cutter radius compensation, tool length offset……)

• M: miscellaneous word

to control miscellaneous functions (spindle on/off, start/stop the machine, turn on/off the coolant, change the tool, and rewind the program tape)

6.1.5 NC Words
• Modal codes and non modal codes/
• modal functions

Modal functions stay activeuntil some other command changes it. Modal commands are arranged in sets called “modal groups”, and only one member of a modal group may be in forces at any given time.

• non-modal functions

Non-modal functions have effect only on the lines on which they occur.

6.1.5 NC Words

modal groups

6.1.5 NC Words

modal groups

M CODES

6.1.5 NC Words

N, G, X, Y , Z, A, B, C, I, J, K, F, S, T, R, M

• F: feed rate of the tool motion
• S: cutting-speed
• T: tool number
6.1.5 NC Words
• X, Y, Z, A, B, C: provide the coordinate positions of the tool. X, Y, and Z define the three translational (Cartesian) axes of a machine. A, B and C are used for the three rotational axes about the X, Y, and Z axes.
• I, J, K: specify the center for circular motion

N, G, X, Y , Z, A, B, C, I, J, K, F, S, T, R, M

6.1.5 NC Words

N, G, X, Y, Z, A, B, C, I, J, K, F, S, T, R, M

• R: specify the clearance height in canned-cycle

N0010 G81 X1.000 Y2.000 Z0.000 R1.300

Operations in drill cycle G81 :

1. Rapid to location (1,2,2).

2. Rapid down to the R plane:(1,2,1.3)

3. Feed to the Z point, the bottom of the hole:(1,2,0)

4. Operation at the bottom of the hole .

5. Rapid or feed to either the R plane or the initial height.

G codes
• Unit selection:
• G70 (inch), G71(metric)
• Coordinates selection:
• G90(absolute), G91(incremental)
• Working plane selection:
• G17(X-Y), G18(Z-X), G19(Y-Z)

Z

23

X

25.2

G92 X25.2 Z23.0

G55

G56

G57

G58

G59

G54

Machine zero

Set up working coordinate
• Machine zero
• is unchangeable and usually is set up with the machine
• Working coordinate

(is decided by the offset from the machine zero)

• G92
• Be defined in program

End

Start

Rapid traverse: G00
• G00:
• to make the machine move at maximum speed.
• It is used for positioning motion.

G90G00 X20.0 Y10.0

G90: absolute coordinates

(20,10)

(10,10)

(0,0)

Y

End

100.0

200.0

X

Start

Linear interpolation: G01
• G01:
• linear interpolation at feed speed.

G91 G0l X200.0 Y100.0 F200.0

G91: incremental coordinates

Circular interpolation: G02, G03
• G02, G03:
• For circular interpolation, the tool destination and the circle center are programmed in one block
• G02 is clockwise interpolation, G03 is counterclockwise interpolation

End point

Y

End

X

Start

j

Center

i

Circular interpolation: G02, G03
• Specify Center with I, J, K
• I, J, K are the incremental distance from the start of the arc;
• Viewing the start of arc as the origin, I, J, K have positive or negative signs.

Y

100

R50

R60

60

40

X

O

90 120 140 200

Circular interpolation: G02, G03

N0010 G92 X200.0 Y40.0 Z0；

N0020 G90 G03 X140.0 Y100.0 R60.0 F300；

N0030 G02 X120.0 Y60.0 R50.0；

G92:

To define working coordinate

G90: absolute coordinates

Circular interpolation: G02, G03

Annotation for Circular Interpolation

• I0.0, J0.0, and K0.0 can be omitted.
• If X,Y,Z are all omitted in the program, that means start and end of arc are same points.

N0020 G02 I20.0 (a full circle)

• If I, J, K, and R all appears in circular interpolation instruction, R is valid and I, J, and K are invalid

Machine Zero

Specified point

A

G28

• The machine passes by the specified point, and then move to the machine zero.

G91 G28 X_, Y_, Z_

• X,Y,Z are the coordinate of specified point that is saved in memory of machine.
• Usually this instruction is used in the beginning and end of program.

G91: incremental coordinates

Machine Zero

Specified point in G28

A

New specified point in G29

G29

• The machine passes from the machine zero by the point that is specified in G28, and then move to the new specified point.

G29 X_, Y_, Z_

• X, Y, Z are the coordinate of new specified point
• G28,G29 are usually used to change tool
M code
• miscellaneous word
• miscellaneous functions:
• turn the spindle on/off
• start/stop the machine
• turn on/off the coolant
• change the tool
• rewind the program (tape)

M code

modal groups

M code: M00, M01
• M00 and M01 both stop the machine in the middle of a program.
• M01 is effective only when the optional stop button on the control panel is depressed. The program can be resumed through the control panel.
M code: M03, M04, M05
• M03 turns on the spindle clockwise.
• M04 turns the spindle on counterclockwise.

