emco winnc 810M, 820 M User Manual

EMCO WinNC SINUMERIK 810/820 M

Software Description/ Software Version from 13.70

S I E M E N S

SINUMERIK

							%	/	N	G
							7	8	9
							X	C	Z	4 .	@
							4	5	6		*
							I	J	K	U	A
							1	2	3		-
							F	D	L	P	R
							+/-	0	.	=	+
							M	S	T	H	L F
										1 . n
GESFanucI E M ESeriesN 21						SINUMERIK
<						>	USB			RS232
SKIP	DRY	-4	+Z		+Y		1			60 7 0	80
	RUN						10		40		90
1 x	STOPOPT.	-X			+X		100		2 0		100
							1000		10
	SBL	-Y	-Z		+4		EDIT		6		110
							10000		2
					100%				0		120
					AUX	AUX
			0		0
				1	1

S I E M E N S

<

SINUMERIK

>

S I E M E N S							SINUMERIK
%	A	B	C	D	E	F	G	H
I	J	K	L	M	N	O	P	Q
R	S	T	U	V	W	X	Y	Z
		:	=	@	(	)		LF
				7	8	9
				4	5	6		*
				1	2	3		-
1...n				+/-	0	.		+

USB RS232

SKIP	DRY	-4	+Z		+Y	1	60 70	80
	RUN					10	40	90
1 x	STOPOPT.	-X			+X	100	20	100
						1000	10
	SBL	-Y	-Z		+4	EDIT	6	110
						10000	2
					1 0 0 %		0	120
					AUX	AUX
			0		0
				1	1

Software Description

EMCO WinNC SINUMERIK 810/820 M

Ref.No. EN 1803

Edition J2003-10

EMCO Maier Ges.m.b.H.

P.O. Box 131

A-5400 Hallein-Taxach/Austria Phone ++43-(0)62 45-891-0 Fax ++43-(0)62 45-869 65 Internet: www.emco.at

E-Mail: [e-mail]

EMCO WINNC SINUMERIK 810/820 M

PREFACE

Preface

The EMCO WinNC SINUMNERIK 810/820 M Milling Software is part of the

EMCO training concept on PC-basis.

This concept aims at learning the operation and programming of a certain machine control on the PC.

The milling machines of the EMCO PC MILL und CONCEPT MILL series can be directly controlled via PC by means of the EMCO WinNC for the EMCO MILL.

The operation is rendered very easy by the use of a digitizer or the control keyboard with TFT flat panel display (optional accessory), and it is didactically especially valuable since it remains very close to the original control.

This manual does not include the whole functionality of the control software SINUMNERIK 810/820 M Milling, however emphasis was laid on the simple and clear illustration of the most important functions so as to achieve a most comprehensive learning success.

In case any questions or proposals for improving this manual should arise, please contact us directly:

EMCO MAIER Gesellschaft m. b. H.

Department for technical documentation

A-5400 Hallein, Austria

All rights reserved, reproduction only by authorization of Messrs. EMCO MAIER © EMCO MAIER Gesellschaft m.b.H., Hallein 2003

2

EMCO WINNC SINUMERIK 810/820 M

CONTENTS

Contents

A: Key Description

Control Keyboard, Digitizer Overlay .....................................	A1
Key Functions ....................................................................	A2
Address and Numeric Keyboard .........................................	A2
Machine Control Keys ........................................................	A4
PC Keyboard .....................................................................	A6
Screen with Softkeys ..........................................................	A7

B: Basics

Reference Points of the EMCO Milling Machines .................	B1
Zero offset .........................................................................	B2
Coordinate System .............................................................	B2
Coordinate System with Absolute Programming .............	B2
Coordinate System with Incremental Programming ........	B2
Input of the Zero Offset .......................................................	B3
Input of the Coordinate Rotation .........................................	B3
Tool Data Measuring ..........................................................	B4
Input of Tool Data ...............................................................	B5
Tool Data Measuring with a Metering Clockwork
or a Measuring Cell ............................................................	B6

C: Operating Sequences

Survey Modes ...................................................................	C1
Approach the Reference Point ...........................................	C2
Input of the Gear Position ..................................................	C2
Setting of Language and
Workpiece Directory ..........................................................	C2
Input of Programs .............................................................	C3
Program Input with Guiding Function ............................	C4
Program Input with CAD/CAM Systems ........................	C4
Data Input-Output .............................................................	C5
Program Administration .....................................................	C5
Copy Program .............................................................	C5
Rename Program ........................................................	C5
Delete Program...........................................................	C5
Data Input via COM1 / COM2 ......................................	C6
Data Import .................................................................	C6
Data Output ................................................................	C7
Print Data ...................................................................	C7
Adjusting the Serial Interface .......................................	C8
Program Run ....................................................................	C9
Start of a Part Program ................................................	C9
Messages while Program Run .....................................	C9
Program Influence .......................................................	C9
Overstore ..................................................................	C10
Block Search .............................................................	C10
Program Interruption ..................................................	C10
Status Display of the PLC ...........................................	C10
Display of the Software Versions .................................	C10
Graphic simulation ...........................................................	C11

