Manual Centro Mecanizado Doosan PDF

Preview

Summary

Manual operación de máquinas...

Description

Programming Manual For all Doosan Machining Centers Using Fanuc Controls

©Phil Misseldine 2007

Forward While similar in appearance your CNC Machining Center operates somewhat differently from your conventional mill. Although they may share the same work envelope and number of axis the CNC does not have the array of knobs, levers or handles associated with the manual machine. In place of these are motors that move the X, Y, and Z-axis. The axis motors receive commands from the control, which is user programmed with a series of instructions. It is these instructions which determine the shape of the part to be machined.

Notice of Disclaimer This manual is intended not to replace but to supplement the control manufactures original manual. The control manufactures manual will be the final say in any discrepancy that may evolve.

2

Introduction to Programming Programming of your Doosan Machining Center involves the sequential study of the operations required to produce a component, using established engineering methods.

Finished Part

Study Part Drawing

Methodize the Part

Set up Machine

Program the Part

Machine Part

Example S4000 M03 Set spindle speed to 4000 (S4000) and turn on spindle clockwise (M03). A number of Words can be programmed on the same line. Once the line is complete this forms a ‘Block’ of information.

Example of a Block N40 G1 X20.0 Y-8.0 F80. It contains the Words: N40, G1, X20.0, Y-8.0, F80. The Addresses used are N, G, X, Y, and F, and the values are 40, 1, 20.0, -8.0 and 80.

3

Most Commonly Used G-Codes G-Code

Function

G00 G01 G02 G03 G04 G05 G08 G09 G10 G11 G17 G18 G19 G20 G21 G28 G30 G40 G41 G42 G43 G49 G54 G55 G56 G57 G58 G59 G65 G73 G80 G81 G83 G84 G86 G90 G91 G92 G94 G95 G98 G99

Rapid Positioning Feedrate Positioning Arc Clockwise Arc counter Clockwise Dwell High Speed Machining Look Ahead Control Exact Stop Data Setting Data Setting Cancel X and Y Plane Selection Z and X Plane Selection Y and Z Plane Selection Input in Inch Input in Metric Return to Reference Position Return to 2nd Reference Position Cutter Compensation Cancel Cutter Compensation Left Cutter Compensation Right Tool Length Compensation Tool Length Compensation Cancel Work piece Coordinate System 1 Work piece Coordinate System 2 Work piece Coordinate System 3 Work piece Coordinate System 4 Work piece Coordinate System 5 Work piece Coordinate System 6 Macro Call High Speed Peck Drilling Canned Cycle Cancel Drilling Cycle Peck Drilling Cycle Tapping Cycle Boring Cycle Absolute Command Incremental Command Setting Work Coordinate System Feed Per Minute Feed Per Rotation Return to Initial Point in Canned Cycle Return to R Point in Canned Cycle

Standard Standard Standard Standard Standard Optional Optional Standard Optional Optional Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard

For a complete G-code list please refer to your Fanuc manual. 4

Most Commonly Used M-Codes M Code Function M00 Program Stop M01 Optional Stop M02 Program End M03 Spindle Clockwise Rotation M04 Spindle Anti - Clockwise Rotation M05 Spindle Stop M06 Tool Change M07 Thru-Spindle Coolant On M08 Flood Coolant On M09 Coolant Off (all coolant) M10 Table (Pallet) Clamp M11 Table (Pallet) Unclamp M12 Shower Coolant On M14 Spindle Air Blow On M15 Spindle Air Blow Off M16 Air Blast for Tool Setter M18 Air Blast off M19 Spindle Orientation M29 Rigid Tapping Mode (Fanuc only) M30 Program End & Rewind M50 Auto Door Open M51 Auto Door Close M54 Parts Count M60 Pallet Change M61 Load Pallet 1 M62 Load Pallet 2 M66 ATC & APC Change with one command M76 Fixture 1 Clamp M77 Fixture 1 Unclamp M84 G01 Possible with spindle stopped M86 Fixture 2 Clamp M87 Fixture 2 Unclamp M98 Sub-Program Call M99 Sub-Program End * Not standard on all machining centers

Vertical Standard Standard Standard Standard Standard Standard Standard Standard* Standard Standard N/A N/A Optional Standard Standard Optional Optional Standard Standard Standard Optional Optional Standard Standard Standard Standard Standard Optional Optional Standard Optional Optional Standard Standard

Horizontal Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Standard Optional Standard Standard Optional Optional Standard Standard Standard Optional Optional Standard Standard Standard Standard Standard Optional Optional Standard Optional Optional Standard Standard

For a complete M-code list please refer to your Doosan Manual. 5

Control Panel

O(

RESET

POWER ON

HELP

N ) GE P C

7

8

9

X U Y V ZW Q ?

