advertisement
CNC 800 M
New Features
(Ref.0204in)
Version 2.1 (July 1995)
1. P627(1). DIVIDING FACTOR FOR ELECTRONIC HANDWHEEL FEEDBACK
SIGNALS
Machine parameter P627(1) is used with P612(6), P626(6) and P627(6) which indicate the multiplying factor for the electronic handwheel feedback signals for the X, Y and Z axis respectively.
Machine parameter P627(1) indicates whether all handwheel feedback signals are to be divided or not.
P627(1)=0 They are not divided.
P627(1)=1 All handwheel feedback signals are divided by two.
Examples for the X axis so the CNC assumes 100 pulses/turn with 25, 50 and 100 line handwheels:
25 line Fagor handwheel:
50 line Fagor handwheel:
100 line Fagor handwheel:
P612(6)=0 and P627(1)=0
P612(6)=1 and P627(1)=0
P612(6)=1 and P627(1)=1
25 x 4 / 1 = 100 lines
50 x 2 / 1 = 100 lines
100 x 2 / 2 = 100 lines
Version 2.4 (June 1996)
1. HANDWHEELS AFFECTED BY FEED-HOLD.
Until now, it was assumed that electronic handwheels operated like mechanical handwheels and, therefore, were not affected by Feedhold.
However, some applications require the electronic handwheels (manual pulse generators) to be affected by Feed-hold.
Machine parameter "P628(2)" indicates whether they are or not affected by Feed-hold.
P628(2) = 0
P628(2) = 1
Not affected
Affected.
2. AUTOMATIC TOOL CHANGERS (ATC)
With this feature, it is possible to manage tool changers at any time.
Until now, this was only possible while executing a program (P99996) in Automatic Mode.
Parameter setting:
Machine parameter "P628(3)" indicates whether the machine has an ATC or not.
P628(3) = 0
P628(3) = 1
No ATC.
The machine has an ATC.
In either case, the CNC considers machine parameter "P743" and "P745" .
P743
P745
Standard subroutine to be executed prior to a T function
Standard subroutine to be executed after a T function
The subroutines associated with the T function must contain the tool selection sequence and must be defined by the manufacturer in one of the special ISO-coded user programs: P99994 or P99996.
Both subroutines are defined by an integer between 0 and 89.
If set to 0, the CNC assumes that no subroutine is to be executed.
- 2 -
2.1 MACHINE WITH MANUAL TOOL CHANGER
Machine parameter "P628(3)" must be set to "0" (no ATC available).
Basic operation in JOG or DRO mode
Every time a new tool is selected, (T?? - START), the CNC acts as follows:
1.If machine parameter "P743" is set to a value other than "0", the CNC executes that standard subroutine.
2.The CNC outputs the BCD code and assumes the new tool.
3.If machine parameter "P745" is set to a value other than "0", the CNC executes that standard subroutine.
Basic operation while executing an automatic operation
Every time the execution of an automatic operation requires a tool change, (T01 active and the cycle requests T02), the CNC behaves as follows:
1.If machine parameter "P743" is set to a value other than "0", the CNC executes that standard subroutine.
2.It displays the message: "TOOL CHANGE" and interrupts program execution.
3.When the operator presses the [CYCLE START] key, the CNC outputs the BCD code and assumes the new tool.
4.If machine parameter "P745" is set to a value other than "0", the CNC executes that standard subroutine.
5.The CNC resumes the execution of the automatic operation.
Basic operation while executing the ISO-coded user program (99996) a ) One or both machine parameters "P743" and "P745" have been set to a value other than "0".
Every time the execution of the ISO program (99996) requires a tool changer, the CNC behaves as follows:
1.If machine parameter "P743" is set to a value other than "0", the CNC executes that standard subroutine.
2.The CNC outputs the BCD code and assumes the new tool.
3.If machine parameter "P745" is set to a value other than "0", the CNC executes that standard subroutine.
4.The CNC resumes program execution.
b) Both machine parameters "P743" and "P745" have been set to "0".
Every time the execution of the ISO program (99996) requires a tool changer, the CNC behaves as follows:
1.The CNC outputs the BCD code and assumes the new tool.
2.It executes the internal standard subroutine N99, which:
Displays the message: "TOOL CHANGE" and interrupts program execution (M00).
3.When the operator presses the [CYCLE START] key, the CNC resumes program execution.
- 3 -
2.2 MACHINE WITH AUTOMATIC TOOL CHANGER (ATC)
Machine parameter "P628(3)" must be set to "1" (ATC available).
Basic operation in JOG or DRO mode
Every time a new tool is selected, (T?? - START), the CNC acts as follows:
1.If machine parameter "P743" is set to a value other than "0", the CNC executes that standard subroutine.
2.The CNC outputs the BCD code and assumes the new tool.
3.If machine parameter "P745" is set to a value other than "0", the CNC executes that standard subroutine.
Basic operation while executing an automatic operation
Every time the execution of an automatic operation requires a tool change, (T01 active and the cycle requests T02), the CNC behaves as follows:
1.If machine parameter "P743" is set to a value other than "0", the CNC executes that standard subroutine.
2.The CNC outputs the BCD code and assumes the new tool.
3.If machine parameter "P745" is set to a value other than "0", the CNC executes that standard subroutine.
4.The CNC resumes the execution of the automatic operation.
Basic operation while executing the ISO-coded user program (99996) a ) One or both machine parameters "P743" and "P745" have been set to a value other than "0".
Every time the execution of the ISO program (99996) requires a tool changer, the CNC behaves as follows:
1.If machine parameter "P743" is set to a value other than "0", the CNC executes that standard subroutine.
2.The CNC outputs the BCD code and assumes the new tool.
3.If machine parameter "P745" is set to a value other than "0", the CNC executes that standard subroutine.
4.The CNC resumes program execution.
b ) Both machine parameters "P743" and "P745" have been set to "0".
Every time the execution of the ISO program (99996) requires a tool changer, the CNC behaves as follows:
1.The CNC outputs the BCD code and assumes the new tool.
2.It executes the internal standard subroutine N99, which:
Displays the message: "TOOL CHANGE" and interrupts program execution (M00).
3.When the operator presses the [CYCLE START] key, the CNC resumes program execution.
- 4 -
3. TREATMENT OF THE M19 (SPINDLE ORIENT)
When using ATC, the spindle must be oriented before changing tools.
This features implements function M19 to manage spindle orientation.
M19 should be included in the standard subroutine to be executed before the T function (machine parameter P743).
Requirements:
The spindle must have a spindle encoder installed.
This encoder must be connected via connector "A5", which is the same one used for the electronic handwheel associated with the Z axis.
To use this feature on machines having a handwheel associated with the Z axis, connector "A5" must be shared by the handwheel and the spindle encoder.
Precautions on machines having a Z axis handwheel:
· Both feedback devices must be commutated (handwheel and spindle encoder).
· The CNC interprets the feedback signals at connector "A5" as follows:
In "Spindle Orient" mode" (M19) as spindle feedback.
In "Open Loop Spindle" mode (M3, M4, M5) as handwheel pulses.
· If the spindle switches from "Spindle Orient" mode to "Open Loop" mode without swapping the feedback device at connector
"A5", the CNC will take the spindle pulses as handwheel pulses.
Parameter setting:
Machine parameter "P800" indicates whether there is a spindle encoder installed or not and, consequently, whether "Spindle
Orientation" is available or not.
P800 = 0 No spindle encoder installed. "Spindle Orient" not available.
P800 <>0 Spindle encoder line count (number of pulses/rev).
Besides having an spindle encoder (P800 other than 0), the following machine parameters must also be set:
P609(2)
P700
P601(7)
P612(8)
P619(6)
P719
P717
P718
P916
Spindle counting direction
Spindle speed when operating in M19
Sign of the spindle analog output associated with M19.
Type of spindle encoder reference mark (home).
Spindle orient in both directions (Negative S also possible).
Minimum analog spindle output when in M19.
Spindle in-position zone when in M19
Proportional gain K of the spindle when in M19
Spindle Orient position when executing M19 without an "S" value.
Programming format
Spindle Orient is programmed as: "M19 S4.3", where:
M19 Indicates that the spindle is now moving in Closed loop.
S4.3
Indicates the number of degrees it has to move from the reference zero mark
Programming format while in DRO mode
To orient the spindle, proceed as follows:
* Press the keystroke sequence: [F] - [BEGIN] - [END]
* Key in [1] - [9] - [S] - (desired value) - [CYCLE START]
- 5 -
Basic operation
A "M19 S4.3" type block is executed as follows:
* The CNC outputs the M19 code as any other "M" function so the electrical cabinet can execute it.
* If the spindle was in open loop (M3, M4), the CNC slows the spindle down until its speed is below the value set by machine parameter "P700" and, then, homes the spindle.
* The CNC orients the spindle to the preset position (S4.3) and at the speed set by machine parameter "P700".
If a block containing only an "M19" is executed (without "S4.3"), the CNC orients the spindle to the position set by machine parameter "P916". If "P916=0", the spindle spins indefinitely at the rpm set for M19.
using machine parameter "P619(6)".
* The spindle will remain in closed loop until:
An M3, M4 or M5 is executed
An S ???? is executed
A Reset is carried out
An M30 is executed
An execution error comes up
Example:
M3 S1000
M19
M19 S100
S1000
M19 S200
Spindle in open loop and turning clock-wise.
Orient to 100° (from reference mark, home)
Spindle in open loop recovering its previous turning direction (M3):
Spindle in closed loop, home search and orientation to 200º from reference mark.
- 6 -
Version 3.1 (November 1997)
1. GENERATING AN ISO-CODED PROGRAM
With this CNC, the ISO code (low level) for an operation or a part-program may be generated.
To use this feature, machine parameter "P630(1)" must be set to "1".
This ISO program always has the number: 99996 and can be stored either at the CNC or at a PC.
Program 99996 is a special user program in ISO code and can be:
Generated from an operation or a part-program.
Edited at the CNC itself via menu option: "Auxiliary Modes - Edit program 99996"
Loaded into the CNC after being generated at a PC.
Generating the ISO program (99996) at the CNC.
This CNC has 11 K of memory space to store program 99996. If the generated program is larger than that, the CNC will issue the relevant error message.
To generate program 99996, proceed as follows:
* If it is an operation, select or define the desired operation.
* If it is a part-program, select the desired one in the part-program directory and place the cursor on its header ("PART 01435".
A listing of the operations it consists of must appear).
* Press the keystroke sequence: [CALC] [7]. The CNC will show the graphic simulation screen.
* Press . The CNC starts simulating the part and generating its ISO-coded program 99996.
* When done with the simulation, program 99996 stored in CNC memory will contain all simulated blocks in ISO code.
Generating the ISO program (99996) at a PC
Usually, the 99996 program generated from a part-program exceeds the available memory space of the CNC.
By using "DNC30", this program may be generated at a PC.
To do this, proceed as follows:
* Activate DNC communications and execute the DNC30 program at the PC.
* Select at the PC the menu option: "Program Management - Receive Digitizing".
* At the CNC, select the operation or place the cursor on the part-program header ("PART 01435"). A listing of the operations it consists of must appear).
* Press [CALC] [8]. The CNC will display the graphic simulation screen.
* Press . The CNC starts simulating the part and generating program 99996.
* When done with the simulation, the 99996 program generated at the PC will contain all the blocks simulated by the CNC in
ISO code.
This program can be executed at the CNC through the menu option: "Execute infinite program" of the DNC30.
Note: While generating the ISO-coded program, no tool compensation is applied when simulating. However, the generated program will have the corresponding G41 and G42.
- 7 -
2. RIGID TAPPING IS NOW AVAILABLE
From this version on, typical tapping is possible (with a clutch) "P630(3)=0" as well as rigid tapping "P630(3)=1".
For rigid tapping, the CNC must control the spindle checking its turning speed at all times and supplying the necessary analog voltage for the spindle to turn at the selected speed.
General considerations:
Rigid tapping is an interpolation between the spindle and the Z axis.
The acceleration and deceleration time for the spindle and the Z axis should be the same.
The following error (lag) of the spindle and that of the Z axis must be proportional. For example, if when tapping at F1000mm/min,
S1000rpm (pitch=1mm) the observed following error is Z=1mm and S=360º, it means that they are both perfectly synchronized.
A machine parameter is now available to adjust the spindle's response (acc/dec) for each spindle range (gear).
Since the Z axis gain is different for machining and for rigid tapping, the CNC offers 2 parameters, one for each case.
Output THREADING_ON (I97) is active when carrying out a rigid tapping.
Machine parameters related to the spindle:
P800 Number of spindle encoder pulses (0...9999)
P601(7) Sign of the analog S associated with M19 (0 or 1)
P609(2) Spindle counting direction (0 or 1)
P612(8) Type of spindle home marker pulse (0 = -, 1 = +)
P719 Minimum spindle analog voltage (0...255)
P719=0 ==> 2,5 mV
P719=1 ==> 2,5 mV
P719=10 ==> 25.0 mV (10 x 2.5)
P719=255 ==> 637.5 mV (255 x 2.5)
P717
The CNC internally applies a x4 multiplying factor to the pulses coming from the encoder.
Thus, with a 1000 line encoder and P717= 100, the in-position zone will be: (360°/4000)x100= ±9°
P718 Proportional spindle gain K (0...255)
It sets the analog voltage corresponding to a following error of 1 spindle encoder pulse.
Analog (mV.) = P718 x Following error (pulses) x 2.5 mV / 64
P751, P747, P748, P749 Duration of the spindle acc/dec ramp in ranges 1, 2, 3, 4 (0...255) Value 1=20 ms
P746 Feed-forward gain in rigid tapping (0...255)
P750 Z axis proportional gain K1 in rigid tapping (0...255)
P625(1) The tap entry is synchronized with the spindle home marker pulse
Feedback inputs:
P630(4) = 0 Connector A5 is used for spindle feedback and for the Z axis handwheel.
Both feedback devices must be switched externally.
P630(4) = 1 Connector A5 is only used for spindle feedback.
Connector A6 is used for the X axis handwheel.
Connector A4 is used for Y and Z axes handwheels.
PLC output O46 indicates which axis moves when turning the handwheel connected to A4.
"O46=0" for the Y axis and "O46=1" for the Z axis.
ISO Programming
It is programmed by means of function G33 (threading) indicating axis feedrate and spindle speed.