D: Programming

Program Structure .............................................................		D1
Used Addresses ................................................................		D1
Survey of M commands .....................................................		D2
Survey of cycles ................................................................		D2
Command Description GCommands .................................		D3
G00	Rapid Traverse ..........................................................	D3
G01	Linear Interpolation ....................................................	D3
G02	Circular Interpolation Clockwise ..................................	D4
G03	Circular Interpolation Counterclockwise .......................	D4
Helix Interpolation .............................................................		D4
G04	Dwell .........................................................................	D5
G09	Exact Stop .................................................................	D5
G10	- G13 Polar Coordinate Interpolation ...........................	D5
G17-G19 Plane Selection ..................................................		D6
G25/G26 Programmierbare Arbeitsfeldbegrenzung ..........		D6
G33	Thread Cutting ...........................................................	D7
Cutter Radius Compensation .............................................		D8
G40	Cancel Cutter Radius Compensation ..........................	D8
G41	Cutter Radius Compensation Left ...............................	D8
G42	Cutter Radius Compensation Right .............................	D8
G48	Leave as Approached ..............................................	D10
G50	Cancel Scale Modification ........................................	D10
G51	Scale Modification ....................................................	D10
G53	Cancel Zero Offset Blockwise ....................................	D11
G54 - G57 Zero Offset 1 - 4 / Coordinate Rotation 1-4 ........		D11
G58/G59 Programmable Zero Offset / Coordinate Rotation D11
G60	Exact Stop Mode......................................................	D12
G62,G64 Deselection Exact Stop Mode ............................		D12
G70	Measuring in Inch ....................................................	D12
G71	Measuring in Millimeter ............................................	D12
G80	Delete G81 bis G89 .................................................	D13
G81	Call Cycle L81 .........................................................	D13
G82	Call Cycle L82 .........................................................	D13
G83	Call Cycle L83 .........................................................	D13
G84	Call Cycle L84 .........................................................	D13
G85	Call Cycle L85 .........................................................	D13
G86	Call Cycle L86 .........................................................	D13
G87	Call Cycle L87 .........................................................	D13
G88	Call Cycle L88 .........................................................	D13
G89	Call Cycle L89 .........................................................	D13
G90	Absolute Programming .............................................	D13
G91	Incremental Programming ........................................	D13
G 92 Cylindrical interpolation ..........................................		D14
G94	Feed Rate in Minutes ...............................................	D15
G95	Feed Rate in Revolutions .........................................	D15
G147 Soft Approach to Contour with Linear ......................		D16
G247 Soft Approach to Contour with Quarter Circle ...........		D16
G347 Soft Approach to Contour with Semicircle ................		D16
G148 Soft Leaving the Contour with Linear .......................		D16
G248 Soft Leaving the Contour with Quarter Circle ...........		D16
G348 Soft Leaving the Contour with Semicircle .................		D16

3

EMCO WINNC SINUMERIK 810/820 M

CONTENTS

Description of M Commands .............................................		D17
M00	Programmed Stop ....................................................	D17
M01	Programmed Stop, Conditional ..................................	D17
M02	Main Program End ....................................................	D17
M03	Milling Spindle ON Clockwise ....................................	D17
M04	Milling Spindle ON Counterclockwise .........................	D17
M05	Milling Spindle OFF ..................................................	D17
M06 Tool Change .............................................................		D17
M08	Coolant ON ..............................................................	D17
M09	Coolant OFF ............................................................	D17
M17	Subroutine End ........................................................	D17
M27	Swivel Dividing Head ................................................	D17
M30	Main Program End ....................................................	D17
M53	- M58 Mirror Functions ..............................................	D18
M71	Puff Blowing ON .......................................................	D18
M72	Puff Blowing OFF .....................................................	D18
Description of Cycles ........................................................		D19
L81 Drilling, Centering ......................................................		D20
L82 Drilling, Spot Facing ...................................................		D20
L83 Deep-hole Drilling ......................................................		D21
L84 Thread Tapping with/without Encoder .........................		D22
L85 Boring 1 ....................................................................		D23
L86 Boring 2 ....................................................................		D23
L87 Boring 3 ....................................................................		D24
L88 Boring 4 ....................................................................		D24
L89 Boring 5 ....................................................................		D24
L96 Cycle for Tool Change ................................................		D25
Drilling and Milling Patterns ..............................................		D25
L900 Drilling Pattern Hole Circle .......................................		D26
L901 Milling Pattern Slot ...................................................		D26
L902 Milling Pattern Elongated Hole .................................		D27
L903 Milling Rectangular Pocket .......................................		D27
L904 Milling Pattern Circular Slot ......................................		D28
L905 Drilling Pattern Single Hole ......................................		D28
L906 Drilling Pattern Row of Holes ....................................		D29
L930 Milling Pattern Circular Pocket ..................................		D29
L999 Clear Buffer Memory ................................................		D30
Contour Definition ............................................................		D31
Insert Chamfer ...........................................................		D31
Insert Radius .............................................................		D31
Line ...........................................................................		D31
Arc ............................................................................		D31
Line - Line .................................................................		D32
Line - Arc (tangential) .................................................		D32
Arc - Line (tangential) .................................................		D32
Arc - Arc (tangential) ...................................................		D32
Subroutines .....................................................................		D33
Subroutine Call in Part Program ..................................		D33
Subroutine End with M17 ............................................		D33
Subroutine Nesting .....................................................		D33
E: @-Codes
G: Survey Pages
Survey Softkey Explanations ..............................................		G1
Softkey Menu Survey ........................................................		G6
Survey Guiding .................................................................		G8
H: Alarms and Messages
Startup Alarms ..................................................................		H1
Control Alarms ..................................................................		H3
Machine Alarms ...............................................................		H10

