FAGOR 800T CNC SELF-TEACHING Manual
Ref. 9804 (ing)
INDEX Chapter 1 Theory on CNC machines 1.1.- Machine axes ……………………………………………..……………..………….3 1.2.- Machine reference zero and part zero ………..…………………………..………...4 1.3.- Home Search ……………………...………………...……………………..……….5 1.4.- Travel limits ……...………………………………...………………………..…….. 6 1.5.- Part zero preset ……….……………………………...…...…………………..…….7 1.6.- Programming units ………..………………………………………………….…….8 1.7.- Spindle speed …………..…………………………………………………...…..…. 9 1.8.- Axis feedrate ………………………….…………………………………………...11 Chapter 2 Theory on tools 2.1.- The tool turret …………………………………………………………………...….3 2.2.- Tool table …………….………………………………………………….…...…..... 4 2.3.- Tool calibration …………………………………………………………….……...11 Chapter 3 Hands-on training 3.1.- Screen and keyboard description …………………………………………………...3 3.1.1.- Power-up ……...……………………………………………………….…...…...3 3.1.2.- Keyboard description ….……………………………………………………......4 3.1.3.- Description of the screen …..………………………………….……………......6 3.2.- Home Search ………………………….………………………...………………….7 3.3.- Spindle ………………………………..…………………………...………………..8 3.3.1.- Speed ranges (gears) …………….…...…………………………...…………….8 3.3.2.- Work in RPM (Revolutions per minute) ………………...……….…………... 10 3.3.3.- Work at Constant Surface Speed (CSS) ………………..………….…………. 11 3.4.- Axis jog …………………………………………………………….…………….. 13 3.4.1.- Handwheels ……………...……………..……………………….……………..14 3.4.2.- Incremental JOG …………………….….……………………….….…………15 3.4.3.- Continuous JOG mm/min …………..…………………………….…..……….16 3.4.4.- Continous JOG mm/rev ……………………………………………...………..17 3.4.5.- Rapid jog key ………………………………………………………..….……..19 3.4.6.- Move the axes with keystroke sequence: “BEGIN+start” or “END+start” ….. 20 3.5.- Tools ………...…………………………..……………………….………………..22 3.5.1.- Tool selection ………………………..……………………….………………..22 3.5.2.- Tool calibration …………..…………..………………………….…………….24 3.5.3.- How to complete the tool table ……….………………………….……………27 3.6.- Checking for proper calibration ……….……………………………….…………28
Chapter 4 Automatic operations 4.1.- Operating modes ……...……………………………………………………….…... 3 4.2.- Example of turning in “Semiautomatic” mode .…….………………………….......7 4.3.- Example of turning in “Automatic” mode ……..…………………………...….…10 4.3.1.- Programming …………………………………………………………….….... 10 4.3.2.- Simulate an operation ……...….……………………...…………..………...…13 4.3.3.- Executing an operation ………...……………………………………………...16 Chapter 5 Summary of work cycles 5.1.- Facing. “Automatic” ….………………………………………………………..….. 2 5.2.- Taper turning. “Automatic” ……….………………………………………….….... 3 5.3.- Rounding. “Automatic 1” ….…...…………………………………………...…..….4 5.4.- Rounding. “Automatic 2” ………..…………………………………………..…..…5 5.5.- Profile rounding ……………..…….……………………………………………..…6 5.6.- Threading. “Automatic” …...………………………………………………...……..8 5.7.- Grooving ……………………….……………………………………………..…… 9 5.8.- Simple drilling …...……………………………………………………………..…10 5.9.- Tapping ……………………..………………………………………….……….…11 5.10.- Profiles …...………………………………………………………...…………… 12 Chapter 6 Part-programs 6.1.- Conversational part-programs …….………………………………………...……...3 6.1.1.- What is a conversational part-program? …...…………………………....……...3 6.1.2.- Edit a part-program …………….………………………………….…….……...4 6.1.3.- Modify a part-program ……...…………………….…………………….……... 7 6.1.4.- Simulate an operation of a part-program ……………….…………….……….10 6.1.5.- Simulate a part-program ……………….…………………………….…….….11 6.1.6.- Execute an operation of a part-program ………………………………..……..12 6.1.7.- Execute a part-program from a particular operation on …….………….….…..13 6.1.8.- Execute a part-program ……………..………………………………………....14 6.1.9.- Delete a part-program ……....……………………………………………..…..17 6.2.- Program P99996 …….………………………………………………...……….….18 6.2.1.- What is it? ……………………………………………………………..….…...18 6.2.2.- How is it edited? ..……………………………………………………...…...…19 6.2.3.- Execute/simulate program P99996 ……………..…………………...…….......22
Appendix I Other machining operations on a lathe I.1.- Introduction ……………………………………………………….…………....…...2 I.2.- Spindle orientation ……………………………………...……….…...………….….3 I.3.- Live tool ……………………….……………………………………………………4 I.4.- Multiple drilling ………………………………………………………………..…...5 I.5.- Slot milling ……………………………………………………….………...……… 6 Appendix II Peripherals II.1.- Peripherals …...…………………………………………………………………….2 II.1.1.- Peripheral mode ….…………………………………………………………..... 2 II.2.- Lock/Unlock ………………..……………………………………………..…..…...4
1.- Theory on CNC machines
800T CNC This chapter describes: • How to name the axes of the machine. • What machine reference zero and part zero are. • What “Home Search” is. • What travel limits are. • How to preset a part zero. • Which are the programming units. > millimeters/inches. > radius/diameter. • Ways to operate with the spindle. > RPM/CSS. (Revolutions Per Minute/Constant Surface Speed). • Ways to move the axes. > mm/min or mm/rev.
Self-teaching Manual
Chapter 1 Page 2
800T CNC 1.1 Machine Axes.
Z axis: Along the machine. X axis: Across the machine. Self-teaching Manual
Chapter 1 Page 3
800T CNC 1.2 Machine reference zero and part zero. They are the references the machine needs in order to work: – Machine ref. zero (OM): Is set by the manufacturer and it is the origin point for the axes. – Part zero (OP): Is set by the operator. It is the part’s origin or datum point with respect to which the movements are programmed. It could be set anywhere on the part.
Home
Self-teaching Manual
Chapter 1 Page 4
800T CNC 1.3 Home Search. When the CNC is off, the axes may be moved by hand or by accident. In these situations, the CNC no longer keeps track of the real position of the axes. That is why a “Home Search” should be carried out on power-up. When searching home, the axes move to the home point set by the manufacturer and the CNC assumes the value of the coordinates set by the manufacturer for that point. When searching home, the part zero is lost. Home Home Turrent Ref. Real X
Real Z
– Home: Set by the manufacturer. It is the point where the axes move during “Home Search”. – Turret Ref.: Set by the manufacturer. Point moving with the turret. It is the point that moves during “Home Search”. Self-teaching Manual
Chapter 1 Page 5
800T CNC 1.4 Travel limits. There are two types of limits: – Hard limits: Mechanical limits set on the machine to prevent the carriage from moving beyond the ways. – Software limits: Software limits set at the CNC by the manufacturer to prevent the carriage from running into the machine’s hard limits.