Examples: G33 Z -10 F1000 S1000 M3 F1000 S1000 M3
G33 Z-10
Functions G00, G01, G02 and G03 cancel function G33.
3. CURRENT CNC SOFTWARE VERSION
From this version on, when accessing the EPROM checksum screen [Auxiliary Modes] [Special Modes] [8]
The CNC will show the checksum of each EPROM and the current CNC software version. For example: Version 3.1
4. SCREEN SAVER
When machine parameter “P626(7)=1” the screen saver function acts as follows:
After 5 minutes without pressing any key or the CNC not receiving any new data for refreshing (updating) the screen, it goes blank. Video is restored when pressing any key or when the CNC receives data to update the screen.
- 8 -
5. SEMIAUTOMATIC LINEAR MILLING
To access this mode, select the linear milling mode and press to get into semiautomatic mode.
This operation cannot be stored as in a part-program.
The path angle (
α
) and length (L) must be defined.
Jog the axes with the handwheel up to the starting point and press the corresponding JOG key (just press it once, it does not have to be held down).
The axes will travel the indicated distance "L" in the indicated direction and at an angle " " or until the key is pressed.
6. SEMIAUTOMATIC ARC MILLING
To access this mode, select the arc milling mode and press to get into semiautomatic mode.
This operation cannot be stored in a part-program.
The rounding radius (R) must be defined. Its sign indicates the turning direction (R+ and R-)
Jog the machines with the handwheels to the desired starting point and press the corresponding JOG key (just press it once, it does not have to be held down). The machine will make a 90º arc in the indicated direction.
7. CROSS COMPENSATION
Besides compensating for measuring errors due to inaccurate leadscrews (leadscrew error), this CNC offers cross compensation in order to compensate for errors caused by one axis onto another. A typical case would be beam (ram) sag compensation.
To use cross compensation, one must define the axis to be compensated and the one inflicting the error onto the other one when moving.
Machine parameters related to cross compensation:
P623(1)
P620(5)
Cross compensation applied to the X axis (0=No, 1=Yes)
Cross compensation applied to the Y axis (0=No, 1=Yes)
P620(4) Cross compensation applied to the Z axis (0=No, 1=Yes)
P623(2), P623(3) Axis inflicting the error onto the other one.
X
Y
Z
Affected (compensated) axis
P623(1) P620(5) P620(4)
1
0
0
0
1
0
0
0
1
X
Y
Z
Moving ("guilty") axis
P623(3) P623(2)
0
1
1
1
0
1
Examples: Compensate Y for Z axis movementP620 ( * * * 1 0 * * *)
Compensate X for Y axis movementP620 ( * * * 0 0 * * *)
P623 ( * * * * * 0 0 0)
P623 ( * * * * * 1 0 1)
8. FUNCTION M80 WHEN "Z" AS A DRO AXIS
This feature is available when the Z axis is set to work as a DRO axis. "P617(4)=1".
Whenever the Z axis has to be moved, the CNC shows the text: "Act upon Z".
Also, from this version on, it executes the auxiliary function M80. With this function, it is possible to act upon the hydraulic or mechanical device that controls the Z axis.
- 9 -
9. MACHINE SAFETY REGULATION
This CNC offers the following features to comply with machine safety regulations.
Enabling of the CYCLE START key from the PLC
This feature is available when machine parameter "P630(5)=1"
PLC output O25 indicates whether the CYCLE START key is enabled (=1) or not (=0)
Axes movements controlled by Feed-Hold. (It was already available)
Feed-Hold input, pin 15 of connector I/O 1, must be normally high.
If while moving the axes, the Feed-Hold input is brought low, the CNC keeps the spindle turning and stops the axes with 0V or velocity command (analog signal) and keeping their enables ON.
When this signal is brought back up, the CNC will resume the movement of the axes.
Axes jogging feedrate limited by PLC.
This feature is available when machine parameter "P630(5)=1"
When activating PLC output O26, the CNC assumes the feedrate set by machine parameter "P814"
Handwheel managed by the PLC.
Machine parameter "P628(2)" indicates whether the axes movements with handwheels are affected by Feed-Hold (=1) or not (=0)
Machine parameter "P630(2)" indicates whether the multiplying factor indicated by the MFO switch position is applied (=0) or the one indicated by the PLC outputs O44 and O45 (=1) (already available)
O44
0
1
0
Spindle control from the PLC.
1
O45
0
0
1
1
According to switch setting
Same as x1 setting of the switch
Same as x10 setting of the switch
Same as x100 setting of the switch
This feature is available when "P630(5)=1"
Output O27 =1 "tells" the CNC to apply the spindle analog voltage set by the PLC. The value of this analog signal is set at register
R156 and sent to the CNC by mark M1956.
R156= 0000 1111 1111 1111 => + 10V.
R156= 0000 0111 1111 1111 => + 5V.
R156= 0000 0011 1111 1111 => + 2,5V.
R156= 0000 0000 0000 0000 => + 0V.
R156= 0001 1111 1111 1111 => -
R156= 0001 0111 1111 1111 => -
10V.
5V.
R156= 0001 0011 1111 1111 => 2,5V.
R156= 0001 0000 0000 0000 => 0V.
Also, PLC output O43, lets you control the rotation of the spindle. (Already available).
It must be normally low.
If it is brought up, the CNC stops the spindle.
When it is brought back up, the CNC restarts the spindle.
Information for the PLC on the status of the machine reference (home) search
I88 Home search in progress.
I100 X axis home search done.
I101 Y axis home search done.
I102 Z axis home search done.
- 10 -
Additional CNC information for the PLC
R120 The lower half of this register indicates the last key pressed.
This value is maintained for 200 milliseconds unless another key is pressed before then.
This register can be canceled from the PLC after being processed.
R121 bit 1 Indicates that the Milling operation is selected (=1) bit 2 Indicates that the Positioning operation is selected (=1) bit 3 Indicates that the Pocket Milling operation is selected (=1) bit 4 Indicates that the Boss Milling operation is selected (=1) bit 5 Indicates that the Corner Roughing operation is selected (=1) bit 6 Indicates that the Surface Milling operation is selected (=1) bit 7 Indicates that one of the machining operations (Center punching, Drilling, etc.) is selected (=1) bit 8 Indicates that the "Auxiliary Modes" option is selected (=1) bit 9 Indicates that the "Tool Calibration" option is selected (=1) bit 10 Indicates that the "Graphic Simulation" mode is selected (=1) bit 16 Indicates that the mode relevant to following cycle parameters: "finising pass, finishing feedrate, finishing tool and safety distances on X and Z" is selected (=1)
- 11 -
Version 3.3 (March 1998)
1. MODULAR CNC
The modular 800M CNC consists of the Central Unit module (CPU), the Monitor and the keyboard.
Central Unit.
It is usually located in the electrical cabinet and is mounted by means the holes it has for this purpose on its support lid. Dimensions in mm.
When installing it, observe enough clearance to swing the
Central Unit open for future access to its interior.
To swing the central unit open, undo the two knurled nuts at the top and swing it open while holding its body.
Monitor.
It may be mounted anywhere on the machine, preferably at operator's eye level.
9" Amber and 10" Color Monitor
1.Contrast
2.Brightness
3.Two 3.15A/250V fast fuses (F), one per mains line, to protect the mains input.
4.Power switch.
5.220 Vac mains and ground connection.
6.General ground connection terminal. Metric 6mm
7.15-pin SUB-D type male connector for connecting it with the Central Unit.
- 12 -
14" Color Monitor
X2 15-pin SUB-D type male connector for connecting it with the Central Unit.
1.General ground connection terminal. Metric 6mm
2.220 Vac mains and ground connection.
Monitor enclosures.
9" & 10 Monitor
14" Monitor
A, B, C, D
25 mm
100 mm
E
150 mm
50 mm
Keyboard.
It may be mounted anywhere on the machine.
Rear panel
1.25-pin SUB-D type female connector for connecting it with the Central Unit.
2.Buzzer volume adjusting potentiometer.
3.Buzzer.
- 13 -
Connector for connecting the Central Unit with the Monitor.
FAGOR AUTOMATION provides the cable required for this connection. It comes with a 15-pin SUB-D type male connector at one end and a 15-pin SUB-D type female connector at the other.
Both connectors have a latching system UNC4.40 by means of two screws.
The supplied cable has 6 twisted pairs of 0.34 mm² wires (6 x 2 x 0.34mm²), with overall shield and acrylic cover. It has a specific impedance of 120 Ohms. Its maximum length must be 25 meters (82 feet).
The cable shield is soldered to the metal hoods (housings) of both connectors and connected to pin 1 at both the Central Unit and Monitor/keyboard connectors.
PIN SIGNAL
10
11
12
13
7
8
9
5
6
3
4
1
2
14
15
Metal hood
GND
H
R
G
V
I
B
Not connected
Not connected
I
R
H
V
G
B
Shield
Shield
Heat shrink
Outside shield soldered to metal hood
Metal hood
Connector for connecting the Central Unit with the keyboard.
FAGOR AUTOMATION provides the cable required for this connection. It comes with a 25-pin SUB-D type male connector at each end.
Both connectors have a latching system UNC4.40 by means of two screws.
The supplied cable has 25 wires of 0.14 mm² (25 x 0.14mm²), with overall shield and acrylic cover. Its maximum length must be 25 meters (82 feet).
The cable shield is soldered to the metal hoods (housings) of both connectors and connected to pin 1 at both the Central Unit and Monitor/keyboard connectors.
PIN SIGNAL
14
15
16
17
9
10
11
12
13
4
5
6
7
8
1
2
3
18
19
20
21
22
23
24
25
Metal hood
C8
C10
C12
C14
C7
D1
D3
D5
D7
GND
C9
C11
C13
C15
C1
C3
C5
C0
C2
C4
C6
D0
D2
D4
D6
Shield
Shield
Heat shrink
Outside shield soldered to metal hood
Metal hood
- 14 -
2. PROGRAMMING IN ISO CODE. NEW FUNCTION F34
P1 = F34 Parameter P1 takes the value of the tool causing the call to the subroutine associated with the tools.
Do not mistake it with function F24 which returns the number of the tool currently being used.
3. PROGRAMMING IN ISO CODE. RIGID TAPPING
When carrying out rigid tapping in 800M mode, the CNC acts as follows:
1.Internally generates function M81 (switching feedback)
2.Carries out rigid tapping.
3.Internally generates function M82 (switching back to previous feedback)
Therefore, when programming rigid tapping in ISO code, function M81 must be programmed in block preceding rigid tapping and function M82 in the one following it.
4. 1000 LINE ENCODER AS A 1250 LINE ENCODER
With this feature, the CNC can use a 1000 line encoder as it were a 1250 line encoder.
P630(6) X axis 1000 line encoder as 1250 line encoder (0=No, 1=Yes)
P630(7) Y axis 1000 line encoder as 1250 line encoder (0=No, 1=Yes)
P630(8) Z axis 1000 line encoder as 1250 line encoder (0=No, 1=Yes)
A typical case: When using a motor with 1000 line encoder on a 5 mm pitch ballscrew.
The necessary calculations for setting axis resolution will be made using the selected line count (1000 or 1250 pulses).
5. PLCI. INPUT I104
When the Feedrate Override Switch on the operator panel is set on one of the handwheel positions (x1, x10, x100), input I104 is set to "1".
6. PLCI. R120 AND THE
From this version on, even when the
KEY
is disabled by parameter P618(1), PLCI register R120 contains its code when it is pressed.
Version 3.04 (March 2002)
1. TOOL COMPENSATION CANCELATION
Sometimes, it may be interesting to move the tool to a set position without applying its length compensation.
In these cases, program "T.0" and the CNC will acts as follows:
•
It does not change the tool (it does not call its associated subroutine).
•
It cancels its associated offset (assuming a zero length and radius compensation).
The "T.xx" instruction may be programmed at any time, even inside the program P99996 or in its associated subroutine. The CNC assumes the new "xx" offset. When programming "T.0", it assumes a zero tool length and radius compensation.
2. FEEDBACK SIGNAL DIVIDING FACTOR
Parameters P631(8), P631(7), P631(6), P631(5) and P631(4) are used with parameters P604(8), P604(7), P604(6), P604(5) and P616(8) that indicate the multiplying factor for the feedback signals of the X, Y, Z, W, V axes respectively.
X axis
P604(8)
Y axis
P604(7)
Z axis
P604(6)
W axis
P604(5)
V axis
P616(8)
P631(8) P631(7) P631(6) P631(5) P631(4)
They indicate whether the feedback signals are divided (=1) or not (=0).
P631(8)=0, P631(7)=0, P631(6)=0, P631(5)=0 and P631(4)=0 They are not divided
P631(8)=1, P631(7)=1, P631(6)=1, P631(5)=1 and P631(4)=1 They are divided by 2.
Example: To obtain a 0.01 mm resolution using a square-wave encoder mounted on the X axis whose pitch is 5 mm/turn.
Nr of pulses = Leadscrew pitch / (Multiplying factor x Resolution)
If P604(8)=0 & P631(8)=0
If P604(8)=1 & P631(8)=0
If P604(8)=0 & P631(8)=1
If P604(8)=1 & P631(8)=1 x4 multiplying factor x2 multiplying factor x2 multiplying factor x1 multiplying factor
Nr of pulses = 125
Nr of pulses = 250
Nr of pulses = 250
Nr of pulses = 500
- 15 -
3. FEEDBACK FACTOR.
The resolution of the axis is determined by the leadscrew pitch and the number of pulses of the encoder mounted on the motor.
Sometimes, the resolution resulting from the available leadscrew / encoder combination does not match any of the resolution values allowed for the machine parameters (1, 2, 5, 10 microns or ten-thousandths of an inch).
Example: With a 6 mm/turn leadscrew pitch and a 2500 line encoder, the resulting resolution values are:
Resolution = Leadscrew pitch / ( Nr of encoder pulses x multiplying factor).
With x1 multiplying factor2.4 micron resolution
With x2 multiplying factor1.2 micron resolution
With a x4 multiplying factor 0.6 micron resolution
A new axis machine parameter is now available to solve these cases and it is referred to as Feedback Factor in order to adapt the resulting resolution to the existing setup.
P819 Feedback factor for the X axis P820 Feedback factor for the Y axis P821 Feedback factor for the Z axis
Values between 0 and 65534, a "0" value means that this feature is not being used.