Starting Information

see attachment

4

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

A: Key Description

Control Keyboard, Digitizer Overlay

						6,(0 (16						6,180(5,.
										1	*
								;	&	=		#
								,	-	.	8	$
								)	'	/	3	5
								0	6	7	+	/ )
											Q
*( )DQXF,(0 6HULHV16						6,180(5,.
								86%			56
6.,3	'5<
	581		=		<
[	237	;			;
	6723
						(',7
	6%/
		<	=
					$8;	$8;
						6,(0 (16						6,180(5,.
							$	%	&	'	(	)	*	+
						,	- .		/	0	1	2	3	4
						5	6	7	8	9	:	;	<	=
										#				/)
						Q
6,(0 (16						6,180(5,.
						!		86%			56
6.,3	'5<
	581		=		<
[	237	;			;
	6723
						(',7
	6%/
		<	=
					$8;	$8;
					A 1

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

		1	*
				#
;	&	=	4
,	-	.	%	$
)	'	/	3	5
0	6	7	+	/ )

AddressandnumerickeyboardoftheSINUMERIK

810 M

Key Functions

Inputkey

Deleteinput/operatormessage

Deleteword/block

Alterword

Searchaddress/block/word

Cursorup/down

Cursor left / right

Pageup/down

Acknowledgealarm

Actualpositionindoublesizeletters

Address and Numeric Keyboard

SINUMERIK 810M:

With the SHIFT key (at the top right edge) you can selectthesecondkeyfunction.

Pressing again this key selects the first function again.

AfterinputofaNCaddress(letter)theSHIFTfunctions isactiveautomatically

. functionK

.function6

SINUMERIK 820M:

Every address or number has its own key.

A 2

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

A 3

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

Machine Control Keys

Themachinekeysareinthelowerpartofthecontrol keyboardordigitizeroverlay.

Dependingontheusedmachineandaccessorynot allofthesefunctionsareactive.

	; 4
	(',7
=	=
4	;

Machinecontrolkeyboard

6.,3	'5<		=		<
	581
[	237
	6723	;			;
						(',7
	6%/
		<	=
					$8;	$8;

MachinecontrolkeyboardoftheEMCOPC-MillSerie

= <

; ;

< =

SKIP (skip blocks will not be executed)

DRY RUN (test run of programs) OPT STOP (program stop at M01) R E S E T

Singleblockmachining

Programstop/programstart

manualaxismovement

Approachingthereferencepointinallaxes

Feedstop/feedstart

Spindleoverridelower/100%/higher

A 4

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

(',7

Spindelstop/spindlestart;spindlestartinJOGandINC1...INC10000mode: Clockwise: perss key short, Counterclockwise: press min. 1 sec. Open/closedoor

Swiveldividinghead

Open/closeclampingdevice

Swiveltoolturret

Coolanton/off

AUX OFF / AUX ON (auxiliary drives off / on)

Modeselector

Feed/rapidfeedoverrideswitch

EMERGENCY OFF (Unlock: pull out button)

Keyswitchforspecial operations(sieheMaschinenbeschreibung)

AdditionalNCstartkey

Additionalkeyclampingdevice

Consentkey

Nofunction

A 5

EMCOWINNC SINUMERIK 810/820 M	KEYDESCRIPTION

PC Keyboard

				!			1&
					+X

			+Z
				X -

	Z
	-

!
!

	C •
" ‰
		8
			#
	ƒ A

& '
%
	4
3
$	2
1
#
/	0
"
	.
!
	-
	,
	+
	*

)

(

5 6

7

7

		The machine functions in	the numeric key block are active only with active NUM	lock.
		F12Withthe function keys PRESET, MDI-	AUTOM.,JOG, REPOS, AUTOMATIC and POINTREF will be displayed in the softkey		line.
		*
		acknowledgedbewillalarmsSomewith the key ESC.	modestheF1keythepressingBy (JOG, AUTOMATIC,...) will be	line.softkeytheindisplayed	functionsaccessorytheofassignementThe is described int the chapter Functions"."Accessory	combinationkeytheofmeaningThectrl 2 depends on the machine: 50/55:MILLPCEMCOPuff blowing ON/OFF 100/125/155:MILLPCEMCOcoolant ON/OFF
	7

A 6

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

Screen with Softkeys

	:LQ1& 6LQXPHULN 7 F (0&2					[
6,(0(16						6,180(5,.