Home
Self-teaching Manual
Hard limits Software limits
Chapter 1 Page 6
800T CNC 1.5 Part zero preset. It is easier to program movements from a part zero. The part zero is only set on the Z axis.
OM: Machine Ref. zero. OP: Part zero.
Self-teaching Manual
Chapter 1 Page 7
800T CNC 1.6 Programming units. The movement units of the CNC can be millimeters or inches.
millimeters
inches
The X axis movements may also be programmed in radius or in diameter.
Radius
Diameter
A
X=0 Z=0
X=0 Z=0
B
X=12 Z=-12
X=24 Z=-12
C
X=12 Z=-42
X=24 Z=-42
D
X=22 Z=-52
X=44 Z=-52
Self-teaching Manual
Chapter 1 Page 8
800T CNC 1.7 Spindle speed. It could be defined in two ways: –Cutting speed (V): It is the linear speed between the part and the tool at the contact point. –Turning speed (N): It is the angular speed of the part. The relationship between them is: V=2*π*R*N/1000 The CNC offers two ways to operate with the spindle: CSS: Constant Surface Speed.
RPM: Revolutions per minute.
V1=V2 N1V2
The CNC maintains the cutting speed (V) constant while varying the turning speed (N).
The CNC maintains the turning speed (N) constant while varying the cutting speed (V).
Self-teaching Manual
Chapter 1 Page 9
800T CNC To work at CSS, two things must be borne in mind: The part zero must be at the part’s turning axis so that the calculated turning speed is the same as the best cutting speed.
The maximum turning speed must be programmed because the turning speed increases as the diameter decreases and a particular speed should not be exceeded on parts with a large diameter. The CNC works at Constant Surface Speed (Vc) and, starting at diameter Dc (when N=Nmax), it works at constant turning speed (N).
Self-teaching Manual
Chapter 1 Page 10
800T CNC 1.8 Axis feedrate. The feedrate of the axes can be programmed in two ways: – mm/rev: The axis feedrate changes depending on spindle speed. If the spindle is stopped, the axes do not move. – mm/min: The axis feedrate is independent of the spindle speed. The axes move even when the spindle is stopped.
NOTE It is recommended to work at Constant Surface Speed (CSS) and with the feedrate in mm/rev. This way, the tool lasts longer and the resulting part finish is better.
Self-teaching Manual
Chapter 1 Page 11
2.- Theory on tools
800T CNC This chapter describes: • What the tool turret is. • What the tool table is and what information it contains. • What tool presetting is. • Defects due to errors in the tool table. > Due to wrong tool calibration. > Due to wrong tool location codes (tool shapes). > Due to wrong tool radius values.
Self-teaching Manual
Chapter 2 Page 2
800T CNC 2.1 The tool turret. The tools this CNC can use are placed on the tool turret. This turret may have either a manual or automatic tool changer. When manual, the tool change is carried out like on a conventional machine. When automatic, all the tools will be placed on the turret and the CNC will rotate the whole turret to put the tool at the work position.
Turret with manual tool change
Self-teaching Manual
Turret with automatic tool changer Chapter 2 Page 3
800T CNC 2.2 Tool table. The tool table contains tool information such as their position on the turret, dimensions, etc. When changing the tool, the CNC takes this tool information. The information kept in the tool table refers to: T, X, Z, F, R, I, K:
T: Tool number. X: Tool length (in radius) along the X axis Z: Tool length along the Z axis.
Self-teaching Manual
Tool Ref.
Chapter 2 Page 4
800T CNC R: Tool radius.
I: Tool wear along the X axis. K: Tool wear along the Z axis.
Self-teaching Manual
Chapter 2 Page 5
800T CNC F: Location code or tool shape as it has been calibrated. Once the tool dimensions are known;
The CNC must know which is the calibration point for that tool (location code) to compensate for the shaded area (radius compensation).
The location code depends on the orientation of the machine axes.
Self-teaching Manual
Chapter 2 Page 6
800T CNC Table of location codes.
F7
F3
F6
F2
F5
F1
F4
F8
F0
Self-teaching Manual
Chapter 2 Page 7
800T CNC Most common location codes.
Self-teaching Manual
Chapter 2 Page 8
800T CNC Table of location codes
F1
F5
F2
F6
F3
F7
F4
F8
F0
Self-teaching Manual
Chapter 2 Page 9
800T CNC Most common location codes.
Self-teaching Manual
Chapter 2 Page 10
800T CNC 2.3 Tool calibration. By calibrating a tool, we indicate to the CNC the tool dimensions. It is essential to carry this operation out properly for obtaining the parts with the right dimensions and for controlling the same point after changing a tool.
Different tool dimensions, same point.
Self-teaching Manual
Chapter 2 Page 11
800T CNC DEFECTS DUE TO WRONG LENGTH CALIBRATION
Part to be machined
X1: Real dim. Z1: Real dim.
X2: Wrong dim. X2 What the speed ranges (gears) are. > Operate at CSS or in RPM. • Ways to move the axes. > Selection of feedrate type. (mm/min or mm/rev) > Jog modes. (Handwheels, incremental JOG, continuous JOG...) • Tool handling. > Types of tool changer. (Manual or automatic). > Tool calibration. > Tool table. • Calibration verification.
Self-teaching Manual
Chapter 3 Page 2
800T CNC 3.1 Screen and keyboard description. 3.1.1 Power-up.
After the message: PASSED press any key to get into work mode.
GENERAL TEST PASSED
Welcome screen
Self-teaching Manual
Chapter 3 Page 3
800T CNC 3.1.2 Keyboard description.
Compact keyboard
Modular keyboard
1.- Screen. (On the modular, the CRT is separate from the keyboard). 2.- Keyboard to define special operations and their parameters. 3.- Alpha-numeric keyboard. 4.- Operator panel. NOTE: Refer to the Operation Manual Chapter 1 Sections. 1.2/1.2.1/1.2.2 Self-teaching Manual
Chapter 3 Page 4
800T CNC Description of the operator panel.
Compact’s operator panel
Modular’s operator panel
1. Axes jogging keys. 2. Work mode selector. (Continuous jog (FEED), incremental (JOG) or with handwheel ( )). 3. Selection of the turning direction ( ) and spindle start-up. Spindle speed override ( ) between 50% and 120% 4. Keyboard for CYCLE START ( ) and CYCLE STOP ( ). 5. Emergency stop. NOTE: Refer to the Operation Manual Chapter 1 Section 1.2.3 Self-teaching Manual
Chapter 3 Page 5
800T CNC 3.1.3 Description of the screen.