Use the following formula to calculate the "Feedback factor":
Feedback Factor = (Gear ratio x Leadscrew Pitch / Encoder pulses) x 8.192
Examples: Gear ratio
Leadscrew Pitch
Encoder
Feedback factor
1
4000
2500
13,107.2
1
6000
2500
19,660.8
2
6000
2500
39,321.6
1
8000
2500
26,214.4
(microns)
(pulses/turn)
The machine parameters only admit integers, but the Feedback Factor sometimes may have decimals. In those cases, set the machine parameter to the integer part of that value and use the leadscrew error compensation table to make up for the decimal part.
The values for this table are calculated using the following formula:
Leadscrew position = Leadscrew error (microns) x Integer portion of feedback factor /Decimal portion of feedback factor
In this case: Gear ratio = 1 Pitch = 6000 Encoder = 2500
Feedback factor = 19,660.8
Machine parameter = 19660
For leadscrew error of 20 microns Leadscrew position = 20 x 19,660 / 0.8 = 491,520
The following table is obtained by using this calculation.
Leadscrew position Amount of error at that position
P0 = -1966,000
P2 = -1474,500
P4 = -983,000
P6 = -491,500
P1 =
P3 =
P5 =
P7 =
-0.080
-0.060
-0.040
-0.020
P8 = 0
P10 = 491,500
P12 = 983,000
P14 = 1472,500
P16 = 1966,000
P9 = 0
P11 = 0.020
P13 = 0.040
P15 = 0.060
P17 = 0.080
Headquarters (SPAIN): Fagor Automation S. Coop.
Bº San Andrés s/n, Apdo. 144
E-20500 Arrasate - Mondragón
Tel: +34-943-719200/039800
Fax: +34- 943-791712
+34-943-771118 (Service Dept.) www.fagorautomation.com
E-mail: [email protected]
FAGOR 800M CNC
OPERATING MANUAL
Ref. 9701 (in)
ABOUT THE INFORMATION IN THIS MANUAL
This manual is addressed to the machine operator.
It includes the necessary information for new users as well as advanced subjects for those who are already familiar with the 800M CNC product.
It may not be necessary to read this whole manual. Consult the list of "New Features and
Modifications".
This manual explains all the functions of the 800M CNC family. Consult the Comparison
Table for the models in order to find the specific ones offered by your CNC.
Chapters 1, 2, 3, 4 and 5 show how to operate with this CNC.
Chapter 6 "Working with Part-programs" shows how to create parts consisting of Automatic
Operations. The Part-programs are stored in the internal CNC memory and may be sent out to a peripheral device or PC.
There is also an appendix on error codes which indicates some of the probable reasons which could cause each one of them.
Notes: The information described in this manual may be subject to variations due to technical modifications.
FAGOR AUTOMATION, S.Coop. reserves the right to modify the contents of the manual without prior notice.
INDEX
Section Page
Section Page
Chapter 4 AUTOMATIC OPERATIONS
Section Page
Chapter 5 MACHINING OPERATIONS
Chapter 6 WORKING WITH PART-PROGRAMS
Execution of an operation previously stored in a part-program .................................... 7
COMPARISON TABLE
FOR FAGOR 800M
CNC MODELS
AVAILABLE 800M CNC MODELS
X, Y axes control
Z axis as DRO
Controlled Z axis
Spindle
Tools
Tool Radius Compensation
Tool Length Compensation
Electronic Handwheels
RS 232C Communications
Integrated PLC (PLCI)
ISO-coded program editing
(P99996)
Execution of ISO-coded program (P99996)
Graphics
800-MG 800-MGI l l l l l l l l l l
99 l l
3 l l l l
99 l l
3 l l l
NEW FEATURES
AND
MODIFICATIONS
Date:
FEATURE them to "0".
July 1995
Clear all arithmetic parameter contents setting
ISO Programming.
Editing of program P99996 at the CNC.
When interrupting execution, the keys for the spindle, the coolant and for O1, O2, O3 and
TOOL are enabled.
Subroutine associated to the execution of a tool
(only when executing program P99996)
ISO codes of the 800T CNC
Software version: 2.1 and newer
AFFECTED MANUAL AND SECTION
Installation Manual
Operating Manual
Programming Manual
Section 3.9
Section 3.8&6.9
Installation Manual
Operating Manual
Installation Manual
Operating Manual
Operating Manual
Installation Manual
Programming Manual
Programming Manual
Section 3.10
Section 3.9
Section 3.5.1
Section 2.5.1
Section 6.5
Section 4.3
Chapter 9.
Date:
FEATURE
November 1995
Subroutines to be executed before and after the "T" function.
"M" functions associated with automatic operations.
"M" functions associated with machining operations.
Software version: 2.2 and newer
AFFECTED MANUAL AND SECTION
Installation Manual
Programming Manual
Operating Manual
Section 4.3
Chapter 9
Section 4.1.2
Operating Manual Section 5.1.1
INTRODUCTION
Introduction - 1
SAFETY CONDITIONS
Read the following safety measures in order to prevent damage to personnel, to this product and to those products connected to it.
This unit must only be repaired by personnel authorized by Fagor Automation.
Fagor Automation shall not be held responsible for any physical or material damage derived from the violation of these basic safety regulations.
Precautions against personal damage
Before powering the unit up, make sure that it is connected to ground
In order to avoid electrical discharges, make sure that all the grounding connections are properly made.
Do not work in humid environments
In order to avoid electrical discharges, always work under 90% of relative humidity
(non-condensing) and 45º C (113º F).
Do not work in explosive environments
In order to avoid risks, damage, do no work in explosive environments.
Precautions against product damage
Working environment
This unit is ready to be used in Industrial Environments complying with the directives and regulations effective in the European Community
Fagor Automation shall not be held responsible for any damage suffered or caused when installed in other environments (residential or homes).
Install the unit in the right place
It is recommended, whenever possible, to instal the CNC away from coolants, chemical product, blows, etc. that could damage it.
This unit complies with the European directives on electromagnetic compatibility.
Nevertheless, it is recommended to keep it away from sources of electromagnetic disturbance such as.
- Powerful loads connected to the same AC power line as this equipment.
- Nearby portable transmitters (Radio-telephones, Ham radio transmitters).
- Nearby radio / TC transmitters.
- Nearby arc welding machines
- Nearby High Voltage power lines
- Etc.
Ambient conditions
The working temperature must be between +5° C and +45° C (41ºF and 113º F)
The storage temperature must be between -25° C and 70° C. (-13º F and 158º F)
Introduction - 3
Protections of the unit itself
It carries two fast fuses of 3.15 Amp./ 250V. to protect the mains AC input
All the digital inputs and outputs are protected by an external fast fuse (F) of 3.15 Amp./
250V. against a voltage overload (greater than 33Vdc) and against reverse connection of the power supply.
Precautions during repair
Do not manipulate the inside of the unit
Only personnel authorized by Fagor Automation may manipulate the inside of this unit.
Do not manipulate the connectors with the unit connected to AC power.
Before manipulating the connectors (inputs/outputs, feedback, etc.) make sure that the unit is not connected to AC power.
Safety symbols
Symbols which may appear on the manual
WARNING. symbol
It has an associated text indicating those actions or operations may hurt people or damage products.
Symbols that may be carried on the product
WARNING. symbol
It has an associated text indicating those actions or operations may hurt people or damage products.
"Electrical Shock" symbol
It indicates that point may be under electrical voltage
"Ground Protection" symbol
It indicates that point must be connected to the main ground point of the machine as protection for people and units.
Introduction - 4
MATERIAL RETURNING TERMS
When returning the CNC, pack it in its original package and with its original packaging material. If not available, pack it as follows:
1.- Get a cardboard box whose three inside dimensions are at least 15 cm (6 inches) larger than those of the unit. The cardboard being used to make the box must have a resistance of 170 Kg (375 lb.).
2.- When sending it to a Fagor Automation office for repair, attach a label indicating the owner of the unit, person to contact, type of unit, serial number, symptom and a brief description of the problem.
3.- Wrap the unit in a polyethylene roll or similar material to protect it.
When sending the monitor, especially protect the CRT glass.
4.- Pad the unit inside the cardboard box with poly-utherane foam on all sides.
5.- Seal the cardboard box with packing tape or industrial staples.
Introduction - 5
FAGOR DOCUMENTATION
FOR THE 800M CNC
800M CNC OEM Manual Is directed to the machine builder or person in charge of installing and starting up the CNC.
It has the Installation manual inside. Sometimes, it may contain an additional manual describing New Software Features recently implemented.
800M CNC USER Manual Is directed to the end user or CNC operator.
It contains 2 manuals:
Operating Manual describing how to operate the CNC.
Programming Manual describing how to program the CNC.
Sometimes, it may contain an additional manual describing New Software
Features recently implemented.
DNC 25/30 Software Manual Is directed to people using the optional DNC communications software.
DNC 25/30 Protocol Manual Is directed to people wishing to design their own DNC communications software to communicate with the 800 without using the DNC25/30 software..
PLCI Manual To be used when the CNC has an integrated PLC.
DNC-PLC Manual
Is directed to the machine builder or person in charge of installing and starting up the PLCI.
Is directed to people using the optional communications software: DNC-PLC.
FLOPPY DISK Manual Is directed to people using the Fagor Floppy Disk Unit and it shows how to use it.
Introduction - 6
MANUAL CONTENTS
The operation manual consists of the following sections:
Index
Comparative Table for Fagor 800M CNC models
New Features and modifications
Introduction Safety Conditions
Material returning conditions
Fagor documents for the 800M CNC
Manual Contents
Chapter 1 Concepts
Indicates the layout of the keyboard, operator panel and information on the monitor.
Describes the display units and how to modify them
Indicates the reference systems to be set.
How to reference the machine and how to preset coordinates.
How to operate with absolute and incremental coordinates
Chapter 2 Basic operations
Indicates how to select the axis feedrate.
How to jog the machine with jog keys or with the electronic handwheel.
How to select the starting point (BEGIN) and the end point (END).
How to position the tool at the BEGIN or END point.
Spindle control. Speed selection, range change and turning direction.
How to activate and deactivate external devices.
Chapter 3 Auxiliary functions:
Indicates how to select working units (mm/inches).
How to set the tool table.
How to calibrate and inspect tools.
How to operate with peripherals.
How to lock and unlock the program memory.
How to edit, execute and simulate program 99996.
Chapter 4 Automatic operations.
Indicates how to select and program each automatic operation.
Operating modes: "Semi-automatic and automatic"
How to select the machining conditions of the automatic operations.
How to execute and simulate an automatic operation.
Chapter 5 Machining operations.
Indicates how to select and program each machining operation.
How to associate a machining operation with an automatic operation.
How to associate auxiliary "M" functions with the machining operation.
Chapter 6 Working with parts.
Indicates how to access the part-program directory.
How to select a part-program, edit it, simulate it and execute it.
How to execute an operation previously stored in a part-program.
How to modify a part-program.
How to delete a part-program.
How to operate with peripherals.
How to lock and unlock the part-program memory.
Error codes.
Introduction - 7
1.
CONCEPTS
After powering the 800M CNC, the screen shows the CNC model name and the message:
*** GENERAL TEST *** Passed
Press any key to access the CNC standard operating mode.
If the GENERAL TEST was not successful, the CNC will display the detected errors which must be corrected before operating with the machine.
1.1 CRT DESCRIPTION
The CRT of this model is divided into the following areas or display windows:
1.- This window indicates the selected operating mode: DRO, Linear Milling, Inside
Pocket, etc.
It also shows the CNC status during the execution of the automatic operations (in execution, interrupted or in position).
Chapter: 1
CONCEPTS
Section:
CRT DESCRIPTION
Page
1
2.- Main window.
This window shows the current tool position (X, Y and Z coordinates) and the number of the tool currently selected.
When an automatic operation is selected, this window shows the position of the axes on a single line. The rest of the window is used to show a graphic representation of the selected automatic operation.
3.- This window shows the following information:
* The axis feedrate (F) currently selected and the override percentage (%) being applied at the time.
* The currently selected (active) spindle speed (S) and the override percentage (%) being applied at the time.
* The currently selected spindle turning direction
* The currently selected tool (T).
4.- This area shows the coordinates of the BEGIN point (BEG) and END point.
When an automatic operation is selected, this window shows the definition parameters of that operation.
5.- Editing and CNC message display window.
Page
2
Chapter: 1
CONCEPTS
Section:
CRT DESCRIPTION
1.2 KEYBOARD DESCRIPTION
With this keyboard, it is possible to communicate with the CNC and it is divided into the following areas:
1.- Function keys.
2.- Operator Panel.
3.- Area for functions and automatic operations.
4.- Main area.
Chapter: 1
CONCEPTS
Section:
KEYBOARD DESCRIPTION
Page
3
1.2.1 MAIN AREA
It consists of the following keys:
Numeric keyboard. with the following keys: . , -, 0, 1, 2, ,3 ,4 ,5 ,6 ,7 ,8 ,9 to enter integer and decimal values with or without sign.
To assign values to the machine parameters.
When pressing the keystroke sequence: the normal display back, just press any key.
the CRT goes blank. To get
If while the screen is blank, an error occurs at the CNC, the screen will come back on.
After pressing this key, it is possible to set the X axis coordinate value. Once this value has been keyed in, press [ENTER] to validate it.
After pressing this key, it is possible to set the Y axis coordinate value. Once this value has been keyed in, press [ENTER] to validate it.
After pressing this key, it is possible to set the Z axis coordinate value. Once this value has been keyed in, press [ENTER] to validate it.
After pressing this key, it is possible to set the axis feedrate value. Once this value has been keyed in, press to validate it.
After pressing this key, it is possible to set the spindle speed value. Once this value has been keyed in, press [ENTER] to validate it.
After pressing this key, it is possible to define the new tool to be selected. Once this is done, one may:
* Press for the CNC to select the new tool or
* Press [ENTER] for the CNC to store this value without selecting a new tool.
This option is useful when editing operations that will be stored later on.
After pressing this key, it is possible to select the number of the part-program to be either edited or executed. Once this is done, press [ENTER] to validate the choice.
It is used to validate the CNC commands generated in the editing window.
Used to recover previously entered data from the part-program memory or CNC tables, in order to check it or modify it.
Before pressing this key, select the operation or value to be analyzed, by means of the cursor and up and down arrow keys.