Attheoperatingfieldthefollowingpartsaredefined:

1Displayofthemode

2Displayoftheoperatingconditions

3Displayofalarmnumber,text(comment)

4Displayofnotestotheoperator

5Displayofinputsfromthekeyboard

6Displayofthechannelnumber

7Displayofthesoftkeyfunctions

8Key"jumpbacktoahigherlevelmenu"(key F2at thePC)

9Softkeys (keys F3 - F7 at the PC)

10Key "Further functions in the same menu" (key F11 at the PC)

Softkeys (9) are keys with multiple meaning. The validmeaningwillbedisplayedatthebottomline(7) ofthescreen.

Screenwithsoftkeys

A 7

EMCO WINNC SINUMERIK 810/820 M

KEY DESCRIPTION

A 8

EMCO WINNC SINUMERIK 810/820 M

BASICS

B: Basics

	1
0
:	5

Referencepointsintheworkingarea

Reference Points of the EMCO

Milling Machines

M = Machine zero point

Anunchangeablereferencepointestablishedbythe machinemanufacturer.

Proceeding from this point the entire machine is measured.

Atthesametime"M"istheoriginofthecoordinate system.

R = Reference point

A position in the machine working area which is determinedexactlybylimitswitches.Theslidepositions are reported to the control by the slides approachingthe„R“.

Requiredaftereverypowerfailure.

N = Tool mount reference point

Startingpointforthemeasurementofthetools.„N“ liesatasuitablepointonthetoolholdersystemand isestablishedbythemachinemanufacturer.

W = Workpiece zero point

Startingpointforthedimensionsinthepartprogram. Canbefreelyestablishedbytheprogrammerand movedasdesiredwithinthepartprogram.

B 1

EMCO WINNC SINUMERIK 810/820 M

BASICS

0

:

ZerooffsetfrommachinezeropointMto workpiecezeropointW

	=
Incremental
	=
<
	;
;
	<
=
<	Absolute
=	;
;
	<

Absolutecoordinatesrefertoafixedpoint,incrementalcoordinatestothetoolposition

Zero offset

WithEMCOmillingmachinesthemachinezeropoint "M"liesontheleftfrontedgeofthemachinetable. This position is unsuitable as a starting point for dimensioning. With the so-called zero offset the coordinatesystemcanbemovedtoasuitablepoint intheworkingareaofthemachine.

Inthesettingdatazerooffsetarefouradjustablezero offsetsavailable.

When you define a value in the offset register, this valuewillbeconsideredwithcallupinprogram(G54 -G57)andthecoordinatezeropointwillbeshifted fromthemachinezeroMtotheworkpiecezeroW.

The workpiece zero point can be shifted within a program with "G58, G59 - programmable zero offset" in any number.

MoreinformationsseeincommanddescriptionG58, G59.

Coordinate System

TheXcoordinateliesparalleltothefrontedgeofthe machinetable,theYcoordinateliesparalleltothe sideedgeofthemachinetable,theZcoordinateis verticaltothemachinetable.

Z coordinate values in minus direction describe movementsofthetoolsystemtowardstheworkpiece, valuesinplusdirectionawayfromtheworkpiece.

Coordinate System with Absolute Programming

Theoriginofthecoordinatesystemliesinthemachine zeropoint"M"orafterazerooffsetintheworkpiece zero point "W".

Alltargetpointsaredescribedfromtheoriginofthe coordinatesystembyindicationoftherespectiveX, Y and Z distances.

Coordinate System with Incremental Programming

The origin of the coordinate system lies at the tool mountreferencepoint"N"oratthetooltipafteratool call-up.

Withincrementalprogrammingtheactualpathesof thetool(frompointtopoint)aredescribed.

B 2

EMCO WINNC SINUMERIK 810/820 M

BASICS

:LQ1& 6LQXPHULN 0 F (0&2			[

$8720$7,&

6(77,1*'$7$ =(52 2))6(7 *

=(52 2))6(7		=(52 2))6(7 $'',7,9(
;		;
<		<
=		=

* )	* )	* )	* )	)

InputpatternforzerooffsetG54

Input of the Zero Offset

Fourzerooffsetscanbeentered(e.g.forfourdifferentclampingdevices).

•Press the softkey SETTING DATA in any mode.

•Press the softkey ZERO OFFSET.

•Thescreenshowstheinputpatternforzerooffset G54. The particular offsets G54 - G57 can be selectedwithsoftkeys.

•BelowZEROOFFSETthemeasuredvalues(e.g.: X,Y,Z=distancemachinezeropoint-workpiece zeropoint)areentered.

•Correctionstothisvaluescanbeenteredbelow ZO ADDIT.. These corrections will be added.

•MovetheCursortothevaluetobealteredwiththe

keys

.

•Enternewvalueandpressthekey.

•The inverse input mark jumps to the next input field.

:LQ1& 6LQXPHULN 0 F (0&2			[

-2* 6(77,1*'$7$ &225',1$7( 527$7,21

$		*
$		*
$		*
$		*
$		*
$		*

)	)	)	)	)

Inputpatternforcoordinaterotation

Input of the Coordinate Rotation

Acoordinaterotationcanbeprogrammedforevery zerooffset.Thiscoordinaterotationbecomesactive withcallingupthezerooffset.