1.- Work mode: Standard, Automatic, turning, threading... Status during execution: In execution, interrupted or in position. 2.- Tool position in X and Z, spindle speed “S” and active tool. Information on work units and active spindle speed range. 3.- Programmed cutting conditions and percentage being applied. Work mode: RPM or CSS Active tool. 4.- BEGIN and END coordinates. When selecting an operation, it shows a drawing and the associated parameters. 5.- Editing area and CNC messages. 6.- PLC messages.
NOTE: Refer to the Operation Manual Chapter 1 Section 1.1 Self-teaching Manual
Chapter 3 Page 6
800T CNC 3.2 Home Search. After powering the machine up, carry out the “Home Search” just in case the axes of the machine have moved while the CNC was off. 1st.- The CNC does not know the position of the carriages. X?, Z? different from the X, Z displayed.
2nd.-Home the X axis. Press [X]+ + Home
Home
4th.-The CNC shows the coordinates referred to machine ref. zero Home (OM) taking the tool’s X, Z dimensions.
3rd.-Home the Z axis. Press [Z]+ +
Home
Home
Home X
Home Z
NOTE: Refer to the Operation Manual Chapter 1 Section 1.4.1 Self-teaching Manual
Chapter 3 Page 7
800T CNC 3.3 Spindle. The spindle of a machine can work in two modes: – RPM: At constant turning speed. (Section 1.7) – CSS: At constant surface speed.(Section 1.7) Press [CSS] to select the work mode. 3.3.1 Speed ranges (gears). With this CNC the machine can have a gear box. By means of RANGES, we can choose the best gear ratio for the programmed spindle speed. P
Constant Power
P
Constant Power
RANGE 2
RANGE 1
If the work speed is between N1 and N2, RANGE 1 should be used and if between N2 and N3, RANGE 2. Always try to work at constant power. Self-teaching Manual
Chapter 3 Page 8
800T CNC There are two types of gear changers: • Automatic. If the machine has an automatic gear changer, the CNC selects the right range when it has to be changed. •Manual. If the machine does not have an automatic gear changer, when a gear change is required, the CNC acts as follows: – The editing window of the CNC (last row) shows the range to be selected. – Make the change and press [ENTER]. – The CNC considers the range change completed and starts the spindle.
NOTE: Refer to the Operation Manual Chapter 4 Section 4.4/4.4.1/4.4.2 Self-teaching Manual
Chapter 3 Page 9
800T CNC 3.3.2 Work in RPM mode. (Revolutions per minute) To select the work speed (in rpm), press: [S] + (turning speed) + If the machine has a manual gear changer, the CNC will ask the user to change gears if so required. If the machine has an automatic gear changer, the CNC will assume the new range. The CNC shows the following information: F 0000.000
100%
RPM 1250
Selected speed
100%
T2
Applied override
Use the JOG keys of the operator panel to start the spindle. Spindle clockwise. Stop the spindle. Spindle counter-clockwise. Increase or decrease the applied override % in increments of 5% (between 50% & 120%).
NOTE: Refer to the Operation Manual Chapter 4 Section 4.2/4.5/4.6/4.7 Self-teaching Manual
Chapter 3 Page 10
800T CNC 3.3.3 Work at Constant Surface Speed. (CSS) Before programming the cutting speed, the working speed range must be selected. The CNC assumes the current range by default. To change the range, select a turning speed in RPM within the range to be used. Once the change is completed, enter the CSS mode and press [CSS]. To select the cutting speed (m/min) , press: [S] + (cutting speed) + To select the maximum turning speed (in rpm), press: [S] + + (maximum speed) + [ENTER] The CNC shows the following information: F 0000.000
100%
CSS 250 Selected cutting speed
100%
SMAX 1500 T2
Applied override
Maximum turning speed selected
Self-teaching Manual
Chapter 3 Page 11
800T CNC Start the spindle using the JOG keys of the operator panel. Spindle clockwise. Stop the spindle. Spindle counter-clockwise. Increases or decreases the applied override % in increments of 5% (between 50% and 120%). Depending on the position of the axes, the turning speed will be different: If X decreases, the RPM increase. If X increases, the RPM decrease. NOTE While machining an operation, NO range change will take place. To work at constant surface speed, the tools MUST BE calibrated. NOTE: Refer to the Operation Manual Chapter 4 Section 4.3/4.3.1 Self-teaching Manual
Chapter 3 Page 12
800T CNC 3.4 Axis jog. To jog the axes, we will use: Each key is used for moving the axis in one direction according to the axes of the machine. (Section 1.1) JOG keys
It can have one or two handwheels. The axes move in the turning direction of the handwheels. Handwheel
To select the jog mode, use the selector switch: Incremental jog
Continuous jog
Handwheel jog
Self-teaching Manual
Chapter 3 Page 13
800T CNC The axes may be moved in mm/min or mm/rev. To select the type of feedrate, press:
[AUX] + [2] < F mm(inches)/min F mm(inches)/rev > To quit this option, press [AUX], [END] or [CLEAR]. 3.4.1 Handwheels. – Select the feedrate of the carriages with the selector switch. ( It does not matter if it is in mm/min. mode or in mm/rev. mode.
position)
POSITION
1 10 100
Handwheel
Selector switch
D istance per increment on the handwheel dial 1 m icron. 10 m icrons 100 m icrons
Jogging distance table
– Jog the axes with the handwheels. • If the machine has 1 handwheel: Select an axis with the JOG keys. The machine moves the axis as the handwheel is being turned. • If the machine has 2 handwheels: The machine moves an axis with each handwheel.
NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.3 Self-teaching Manual
Chapter 3 Page 14
800T CNC 3.4.2 Incremental JOG . Every time a JOG key is pressed, the axis will move the selected increment. – Select the distance to move at the selector (JOG position). – Move the axes with the JOG keys. Only in mm/min. mode.
Actual displacement: 0.001 mm
JOG keys Actual displacement: 1 mm
NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.2 Self-teaching Manual
Chapter 3 Page 15
800T CNC 3.4.3 Continuous JOG. mm/min. – Select the type of feedrate: mm/min . – Enter the feedrate value: [F] + 120 + [ENTER] – Change the % override of the axes with the selector switch in FEED position. – Jog the axis with JOG keys.
Actual displacement: 60 mm/min (50%)
Actual displacement: 120 mm/min (100%) JOG keys
Selector Switch
NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.1 Self-teaching Manual
Chapter 3 Page 16
800T CNC 3.4.4 Continuous JOG. mm/rev. In this mode, the feedrate is a function of the spindle rpm. Thus, the spindle must be turning in order for the axes to be able to move. Select the type of feedrate: mm/rev. – Enter the feedrate value: [F] + 0.1 + [ENTER] – Try to jog the axes with JOG keys. The axes will not move because the spindle is stopped. – Start the spindle in RPM mode. – Change the % override for the axes with the selector switch in FEED position. – Jog the axes with JOG keys. Actual displacement: 0.05 mm/rev. (50%)
JOG keys
Selector Switch
Actual displacement: 0.1 mm/rev. (100%)
Self-teaching Manual
Chapter 3 Page 17
800T CNC – – – –
Stop the spindle. Change the spindle work mode to Constant Surface Speed (CSS), Start the spindle. Check how the spindle speed varies while moving the X axis. • If X decreases, the spindle speed increases. • If X increases, the spindle speed decreases. – Stop the spindle.
NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.1 Self-teaching Manual
Chapter 3 Page 18
800T CNC 3.4.5 Rapid jog key. – Jog the axes with the JOG keys and press the Rapid jog key at the same time. It does not matter if it is in mm/min. or mm/rev. mode, the axes will move as fast as possible. (Set by the manufacturer).
Actual movement: Rapid feedrate Rapid jog key JOG keys
Any position
NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.1 Self-teaching Manual
Chapter 3 Page 19
800T CNC 3.4.6 Move the axes with keystroke sequence: “BEGIN + start” and “END + start”. 1.- Select the feedrate value. 2.- Select the BEGIN and END points. –Moving the machine by hand: BEGIN or END
•[BEGIN] or [END] •[ENTER]
BEGIN or END
BEGIN or END
•[BEGIN] or [END] •[X] •[ENTER]
– At the keyboard: 1. Press [BEGIN] or [END] 2. [X] 3. (X value)
•[BEGIN] or [END] •[Z] •[ENTER]
4. [Z] 5. (Z value) 6. [ENTER]
Self-teaching Manual
Chapter 3 Page 20
800T CNC 3.- Moving to the BEGIN or END points. Moving two axes: 1.[BEGIN] + 2.[END] +
Moving one axis: 1.[BEGIN] + [X] + 2.[BEGIN] + [Z] + 3.[END] + [X] + 4.[END] + [Z] +
:Interrupts the movements. : Resumes execution. [RESET]+[RESET]: Cancels the execution. NOTE: Refer to the Operation Chapter 2 Section 2.4 Self-teaching Manual
Chapter 3 Page 21
800T CNC 3.5 Tools. 3.5.1 Tool selection. Depending on the machine, there are two possibilities: • Machine with manual tool changer. The tool change is carried out like on a conventional machine: – Change the tool on the machine.
Remove the old tool
Put the new tool in
– Press [TOOL]. – Enter the tool number so the CNC assumes the values of the corresponding tool table. – Press NOTE: If when executing a part, a tool change is necessary, the CNC stops the spindle and shows a message requesting the number of the required tool. Self-teaching Manual
Chapter 3 Page 22
800T CNC •
Machine with automatic tool changer. No tool has to be removed. – Press [TOOL]. – Enter the tool number. – Press – The CNC rotates the turret until the new tool is in work position.
NOTE: If while making a part, a tool change is necessary, the CNC makes the change automatically, takes the turret to the change position and makes the change.
NOTE: Refer to the Operation Manual Chapter 2 Section 2.2 Self-teaching Manual
Chapter 3 Page 23
800T CNC 3.5.2 Tool calibration. – Just before calibrating the tools,a “Home Search” must be carried out on all axes. Homing the X axis. [X]+ +
Homing the Z axis. [Z]+ + Home
Home
– To calibrate a tool, a part previously turned and faced is needed.
Use continuous JOG or handwheels
Self-teaching Manual
Chapter 3 Page 24
800T CNC – Measure the part. – Enter in calibration mode [AUX] + [3] + [2] – To calibrate, start the spindle. – Answer the questions asked by the CNC. 1.- Part’s X dimension. (radius or diameter) + [ENTER] 2.- Part’s Z dimension. (Length) + [ENTER] 3.- Tool number. [TOOL] + (tool number) +
Self-teaching Manual
Part dimensions
Chapter 3 Page 25
800T CNC 4.- Move the axes in JOG and touch the part along the X axis. Press: [X] + [ENTER] The CNC shows the X coordinate. 5.- Move the axes in JOG and touch the part along the Z axis. Press: [Z] + [ENTER] The CNC shows the Z coordinate.
[X] + [ENTER]
[Z] + [ENTER]
To calibrate another tool, repeat steps 3, 4, and 5. Stop the spindle. To exit this mode, press [END]. NOTE: Refer to the Operation Manual Chapter 3 Section 3.4.2 Self-teaching Manual
Chapter 3 Page 26
800T CNC 3.5.3 How to complete the tool table. The I, K values are set to zero when calibrating. To enter the other values (F, R), press: – [AUX] + [3]< Tools > + [1] – Select the tool data to be changed: (Tool number) + [RECALL] – Use the keys to place the cursor over the value to be changed. – Key in the new value. – Press [ENTER]. – To change another value, place the cursor over it and change it. – To quit this option, press [END].
NOTE: Refer to the Operation Manual Chapter 3 Section 3.4.1 Self-teaching Manual
Chapter 3 Page 27
800T CNC 3.6 Checking for proper calibration. – Preset the part zero.
Select a tool. e.g. Location code 3
Approach the tool along Z. Press [Z]+[0]+[ENTER]
Withdraw the tool. Part zero position.
– Start the spindle and touch the part diameter with several tools while checking the value on the screen. – The tools are different but the value on the screen must be the same.
Self-teaching Manual
Chapter 3 Page 28
4.- Automatic Operations
800T CNC This chapter describes: • Which are the keys associated with the automatic operations. • How to execute an operation. > In “Semiautomatic” mode. > In “Automatic” mode (cycle level). • Turning example in “Semiautomatic” mode. • Turning example in “Automatic” mode. > Define the specific parameters for the operation. > Other parameters. (Safety distance, finishing conditions). > Simulate an operation. – ZOOM function. > Execute an operation. – Tool inspection. – Tool wear compensation.
Self-teaching Manual
Chapter 4 Page 2
800T CNC 4.1 Operating modes. Compact keyboard
Modular keyboard
Layout of the automatic function keys
Self-teaching Manual
Chapter 4 Page 3
800T CNC Operation keys
Grooving. Threading. Rounding. Taper turning. Facing. Turning. Profiling. Compact
Modular
Access to simple drilling, tapping. “Semiautomatic” / “Automatic”. Self-teaching Manual
Chapter 4 Page 4
800T CNC It is possible to work in “Semiautomatic” or “Automatic” mode. The choice is made as follows: • Automatic operations in “Semiautomatic” mode. In this mode, the operator controls the machine with the JOG keys and the handwheels. The BEGIN and END points of the section to be machined, chamfer angles, rounding radius, etc. must be defined. The CNC does not apply tool radius compensation.
Turning
Taper turning
Rounding
Examples of “Semiautomatic” mode
NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.1 Self-teaching Manual
Chapter 4 Page 5
800T CNC • Automatic operations in “automatic” mode. In this mode, the operation is defined and it is run automatically. Besides the BEGIN and END points, the operation data must also be defined. The keys for defining this data are: : Depth of cut.
: Rounding radius.
: Angles.
: Thread pitch.
: Diameters.
: Number of passes.
In this mode, the following parameters must also be defined: Finishing pass, finishing feedrate, finishing tool, safety distances in X and Z. Press [AUX]. For a good finish, the tool nose radius and location code must be defined in the tool table. (Section 2.2 of this manual).