It allows access to the data entry mode for any automatic operation.
To quit this mode, press this key again.
To delete the last character entered in the editing window.
Page
4
Chapter: 1
CONCEPTS
Section:
KEYBOARD DESCRIPTION
1.2.2 AREA FOR FUNCTIONS AND AUTOMATIC OPERATIONS
It consists of the following keys:
To select the coordinate of the corresponding BEGIN point (BEG) to either modify it later or command the machine to move to that point.
To select the coordinate of the corresponding END point to either modify it later or command the machine to move to that point.
To access the incremental mode (INC).
When the incremental mode is selected, the right-hand side of the main window shows the text "INC".
To return to standard mode, press this key again.
To select the operating mode for the execution of the automatic operation.
Continuous mode. The selected operation is executed from beginning to end without interruptions.
Single mode. The selected operation is executed one pass at a time, being necessary to press before each pass.
Whenever this single mode is selected, the right hand side of the main window shows the symbol
To associate a machining operation to the selected automatic operation.
To select the automatic operation: "Point to Point Positioning"
To select the automatic operation: "Positioning in a straight line"
To select the automatic operation: "Positioning in an arc pattern" (Bolt-hole)
To select the automatic operation: "Positioning in a Rectangular pattern"
To select the automatic operation: "Positioning in a Grid pattern"
To select the automatic operation: "Linear Milling"
To select the automatic operation: "Circular Milling"
To select the automatic operation: "Profiling"
To select the automatic operation: "Inside Pocket"
To select the automatic operation: "Outside Pocket (Boss)"
To select the automatic operation: "Corner Roughing"
To select the automatic operation: "Surface Milling"
When an automatic operation or a machining operation has been selected, the CNC will show the next available option every time this key is pressed.
Chapter: 1
CONCEPTS
Section:
KEYBOARD DESCRIPTION
Page
5
1.2.3 FUNCTION KEYS
They the following:
To access the menu for auxiliary functions offered by this CNC.
To access the simulation mode for operations and programs.
To access the "Calculator" mode. This option is not available in the current version.
To select the previous and next options when required by the displayed menu and to perform the machine reference (home) search.
To move from one data field to another in the data entry mode for automatic and machining operations.
Also, to select the previous and next data in BEG and END functions.
To turn the coolant on and off.
To activate and deactivate outputs: O1, O2 and O3.
To reset the CNC so it assumes the default values established by machine parameters. This key must also be pressed whenever the settings of the machine parameters have been changed so the new ones are assumed by the CNC.
While executing an automatic operation, it is necessary to stop it first. Besides, the
CNC will ask for confirmation of the command being necessary to press this key again. To cancel the resetting operation, press
If this reset key is pressed while one of the automatic operations is selected, the
CNC will quit that mode and return to the DRO display mode.
Page
6
Chapter: 1
CONCEPTS
Section:
KEYBOARD DESCRIPTION
1.2.4 OPERATOR PANEL
Depending on their function, this panel is divided into the following areas:
1.- Keyboard to jog the axes..
2.- Selector switch consisting of the following elements::
To select the multiplying factor applied by the CNC to the pulses from the electronic handwheel (1, 10, 100).
JOG To select the distance the axis will move (1, 10, 100, 1000 microns or tenthousandths of an inch) when pressing the corresponding key.
FEED To change the programmed feedrate between 0% and 120%.
3.- Keyboard to control the spindle. It can be started in the desired direction stopped or change its turning speed between 50% and 120% of the programmed speed with an incremental step of 5%.
4.- Keyboard for [START] and [STOP] of the programmed movements, automatic operations and part programs.
Chapter: 1
CONCEPTS
Section:
KEYBOARD DESCRIPTION
Page
7
1.3 DISPLAY UNITS (mm/inches)
The main window of this CNC shows at all times the X, Y and Z coordinates of the tool position.
With this CNC it is possible to display the position of the axes in either mm or inches.
To change the type of display units, press [AUX] and select the "MM/INCH" option.
Every time this option is selected, the CNC will toggle the display units from mm to inches and vice versa showing the axis position in the selected units.
To exit the operating mode for auxiliary functions and return to the standard display mode, press [AUX] or [END].
Page
8
Chapter: 1
CONCEPTS
Section:
DISPLAY UNITS
1.4 REFERENCE SYSTEMS
The machine where this CNC is installed needs to have the Machine Reference Zero
(home) for each axis defined. This point is set by the manufacturer as the origin of the coordinate system (Part Zero) of the machine.
It is also possible to establish another origin point for programming the part dimensions,
Part Zero. This new origin point is chosen freely by the operator and the position values shown by the CNC are referred to this point.
Bear in mind that to select the Part Zero, the CNC must be working in absolute coordinates.
If in the incremental mode, message "INC" on the right-hand side of the main window, press the key.
The Part Zero stays selected even when the CNC is off and it will be lost when a new Part
Zero is selected or when the Machine Reference Zero (home) is searched.
1.4.1 HOME SEARCH
The Machine Reference Zero search is done one axis at a time by following these steps:
* Press the key corresponding to the axis to be homed [X], [Y], [Z] and then the up arrow key.
* The editing window will request confirmation of the command. Press the k e y for the CNC to perform the home search on that axis.
If the home search is not desired, press any other key. To cancel the home search once in progress, press [CLEAR]
When doing a home search, the CNC initializes the displays of the axis and it cancels the
Part Zero that was selected.
Chapter: 1
CONCEPTS
Section:
REFERENCE SYSTEMS
Page
9
1.4.2 ZERO PRESET
It is possible to preset the desired Part Zero in order to use the coordinates relative to the blue-prints of the work-piece without having to modify the various points of the part.
To preset the Part Zero, follow these steps:
* The CNC must be working in absolute coordinates. If it is in the incremental mode,
"INC" message on the right-hand side of the main window, press the key.
* Press the key corresponding to the axis to be preset [X], [Y], [Z] and then [ENTER].
The CNC will request confirmation of the command, press [ENTER] again.
* Repeat this operation for the other axes.
Every time this operation is done, the CNC assumes that point as the new coordinate origin.
1.4.3 COORDINATE PRESET
With this feature it is possible to preset the desired coordinate (position) values in order to use the coordinates relative to the blue-prints of the work-piece without having to modify the various points of the part.
Also, this type of preset may be used when it is more convenient to work from coordinate value towards zero instead of doing it from one coordinate value to the next, as usual.
To preset a coordinate value, follow these steps:
* Press the key corresponding to the axis to be preset [X] [Y] [Z].
* Key in the desired position value for that point.
* Press [ENTER]. The CNC will request confirmation of the command, press [ENTER] again.
The CNC assumes that preset value as the new position value (coordinate) for that axis.
* Repeat this operation for the other axes.
Every time a preset is done, the CNC assumes a new Part Zero which will be located at a distance from the preset point equal to the preset value.
Page
10
Chapter: 1
CONCEPTS
Section:
REFERENCE SYSTEMS
1.5 OPERATION IN INCREMENTAL MODE
With this CNC it is possible to set a Floating Zero or Incremental Zero, besides the Part
Zero described earlier, in order to use coordinates relative to any point of the part.
In order to work in the incremental mode, it is necessary that the coordinate values displayed by the CNC be incremental, "INC" message on the right-hand side of the main window. If this message is not being displayed, press
Atention:
Every time the incremental mode is selected, the CNC takes as Floating Zero the Part Zero point currently active. Therefore, it will keep showing the same
X, Y, Z position values.
To set another Floating Zero, another coordinate or Par Zero must be preset. From that moment on, the coordinates shown by the CNC will be referred to the new Floating Zero established.
The CNC keeps the Part Zero preset when working in absolute mode and it will display the X, Y, Z position referred to it when switching back from incremental to absolute mode.
Chapter: 1
CONCEPTS
Section:
OPERATION IN
INCREMENTAL MODE
Page
11
2.
BASIC OPERATIONS
2.1 AXIS FEEDRATE SETTING
With this CNC it is possible to set the feedrate (F) for the axes as often as desired in order to move them at the proper speed each time.
Also, the Operator Panel has a multi-position switch which allows modifying the feedrate during those moves by applying the selected percentage (%) override to the feedrate selected in each case. This percentage amount is indicated by the Feedrate
Override Switch (FEED) and it has a range from 0% through 120% of the set feedrate.
Follow these steps to set the axis feedrate (F):
* Press [F]
* Key in the value via keyboard and press
When working in mm/min., this value must be between 0 & 65535.000mm/min.
When working in inches/min., this value must be between 0 and 25801.1811
inches/min.
The CNC assumes this value and it displays it on the screen. It also displays the percentage of the feedrate override currently selected by the FEED switch. For example:
F120 100%.
Atention:
When the CNC displays a value of "F0000", it applies the maximum feedrate set by the corresponding machine parameter for each axis.
Chapter: 2
BASIC OPERATIONS
Section:
FEEDRATE SETTING
Page
1
2.2 WORK TOOL SELECTION
The CNC must know at all times which tool is being used for machining. To achieve this, every time a new tool is selected, after it has been changed, press
[TOOL] followed by the selected tool and, then, press
The CNC assumes all the offset values corresponding to the new selected tool.
These offset values (tool length and radius) will be taken into account by the
CNC when performing any operation from this moment on.
If a new tool is to be selected when executing a cycle or preprogrammed part, the CNC acts as follows:
* It interrupts the execution.
* It executes the auxiliary function M05 to stop the spindle.
* It deactivates the coolant.
* Displays a message indicating the number corresponding to the new tool to be selected.
Once the tool change has been completed, press [ENTER]. The CNC will turn the coolant back on, the spindle will recover its turning direction and speed and the CNC will resume the execution of the part or cycle.
Page
2
Chapter: 2
BASIC OPERATIONS
Section:
TOOL SELECTION
2.3 AXES JOG
2.3.1 CONTINUOUS JOG
With this option it is possible to jog the axes of the machine one at a time.
Once the axis feedrate has been preset and the feedrate override (0% through 120%) has been selected at the operator panel switch (FEED), press the JOG key corresponding to the desired axis and its jogging direction.
Depending on the value assigned to machine parameter P12, this movement will be carried out as follows:
* If P12=Y, the axis will move while the selected JOG key is kept pressed.
* If P12=N, the axes will start moving when the JOG key is pressed and it will stop when either the key or the JOG key for another axis is pressed. In this latter case, the other axis will start moving.
If while an axis is being jogged, the override indicated by the table below:
% selected
% applied
0
0 key is pressed, the CNC will apply the %
2 4 10 20 30 40 50
102 104 110 120 130 140 150
60 70 80 90 100 110 120
160 170 180 190 200 200 200
This % override will be maintained as long as this key is kept pressed and it will recover the previous feedrate percentage (0% through 120%) when releasing this key.
2.3.2 INCREMENTAL JOG
With this option it is possible to jog the desired axis and in the desired direction a distance selected by the JOG positions of the FEED switch on the operator panel.
The feedrate used in these incremental moves is set by the machine manufacturer.
The positions available at this switch are 1, 10, 100, 1000 and 10000, which indicate the number of units to be moved. These units are those used in the display format.
Example:
Switch position
1
10
100
1000
10000
Incremental move
0.001 mm or 0.0001 inch
0.010 mm or 0.0010 inch
0.100 mm or 0.0100 inch
1.000 mm or 0.1000 inch
10.000 mm or 1.0000 inch
After selecting the desired switch position, every time the jog key is pressed, the axis will move the indicated amount and in the chosen direction.
Chapter: 2
BASIC OPERATIONS
Section:
AXES JOG
Page
3
2.3.3 AXES JOG VIA ELECTRONIC HANDWHEEL
With this option it is possible to jog the axes of the machine by means of an electronic handwheel.
To do this, first select any of the positions at the FEED switch of the Operator
Panel which correspond to the electronic handwheel.
The available positions are 1, 10 and 100 which indicate the multiplying factor to be applied to the pulses coming from the electronic handwheel.
This way, and after applying this factor, the desired distance units are obtained for axis jog. These units correspond to the display units being used.
Example: Handwheel resolution: 250 pulses per turn
Switch position Distance jogged per turn
1
10
100
0.250 mm or 0.0250 inch
2.500 mm or 0.2500 inch
25.000 mm or 2.5000 inches
Depending on the setting of machine parameter "P628(5)", the CNC behaves as follows at the rest of the positions of the Feedrate Override Switch of the operator panel.
P628(5)=0 The axes may be jogged with the handwheel as if the MFO switch were at the "x1" position.
P628(5)=1 The axes may not be jogged with the handwheel.
When attempting to move an axis faster than the feedrate value set by machine parameters "P110, P210 and P310", the CNC will limit it to those values ignoring the rest of the handwheel pulses thus preventing any following errors from being issued..
The machine has one electronic handwheel.
Once the desired switch position has been selected, press one of the JOG keys corresponding to the axis to be jogged. The selected axis will be highlighted on the screen.
When using a FAGOR handwheel with axis selector button, the axis can be selected as follows:
* Press the button located on the rear of the handwheel. The CNC will select the first axis and it will show it highlighted on the screen.
* If this button is pressed again, the CNC will select the next axis and so on in a rotary fashion (selecting the first one after the last one).
* If this button is maintained pressed for more than 2 seconds, the CNC will unselect the axis.
The machine will move the selected axis as the handwheel is being turned in one direction or the other depending on the turning direction of the handwheel.
The machine has two or three handwheels.
The machine will move each one of the axes as the corresponding handwheel is turned according to the selected switch position and turning direction.
Page
4
Chapter: 2
BASIC OPERATIONS
Section:
AXES JOG
2.4 BEGINNING (BEG) AND END POINT
With this CNC it is possible to set a beginning point (BEG) and an END point to facilitate the machining tasks.
These points may be re-defined as often as desired and may be used to set the ends of the part, the boundaries (limits) of a particular machining area, etc.
2.4.1 BEGIN AND END POINT SETTING
Press the [DATA] key or the one corresponding to the point to be set, [BEG] or
[END]. The CNC will highlight that value.
The X, Y and Z values of that point must be set one by one following these steps:
1. Press the key of the axis to be set [X], [Y] or [Z]. The CNC will highlight this field.
2. Assign the desired value to this field by following one of these two methods:
* By keying in the desired postion value for this field and pressing [ENTER] or...
* By moving the axes of the machine to the desired point by means of the mechanical or electronic handwheels or by using the JOG keys on the operator panel and then pressing [ENTER].