4

5

6

I

1

2

3

,

M

#

F[

SHIFT

OFF

J

A

S

=

D]

K@ R T H

_

L

ALTER

INSERT

DELETE

0

* &

B

/

SP

POS

EOB

CAN

INPUT

PROG

OFFSET SETTING

CUSTOM

PAGE

PAGE SYSTEM MESSAGE GRAPH

MODE

80 REF.RTN.

25 REF. POI NT

120

100

ON

130

50

FO

EDIT

40 OFF

140 HANDLE

EMERGENCY STOP

100

60

JOG

MEMORY

WORK LIGHT

SPINDLE

FEEDOPERATION

MDI TAPE

20 Y

MODE SELECT

180

RAPID OVERIDE

0 FEEDRATEOVERIDE

Z

X

4TH

_

+

40

ALARM

50 60

30 80 M02/M30 LUB. MACHINE

20 90 10 0

AXIS SELECT MACHIN E READY EMERGENCY REL EASE

FEED HOLD

RAPID

100

SPINDLE OVERIDE

CYCLE START

RESET

FUNCTION FLOOD

ON

MANUAL

THROUGH

AUTO OFF SI NGLE BLOCKOPTI ONAL STOPOPI ONAL BLOCK SKI PDRY RUN

PROGRAM RESTART

CONVEYOR

OFF COOLANT

MACHINE LOCK

PROGRAM PROTECT

CW

STOP

CCW

Doosan Machining Centers uses the following Fanuc Controls:

0i MB 21i MB 18i MB 16i MB

All screen pictures in this manual are from the 18i control and may differ from the control you are running.

6

Axis Movement

Every Vertical Machining Center has three axes: X - side to side Y - forwards and backwards Z - up and down

All Horizontal Machining Centers have four axes: X - side to side Y - up and down Z - forwards and backwards B - rotary

7

Manual Pulse Generator

Y X

Z

X1

4TH

_

X10

X100

+ 0 90

10

80

20

70

30 60

40 50

The Manual Pulse Generator (MPG) or Hand Wheel is used during the setup of the machine. This is separate from the machine control and gives better control of all axis during setup.

8

TOOL LENGTH OFFSET When a cutting tool is inserted into its holder, the cutting edge is located at an imprecise distance from the gauge line of the holder. By specifying G43 and the corresponding offset value (H) it is possible to compensate the difference without changing the part program. This is known as the ‘Tool Offset Value’ and is unique to the tool in the spindle.

Z Axis Home Position

Tool Length Offset Distance

Workpiece

9

Tool Length Setting Method

Using a combination of the jog buttons and MPG, bring the tool down to the predetermined "Z" point.

Work piece

Press the function key

Operators choice of 'Z' zero position. (This example uses the top of the work piece).

OFFSET SETTING

and then the [OFFSET] soft key to display the following screen.

Cursor down to Tool Number to be set. Key in value displayed in Actual Position (Relative) and press INPUT. 10

Tool Offset Memory 'C' (Optional) Tool Offset Memory 'C' allows you to use the same number for Length (H) and Diameter (D) offsets.

Press the function key

OFFSET SETTING

and then the [OFFSET] soft key to display the following screen.

Cursor down to tool number to be set. Press 'Z' and then the 'INP.C' soft key. Position value is automatically transferred in to the offset.

If using height and cutter compensation for the same tool the program should look like this N15 G43 Z.10 H1 N20 G41 X-5.0 D1 You also have the ability to adjust the tool length and diameter in the wear column.

11

Work Coordinates Every CNC machine has a reference or machine zero. This is a position that is constant to the machine. When a machine is turned on or powered up by the operator it must first be referenced. When the machine reaches its limit switches the control registers this location as home. Using the home position as a reference you can now tell the control where the work piece is located on the machine table.

Machine Home Position (X, Y, Z Ref. Point)

'X' Zero point

'Y' Zero point

Work Piece

Machine Table

12

Work Coordinate System Setting Method To set the work piece co-ordinates the user has the choice of six co-ordinate systems to choose from G54 to G59.

Press function key

OFFSET SETTING

and then the [WORK] soft key to display the following page.

Method Using an edge finder or indicator locate the part datum position. Without moving go to the work offset screen and highlight desired offset. Press hard key X, hard key 0 soft key [measure] hard key Y, hard key 0 soft key [measure] (Position value is automatically transferred in to Offset).