NOTE: Refer to the Operation Manual
Chapter 5 Section 5.1.2
Self-teaching Manual
Chapter 4 Page 6
800T CNC 4.2 Example of turning in “Semiautomatic” mode. – Select the turning operation. Press – Select the “Semiautomatic” mode. Press
Diagram for “Semiautomatic” mode
– Set the BEGIN and END values. [BEGIN] + [Z] + (Value) + [ENTER] [END] + [Z] + (Value) + [ENTER] – Set the cutting conditions (feedrate, spindle speed and tool). – Start the spindle.
Self-teaching Manual
Chapter 4 Page 7
800T CNC – Carry out the turning operation. Move the X axis with the JOG keys and the handwheel up to the desired depth. Move the Z axis by pressing “[BEGIN]+start” or “[END]+start”. Only the Z axis moves.
1. Approach manually.
2. Turn with [END]+
3. Move away manually.
4. Withdraw with [BEGIN]+
NOTE: Refer to the Operation Manual Chapter 5 Section 5.2.1 Self-teaching Manual
Chapter 4 Page 8
800T CNC NOTE: Remember that in “Semiautomatic” mode and depending on which operation has been selected, the “[BEGIN]+start” or “[END]+start” will execute it differently. – When turning or threading, movements parallel to the Z axis. – When facing, movements parallel to the X axis. If no operation has been selected, when doing “[BEGIN]+start” or “[END]+start” both axes move. “Semiautomatic” mode
DRO mode
[BEGIN]+
Self-teaching Manual
[END]+
Chapter 4 Page 9
800T CNC 4.3 Example of turning in “automatic” mode. 4.3.1 Programming. – Select the turning operation. Press – Select the “Automatic” mode. Press
Diagram for the “Automatic” mode
– Define these parameters: Φ:( ): Final turning diameter. ∆ :( ): Pass (depth of cut). N:( ): Total number of passes for the turning operation. The “N” value is only taken into account when ∆=0. Self-teaching Manual
Chapter 4 Page 10
800T CNC – Other parameters: With this CNC it is possible to change the finishing feedrate, the depth of the pass and finishing tool. To access this option, press [AUX]. The screen will show the following menu: 1.- % ∆ CYCLE FINISHING PASS
(% of pass for the finishing pass)
2.- %Φ CYCLE FINISHING PASS. 3.- T CYCLE FINISHING PASS. 4.- SAFETY DISTANCE X. 5.- SAFETY DISTANCE Z.
(% of feedrate for the finishing pass) (Finishing tool)
With options [4] and [5], we set the safety distances along the X and Z axes. These safety distances are programmed to prevent the tool from running into the part when approaching in rapid.
Example of how to apply safety distances.
NOTE: Refer to the Operation Manual Chapter 5 Section 5.2.2 Self-teaching Manual
Chapter 4 Page 11
800T CNC With option [1], we select the finishing pass. If ∆=2mm and %D=50, the finishing pass will be 1mm (50%). If ∆=2mm and %D=100, the finishing pass will be 2mm (100%). If ∆=2mm and %D=0, the finishing pass will be 2mm (100%). With option [2], we select the feedrate for the finishing pass. If %F=50, the finishing feedrate will be 50% of the programmed F. If %F=100, the finishing feedrate will be100% of the programmed F. With option [3], we select the tool for the finishing pass. If T=0, the roughing tool will be used for the finishing pass.
Self-teaching Manual
Chapter 4 Page 12
800T CNC 4.3.2 Simulate an operation. It is used for checking the tool path on the screen. – Press [SIMUL] (at the compact) or [AUX]+[S] (at the modular). The CNC will display the graphics menu. – To define the display area, press [AUX].
X,Z: Point on the part that will appear at the center of the screen. WIDTH: Width of the graphics on the screen. After setting the display area, to start the simulation, press The simulation speed is controlled with the Feedrate Override Switch. Other useful keys are: : Interrupt simulation. While interrupted: : Resume simulation. [CLEAR] : Delete the graphics on the screen. [END] : Exit the simulation mode. Once the simulation is over. Press [END].
NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.3 Self-teaching Manual
Chapter 4 Page 13
800T CNC NOTE: When simulating the path, the screen only shows half the part. This is because only the path of the tool tip is shown and not the part.
Graphics The screen shows: Rapid movement. Movement at programmed F.
NOTE: To check the part dimensions on the simulation screen, the simulation has to be made with a tool with a nose radius R=0.
Self-teaching Manual
Chapter 4 Page 14
800T CNC ZOOM function: Only when the simulation is interrupted or finished. It is used for enlarging or decreasing the drawing or a section of it. Press [Z]
MODULAR
COMPACT
[AUX]
[SIMUL]
Move the rectangle. Increase the size of the rectangle. Decrease the size of the rectangle. Draw the selected section. Draw the selected section and assume the new display area. End of the ZOOM function.
[ENTER] [END]
NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.3.1 Self-teaching Manual
Chapter 4 Page 15
800T CNC 4.3.3 Execute an operation. The operations in “Automatic” mode may be executed from beginning to end or a pass at a time. This choice is made by the key. To start the execution, press Once the execution has started: : Interrupts the execution. While interrupted: : Resumes the execution. [CLEAR] : Cancels the execution. The execution can be interrupted at any time, except during a threading pass. In that case, the execution will stop at the end of the pass. When interrupting a program, the active keys are:
NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.4 Self-teaching Manual
Chapter 4 Page 16
800T CNC Tool inspection. With this option, the operation may be interrupted for inspecting and replacing the tool. – Press + [TOOL]. The CNC stops the spindle and displays the message: JOG KEYS AVAILABLE EXIT – Move the tool with the JOG keys or the handwheels. – Check the tool. – Press [END]. The CNC starts the spindle and displays the message: RETURN AXES OUT OF POSITION – With the JOG keys or handwheels, take the axes back to their position when the execution was interrupted. The CNC will not let the axes go beyond this point. The CNC displayes the message: RETURN AXES OUT OF POSITION NONE – Press
NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.4.1 Self-teaching Manual
Chapter 4 Page 17
800T CNC Changing the tool wear values: With this option, it is possible to change the I, K values while the program is either running or interrupted. The entered values are incremental and will be added to the ones stored before. – Press . The CNC shows the message “T”. – Key in the tool number and press [RECALL]. – The CNC shows the table for that tool and requests the I value. – Enter the I value and press . The CNC requests the K value. – Enter the K value and press [ENTER]. – To change the offset of another tool, press [TOOL]. – To quit this option, press [END].
NOTE: Refer to the Operation Manual Chapter 3 Section 3.4.4 Self-teaching Manual
Chapter 4 Page 18
5.- Summary of work cycles
800T CNC 5.1 “Automatic” Facing. Cycle parameters BEGIN, END: First and last points of the cycle.