This option is not available for the Z axis.
The CNC only modifies the position value (coordinate) of the selected axis leaving the values of the other axes intact.
3. The CNC shows the next field as being selected.
To select another field, either press the key of the axis to be set [X], [Y] or [Z] or use the keys.
4. Repeat step 2 to set this new field.
5. Repeat steps 3 and 4 as many times as necessary.
6. To quit the selecting mode, press [CLEAR] or [DATA].
Chapter: 2
BASIC OPERATIONS
Section:
BEGIN and END
Page
5
2.4.2 POSITIONING AT "BEGIN" OR "END" POINTS
To move the tool up to the Begin or End point, do the following:
* Press [BEG] to move to the beginning point or [END] to move to the end point.
* Press
The CNC moves the Z axis first and then the X and Y together to position the tool at the selected point. These movements are carried out at the programmed feedrate.
When only one axis is to be moved, follow these steps:
* Press [BEG] to move to the beginning point or [END] to move to the end point.
* Press the corresponding axis key [X], [Y] or [Z].
* Press
The CNC will automatically move the tool to the selected point along that axis and at the programmed feedrate. The other axes will not move.
Also, the next field will appear selected in case another movement is to be made.
To select another field, one may press the corresponding axis key [X], [Y] or [Z] or use the keys.
Page
6
Chapter: 2
BASIC OPERATIONS
Section:
BEGIN and END
2.5 SPINDLE CONTROL
2.5.1 SPINDLE SPEED SETTING
To set the spindle speed, press [S] and after keying in the desired value, press
It is possible to set a value between S0 and S9999 rev/min. However, the maximum turning speed is set by the manufacturer as indicated in the instruction book of the machine. The CNC will apply this manufacturer-set value whenever a higher speed is selected by the operator.
Once the new speed is selected, the CNC will act as follows:
* When the spindle is already turning, the CNC will output the analog voltage corresponding to the new selected speed.
If the selected RPM correspond to another gear range, the CNC will generate a range change before outputting the new analog voltage.
* When the spindle is stopped, the CNC will store the selected value in order to provide its corresponding analog voltage when starting the spindle.
If the new selected RPM correspond to another gear range, the CNC will generate a range change.
The set spindle speed may be varied between 50% and 120% in incremental steps of
5% by means of the keys located on the operator panel.
2.5.2 SPINDLE SPEED RANGE CHANGE
With this CNC, the machine can have a gear box in order to adapt the speeds and torques of the spindle motor to the various machining requirements.
When the new selected spindle speed "S" involves a gear change, the CNC will manage the electrical cabinet to carry out this change without the intervention of the operator.
Chapter: 2
BASIC OPERATIONS
Section:
SPINDLE CONTROL
Page
7
2.5.3 CLOCKWISE SPINDLE ROTATION
To turn the spindle clockwise once the spindle speed has been selected, press
When the spindle is turning, a new speed may be selected or change the current speed by means of the following keys:
Every time this key is pressed, the CNC increases the spindle speed by 5%.
The maximum being 120% of the programmed speed.
It must be borne in mind that the maximum speed is limited by the value assigned to the range currently selected.
Every time this key is pressed, the CNC decreases the spindle speed by 5%.
The minimum being 50% of the programmed speed.
2.5.4 COUNTER-CLOCKWISE SPINDLE ROTATION
To turn the spindle counter-clockwise once the spindle speed has been selected, press
When the spindle is turning, a new speed may be selected or change the current speed by means of the following keys:
Every time this key is pressed, the CNC increases the spindle speed by 5%.
The maximum being 120% of the programmed speed.
It must be borne in mind that the maximum speed is limited by the value assigned to the range currently selected.
Every time this key is pressed, the CNC decreases the spindle speed by 5%.
The minimum being 50% of the programmed speed.
2.5.5 SPINDLE STOP
To stop the spindle rotation, press
The CNC stores the "S" speed which was selected before stopping and the spindle resumes this speed when pressing the or key.
Page
8
Chapter: 2
BASIC OPERATIONS
Section:
SPINDLE CONTROL
2.6 ACTIVATING/DEACTIVATING EXTERNAL DEVICES
With this CNC it is possible to activate and deactivate 4 external devices including the coolant. The other devices depend on the type of machine.
These devices may be activated or deactivated at any time unless indicated otherwise by the machine manufacturer.
To do this, the following keys are available:
Every time one of these keys is pressed, the status of the corresponding device will toggle (activated/deactivated).
Chapter: 2
BASIC OPERATIONS
Section:
EXTERNAL DEVICES
Page
9
3.
AUXILIARY FUNCTIONS
To access this option, press the [AUX] once the CNC is in DRO mode.
Then, the CNC will display a list of options. To select one of then, press the key for its corresponding number.
The operator may access all the shown options except the one referred to as
"AUXILIARY MODES". When selecting this option, the CNC requests a password or access code for entering the various tables and modes available to the manufacturer.
To quit any of these options and return to the standard display, press [END].
3.1 MILLIMETERS <—> INCHES
When selecting this option, the CNC changes the display units from mm to inches and vice versa showing the new X, Y and Z coordinates of the axes in the new selected units.
The axis feedrate (F) will also be shown in the new selected units.
It must be borne in mind that the values stored for BEGIN and END and the data for special operations have no units. Therefore, the values will remain the same when toggling from mm to inches or vice versa.
3.2 TOOL LENGTH COMPENSATION
When choosing this option, the CNC activates or cancels tool length compensation.
When not working with tool length compensation, the CNC displays the position value (coordinate) of the tool base.
When working with tool length compensation, the CNC displays either the tool tip position or that of the tool base depending on the setting of machine parameter P626(1).
The right-hand side of the main window shows the length compensation is active.
symbol whenever tool
Chapter: 3
AUXILIARY FUNCTIONS
Section: Page
1
3.3 TOOL TABLE
When selecting this option, the CNC shows the values assigned to each offset; that is, the dimensions of each tool being used to machine the parts.
Once the tool offset table is selected, the operator may move the cursor one line at a time by using the up and down arrow keys.
Each tool offset has several fields which define the dimensions of the tool. These fields are the following:
R Tool radius.
It is given in the currently active work units. Its maximum value being:
R 1,000.000 mm or R 39.3700 inches.
The CNC will take this "R" value into account when applying tool radius compensation.
L Tool length
It is given in the currently active work units. Its maximum value being:
L 1,000.000 mm or L 39.3700 inches.
The CNC will take this "L" value into account when applying tool length compensation.
I Tool radius wear.
It is given in the currently active work units. Its maximum values being:
I ±32.766 mm or I ±1.2900 inches.
The CNC will add this value to the nominal "R" to calculate the real radius (R+I).
K Tool length wear.
It is given in the currently active work units. Its maximum values being:
K ±32.766 mm or K ±1.2900 inches.
The CNC will add this value to the nominal "L" to calculate the real length (L+K).
Page
2
Chapter: 3
AUXILIARY FUNCTIONS
Section:
TOOL TABLE
3.3.1 MODIFICATION OF TOOL DIMENSIONS
To initialize a table by setting all the fields of each tool to "0", key in the following sequence: [F] [S] [P] [ENTER].
This CNC offers the option for "TOOL CALIBRATION" which is described next.
Once they have been calibrated, the CNC assigns to each tool offset the dimensions of the corresponding tool.
To modify the table values of a tool, ("R", "L", "I" and "K" values), select the corresponding offset at the CNC by keying the desired tool number and then pressing
[RECALL].
The editing area will show the current values assigned to that tool offset.
To change these values, move the cursor by means of the up and down arrow keys until it is placed over the current value. The new values must be keyed in over the current ones.
Once the new values have been keyed in, press [ENTER] so that they are stored in memory.
To quit this mode, move the cursor to the right until it is out of the edited area and then press [END].
Chapter: 3
AUXILIARY FUNCTIONS
Section:
TOOL TABLE
Page
3
3.4 TOOL CALIBRATION
With this option, it is possible to calibrate and load the tool dimensions onto the tool offset table of the CNC.
The CNC shows a graphic at a lower right-hand side of the monitor used as a user guide during tool calibration highlighting the data being requested at the time.
The procedure to calibrate a tool is as follows:
1.- The CNC requests the Z dimension of the part (contact point) being used to calibrate the tool.
Key in that value and press [ENTER].
2.- The CNC requests the number of the tool (T) to be calibrated.
Key in the tool number and press [ENTER].
3.- Jog the axes by means of the mechanical or electronic handwheels or by using the JOG keys of the operator panel until the tool touches the part along the Z axis.
Then press [ENTER]. The CNC will calibrate the tool in length and will update the corresponding tool offset.
The CNC will request a new tool to be calibrated. Repeat steps 2 and 3 as often as necessary.
Press [END] to quit this mode and return to the standard display mode.
Atention:
While calibrating a tool, it is possible to use, at any time, the electronic handwheels, the JOG keys and the spindle of the operator panel.
Page
4
Chapter: 3
AUXILIARY FUNCTIONS
Section:
TOOL CALIBRATION
3.5 EXECUTION / SIMULATION PROGRAM 99996
Program P99996 is a special user program in ISO code. It must be edited (written) on a PC and sent to the CNC via the Peripherals option.
When selecting the option: "Execution of program P99996", it is possible to either execute it or simulate by pressing
3.5.1
EXECUTION OF PROGRAM P99996
When selecting the option: "Execution of program P99996", the CNC displays the following information:
The top line shows the message "AUTOMATIC", the program number (P99996) and the number of the first block of the program or that of the block being in execution.
Then, the CRT shows the contents of the first program blocks. If the program is being executed, the first block of the list will be the one being executed at the time.
The position values along X, Y and Z indicate the programmed values (COMMAND), the current position (ACTUAL) and the distance remaining (TO GO) for the axes to reach the "command" position.
The bottom of the screen shows the machining conditions currently selected. The programmed feedrate F, the % F override, the programmed spindle speed S, the %S override, the programmed Tool as well as the active G and M functions.
. It always starts executing from the first To execute program P99996, press block.
To interrupt the program, press enabled:
. Once interrupted, the following keys are
To resume execution, press
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
Page
5
3.5.1.1
TOOL INSPECTION
With this option it is possible to interrupt the execution of program P99996 and inspect the tool to check its status and change it if necessary.
To do this, follow these steps: a) Press to interrupt the program.
b) Press [TOOL]
At this time, the CNC executes the miscellaneous function M05 to stop the spindle and it displays the following message on the screen:
JOG KEYS AVAILABLE
OUT c) Move the tool to the desired position by using the JOG keys.
Once the tool is "out of the way", the spindle may be started and stopped again by its corresponding keys at the Operator Panel.
d) Once the tool inspection or replacement is completed, press [END].
The CNC will execute an M03 or M04 function to start the spindle in the direction it was turning when the program was interrupted.
the screen will display the following message:
RETURN
AXES OUT OF POSITION
"Axes out of position" means that they are not at the position where the program was interrupted.
e) Jog the axes to the program interruption position by means the corresponding jog keys. The CNC will not allow to move them passed (overtravel) this position.
When the axes are in position, the screen will display: f) Press
RETURN
AXES OUT OF POSITION
NONE to resume the execution of program P99996.
Page
6
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
3.5.1.2
EXECUTION MODES
With this CNC, it is possible to execute program P99996 from beginning to end without interruptions or block by block by pressing
The top line of the screen shows the selected operating mode: "Automatic" or "Single
Block".
To switch modes, press again.
Once the desired execution mode has been selected, press program.
to run the
3.5.1.3 CNC RESET
This option is used to reset the CNC setting it to the initial conditions established by the machine parameters. When quitting this operating mode, the CNC displays the
DRO mode.
To reset the CNC, interrupt the program if running and simply press
The CNC will request confirmation of this function by blinking the message:
"RESET?".
To go ahead with reset, press again; but to cancel it, press
3.5.1.4 DISPLAYING PROGRAM BLOCKS
To display the previous or following blocks to those appearing on the screen, press:
Displays the previous blocks
Displays the following blocks
Atention:
Bear in mind that P99996 always starts executing from the first block of the program, regardless of the blocks currently displayed on the screen.
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
Page
7
3.5.1.5 DISPLAY MODES
There are 4 display modes which can be selected by means of the following keys:
[0] STANDARD
[1] ACTUAL POSITION
[2] FOLLOWING ERROR
[3] ARITHMETIC PARAMETER
STANDARD display mode
It is the mode described before. When accessing the "Execution of program P99996" option, the CNC selects this display mode.
ACTUAL POSITION display mode
FOLLOWING ERROR display mode
Page
8
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
ARITHMETIC PARAMETERS display mode
This mode shows a group of 8 arithmetic parameters. To view the previous and following ones, use these keys:
Displays the previous parameters
Displays the following ones
The value of each parameter may be expressed in one of the following formats:
P46 = -1724.9281
P47 = -.10842021 E-2
Decimal notation
Scientific notation
Where "E-2" means 10 -2 (1/100). Therefore, the two types of notation for the same parameter below have the same value:
P47= -0.001234
P48= 1234.5678
P47= -0.1234 E-2
P48= 1.2345678 E3
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
Page
9
3.5.2 SIMULATION OF PROGRAM P99996
With this CNC, it is possible to check program P99996 in dry-run before executing it.
To do this, press . The CNC will show a graphic representation.
The lower left-hand side of the screen shows the plane being represented (XY, YZ or YZ) or three-dimensional XYZ.
To have any other plane displayed, press its corresponding key:
[0] XY Plane
[1] XZ Plane
[2] YZ Plane
[3] Three-dimensional XYZ
This CNC can show up the graphics on up to 3 planes. Therefore, it will only show the selected ones. To select other planes, proceed as follows:
Press and the CNC will ask whether each one of the possible planes is to be selected or not.
To select the plane press [Y] and, if not, press [ENTER].
Once the planes have been defined, the display area must be set by indicating the XYZ coordinates of the center of the screen and the width of the display area. After keying in each value, press [ENTER].
To check the part, press . This will start the corresponding graphic simulation.
While simulating, it is possible to access any other plane (keys: 0, 1, 2 and 3) but it is not possible to set them. To set other planes or modify the display area, it is necessary to interrupt the simulation of the program by pressing .
Press [CLEAR] to clear the screen, and [END] to quit the simulation mode.