•Press the softkey SETTING DATA in any mode.

•Extendthesoftkeyline(key ! )andpressthe softkey ROTAT. ANGLE.

•The screen shows the input pattern for the coordinaterotation.ThesinglerotationsforG54 -G57canbeenteredinthispattern,therotations forG58andG59willbedeterminedintheCNC program.

•Movethecursortothevaluetobealteredwiththe keys .

•Enterthenewvalueandpressthekey.

•The inverse input mark jumps to the next input field.

B 3

EMCO WINNC SINUMERIK 810/820 M

BASICS

1

=

Lengthcorrection

5 5

Cutter radius R

1	1
/	/
	5

W\SH

W\SH

Tooltype

Tool Data Measuring

Aimofthetooldatameasuring:

Thecontrolshouldusethetooltiporthetoolcentre pointforpositioning,notthetoolmountreference point.

Every tool which is used for machining has to be measured.Thedistancebetweentooltipandtool mountreferencepointistobemeasured.

In the so-called tool register the measured length corrections,thecutterradiusandthecutterposition canbestored.

Every tool offset number D1 - D99 is related to a tool.

Thecorrectionnumbercanbeanyregisternumber, buthastobeconsideredwithtoolcallinprogram.

Example

Thelengthcorrectionsofatoolintetoolturretstation 4havebeenstoredascorrectionnumber41.

Toolcallinprogram:	T4	D41 L96
or:	T4 D41 M6

The address T marks the position in the tool turret, theaddressDmarksthecorrectionnumberbelonging toit.ThecycleL96includestheexecutionofthetool change(dependingonthemachine)intheprogram. UsethecommandM6,ifyouwanttochangethetool with OVERSTORE.

Inserting cutter radius is only necessary for using cutter radius compensation with this tool.

ForactiveX-Yplane(G17):

Thetooldatameasuringoccursfor:

L1: inZdirectionabsolutefrompoint"N"

R:cutterradius

Type: cutter position 1 - 9

Thetooldatameasuringoccursfortype10:

L1: inZdirectionabsolutefrompoint"N"

Type: drilling tool 10, milling tool 20

ForallotheractiveplanesL1isalwayscalculatedas verticalaxistotheactiveplane.

InthefollowingthecommoncaseG17isdescribed.

With "WEAR" occurs the correction of not exact measured tool data or of worn tools after several machiningruns.Theinsertedlengthwillbeaddedor subtractedfromthegeometryofthetoolincrementally.

L1 +/- .....Incremental

R +/- ......Incremental

B 4

EMCO WINNC SINUMERIK 810/820 M

BASICS

:LQ1& 6LQXPHULN 0 F (0&2										[
$8720$7,&
722/ 2))6(7
$FWXDO WRRO RIIVHW QR						'
'	7RRO QXPEHU
	7\SH
	/ *HRPHWU\
	/ *HRPHWU\
	'LDPHWHU 5DGLXV
	/ :HDU
	/ :HDU
	'LDPHWHU 5DGLXV
	/ %DVH
	/ %DVH
	)		)		)	)			)

Inputpatternfortooldata

Input of Tool Data

Select the softkey TOOL OFFSET in any mode. Thescreenshowstheinputpatternfortooldata.

•Select the desired tool offset number with the keys andorbyentryofthecorrection numberandthekey"search"(e.g. ).

•Position the Cursor (invers mark) with the keys

and to the desired input field. Enterthedesiredvaluewiththenumerickeyboard. Theenteredvaluewillbeshownattheinputline ofthescreen.

•Storethecorrectionvaluewiththekeyinthe tooloffsetregister.

Thecursorjumpstothenextinputpositionresp. afterinputofthelastvaluetothefirstvalueofthe nexttooloffsetnumber.

Additiveinputwith,deletewith.

B 5

EMCO WINNC SINUMERIK 810/820 M

BASICS

1

1

Traversewiththetoolmountreferencepointonto themeteringclockworkormeasuringcell

Tool Data Measuring with a MeteringClockwork

or a Measuring Cell

Sequence of operation

•Setupthemeteringclockworkorthemeasuring cellsointheworkingarea,thatthemeasuringpoint canbereachedwiththetoolmountreferencepoint andwithalltoolstobemeasured.

•ChangetothemodeJOG.

•Traversewiththetoolmountreferencepointonto themeteringclockworkandsetittozeroorontothe measuringcelluntilthelamplightsup.

•NotethefirstZvalue(Z1),whichisdisplayedatthe screen.

Note

AttheEMCOPCMILL100thetoolmountreference point is on the face centre of the reference tool. Clampthistoolforthesequencedescribedabove.

• Clampthetooltobemeasuredandtraversewithit ontothemeteringclockworkuntil0isdisplayedor ontothemeasuringcelluntilthelamplightsup.

• NotethesecondZvalue(Z2),whichisdisplayedat

thescreen.

• ThedifferenceZ2-Z1isthelengthcorrectionL1of

thetool.

• Insert L1 for the corresponding tool correction numberintotheinputpatternfortooldata.