13

Work Coordinate System G54 - G59 and G54.1 P1 -P300 The desired Work Coordinate number should always be called at the start of every tool. Example. N4 (.75 DIA. ENDMILL ) N5 G0 G54 G90 X-2.25 Y.625 S8000 M3 N6 G43 Z.1 H1 N7 G1 Z-1. F25

Work Coordinate System Addition This option expands the Work Coordinate System giving the user up to 300 sets of work offsets to chose from.

Work Coordinate System Addition's are called in the following way. Example. N4 (.75 DIA. ENDMILL ) N5 G0 G54.1 P1 G90 X-2.25 Y.625 S8000 M3 N6 G43 Z.1 H1 N7 G1 Z-1. F25

14

PROGRAMMING Linear Interpolation (G00/G01)

GOO Rapid Traverse path (Axis will take the shortest path at 45 degrees)

Y

P2 X

G00 Rapid Path

G01 Feedrate Path

GO1 Feedrate path ( Axis will travel in a staight line)

P1

All axis of the machine tool will move in linear at either RAPID or FEEDRATE traverse rates. Any movement preceded by G00 will occur at RAPID traverse G00 X4.0 Y-3.0 Any movement preceded by G01 will occur at FEEDRATE. G01 X4.00 Y-3.00 F100.

These commands are MODAL and will stay in effect until changed.

15

Co-Ordinate Programming (G90/G91) Absolute co-ordinate programming (G90)

In absolute programming all dimensioning is taken from a fixed point.

Incremental co-ordinate programming (G91)

In incremental programming dimensioning is taken from the last position programmed and NOT from a fixed point.

16

Absolute and Incremental Programming Example

Datum

Y+

X+

Find the absolute and Incremental co-ordinates of the points listed.

ABSOLUTE (G90)

INCREMENTAL (G91)

A X __________ _ Y__

A X__________Y___________

B X __________ _ Y__

B X__________Y___________

C X __________ _ Y__

C X__________Y___________

D X __________ _ Y__

D X__________Y___________

E X __________ _ Y__

E X__________Y___________

F X __________ _ Y__

F X__________Y___________

Answers are on page 100. 17

Plane Selection (G17, G18, G19) Before an arc can be machined the correct plane must be selected.

G17

Y+

X+

When generating an arc in the 'X' and 'Z' axis G17must be selected.

G02

G03

Viewfromtop of machine

G18

Z+

When generating an arc in the 'X' and 'Y' axis G18 must be selected.

G03

G02 X+

View from front of machine

G19

Plane selection is MODAL and will stay effective until another plane is selected.

When generating an arc in the 'Y' and 'Z' axis G19 must be selected.

Z+

Y+

G02

G03

Viewfromleft side of machine

18

Circular Interpolation (G02, G03) There are two directions in which you can produce an arc G02 Clockwise and G03 Counter Clockwise. To machine an arc the machine tool requires the following information. Tool finish position in 'X' Tool finish position in 'Y' Arc offset in 'X' Arc offset in 'Y' 'I' is the Incremental value parallel to the 'X' axis. 'J' is the Incremental value parallel to the 'Y' axis. 'K' is the Incremental value parallel to the 'Z' axis.

Arc offset in 'X' is represented by 'I'. Arc offset in 'Y' is represented by 'J'. Arc offset in 'Z' is represented by 'K'.

G02 Circular Interpolation Clockwise.

Datum

Example G02 X1.0 Y0. I0.0 J-1.0 G02 (Clockwise movement) X 1.0 (Tool finish position in 'X') Y 0.0 (Tool finish position in 'Y') I 0.0 (Arc offset in 'X') J-1.0 (Arc offset in 'Y')

G02

0 000 R1.

J-1.00

G03

Example G03 X1.0 Y0. I-1.0 J0.0 G03 (Counter Clockwise movement) X 1.0 (Tool finish position in 'X') Y 0.0 (Tool finish position in 'Y') I-1.0 (Arc offset in 'X') J 0.0 (Arc offset in 'Y')