Page
10
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
3.5.2.1 ZOOM FUNCTION
With the ZOOM function, it is possible to enlarge or reduce the whole graphic representation or part of it. To do this, the simulation of the program must be either interrupted or finished.
Once the drawing plane to be enlarged or reduced has been selected, press [Z]. The screen will show a rectangle over the original drawing. This rectangle is the zoom window which represents the new display area for the part to be enlarged or reduced.
To change the dimensions of the rectangle, use these keys:
Reduces the size of the rectangle (zoom in)
Use
Increases the size of the rectangle (zoom out) to move the zoom window around.
To set the area selected with the zoom window as the new display area, press [ENTER]
To see the selected area enlarged or reduced while keeping the previous display area values, press
The area contained in the zoom window will now fill out the whole screen.
To return to the previous display area (prior to the zoom), press [END].
To use the zoom again, just press [Z] and proceed as before.
To quit the ZOOM function and return to the graphic representation, press [END].
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EXECUTION / SIMULATION
P99996
Page
11
3.6 AUXILIARY MODES
When selecting this option, the CNC shows the following menu:
1 - SPECIAL MODES
2 - PERIPHERALS
3 - LOCK / UNLOCK
When selecting the "Special Modes" option, the CNC will request the password (access code) described in the installation manual.
After accessing one of these modes and operate with it, press [END] to quit. At this point, the CNC will show this menu again. Press [END] once more to return to the standard display mode.
Page
12
Chapter: 3
AUXILIARY FUNCTIONS
Section:
MODOS AUXILIARES
3.7 PERIPHERALS
With this CNC it is possible to communicate with the FAGOR Floppy Disk Unit, with a general peripheral device or with a computer in order to transfer programs from and to one another. This communication may be managed either from the CNC when in the "Peripheral mode" or from the computer by means of FAGOR's DNC protocol in which case the CNC may be in any of its operating modes.
3.7.1
PERIPHERAL MODE
In this mode, the CNC may communicate with the FAGOR Floppy Disk Unit, with a general peripheral device or with a computer having a standard off-the-shelf communications program.
To access this mode, press [AUX] and select the "Peripherals" option of the
"Auxiliary modes" menu.
The upper left-hand side of The CNC screen will show the following menu:
0 - RECEIVE FROM (Fagor) FLOPPY DISK UNIT
1 - SEND TO (Fagor) FLOPPY DISK UNIT
2 - RECEIVE FROM GENERAL DEVICE
3 - SEND TO GENERAL DEVICE
4 - (Fagor) FLOPPY DISK UNIT DIRECTORY
5 - (Fagor) DELETE FLOPPY DISK UNIT PROGRAM
6 - DNC ON/OFF
In order to use any of these options, the DNC mode must be inactive. If it is active
(the upper right-hand side of the screen shows: DNC), press [6] (DNC ON/OFF) to deactivate it (the DNC letters disappear).
With options 0, 1, 2 and 3 it is possible to transfer machine parameters, the decoded
M function table and the leadscrew error compensation table to a peripheral device.
The lower right-hand side of the CNC screen will show a directory of up to 7 partprograms of the CNC.
To do this, key in the desired number when the CNC requests the number of the program to be transferred and press [ENTER].
P00000 to P99990 Corresponding to part-programs
P99994 and P99996 Special user programs in ISO code
P99997
P99998
P99999
For internal use and CANNOT be transmitted back and forth
Used to associate texts to PLCI messages
Machine parameters and tables
Atention:
The part-programs cannot be edited at the peripheral device or computer.
The CRT will show the message: "RECEIVING" or "SENDING" during the program transfer and the message: "PROGRAM NUM. P23256 (for example) RECEIVED" or "SENT" when the transmission is completed.
Chapter: 3
AUXILIARY FUNCTIONS
Section:
PERIPHERALS
Page
13
When the transmission is not correct, it will display the message: "Transmission error" and when the data received by the CNC is not recognized (different format) by the CNC, it will issue the message: "Incorrect data received".
The CNC memory must be unlocked in order to perform any data transmission; if not so, the CNC will return to the menu of the peripheral mode.
When transmitting from a peripheral device other than a FAGOR Floppy Disk Unit, the following aspects must be considered:
* The program must begin with a "NULL" character (ASCII 00) followed by "%"
"program number" (for example %23256) and a "LINE FEED" character (LF).
* Blank spaces, the carriage-return key and the "+" sign are ignored.
* The program must end with either 20 "NULL" characters (ASCII 00) or with one "ESCAPE" character or with one "EOT" character.
* Press [CL] to cancel the transmission. The CNC will issue the message: PROCESS
ABORTED".
FLOPPY DISK UNIT DIRECTORY
This option displays the programs stored on the disk inserted in the FAGOR
Floppy Disk Unit and the number of characters (size) of each one of them.
It also shows the number of free characters available (free memory space) on the tape.
DELETE FLOPPY DISK UNIT PROGRAM
With this option it is possible to delete a program contained at the FAGOR Floppy
Disk Unit.
The CNC requests the number of the program to be deleted. After keying in the desired number, press [ENTER].
Once the program has been deleted, the CNC will display the message:
"PROGRAM NUM: P____ DELETED".
It also shows the number of free characters on the disk (free memory space).
3.7.2
DNC COMMUNICATIONS
To be able to use this feature, the DNC communication must be active (the upper right-hand side of the screen shows: DNC). To do this the corresponding parameters [P605(5,6,7,8); P606(8)] must be set accordingly and option [6] of the "Peripherals" mode selected if it was not active.
Once active and by using the FAGORDNC application software supplied, upon request, in floppy disks it is possible to perform the following operations from the computer:
. Obtain the CNC's part-program directory.
. Transfer part-programs and tables from and to the CNC.
. Delete part-programs at the CNC.
. Certain remote control of the machine.
Atention:
Any operating mode may be selected at the CNC.
Page
14
Chapter: 3
AUXILIARY FUNCTIONS
Section:
PERIPHERALS
3.8 LOCK/UNLOCK
With this option it is possible to lock/unlock the part-program memory.
To access this mode, press [AUX] and after selecting "Auxiliary Modes", press the key corresponding to the "LOCK/UNLOCK" option.
The codes used to do this are:
[BEG] 0000 [ENTER] Unlocks part-program memory.
[BEG] 1111 [ENTER] Locks part-program memory.
[P] F000 [ENTER] Erases the contents of all arithmetic parameters (data of the automatic operations) and sets them to "0".
Chapter: 3
AUXILIARY FUNCTIONS
Section:
LOCK/UNLOCK
Page
15
3.9 EDITING PROGRAM 99996
Program 99996 is a special ISO-coded user program. It can be edited either in this operating mode or at a PC and then sent out to this CNC.
To select this option, press [AUX] and after selecting "Auxiliary Modes", press the key corresponding to "EXECUTION OF PROGRAM P99996".
The CNC displays the editing page for this program.
If the program is currently being edited, the CNC shows a group of program blocks
(lines).
Use the to display the display the previous and following lines.
To edit a new line, follow this procedure:
1.- If the program line number appearing at the bottom of the screen is not the desired one, clear it by pressing [CL] and key in the desired line number.
2.- Key in all the pertinent data for that line and press [ENTER].
The programming format to be used is described in the programming manual.
The keys on the front panel may be used: [X], [Y], [Z], [S], [F], [N] as well as:
[TOOL] for T, for P, for R and for A.
However, since some function keys are missing (G, M, I, K, etc.), an assisted editor is also available.
To access it, press [AUX]. After analyzing the syntax of what has been edited so far, the CNC will display, one by one, all the functions which can be edited at the time.
Press [CL] to delete characters.
To modify a previously edited line, proceed as follows:
1.- If the program line number appearing at the bottom of the screen is not the desired one, clear it by pressing [CL] and key in the desired line number.
2.- Press [RECALL]. The bottom of the screen of the CNC, editing area, will show the contents of that line.
3.- Use one of these methods to modify the contents: a) Use the [CL] key to delete characters and edit it as described above.
b) Use the keys to position the cursor over the section to be modified and use the [CL] key to delete characters or [INC/ABS] to insert data.
Page
16
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EDITING P99996
While in the data inserting mode, the characters behind the cursor appear blinking. It is not possible to use assisted programming (the [AUX] key).
Key in all the desired data and press [INC/ABS]. If the syntax of the new line is correct, the CNC will display it without blinking and, if not, it will show it blinking until it is edited correctly.
4.- Once the line has been modified, press [ENTER]. The CNC will assume it replacing the previous one.
To delete a program line, proceed as follows:
1.- If the program line number appearing at the bottom of the screen is not the desired one, clear it by pressing [CL] and key in the desired line number.
2.- Press [DATA] and the CNC will delete it from memory.
Chapter: 3
AUXILIARY FUNCTIONS
Section:
EDITING P99996
Page
17
4.
AUTOMATIC OPERATIONS
This CNC has a series of keys to access each one of its automatic operations.
The basic operations selected by pressing their corresponding key are:
To select "Point to Point positioning"
To select "Positioning in a straight line"
"Positioning in an Arc" (bolt-hole pattern)
"Positioning in a Rectangular Pattern"
"Positioning in a grid pattern"
"Linear Milling"
"Circular Milling"
"Profiling"
"Inside Pocket"
"Outside Pocket" (Boss"
"Corner Roughing"
"Surface Milling"
Whenever one of these operations is selected, the CNC shows:
* At the main window, a graphic representation of the selected automatic operation.
* At the bottom of the screen, the data corresponding to the selected automatic operation.
Chapter: 4
AUTOMATIC OPERATIONS
Section: Page
1
4.1 GENERAL CONCEPTS
Once the desired operation has been selected, press [DATA] to access the data entry mode.
The CNC will highlight the first data on the graphic as well as in the data editing area.
To assign the desired value to that data, key it in and press [ENTER]. The CNC assumes the new value and highlights the next data.
To select any other data use the keys.
Once all the data has been defined, press [DATA] to quit the data entry mode.
A machining operation may be associated to the automatic positioning operations.
The machining operation will take place at each positioning point.
To find out how to define and associate a machining operation, refer to the chapter on "Machining Operations".
Then, it is possible to:
* Check the operation by pressing [SIMUL].
* Execute the operation by pressing
* Store the operation into memory as a section of a part-program.
To quit the automatic operation, press [END]. The CNC all store all the set data and it will show them again when selecting this operation.
4.1.1 CONTROL OVER THE Z AXIS
The "Z SAF" data (safety coordinate along Z) must be set in all automatic operations.
Before machining as corresponds to the automatic operation, the CNC will first move the tool to the set safety position "Z SAF".
When the Z axis is a DRO axis (not controlled by the CNC) and it is below the "Z
SAF" coordinate, the CNC will instruct the operator, by issuing a message, that the
Z axis must be moved to this safety point. Then, the resume execution.
key must be pressed to
If the operation involves several machining tasks, the CNC will position the tool at the "Z SAF" point before going on to the next one.
Page
2
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
4.1.2
MISCELLANEOUS FUNCTIONS "M" EXECUTED BEFORE
AND AFTER THE CYCLE
It is possible to associate two "M" functions to each cycle. One of them will be executed before the cycle and the other one afterwards.
The help screens show, to the right of the cycle defining data, the "M" functions selected for each cycle.
The top "M" indicates the one executed before the cycle and the bottom "M" the one executed after the cycle.
If any of them shows "M--", it means that no "M" function has been associated
To select the "M" function to be executed before the cycle, proceed as follows:
- Press the keystroke sequence: [F] [BEGIN]
- Key in the desired "M" function number.
- Press [ENTER]
To select the "M" function to be executed after the cycle, proceed as follows:
- Press the keystroke sequence: [F] [END]
- Key in the desired "M" function number.
- Press [ENTER]
To delete any of the selected "M" functions, do the following:
- Press the keystroke sequence: : [F] [BEGIN] or [F] [END]
- Press [ENTER]
The CNC will show: "M--"
Atention:
When storing an automatic operation, the CNC stores the selected "M" functions together with the data and parameters defining the automatic operation.
This way, every time a previously stored part is executed, the CNC executes each operation with the machining conditions previously set for it.
On power-up or after RESET, the CNC initializes all the cycles (not the ones stored) setting the associated "M" functions to "M--" (no associated
"M" function).
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
Page
3
4.1.3 MACHINING CONDITIONS
The CNC displays the following information:
F Currently selected axis Feedrate.
% Currently applied % of feedrate "F" override.
S Spindle speed to perform the machining operation.
When setting the spindle speed one may proceed as follows:
* Press [S], key in the desired value and press [ENTER].
The CNC assumes that this value is to be used when later executing the automatic operation now being edited. Therefore, it does not change the actual spindle speed.
* Press [S], key in the desired value and press
The CNC changes the actual spindle speed to the new one just set.
It also assumes the new value as the spindle speed to be used when later executing the automatic operation now being edited.
% Currently applied percentage of spindle speed override.
The spindle turning direction for machining.
T
To change the turning direction press [3]. The CNC will show the new turning direction but it will not change the actual turning direction of the spindle.
The tool to be used for machining.
To select the machining tool press [T] and, after keying in the desired tool number, press [ENTER].
The CNC assumes this new tool number as the one to be used with the automatic operation now being edited. Therefore, it maintains the actual tool number shown in the main window.
Atention:
When storing an automatic operation into memory, the CNC stores all these machining conditions, except the override %, together with the data and parameters defining the automatic operation.
This way, every time a previously programmed part is executed, the CNC will execute each one of the automatic operations with the machining conditions set for it.
Page
4
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
4.1.4 SIMULATION
With this CNC, it is possible to check an automatic operation in dry-run before executing it.
To do this, press . The CNC will show a graphic representation.
The lower left-hand side of the screen shows the plane being represented (XY, YZ or YZ) or three-dimensional XYZ.
To have any other plane displayed, press its corresponding key:
[0] XY Plane
[1] XZ Plane
[2] YZ Plane
[3] Three-dimensional XYZ
This CNC can show up the graphics on up to 3 planes. Therefore, it will only show the selected ones. To select other planes, proceed as follows:
Press and the CNC will ask whether each one of the possible planes is to be selected or not.
To select the plane press [Y] and, if not, press [ENTER].
Once the planes have been defined, the display area must be set by indicating the XYZ coordinates of the center of the screen and the width of the display area. After keying in each value, press [ENTER].
To check the part, press . This will start the corresponding graphic simulation.