(The spindle rpm must be specified in the same line or in a previous line. )

• M05 turns off the spindle.
M code: M07, M08, M09
• M07 and M08 turn on different modes of coolant.
• M07: flood coolant on
• M08: mist coolant on
• M09 turns off the coolant.
M code: M06
• M06 signals the tool-change operation.
• On a machine equipped with an automatic tool changer, it stops the spindle, retracts the spindle to the tool-change position, and then changes the tool to the one specified in the T-code.
M code: M02, M30
• M02 marks the end of the program.
• M30 marks the end of the tape. It stops the spindle and rewinds the program (tape)
Example
• A 2.0-in 2.0-in. square is to be milled using a 1/2-in. end milling cutter (end mill). Write an NC part program to make the square.
G codes with animations

http://www.cncezpro.com/gcodes.cfm

Manual Part Programming Example

Tool size = 0.25 inch,

Feed rate = 6 inch per minute,

Cutting speed = 300 rpm,

Tool start position: 2.0, 2.0

Programming in inches

Motion of tool:

p0  p1  p2  p3  p4  p5  p1  p0

1. Set up the programming parameters

Programming in inches

Use absolute coordinates

Feed in ipm

N010 G70 G90 G94 G97 M04

Spindle speed in rpm

Spindle CCW

2. Set up the machining conditions

Machine moves in XY-plane

Use full-circle interpolation

Feed rate

Spindle speed

N020 G17 G75 F6.0 S300 T1001 M08

Tool no.

Flood coolant ON

3. Move tool from p0 to p1 in straight line

Linear interpolation

target coordinates

N030 G01 X3.875 Y3.698

4. Cut profile from p1 to p2

Linear interpolation

target coordinates

N040 G01 X3.875 Y9.125

or

N040 G01 Y9.125

X-coordinate does not change  no need to program it

5. Cut profile from p2 to p3

Linear interpolation

target coordinates

N050 G01 X5.634 Y9.125

6. Cut along circle from p3 to p4

circular interpolation, CCW motion

target coordinates

N060 G03 X7.366 Y9.125 I6.5 J9.0

coordinates of center of circle

N060 G03 X7.366 Y9.125 I0.866 J-0.125

7. Cut from p4 to p5

Linear interpolation

target coordinates (Y is unchanged)

N070 G01 X9.302

8. Cut from p5 to p1

Linear interpolation

target coordinates (see step 3)

N080 G01 X3.875 Y3.698

Linear interpolation

target coordinates (see step 3)

N090 G01 X2.0 Y2.0 M30

end of data

N100 M00

program stop

10. Complete RS-274 program

N010 G70 G90 G94 G97 M04

N020 G17 G75 F6.0 S300 T1001 M08

N030 G01 X3.875 Y3.698

N040 G01 X3.875 Y9.125

N050 G01 X5.634 Y9.125

N060 G03 X7.366 Y9.125 I0.866 J-0.125

N070 G01 X9.302

N080 G01 X3.875 Y3.698

N090 G01 X2.0 Y2.0 M30

Automatic Part Programming

Software programs can automatic generation of CNC data

Define Tool

CNC data

Make 3D model

Simulate

cutting

Automatic part programming and DNC

Very complex part shapes  very large NC program

NC controller memory may not handle HUGE part program

computer feeds few blocks of

NC program to controller

When almost all blocks executed,

controller requests more blocks

Assignment (Learn this software)
• CNC Simulator

Direct Numerical Control (DNC):

• A system in which a central computer downloads the NC programs block by block to many NC machine tools simultaneously is called Direct Numerical Control (DNC) system.
DNC
• Direct numerical control (DNC) – control of multiple machine tools by a single (mainframe) computer through direct connection and in real time
• 1960s technology
• Two way communication
• Distributed numerical control (DNC) – network consisting of central computer connected to machine tool MCUs, which are CNC
• Present technology
• Two way communication

Direct Numerical Control (DNC):

• This system used to work with the early NC machine tools which can not read more than a block of information at a time. The central computer feed the program information one block at a time. When the machine execute the information, the next block of information would be fed.

Distributed Numerical Control (DNC):

• Distributed NC is known by the same acronym as Direct Numerical Control (DNC). After the introduction of CNC, the machine tools have had the capability of storing large amount of information. Therefore, there have been no need to have drip feed information system, like, Direct Numerical Control. Instead, Distributed Numerical Control is introduced. In such a system, a host computer communicate with many CNC machine tools via networks and download or upload programs.

Distributed Numerical Control (DNC):

• With Distributed Numerical Control systems, it is possible to monitor the activities in individual CNC machine tools on host computer.
• Therefore, better shop floor control can be achieved.
TYPES of CNC CONTROL SYSTEMS
• Open-loop control
• Closed-loop control
OPEN-LOOP CONTROL SYSTEM
• In open-loop control system step motors are used
• Step motors are driven by electric pulses
• Every pulse rotates the motor spindle through a certain amount
• By counting the pulses, the amount of motion can be controlled
• No feedback signal for error correction
• Lower positioning accuracy
CLOSED-LOOP CONTROL SYSTEMS
• In closed-loop control systems DC or AC motors are used
• Position transducers are used to generate position feedback signals for error correction
• Better accuracy can be achieved
• More expensive
• Suitable for large size machine tools