• Insert tool type 10 or 20, for type 20 also the tool radius.

Traversewiththetooltipontothemetering

clockworkormeasuringcell

• Clampnexttoolandtraverseontothemetering clockworkormeasuringcelletc..

B 6

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

C: Operating Sequences

Survey Modes

AUTOMATIC

For working off a part program the control calls up block after block and interprets them.

The interpretation considers all corrections which are called up by the program.

The so-handled blocks will be worked off one by one.

JOG

With the JOG keys the tool can be traversed manually. In the submode OVERSTORE (softkey) you can switch on the spindle and swivel the tool holder.

REFPOINT

This mode is used to approach the reference point. With reaching the reference point the actual position store is set to the value of the reference point coordinates. By that the control acknowledges the position of the tool in the working area.

With the following situations the reference point has to be approached:

•After switching on the machine

•After mains interruption

•After alarm "Approach reference point" or "Ref.- point not reached".

•After collisions or if the slides stucked because of overload.

INC FEED 1 ... INC FEED 10 000

MDI-AUTOMATIC

You can enter blocks of a part program in the intermediate store.

The control works off the inserted block and deletes the intermediate store for new entries.

1 ... 10000

In this mode the slides can be traversed for the desired increment (1 ... 10000 in µm / 10-4 inch) with

means of the JOG keys -X + X - Y +Y

-Z +Z .

The selected increment must be larger than the machine resolution (smallest possible traverse distance), otherwise no movement occurs.

C 1

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

Approach the Reference Point

By approaching the reference point the control will be synchronized with the machine.

•Select the mode REFPOINT (after starting the software REFPOINT is active automatically).

Press the JOG keys -X or + X to approach the reference point in X, analogous for Y and Z.

•With the key REFALL all axes will be approached automatically (PC keyboard).

Danger of collisions

Take care of obstacles in the working area (clamping devices, clamped workpieces, etc.).

After reaching the reference point the position of the reference point will be displayed at the screen as actual position. Now the control is synchronized with the machine.

Input of the Gear Position

(only for EMCO PC Turn 50)

For that the control can supervise the correct spindle speed, the selected gear (belt) position of the machine must be entered.

•Press the softkey SETTING DATA in any mode.

•Extend the displayed softkey menu with

the key > .

•Press the softkey spindle.

•Move the cursor to the input field (Spindle gear stage" and enter the corresponding gear position..

1	gear position 1	120 - 2000 U/rev
2	gear position 2	280 - 4000 U/rev

Setting of Language and

Workpiece Directory

•Press softkey SETTING DATA

• Expand the softkey line with the key > and

press the Softkey GENERAL DATA

•In the input pattern you can set the language and the work piece directory.

Workpiece directory

In the workpiece directory the CNC programs created by the operator will be stored.

The workpiece directory is a subdirectory of the directory in which the software was installed.

Enter the name of the workpiece directory with the PC keyboard, max. 8 characters, no drives or pathes. Not existing directories will be created.

Active language

Selection from installed languages, the selected language will be activates with restart of the software.

Input with PC keyboard:

•DT for German

•EN for English

•FR for French

•SP for Spanish

•NL for Netherlands

C 2

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

Input of Programs

Part programs and subroutines can be entered in the modes

JOG AUTOMATIC

INC 1 ... INC 10 000 and REFPOINT.

Call up an existing or new program

•Press softkey PART PROGRAM

•Press softkey EDIT

•Enter program number %... or L...

•Press softkey SELECT PROGRAM

Blocks in an existing program will be displayed.

			Input of a Block
			Example:
N	5		Block number (not necessary)
G	1		1. word
X	N	3	2. word
... ... ...
LF			LineFeed - block end (with PC keyboard	)
or

Insert Block

Position the cursor before the block, that should follow the inserted block and enter the block to be inserted.

Delete Block

Position the cursor before the block, enter block number (if no block number: N0) and press key .

Insert Word

Position the cursor before the word, that should follow the inserted word and enter the word (address

and value) to be inserted and press .

Alter Word

Position the cursor before the word to be altered, enter word and press .

Delete Word

Position Cursor before the word to be deleted, enter address (e.g. X) and press key .

C 3

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

WinNC Sinumerik M (c) EMCO					x
AUTOMATIC
CONTOUR	LINE - CIRCLE
	G 03
	G 02
Ep2
	R
	Ep1		Wa
X			Wa :	A
			R :	B
			Ep1 :	Z
Z			EP2:	X
				G
MEMORYF3 SELECT F4 STORE		F5	F6 DELETE		F7
MENU	MEMORY		PARAM.

Input pattern for guiding line-circle

Program Input with Guiding Function

In an openend program you can enter blocks guided by menues.

Frequently used G and M commands are displayed as softkey functions.

It is also possible to enter predefined contour drafts without need to calculate intermediate positions.

Example: Program contour draft line - circle

•Press softkey GUIDING

•Press softkey GEOM. PATH

•Press softkey LINE - CIRCLE

•The input pattern beside will be displayed. The selected contour draft (line-circle) is displayed graphically.

•Enter with the keyboard the input values one by one.