Φ : Final facing diameter. ∆ : Depth of each pass. If ∆ =0, “N” will be taken into account. N : Number of facing passes. Finishing parameters. Cutting conditions. Execution 1. Approach to the BEGIN point 2. Roughing the part in several passes. 3. Finish the part in a single pass. If programmed.
Roughing
Finish
NOTE: The CNC starts and stops the spindle.
NOTE: Refer to the Operation Manual Chapter 5 Section 5.3.2 Self-teaching Manual
Chapter 5 Page 2
800T CNC 5.2 “Automatic” Taper Turning. Cycle parameters BEGIN: Theoretical positioning corner. Φ : Smaller final diameter. ∆ : Depth of the Pass. If ∆ =0, “N” will be taken into account. N : Number of taper turning passes. a : Taper angle with the Z axis. % : Slope of the chamfer. When entering a or “%”, another value is updated. : Selection of the profile type. Finishing parameters. Cutting conditions.
Types of profile Execution
Roughing
Finishing
NOTE: Refer to the Operation Manual Chapter 5 Section 5.4.2 Self-teaching Manual
Chapter 5 Page 3
800T CNC 5.3 “Automatic” Rounding (Cycle Level 1). Cycle parameters BEGIN: Theoretical positioning corner. Ρ: Defines the rounding radius. ∆ : Depth of the pass. If ∆ =0, “N” will be taken into account. N : Number of rounding passes. : Selection of the profile type. : Type of rounding.(concave, convex). Finishing parameters. Cutting conditions. Types of profile to be machined Execution
Roughing
Finishing
NOTE: Refer to the Operation Manual Chapter 5 Section 5.5.2 Self-teaching Manual
Chapter 5 Page 4
800T CNC 5.4 “Automatic” Rounding (Cycle Level 2). Cycle parameters BEGIN: First rounding point. END: Last rounding point. R: Defines the rounding radius. ∆ : Depth of the pass. If ∆ =0, “N” will be taken into account. N : Number of rounding passes. : Selection of the profile type. : Type of rounding.(concave, convex). Types of profiles to be machined
Finishing parameters. Cutting conditions.
Execution
Roughing
Finishing
NOTE: Refer to the Operation Manual Chapter 5 Section 5.5.2 Self-teaching Manual
Chapter 5 Page 5
800T CNC 5.5 Profile Rounding. Cycle parameters BEGIN: First rounding point. END: Last rounding point. R: Rounding radius. ∆ : Distance between two passes.
α : Angle with Z of the first rounding section. α1: Angle with Z of the second rounding section. use the key to select this data. αT: Cutter angle with the X axis. Use the keys to select this data. Setting the angles
Setting the angle of the tool
Self-teaching Manual
Chapter 5 Page 6
800T CNC Cycle parameters H: Amount of material to be removed (in radius). use the keys to select this data. With the sign, we choose the roughing type. H(+): Passes parallel to programmed profile. H(-): Passes parallel to the Z axis or X axis depending on the tool. For the finishing pass, the CNC has to know how the tool enters and exits the profile. To select how it enters, press Roughing passes
To select how it exits, press
Finishing parameters. Cutting conditions. Tool entry/exit
NOTE: Refer to the Operation Manual Chapter 5 Section 5.5.3 Self-teaching Manual
Chapter 5 Page 7
800T CNC 5.6 “Automatic” Threading. Cycle parameters BEGIN: First threading point. END: Last threading point. P : Thread pitch. ∆ : Depth of the first pass (in radius). H: Depth of the thread (in radius). α: Penetration angle. :Inside or outside thread.
D: End of thread distance. X, Z: Safety distances.
Finishing parameters. Cutting conditions. Penetration angle Execution
Approach to the BEGIN point.
Making the thread in consecutive passes.
NOTE: Refer to the Operation Manual Chapter 5 Section 5.6.2 Self-teaching Manual
Chapter 5 Page 8
800T CNC 5.7 Grooving. Cycle parameters BEGIN: First grooving point. END: Last grooving point or depth of the groove. F : Last smaller diameter. ∆ : Depth of the pass. If ∆ =0, “N” will be taken into account. N : Number of grooving passes. TW: Tool width. Finishing parameters. Cutting conditions. Execution
Roughing
Finishing
NOTE: Refer to the Operation Manual Chapter 5 Section 5.7 Self-teaching Manual
Chapter 5 Page 9
800T CNC 5.8 Simple drilling. [AUX] + [6] + “Simple drilling. Tapping” Cycle parameters BEGIN: First drilling point. END: Last drilling point. P : maximum penetration in each drilling peck. If P=0, tapping. Finishing parameters. Cutting conditions. Execution
The tool penetrates P and withdraws up to “BEGIN+Z” position to remove material. Rapid approach up to 1 mm off the previous peck. Repeat these steps until reaching the total drilling depth. Rapid Move. The tool stays at the bottom of the Move at programmed F. hole for 400 msec (dwell) for better part finish.
NOTE: Refer to the Operation Manual Chapter 5 Section 5.8 Self-teaching Manual
Chapter 5 Page 10
800T CNC 5.9 Tapping. [AUX] + [6] + “Simple drilling. Tapping” Cycle parameters BEGIN: First tapping point. END: Last tapping point. P=0, tapping. Finishing parameters. Cutting conditions.
Execution
Rapid move. Move at programmed F.
The tool penetrates at the programmed feedrate up to the END point. The spindle starts turning in the opposite direction. Withdrawal at programmed feedrate to the “BEGIN + Z” position.
NOTE: Refer to the Operation Manual Chapter 5 Section 5.8 Self-teaching Manual
Chapter 5 Page 11
800T CNC 5.10 Profiles. Cycle parameters
Roughing passes
Up to 9 points and 6 rounding operations may be defined. If all the points are not used, the first unused point will have the values of the last point used. ∆ : Depth of the pass. Η: Amount of material to be removed. Press Η>0: Roughing passes parallel to the profile. H=0: No roughing. Only finishing pass. H What a conversational part-program is. > How to edit it. > How to change it (Insert or delete operations). > How to simulate an operation or part-program. > How to execute an operation. > How to execute starting at a particular operation. > How to execute a program. > Delete a program. • Program P99996. > What it is. > How to edit it. > How to simulate and execute it.
Self-teaching Manual
Chapter 6 Page 2
800T CNC 6.1 Conversational part-programs. 6.1.1 What is a conversational part-program? It is a set of operations ordered secuentially. Each operation is defined separately (always in “automatic” mode) and they are then stored one after the other in a program. Up to 20 operations. The name of the part-program can be any integer between 00000 and 99990. Besides these, the number 99996 corresponds to a part-program written in CNC language, ISO code (Section 6.2 in this manual). The CNC can store up to 10 part-programs. The rest of them must be stored at a PC. Turning Taper turning Rounding Profile
Facing
PART 32741 1 - FACING 2 - TURNING 3 - TAPER 4 - ROUNDING 567? EXIT
NOTE: The profile occupies two memory positions. Self-teaching Manual
Chapter 6 Page 3
800T CNC 6.1.2 Edit a part-program. To edit a part-program, we first choose the operations needed to execute the part. A part may be executed in various ways. Taper turning Rounding Turning
Profile
Different solutions for the same part
Self-teaching Manual
Chapter 6 Page 4
800T CNC Once the sequence of operations has been chosen (in our case we will make the previous example), we are going to build the part program editing the operations one by one in “automatic” mode.