While simulating, it is possible to access any other plane (keys: 0, 1, 2 and 3) but it is not possible to set them. To set other planes or modify the display area, it is necessary to interrupt the simulation of the program by pressing .
Press [CLEAR] to clear the screen, and [END] to quit the simulation mode.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
Page
5
4.1.4.1 ZOOM FUNCTION
With the ZOOM function, it is possible to enlarge or reduce the whole graphic representation or part of it. To do this, the simulation of the program must be either interrupted or finished.
Once the drawing plane to be enlarged or reduced has been selected, press [Z]. The screen will show a rectangle over the original drawing. This rectangle is the zoom window which represents the new display area for the part to be enlarged or reduced.
To change the dimensions of the rectangle, use these keys:
Reduces the size of the rectangle (zoom in)
Use
Increases the size of the rectangle (zoom out) to move the zoom window around.
To set the area selected with the zoom window as the new display area, press [ENTER]
To see the selected area enlarged or reduced while keeping the previous display area values, press
The area contained in the zoom window will now fill out the whole screen.
To return to the previous display area (prior to the zoom), press [END].
To use the zoom again, just press [Z] and proceed as before.
To quit the ZOOM function and return to the graphic representation, press [END].
Page
6
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
4.1.5 EXECUTION
With this CNC, it is possible to run an automatic operation from beginning to end or execute it step by step (single block) by using the key.
Whenever the "single block" mode is selected, the right-hand side of the screen shows the symbol
To unselect this mode and return to the continuous execution mode, press again.
Once the desired execution mode has been selected, press
The CNC assumes the F, S, T machining values as well as the spindle turning direction chosen and it executes the automatic operation in the following steps:
1.- If the operation has been programmed with a new tool, the CNC will request it to be selected.
Once the tool has been changed, press operation.
to resume the execution of the
2.- The CNC will start the spindle at the selected S and rotating direction.
3.- The tool will position at the pre-established safety point "Z SAF".
4.- The CNC will perform the automatic milling operation.
5.- The tool will withdraw up to the safety position "Z SAF".
6.- The CNC will stop the spindle.
It is possible to inspect and change the tool, if necessary, during the execution of an automatic operation.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
Page
7
4.1.5.1 TOOL INSPECTION
With this option it is possible to interrupt the execution of the automatic operation and inspect the tool to check its status and change it if necessary.
To do this, follow these steps: a) Press to interrupt the program.
b) Press [TOOL]
At this time, the CNC executes the miscellaneous function M05 to stop the spindle and it displays the following message on the screen:
JOG KEYS AVAILABLE
OUT c) Move the tool to the desired position by using the JOG keys.
Once the tool is "out of the way", the spindle may be started and stopped again by its corresponding keys at the Operator Panel.
d) Once the tool inspection or replacement is completed, press [END].
The CNC will execute an M03 or M04 function to start the spindle in the direction it was turning when the program was interrupted.
the screen will display the following message:
RETURN
AXES OUT OF POSITION
"Axes out of position" means that they are not at the position where the program was interrupted.
e) Jog the axes to the program interruption position by means the corresponding jog keys. The CNC will not allow to move them passed (overtravel) this position.
When the axes are in position, the screen will display: f) Press
RETURN
AXES OUT OF POSITION
NONE to resume the execution of the automatic operation
Page
8
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GENERAL CONCEPTS
4.2 POSITIONING
The various automatic positioning patterns offered on this CNC make it easy to define the points where specific machining operations will be performed.
The available positioning choices are:
* Point-to-point positioning. To be used when the points are located at random (with no specific pattern) on the surface of the part.
* Positioning in a straight line.
* Positioning in an arc (bolt-hole pattern).
* Positioning in a rectangular pattern.
* Positioning in a grid pattern.
All positioning movements are carried out in rapid.
When the Z axis is controlled by the CNC (not a DRO axis), it will be possible to associate an automatic machining operation to the positioning patterns as described later on in the chapter on "Machining Operations". These machining operations are:
Drilling
Tapping
Reaming - Boring
Center punching
This way, it will be possible to tap holes that follow a straight line, drill holes that following an arc (or bolt-hole pattern), etc.
If the positioning has no machining operation associated with it, the CNC will ask the operator to act on the Z axis after each positioning move.
Next, each one of the possible positioning choices is described as well as the data required to define them.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
POSITIONING
Page
9
4.2.1 POINT-TO-POINT POSITIONING
This option is selected by means of the key
Up to 8 points may be defined by assigning their X and Y coordinate values. These coordinate values may be entered by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
When using less than 8 points, the coordinate values for the first unused point must be the same as those of the last used point.
Example:
X1
X2
X3
X4
X5
X6
X7
X8
10.278
18.345
27.789
27.789
00.000
00.000
00.000
00.000
Z SAF 10.000
Y1 12.876
Y2 23.456
Y3 90.122
Y4 90.122
Y5 00.000
Y6 00.000
Y7 00.000
Y8 00.000
1st point
2nd point
Last point
Safety point along the Z axis
Page
10
Chapter: 4
AUTOMATIC OPERATIONS
Section:
POINT TO POINT
POSITIONING
4.2.2 POSITIONING IN A STRAIGHT LINE
This option is selected by means of the key
The first point "X1 Y1" must always be defined. This can be done by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
The path must be defined by either one of the following methods:
1.- Set the length "L" and angle "A" of the path.
In this case, one must set either the number of points (N) or the step between consecutive points (I).
2.- Set the last point, "Xn Yn", by positioning the machine at that point and pressing
[ENTER] or by keying it at the keyboard and pressing [ENTER].
In this case, one must set "L0" and the number of points or the steps between consecutive points (I).
3.- Set the "N", "I" and "A" values (number of points, steps between points and path angle respectively).
In this case one must define: "L0", "Xn=X1" and "Yn=Y1"
Programming example:
The following formats may be used:
X1=0 Y1=0 L=60 A=30 N=4
X1=0 Y1=0 L=60 A=30 I=20
X1=0 Y1=0 Xn=51.961
Yn=30 L=0 N=4
X1=0 Y1=0 Xn=51.961
Yn=30 L=0 I=20
X1=0 Y1=0 Xn=0 Yn=0 L=0 N=4 I=20 A=30
Chapter: 4
AUTOMATIC OPERATIONS
Section:
STRAIGHT LINE
POSITIONING
Page
11
4.2.3 POSITIONING IN AN ARC (BOLT-HOLE)
This option is selected by means of the key
The center of the arc, "Xc Yc", must always be defined. This can be done by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
To set the first point either one of the following methods must be used:
1.- Define the radius "R" and the angle "A" of the first point.
The angle "A" of the first point is referred to the X axis and it is given in degrees
(signed or unsigned). Negative value when clockwise and positive when counterclockwise.
2.- Set the first point, "X1 Y1", by either positioning the machine at that point or by keying its coordinates in, and then pressing [ENTER].
In this case one must set: "R0".
The number of points (N) and the angular step between consecutive points (B) must always be defined.
The angular step "B" is given in degrees signed or unsigned and it indicates the stepping direction. Clockwise for negative B and counter-clockwise for positive B.
To make a complete circle, program B0. The positioning movements will be made counter-clockwise.
Page
12
Chapter: 4
AUTOMATIC OPERATIONS
Section:
BOLT-HOLE
POSITIONING
4.2.4 RECTANGULAR PATTERN POSITIONING
This option is selected by means of the key
The first point "X1 Y1" must always be defined. This can be done by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
The following data must also be set:
"A" Angle of the abscissa path with respect to the X axis.
"B" Angle of the ordinate path with respect to the abscissa path.
To make both paths parallel to the X and Y axes, set: A=0 and B=90.
To describe the paths long the X and Y axes, the following options may be used:
1.- Define the length of the path, "LX" "LY", and the number of points on it, "NX"
"NY".
2.- Define the length of the path, "LX" "LY" and the step between consecutive points
"IX" "IY".
3.- Define the step between points "IX" "IY" and the number of points of the path
"NX" "NY".
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
POSITIONING
Page
13
4.2.5 GRID PATTERN POSITIONING
This option is selected by means of the key
The first point "X1 Y1" must always be defined. This can be done by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
The following data must also be set:
"A" Angle of the abscissa path with respect to the X axis.
"B" Angle of the ordinate path with respect to the abscissa path.
To make both paths parallel to the X and Y axes, set: A=0 and B=90.
To describe the paths long the X and Y axes, the following options may be used:
1.- Define the length of the path, "LX" "LY", and the number of points on it, "NX"
"NY".
2.- Define the length of the path, "LX" "LY" and the step between consecutive points
"IX" "IY".
3.- Define the step between points "IX" "IY" and the number of points of the path
"NX" "NY".
Page
14
Chapter: 4
AUTOMATIC OPERATIONS
Section:
GRID PATTERN
POSITIONING
4.3 MILLING
The available milling operations are:
* Linear milling
* Circular Milling
* Profiling
Prior to milling, the Z axis will move to the "Z SAF" position. If the Z axis is a DRO axis (not controlled by the CNC), the corresponding message will be issued.
Then, the tool will position at the programmed milling depth "Z". The CNC permits setting the feedrate override % for this movement.
The part is milled at the selected feedrate F.
When the milling operation is done, the Z axis moves to the "Z SAF" position. If the
Z axis is a DRO axis (not controlled by the CNC), the corresponding message will be issued.
Next, the various available milling operations will be described.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
MILLING
Page
15
4.3.1 LINEAR MILLING
This option is selected by means of the key
The first point "X1 Y1" must always be defined. This can be done by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
The path must be defined by one of the following methods
1.- Set the length "L" and angle "A" of the path.
2.- Set the last point, "X2 Y2", (either by moving the machine or entering the coordinates at the keyboard). In this case, one must set: "L0"
The milling operation may be performed either with or without tool radius compensation. To do this, press [T] and select one of the options below using the keys
-aWithout tool radius compensation.
-bWith left-hand tool radius compensation. The part stays to the right of the tool.
-cWith right-hand tool radius compensation. The part stays to the left of the tool.
To set the milling depth, indicate the "Z" value (by moving the machine or by entering the value at the keyboard) and the Feedrate override % to be applied.
Page
16
Chapter: 4
AUTOMATIC OPERATIONS
Section:
LINEAR MILLING
4.3.2 CIRCULAR MILLING
This option is selected by means of the key
The first point "X1 Y1" and last point "X2 Y2" must always be defined. This can be done by:
* jogging the axes to the desired point using the mechanical or electronic handwheels or the JOG keys of the operator panel and then pressing [ENTER].
* or by keying them in at the keyboard and pressing [ENTER].
The path must be defined by indicating the radius "R" and the moving direction "P".
After pressing [P], press the corresponding key [1], [2], [3] or [4].
The milling operation may be performed either with or without tool radius compensation. To do this, press [T] and select one of the options below using the keys
-aWithout tool radius compensation.
-bWith left-hand tool radius compensation. The part stays to the right of the tool.
-cWith right-hand tool radius compensation. The part stays to the left of the tool.
To set the milling depth, indicate the "Z" value (by moving the machine or by entering the value at the keyboard) and the Feedrate override % to be applied.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CIRCULAR MILLING
Page
17
4.3.3 PROFILING
This option is selected by means of the key
The following data must be set:
* Starting point "BEG"
* First point on the profile "X1Y1"
* Up to 7 sections, straight and/or curved, forming the profile.
* Exit or "END" point
Starting point "BEG"
The beginning point "BEG" and the milling depth "Z" must always be defined.
* The beginning point may belong to the profile or be outside of it.
* To define the milling depth, indicate the "Z" value (by moving the machine or entering it at the keyboard) and the Feedrate override % to be applied.
Tool radius compensation
The milling operation may be performed either with or without tool radius compensation. To do this, press [T] and select one of the options below using the keys
-aWithout tool radius compensation.
-bWith left-hand tool radius compensation. The part stays to the right of the tool.
-cWith right-hand tool radius compensation. The part stays to the left of the tool.
Page
18
Chapter: 4
AUTOMATIC OPERATIONS
Section:
PROFILING
Up to 7 sections, straight and/or curved, that form the profile.
Up to 7 sections may be defined on a profile. To define the type of profile section, press the following keys:
Straight section. The section assumes the indicator:
Curved section. The section assumes the indicator:
The undefined sections have the indicator:
When the CNC runs into an indicator, it assumes that there are no more sections. Therefore, it takes the previous section as the last one of the profile.
To cancel or delete an already defined section, press now assume the indicator
. The section will
Straight section
On a straight section, defined.
indicator, the XY end point of the section must be
The union between this section and the next one must also be defined.
Set "r" to blend them with a radius and, to chamfer the joint, set the "C" distance from it (XY point).
Curve d section
On a curved section, indicator, the XY end point, the radius "R" and the moving direction "P" must be defined.
To set the moving direction, press [P] followed by the corresponding key: [1],
[2], [3] or [4].
When the section being defined is tangent to the previous one, R must be "0"
(R=0).
Chapter: 4
AUTOMATIC OPERATIONS
Section:
PROFILING
Page
19
The transition from this section to the next one must also be defined setting the
"r" value when blending them with a radius.
Exit or "END" point
Once the defined sections have been executed, the tool will position at the exit point "END".
This "END" point must always be defined. To do this, either move the axes to this point and press [ENTER] or key in its coordinate values and press [ENTER].
In order to obtain a good finish, the exit may be tangential. To use this, define its radius "r" on the last section of the profile.
Page
20
Chapter: 4
AUTOMATIC OPERATIONS
Section:
PROFILING
Programming examples:
Starting point "BEG"
ZSAF=2
BEG X=70 Y=20
Z=-10 %F(Z)=50
First point of profile "X1Y1"
X1 =80 Y1 =20 r =3
Profile
X2 =80 Y2 =0 r =5
C =0
X4 =20 Y4 =0
R =15 P =4 r =5
X6 =0 r =10
C =0
Y6 =45
X8 =80 Y8 =20 r =3
Exit point "END"
END X=70 Y=20
Chapter: 4
AUTOMATIC OPERATIONS
X3 =50 Y3 =0 r =5
C =0
X5 =0 Y5 =20
R =20 P =3 r =5
X7 =80 Y7 =45 r =0
C =10
Section:
PROFILING
Page
21
Starting point "BEG"
ZSAF=2
BEG X=0 Y=-10
Z=-10 %F(Z)=50
First point of profile "X1Y1"
X1 =0 r =3
Y1 =0
Profile
X2 =67.57
Y2 =18.27
r =0
C =0
X4 =23
R =0 r =0
Y4 =-28.45
P =3
X6 = r =
C =
Y6 =
Exit point "END"
END X=0 Y=-10
X3 =69.73
Y3 =-1.37
R =0 P=1 r =0
X5 =0
R =0 r =3
Y5 =0
P =1
Page
22
Chapter: 4
AUTOMATIC OPERATIONS
Section:
PROFILING
4.4 POCKETS
There are two keys to select the type of pocket.