•If in the input fields several values are in curved brackets only one of this values must be entered. If you have entered several values, you can delete the odd values with the softkey PARAM. DELETE.

•Press the softkey STORE, SOTRE MENU or STORE SELECT when input is finished.

•Now the contour draft will be stored as block in the program with all the entered geometry values. The software automatically creates a block end (LF) and displays the inserted block.

Program Input with CAD/CAM Systems

Principially NC programs can be read in from CAD/ CAM systems into WinNC SINUMERIK 810/820 M.

Act as following:

•The NC program has to be created in the format of the SINUMERIK 810/820.

•The file has to be renamed.

The NC programs of the Control System are stored as following:

%MPFxxxx ...... main program %SPFxxxx ...... subprogram (xxxx ............... program number)

E.g.: Rename with WINDOWS File Manager: From: PART1.81M

To: %MPF123

•Import the program with DATA IMPORT (see Data Input/Output).

C 4

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

WinNC Sinumerik M (c) EMCO

x

AUTOMATIC

DATA INPUT

Available memory: 62589 Zeichen

Data type:
Interface no. for data in:	2
Interface allocation:	1 = RTS-LINE
	2 = RTS-LINE

DATA-IN F3	DATA-	F4	BTR	F5	DATA F6	STOP F7
START	OUT		START		IMPORT

Input pattern for data input-output

Program Administration

•Press softkey PART PROGRAM

•Press softkey PROGR.- HANDLE

•In the softkey line the functions COPY

RENAME DELETE

will be displayed

Copy Program

Example:

•Enter with keyboard %88=%5

•Press the softkey COPY

•The software copies the program %88 and stores it again with the program number %5.

The program %88 is still existing.

Rename Program

Example:

•Enter with keyboard %12=%15

•Press the softkey RENAME

•The software renames the program %12 to %15. The program %12 will not be kept.

Delete Program

Example:

•Enter with keyboard %22

•Press the softkey DELETE

•The software deletes the program %22.

Data Input-Output

•Press softkey DATA IN-OUT

•The input pattern beside will be displayed

•With "Interface no. for data in:" you can select a serial interface (1 or 2) or a drive (A, B or C).

1 serial interface COM1

2 serial interface COM2 A disk drive A

B disk drive B

C hard disk drive C, workpiece directory (can be determined with installation or with GENERAL DATA in SETTING DATA) or import/export directory (see WinConfig, 4.1 Alter Directories)

C 5

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

WinNC Sinumerik M (c) EMCO										x
AUTOMATIC
DATA IMPORT
Main program:			Subroutine:
Begin: %		0	Begin:		L	0
End:	% 0		End:		L	0
Device for data in:			1
Device allocation:			A= Drive A:
			B= Drive B:
			C= Program path
TOOL-	F3	ZERO- F4	MAIN- F5	SUB-		F6	STOP F7
OFFSET		OFFSET	PROGRAM	ROUTINE

Input pattern for data import

Data Input via COM1 / COM2

•Press softkey DATA IN START. This will start the receiving function of the software.

•At the right top edge of the screen DIO (Data Input/Output) will be displayed. Destination signs the data from the sender (punched tape drive, ...).

•Start the sender.

•With the softkey STOP you can abort the data input at any time, with DATA IN START you can restart data input.

•A direct call-up of certain data by the software is not possible with data input.

Data Import

With the function data import you can load data from the drives A, B and C.

•Press softkey DATA IMPORT

•Select drive (device for data in)

•Enter below "Mainprogram" resp "Subprogram" the following program numbers:

Begin: the first program to read in End: the last program to read in

•Press the softkey MAIN PROGRAM or SUBROUTINE to start reading in the data.

•Transmission of zero offsets, tool data: Press the softkey START.

•With the softkey STOP you can interrupt the data input at any time.

C 6

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

WinNC Sinumerik M (c) EMCO

x

AUTOMATIC

DATA OUTPUT

Available memory: 63548 Zeichen

Interface no. for data out:	2
Interface allocation:	1 = RTS-LINE
	2 = RTS-LINE

TOOL-

F3

ZERO-

F4

MACH.

F5

PART-

F6

PLC-

F7

OFFSET

OFFSET

DATA

PROGRAM

M-DATA

Input pattern for data output

WinNC Sinumerik M (c) EMCO

x

AUTOMATIC

DATA OUTPUT

Main program:

Subroutine:

Begin: %

0

Begin:

L

0

End:

%

0

End:

L

0

Interface no. for data out:

2

Interface allocation:

1=RTS-LINE

2=RTS-LINE

F3

EXT

F4

MAINPRGF5

SUBROUTF6

STOP

F7

START

START

START

Input pattern for data output - part program

WinNC Sinumerik M (c) EMCO		x
AUTOMATIC
DATA OUTPUT ZERO OFFSET/ROTATION
Channel no.0
...	...	...

Data output zero offset - rotation

WinNC Sinumerik M (c) EMCO

x

AUTOMATIC

DATA OUTPUT

Available memory: 36987

Interface no. for data out:	1
...

Input pattern for data output - printer

Data Output

•Press softkey DATA OUT.