DRO MODE
PART 01234 [*] 24832 [*] 12345 [ ] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
Press [RECALL]
PART 01234 [*] 24832 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
Choose position
PART 01234 [*] 24832 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
Press [P]
The dashes indicate that there is no part-program. [*] : The part has been already edited. It contains data. [ ] : The part contains no data. [ENTER] EXIT: Exit the table. If when pressing [P] no other program can be entered, it means that there are already 10 programs in memory.
Self-teaching Manual
PART 01234 [*] 24832 [*] 00000 [ ] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
Enter number
PART 12345 1? 2? 3? 4? 5? 6? 7? EXIT
Chapter 6 Page 5
800T CNC Choose the operation and define the parameters. Choose position
NOTE: To go from the parameter table to the operations table, press
PART 12345 1? 2? 3? 4? 5? 6? 7? EXIT
[ENTER] [ENTER]
PART 12345 1 - TAPER 2? 3? 4? 5? 6? 7? EXIT
Repeat these steps with the other operations. In our case, the finished partprogram will be: Program number Operations
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
Self-teaching Manual
Chapter 6 Page 6
800T CNC 6.1.3 Modify a part-program. The operations making up a part-program can be modified.
Choose program
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
The CNC shows the cycle with all its data. Modify the operation parameters like in the editing mode.
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
[ENTER]
Choose operation
CNC requests confirmation.
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
[ENTER]
[RECALL]
The new operation replaces the old one.
7 Section 7.6 Self-teaching Manual
Chapter 6 Page 7
800T CNC New operations can also be inserted into a part-program.
Choose program
Choose position
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
[ENTER]
Choose operation
CNC requests confirmation.
Define parameters and cutting conditions of the operation to be inserted.
Press [1]
PART 12345 1 - TAPER 2 - GROOVING 3 - ROUNDING 4 - TURNING 5? 6? 7? EXIT
NOTE: Refer to the Operation Manual Chapter 7 Section 7.6 Self-teaching Manual
Chapter 6 Page 8
800T CNC Operations can be deleted from a part-program. PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
CNC requests confirmation.
PART 12345 1 - TAPER 2 - GROOVING 3 - ROUNDING 4 - TURNING 5? 6? 7? EXIT
[ENTER]
PART 12345 1 - TAPER 2 - GROOVING 3 - ROUNDING 4 - TURNING 5? 6? 7? EXIT
[CLEAR]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
NOTE: Refer to the Operation Manual Chapter 7 Section 7.6 Self-teaching Manual
Chapter 6 Page 9
800T CNC 6.1.4 Simulate an operation of a part-program. It is used to check the tool path on the screen. PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
Choose program
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
At the compact model, press [SIMUL] [RECALL]+
At the modular model, press [AUX]+[S]
Graphics screen.
To define a display area, press [AUX]. Self-teaching Manual
Chapter 6 Page 10
800T CNC 6.1.5 Simulate a part-program. The simulation starts with the first operation and ends when finding a free (empty) position. PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
Choose program
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
At the compact model, press [SIMUL] At the modular model, press [AUX]+[S]
Graphics screen
To define a display area, press [AUX]. Self-teaching Manual
Chapter 6 Page 11
800T CNC 6.1.6 Execute an operation of a part-program. The operations of a part-program can be executed separately.
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING [RECALL]+ 4? 5? 6? 7? EXIT
NOTE: Refer to the Operation Manual Chapter 7 Section 7.5.1 Self-teaching Manual
Chapter 6 Page 12
800T CNC 6.1.7 Execute a part-program from a particular operation on. The execution may begin at any operation.
DRO MODE
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
Operations 2 and 3 will be executed.
Self-teaching Manual
Chapter 6 Page 13
800T CNC 6.1.8 Execute a part-program. The execution begins with the first operation and ends when finding a free (empty) position. PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[RECALL]
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
PART 12345 1 - TAPER 2 - ROUNDING 3 - TURNING 4? 5? 6? 7? EXIT
NOTE: Refer to the Operation Manual Chapter 7 Section 7.5 Self-teaching Manual
Chapter 6 Page 14
800T CNC The execution begins with the first operation and ends when finding a free (empty) position. When the CNC executes an operation, the bottom of the screen shows the operation with all its parameters. Once the execution has started: : Interrupts the execution. While being interrupted: : Resumes the execution. [RESET]+[RESET] : Cancels the execution. The execution can be interrupted at any time, except during a threading pass. In that case, the execution will stop at the end of the pass. When interrupting a program, the active keys are:
NOTE: Refer to the Operation Manual Chapter 7 Section 7.5 Self-teaching Manual
Chapter 6 Page 15
800T CNC How does the tool move? After executing an operation, the tool goes to the BEGIN point maintaining the safety distances. When going from one operation to another, the tool moves in a straight line from the BEGIN point of the current one to the BEGIN of the next one. When ending the last operation, the tool goes back to the where the partprogram execution started. If the manufacturer has not set a tool change position, it will be done where the execution started.
Self-teaching Manual
Chapter 6 Page 16
800T CNC 6.1.9 Delete a part-program. Select the program in the table and press [CLEAR].
[RECALL]
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
PART 01234 [*] 24832 [*] 12345 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
[CLEAR]
CNC requests confirmation.
[ENTER]
PART 01234 [*] 24832 [*] ----- [ ] ----- [ ] ----- [ ] ----- [ ] ----- [ ] EXIT
NOTE: Refer to the Operation Manual Chapter 7 Section 7.7 Self-teaching Manual
Chapter 6 Page 17
800T CNC 6.2 Program P99996. 6.2.1 What is it? It is a program written in CNC programming language. (ISO code).
... N100 G01 X20 Z0 N110 G01 X20 Z-30 N120 G03 X34 Z-37 R7 N130 G01 X34 Z-60 N140 G02 X54 Z-70 R10 N150 G01 X54 Z-100 N160 G00 X70 Z20 ...
Self-teaching Manual
Chapter 6 Page 18
800T CNC 6.2.2 How is it edited? It can be edited at the CNC or at a PC. To edit it at the CNC, press: [AUX]+[5]+[5]
Blocks in memory
Block to be edited
Editing screen
Self-teaching Manual
Chapter 6 Page 19
800T CNC When editing blocks: Besides the alphanumeric keys [0]...[9], [F], [S], [T], [X], [Z] we will use: as P. as R. as A. The missing function keys (G, M, I, K) are displayed in the help [AUX]. (The CNC will only offer the right help possibilities). [ENTER]: Save block. [CL]: Delete character. Example: N40 G01 X10 Z-10_ [CL] N40 G01 X10 Z-1_ Self-teaching Manual
Chapter 6 Page 20
800T CNC When modifying blocks: [RECALL] :Call a block. Example: N40 [RECALL] N40 G01 X10 Z-10_ :Delete a block. :To insert or overwrite . :Search for previous or next blocks. To move over a block: N60 [RECALL] N60 G01 G90 X30 Z-20 T2_ N60 G01 G90_ X30 Z-20 T2
at the compact,
at the modular.