I-1.00

Datum

G03 Circular Interpolation Counter Clockwise 19

Circular Interpolation G02 N6

Cutting direction G02

Start N3 Finish N10

Arc offset parallel to the Xaxis. I 1.5

N7 R.75

X&YZERO

R1.5

N8 Arc offset parallel to the Yaxis. J 1.5

N9

O1066 (Program number) N1G17G40G80G90 (Safe start) N2T1M6 (Calls T1 and changes tool) N3G54G90G0X-1.5Y0.S718M3 (Tool moves to start position) N4G43Z.1H1 (Picks up tool length value) N5G1Z-.1F20. (Feeds to Z-depth) N6G2X0.Y1.5I1.5F40. (Clock-wise move) N7G1X3.75Y.75 (Linear move) N8G2Y-.75J-.75 (Clock-wise move) N9G1X0.Y-1.5 (Linear move) N10G2X-1.5Y0.J1.5 (Clock-wise move) N11G0Z.1 (Lifts up in Z) N12G91G28Z0Y0. (Returns Z and Y to home position) N13G90 (Back into absolute) N14M30 (Return to beginning of program)

20

Arc offset parallel to the Yaxis. J -.75

Circular Interpolation G03 Arc offset parallel to the Yaxis. J- 1.5

Arc offset parallel to the Yaxis. J .75

N9

N8 R1.5

X&YZERO

Start N3 Finish N10

Arc offset parallel to the Xaxis. I 1.5 Cutting direction G03

N7

N6

O1066 (Program number) N1G17G40G80G90 (Safe start) N2T1M6 (Calls T1 and changes tool) N3G54G90G0X-1.5Y0.S718M3 (Tool moves to start position) N4G43Z.1H1 (Picks up tool length value) N5G1Z-.1F20. (Feeds to Z-depth) N6G3X0.Y-1.5I1.5F40. (Counter Clock-wise move) N7G1X3.75Y.75 (Linear move) N8G3Y-.75J.75 (Counter Clock-wise move) N9G1X0.Y-1.5 (Linear move) N10G3X-1.5Y0.J-1.5 (Counter Clock-wise move) N11G0Z.1 (Lifts up in Z) N12G91G28Z0Y0. (Returns Z and Y to home position) N13G90 (Back into absolute) N14M30 (Return to beginning of program)

21

R.75

Radius Command (R) As an alternative to using the 'I' and 'J' commands it is possible to program an arc using the 'R' command.

1

8 7

2

6

3 4

5

This example machines a ½” radius on each corner. The datum is the top left-hand corner of the part. The tool diameter is .500”. Position No. G1X3.5Y.25 G2X4.25Y-.5R.75 G1Y-3.5 G2X3.5Y-4.25R.75 G1X.5 G2X-.25Y-3.5R.75 G1Y-.5 G2X.5Y.25R.75

1 2 3 4 5 6 7 8

The R+ command can only be used for arcs up to 180 degrees. The R- command can only be used for arcs greater than 180 degrees.

22

Cutter Compensation (G41/G42) Cutter compensation allows a program to be written without considering the size of the cutter. The three G-codes used to control cutter compensation are G41 - Cutter compensation Left G42 - Cutter compensation Right G40 - Cutter compensation Cancel

If your control has cutter compensation 'B' then different offset numbers have to applied to 'H' and 'D' values. Your program should look like this G0 G43 Z1. H1 G1 G41 Y0. D11 F50.

If your control has cutter compensation 'C' then the same offset numbers can be applied to 'H' and 'D' values. Your program should look like this G0 G43 Z1. H1 G1 G41 Y0. D1 F50.

23

Cutter Compensation (G41)

Endmill is on the left hand side of the work piece

Direction of travel Approach part at 90°applying cutter comp G41

G41 - Cutter compensation to the Left of the work piece.

Always apply cutter compensation at 90 degrees to the work piece. The program for applying cutter compensation should look like this. G1G41Y0 D1 F25. or if using cutter compensation 'B' it should look like this G1G41Y0 D11F25. When turning of cutter compensation the program should be as follows. G1G40Y.5.

G41 and G42 are Modal commands and will stay active until canceled by G40.

24

Cutter Compensation (G42)

Approach part at 90°applying cutter comp G42

Endmill is on the right hand side of the work piece

Direction of travel

G42 - Cutter compensation to the Right of the work piece.

Always apply cutter compensation at 90 degrees to the work piece. The program for applying cutter compensation should look like this. G1G42Y0D1F25. or if using cutter compensation 'B' it should look like this G1G42Y0 D11F25. When turning of cutter compensation the program should be as follows. G1G40Y.5.

G41 and G42 are Modal commands and will stay active until canceled by G40.

25

Canned (Fixed) Cycles (G73, G81, G83, G86) Canned cycles are designed to make it easier for the programmer to create programs. With the use of a single 'G' function the canned cycle can be performed in a single block. This makes programming quicker and also saves on program memory.

The formats for the most commonly used canned cycles are ...