•The screen shows the input pattern beside.

•With "Interface no. for data out" you can enter a serial interface (1 or 2) or a drive (A, B or C).

•If you send data to disks, this data will be sent in the same format as with output to the serial interface. This data have to be read in with DATA IMPORT and must not be copied directly into the workpiece directory.

Example: Program output

•Press softkey PART PROGRAM

•The screen shows the input pattern beside

•Enter below mainprogram resp. subprogram the following numbers:

Begin: the first program to be sent

End:	the last program to be sent

•Press softkey MAINPRG START resp. SUBRROUT START. This will start the send function of the software.

•With the softkey STOP you can interrupt data output at any time, with MAINPRG START resp. SUBROUT START you restart data output with the first program to be sent.

Example: Zero offset output

You can select to put out zero offsets or coordinate rotations.

Channel-no. 0: Output zero offsets Channel-no. 1: Output coordinate rotation

Print Data

•Press softkey DATA OUT

•The screen shows the input pattern beside.

•With "Interface no. for data out" you can enter P to select a printer.

•Act like data output

C 7

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

WinNC Sinumerik M (c) EMCO									x
AUTOMATIC
PARAMETERS OF SERIAL INTERFACES
			COM1		COM2
Baudrate			9600		9600
Parity			E		E
Stopbits			1		1
Databits			7		7
Control parameter			00000000
ETX-Character code			00000011
F3		F4	F5		F6			F7

Input pattern for adjusting the serial interface

Adjusting the Serial Interface

•For transmission the interfaces of sender and receiver have to be set similar.

•Select SETTING DATA - SETTING BITS with softkeys.

Settings:
Baudrate	110, 300, 600, 1200, 2400,
	4800, 9600, 19200
Parity	E, O, N
Stop bits	1, 2
Data bits	7, 8

Data transmission from / to original control in ISOCode only.

ISO: 7 Data bits, Parity even (=E)

Control parameter:

Bit 0: 1...Transmission will be ceased only with ETX- (End of Text) Code (not with M30, M17, M2) - this enables transmitting several programs in one sequence

Bit 7: 1...Overwrite part program without message 0...Message, if a program is already existing

ETX character code:

free setable, has to be conform with the code set at the CNC

Settings at the original control 810/820 with SETTING DATA - SETTING BITS:

5010 - 5013:	first interface
5018 - 5021:	second interface
5028:	ETX sign

5010, 5012: 00000000
5011, 5013: 11000xxx
		coded baud rate:
001:	150 bd	010: 300 bd	011:	600 bd
100:	1200 bd	101: 2400 bd	110:	4800 bd
111:	9600 bd

NOTE

When you use an interface expansion card (e.g. for COM 3 and COM 4), take care that for every interface a separate interrupt is used (e.g.: COM1 - IRQ4, COM2 - IRQ3, COM3 - IRQ11, COM4 - IRQ10).

C 8

EMCO WINNC SINUMERIK 810/820 M

OPERATING SEQUENCES

Program Run

Start of a Part Program

Before starting a program the control and the machine must be ready for running the program.

•Select the mode AUTOMATIC.

•Enter the desired part program number (e.g.:

%59: %

7 9

.

•Press the key .

Messages while Program Run

In the first line on the screen the influences on program run will be displayed.

HALT: AUTO interrupted

The mode was changed or the key was pressed.

HALT: Single block

In single block mode one block was worked off (finished). Go on in program with key .

HALT: Pr. stop M00, M01

Programmed interruption of the program process. Continue the program with key .

HALT: Read enable

Read enable is a PLC output signal. The current block is not finished (e.g. with tool change). The next program block will be worked off after finishing the current block.

HALT: Dwell time

Processing the program is interrupted for the duration of the programmed dwell time.

FST

FEED STOP. This message will be displayed, if the PLC stops the program to execute an operation (e.g. tool change).

Program Influence

By actuating the following softkeys runnig programs can be influenced.

•Press the softkey PROGRAM CONTROL in the mode AUTOMATIC or MDI-AUTOMATIC.

•The menu line shows the following softkeys:

SKIP YES-NO	(skip block)
DRY ON-OFF	(dryrun)
OPT.STOP YES-NO	(programmed stop)
DEC-SBL YES-NO	(decoding single block)

Select this functions by pressing the corresponding softkey, deselect by pressing the softkey again.

Skip block:

Blocks in the program, which are marked by a slash before the block number (/N ...), now will not be worked off while program run.

Dryrun:

For test run without workpiece this function can be activated. All blocks with programmed feed (G01, G02, G03, G33, ...) traverse with dryrun-feed instead of the programmed feed.

The dryrun feed can be set in the setting data.

Programmed stop:

When an M01 is present in the part program, the program normally is not stopped. When the softkey function is marked with YES, the program stops with M01.

Decoding single block:

This function works in a similar way like the function SINGLE BLOCK. If this function is activated by YES, after every block, which is running through decoding, the part program will be stopped.

With the key the program can be continued.

As difference to the normal single block mode the decoding single block mode stops also with calculation blocks.

Application: testing cycles.

C 9