[CL] N60 G01 G9_ X30 Z-20 T2 [1] N60 G01 G91_ X30 Z-20 T2 [ENTER]
NOTE: Refer to the Operation Manual Chapter 3 Section 3.11 Self-teaching Manual
Chapter 6 Page 21
800T CNC 6.2.3 Ejecute/simulate program P99996. To access this mode: – Press [AUX]+[5]+[4] Steps to execute/simulate program P99996. – Choose execution mode AUTOMATIC/SINGLE BLOCK – Choose first block: [N] + [RECALL] or [N]+ (block number) + [RECALL] – To simulate, press [SIMUL], (at the compact model), or [AUX]+[S], (at the modular model). To define the display area, press [AUX]. – To execute program P99996, press the START key NOTE: While executing, press [4] to display the tool path or [0] to return to the previous screen.
NOTE: Refer to the Operation Manual Chapter 3 Section 3.10 Self-teaching Manual
Chapter 6 Page 22
800T CNC Screen for executing program P99996 Execution mode
Block in execution and following ones
Cutting conditions
A: Actual C: Command R: To go
Active functions
COMMAND: Tool’s target point. ACTUAL: Current tool position. TO GO: Distance left to reach the target point.
Self-teaching Manual
Chapter 6 Page 23
Appendix I Other machining operations on a lathe
800T CNC I.1 Introduction. For this type of machining operations, the machine must have a spindle which can be oriented and a live tool. If the machine has these features, the CNC menu will offer the “Multiple drilling” and “Slot milling” choices when pressing [AUX]+[6].
Multiple drilling
Slot milling
Self-teaching manual
Appendix I Page 2
800T CNC I.2 Spindle orientation. With this feature the spindle can be oriented to the desired angular position for drilling holes and milling slots both on the face of the part or on its turning surface. To orient the spindle, press: – [S]+ . The CNC shows the message: “ S POS= ”. – Enter the target angular position for the spindle. – Press The spindle stops, (if it was turning) and it positions at the specified angle. The CNC shows the angular position in degrees. By pressing or , it will return to the conditions prior to orienting the spindle.
Self-teaching manual
Appendix I Page 3
800T CNC I.3 Live tool. To select the speed of the live tool, press: – [TOOL] + [S]. The CNC shows the message: “ T RPM= ”. – Enter the speed of the live tool in rpm. – Press The CNC shows the following information: F 0000.000
100%
RPM 1250
100%
TRPM 800
T2
Live tool speed To stop the live tool, press: – [TOOL] + [S] + [0] + [ENTER].
NOTE: Refer to the Operation manual Chapter 2 Section 2.2.1 Self-teaching manual
Appendix I Page 4
800T CNC I.4 Multiple drilling. [AUX] + [6] + “Multiple drilling”
Cycle parameters
Execution
BEGIN: First drilling point. END: Last drilling point. P : Maximum drilling depth.
α: Angular position of the first hole. D: Angular gap betwen holes. N: Number of holes. Finishing parameters. Cutting conditions.
Rapid move. Move at F.
NOTE: Refer to the Operation manual Chapter 5 Section 5.9 Self-teaching manual
Appendix I Page 5
800T CNC I.5 Slot milling. [AUX] + [6] + “Slots”
Cycle parameters
Execution
BEGIN: First point of the slot. END: Last point of the slot.
α: Angular position of the first slot. D: Angular gap between slots. N: Number of slots. Finishing parameters. Cutting conditions. Rapid move.
Move at F.
NOTE: Refer to the Operation manual Chapter 5 Section 5.10 Self-teaching manual
Appendix I Page 6
Appendix II Peripherals
800T CNC II.1 Peripherals. Peripherals are devices external to the CNC (FAGOR floppy disk unit, PC, etc.) which could be used to store data. This data is transmitted from the CNC (while in Peripheral mode) or by means of the DNC protocol.
II.1.1 Peripheral mode. In this mode, part-programs can be transferred between the CNC and the FAGOR floppy disk unit, a general peripheral device or a PC. To select this option, press: DRO MODE
[AUX] + [5] + [2]
The CNC will show the following menu:
0 - RECEIVE FROM FLOPPY DISK UNIT (Fagor) 1 - SEND TO FLOPPY DISK UNIT (Fagor) 2 - RECEIVE FROM GENERAL DEVICE 3 - SEND TO GENERAL DEVICE 4 - FLOPPY DISK UNIT DIRECTORY (Fagor) 5 - DELETE FLOPPY DISK UNIT PROGRAM (Fagor) 6 - DNC ON/OFF Self-teaching manual
Appendix II Page 2
800T CNC In order to work with these options, the DNC option must be OFF. If ON, (the word DNC will appear at the upper right-hand corner of the screen), press [6] to turn it OFF. The word DNC disappears. 0 - RECEIVE FROM FLOPPY DISK UNIT 1 - SEND TO FLOPPY DISK UNIT 2 - RECEIVE FROM GENERAL DEVICE 3 - SEND TO GENERAL DEVICE Options 0, 1, 2 and 3 are used to exchange programs between the CNC and the peripheraldevices. The numbers of the programs which can be exchanged are: P00000 through P99990 Corresponding to part-programs. P99994 and P99996 Special ISO-coded programs. P99997 CANNOT be transmitted (internal use). P99998 Used to associate texts with PLC messages. P99999 Machine parameters and tables. While working with these options, the screen will show: “RECEIVING” or “SENDING” and, when the transmission is completed, “PROGRAM NUM. P----- RECEIVED” or “SENT”. 4 - FLOPPY DISK UNIT DIRECTORY To see the list of the programs stored in the Fagor Floppy Disk Unit. 5 - DELETE FLOPPY DISK UNIT PROGRAM To delete a program of the Fagor Floppy Disk Unit, key in the program number and press [ENTER]. 6 - DNC ON/OFF To turn the DNC mode ON or OFF.
NOTE: Refer to the Operation manual Chapter 3 Section. 3.8.1 Self-teaching manual
Appendix II Page 3
800T CNC II.2 Lock/unlock. With this option, it is possible to lock or unlock the machine parameters and the part-program memory of the CNC. When the part-program memory is locked, the existing programs cannot be modified and new ones cannot be edited. They can only be displayed and executed. To access this option, press: [AUX] + [5] + [3] The codes which can be used are: N0000 [ENTER] to unlock part-program memory. N1111 [ENTER] to lock part-program memory.
NOTE: Refer to the Operation manual Chapter 3 Section. 3.9 Self-teaching manual
Appendix II Page 4