The
The key for an inside pocket.
key for an outside pocket or boss.
Since this CNC offers 2 inside pockets and 2 outside pockets, use the select the desired one.
key to
The available pockets are:
1.- Rectangular inside pocket.
2.- Rectangular outside pocket (rectangular boss).
3.- Circular inside pocket.
4.- Circular outside pocket (circular boss).
Before making the pocket, the Z axis will move to the safety position "Z SAF". If the Z axis is a DRO axis (not controlled by the CNC) and it is located before this safety position, the corresponding message will be issued.
Next, each one of the possible pockets are described as well as the data required to define them.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
POCKETS
Page
23
4.4.1 RECTANGULAR INSIDE POCKET
The following data must be set:
"X1 Y1"Indicates the corner of the pocket. It can be defined by:
* jogging the axes to the desired point with the mechanical or electronic handwheels or with the JOG keys of the operator panel and then pressing
[ENTER].
"L"
* keying its coordinates in at the keyboard and then pressing [ENTER].
Defines the length of the pocket. The sign indicates the machining direction.
"H" Defines the width of the pocket.
"r", "C" Define the corners of the pocket.
Page
24
For a pocket with rounded corners set "C0" and assign the rounding radius value to "r".
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
INSIDE POCKET
"G"
"E"
For a pocket with chamfered corners, set "r0" and assign to "C" the chamfer distance from the theoretical corner.
When making a regular pocket without rounded or chamfered corners, program "r0" and "C0".
Defines the sweeping step in the XY plane. The whole pocket is milled in identical steps which will be equal or smaller than the one programmed.
When programming a value of "0", the CNC will assume a value equal to
0.75 times the tool diameter.
Defines the finishing pass.
If set to "0", no finishing pass will be run.
"%F" Indicates the percentage of feedrate used for the finishing pass.
If set to 0, the feedrate for the finishing pass will be the same as the one used for the roughing passes.
"A"
"Z"
"P"
"I"
Angle of the pocket with respect to the X axis.
Defines the top Z coordinate of the pocket.
Defines the depth of the pocket.
Defines the milling pass. The CNC runs identical passes for the whole pocket which will be equal or smaller than the one programmed.
"%F (Z)" Indicates the percentage of feedrate used for the Z axis (penetration).
When set to "0", the Z axis is fed at the programmed feedrate.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
INSIDE POCKET
Page
25
Basic operation:
1.- The tool moves to the safety position "Z SAF".
2.- It moves to the center of the pocket.
3.- First penetration move at %F(Z) of the currently selected feedrate "F".
4.- Milling of the surface of the pocket at the currently selected feedrate "F".
The finishing pass will be run at %F of the currently selected feedrate "F".
In order to obtain a good finish on the sides of the pocket, the CNC applies tangential entry and exit on the last pass.
5.- The tool positions at the center of the pocket withdrawing to 1mm off the machined surface.
6.- New milling surfaces until the total depth of the pocket is reached following steps 3, 4 and 5.
7.- Withdrawal to the safety position "Z SAF".
Page
26
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
INSIDE POCKET
4.4.2 CIRCULAR INSIDE POCKET
The following data must be set:
"Xc Yc" Indicates the center of the pocket. It can be defined by:
* jogging the axes to the desired point with the mechanical or electronic handwheels or with the JOG keys of the operator panel and then pressing
[ENTER].
"R"
* keying its coordinates in at the keyboard and then pressing [ENTER].
Defines the radius of the pocket. The sign indicates the machining direction.
"G"
"E"
Defines the sweeping step in the XY plane. The whole pocket is milled in identical steps which will be equal or smaller than the one programmed.
When programming a value of "0", the CNC will assume a value equal to
0.75 times the tool diameter.
Defines the finishing pass.
If set to "0", no finishing pass will be run.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CIRCULAR
INSIDE POCKET
Page
27
"%F" Indicates the percentage of feedrate used for the finishing pass.
If set to 0, the feedrate for the finishing pass will be the same as the one used for the roughing passes.
"Z"
"P"
"I"
Defines the top Z coordinate of the pocket.
Defines the depth of the pocket.
Defines the milling pass. The CNC runs identical passes for the whole pocket which will be equal or smaller than the one programmed.
"%F (Z)" Indicates the percentage of feedrate used for the Z axis (penetration).
When set to "0", the Z axis is fed at the programmed feedrate.
Basic operation:
1.- The tool moves to the safety position "Z SAF".
2.- It moves to the center of the pocket.
3.- First penetration move at %F(Z) of the currently selected feedrate "F".
4.- Milling of the surface of the pocket at the currently selected feedrate "F".
The finishing pass will be run at %F of the currently selected feedrate "F".
In order to obtain a good finish on the sides of the pocket, the CNC applies tangential entry and exit on the last pass.
5.- The tool positions at the center of the pocket withdrawing to 1mm off the machined surface.
6.- New milling surfaces until the total depth of the pocket is reached following steps 3, 4 and 5.
7.- Withdrawal to the safety position "Z SAF".
Page
28
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CIRCULAR
INSIDE POCKET
4.4.3 RECTANGULAR OUTSIDE POCKET
The following data must be set:
"X1 Y1"Indicates the corner of the pocket. It can be defined by:
* jogging the axes to the desired point with the mechanical or electronic handwheels or with the JOG keys of the operator panel and then pressing
[ENTER].
"L"
* keying its coordinates in at the keyboard and then pressing [ENTER].
Defines the length of the pocket. The sign indicates the machining direction.
"H" Defines the width of the pocket.
"r", "C" Define the corners of the pocket.
For a pocket with rounded corners set "C0" and assign the rounding radius value to "r".
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
OUTSIDE POCKET
Page
29
"G"
For a pocket with chamfered corners, set "r0" and assign to "C" the chamfer distance from the theoretical corner.
When making a regular pocket without rounded or chamfered corners, program "r0" and "C0".
Defines the sweeping step in the XY plane. The whole pocket is milled in identical steps which will be equal or smaller than the one programmed.
When programming a value of "0", the CNC will assume a value equal to
0.75 times the tool diameter.
"Q"
"E"
Defines the excess material to be removed along X and Y.
Defines the finishing pass.
If set to "0", no finishing pass will be run.
"%F" Indicates the percentage of feedrate used for the finishing pass.
If set to 0, the feedrate for the finishing pass will be the same as the one used for the roughing passes.
"A"
"Z"
"P"
"I"
Angle of the pocket with respect to the X axis.
Defines the top Z coordinate of the pocket.
Defines the depth of the pocket.
Defines the milling pass. The CNC runs identical passes for the whole pocket which will be equal or smaller than the one programmed.
"%F (Z)" Indicates the percentage of feedrate used for the Z axis (penetration).
When set to "0", the Z axis is fed at the programmed feedrate.
Page
30
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
OUTSIDE POCKET
Basic operation:
1.- The tool moves to the safety position "Z SAF".
2.- First penetration move at %F(Z) of the currently selected feedrate "F".
3.- Milling of the outside surface of the pocket at the currently selected feedrate
"F".
The finishing pass will be run at %F of the currently selected feedrate "F".
In order to obtain a good finish on the sides of the pocket, the CNC applies tangential entry and exit on the last pass.
4.- The tool positions at the starting point of the pocket withdrawing to 1mm off the machined surface.
5.- New outside milling surfaces until the total depth of the pocket is reached following steps 2, 3 and 4.
6.- Withdrawal to the safety position "Z SAF".
Chapter: 4
AUTOMATIC OPERATIONS
Section:
RECTANGULAR
OUTSIDE POCKET
Page
31
4.4.4 CIRCULAR OUTSIDE POCKET
The following data must be set:
"Xc Yc" Indicates the center of the pocket. It can be defined by:
* jogging the axes to the desired point with the mechanical or electronic handwheels or with the JOG keys of the operator panel and then pressing
[ENTER].
"R"
* keying its coordinates in at the keyboard and then pressing [ENTER].
Defines the radius of the pocket. The sign indicates the machining direction.
"G"
"Q"
Defines the sweeping step in the XY plane. The whole pocket is milled in identical steps which will be equal or smaller than the one programmed.
When programming a value of "0", the CNC will assume a value equal to
0.75 times the tool diameter.
Defines the excess material to be removed along the X and Y axes.
Page
32
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CIRCULAR
OUTSIDE POCKET
"E" Defines the finishing pass.
If set to "0", no finishing pass will be run.
"%F" Indicates the percentage of feedrate used for the finishing pass.
If set to 0, the feedrate for the finishing pass will be the same as the one used for the roughing passes.
"Z"
"P"
"I"
Defines the top Z coordinate of the pocket.
Defines the depth of the pocket.
Defines the milling pass. The CNC runs identical passes for the whole pocket which will be equal or smaller than the one programmed.
"%F (Z)" Indicates the percentage of feedrate used for the Z axis (penetration).
When set to "0", the Z axis is fed at the programmed feedrate.
Basic operation:
1.- The tool moves to the safety position "Z SAF".
2.- First penetration move at %F(Z) of the currently selected feedrate "F".
3.- Milling of the outside surface of the pocket at the currently selected feedrate
"F".
The finishing pass will be run at %F of the currently selected feedrate "F".
In order to obtain a good finish on the sides of the pocket, the CNC applies tangential entry and exit on the last pass.
4.- The tool positions at the starting point of the pocket withdrawing to 1mm off the machined surface.
5.- New outside milling surfaces until the total depth of the pocket is reached following steps 2, 3 and 4.
6.- Withdrawal to the safety position "Z SAF".
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CIRCULAR
OUTSIDE POCKET
Page
33
4.5 CORNER ROUGHING
With this CNC it is possible to rough square, round or chamfered corners as shown in the illustration below:
This option is selected by means of the key.
The following data must be set:
Machining direction
To change the machining direction, press [T] and then or
"X1 Y1"Indicates the inside coordinates of the corner referred to Part Zero. It can be defined by:
* jogging the axes to the desired point with the mechanical or electronic handwheels or with the JOG keys of the operator panel and then pressing
[ENTER].
* keying its coordinates in at the keyboard and then pressing [ENTER].
Page
34
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CORNER ROUGHING
"L", "H" Defines the length of the pocket along the X and Y axis respectively.
Depending on the corner to be machined, the sign will be positive or negative as shown below.
"r", "C" Define the type of corner to be machined
For a rounded corner set "C0" and assign the rounding radius value to "r".
For a chamfered corner, set "r0" and assign to "C" the chamfer distance from the theoretical corner.
"G"
"E"
When making a regular sharp corner, program "r0" and "C0".
The "r" and "C" values must be smaller than those of "L" and "H".
Defines the sweeping step in the XY plane. The whole corner is milled out in identical steps which will be equal or smaller than the one programmed.
When programming a value of "0", the CNC will assume a value equal to
0.75 times the tool diameter.
Defines the finishing pass.
If set to "0", no finishing pass will be run.
"%F" Indicates the percentage of feedrate used for the finishing pass.
If set to 0, the feedrate for the finishing pass will be the same as the one used for the roughing passes.
"A"
"Z"
Angle of the corner with respect to the X axis.
Defines the top Z coordinate of the pocket.
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CORNER ROUGHING
Page
35
"P"
"I"
Defines the depth of the pocket.
Defines the milling pass. The CNC runs identical passes for the whole corner which will be equal or smaller than the one programmed.
"%F (Z)" Indicates the percentage of feedrate used for the Z axis (penetration).
When set to "0", the Z axis is fed at the programmed feedrate.
Basic operation:
1.- The tool moves to the safety position "Z SAF".
2.- It moves to the outside of the corner
3.- First penetration move at %F(Z) of the currently selected feedrate "F".
4.- Milling of the corner at the currently selected feedrate "F".
The finishing pass will be run at %F of the currently selected feedrate "F".
5.- New milling surfaces until the total depth is reached.
6.- Withdrawal to the safety position "Z SAF".
Page
36
Chapter: 4
AUTOMATIC OPERATIONS
Section:
CORNER ROUGHING
4.6 SURFACE MILLING
This option is selected by means of the key
Since this CNC offers 4 different types of surface milling, the used to select the desired one.
The available types of surface milling are:
Bidirectional along X key must be
Unidirectional along X
Bidirectional along Y
Chapter: 4
AUTOMATIC OPERATIONS
Section:
SURFACE MILLING
Page
37
Unidirectional along Y
Once the desired surface milling type has been chosen, all the data must be defined.
"X1 Y1"Indicates the corner of the surface to be milled. It can be defined by:
* jogging the axes to the desired point with the mechanical or electronic handwheels or with the JOG keys of the operator panel and then pressing
[ENTER].
* keying its coordinates in at the keyboard and then pressing [ENTER].
"L", "H" Define the length and width of the surface to be milled.
When using unidirectional milling, the sign of these parameters indicates the machining direction.
Page
38
Chapter: 4
AUTOMATIC OPERATIONS
Section:
SURFACE MILLING
"G"
"E"
Defines the step between two consecutive passes. The whole surface is milled with the same step which is the same or smaller than the one programmed.
If programmed with a 0 value, the CNC will assume a value 0.75 times the tool diameter.
Defines the amount the tool runs off each side of the part in order to achieve a good finish on its corners.
"Z SAF" Defines the safety coordinate along Z.
"Z" Defines the height of the plane to be milled.
"P"
"I"
Defines the milling depth.
Defines the milling pass. The CNC assumes the same pass for the whole surface which will be equal or smaller than the one programmed.
Basic operation:
1.- The tool positions at the safety point "Z SAF".
2.- Moves to a point located at an "E" distance from the corner, X1 Y1.
3.- First penetration and milling of the surface at the selected feedrate "F".
In order to obtain a good finish at the corners, the tool overshoots an "E" distance off each side.
4.- The tool moves to the point located at an "E" distance of the corner, X1 Y1, retracting 1mm from the machined surface.
5.- New milling surfaces until the programmed depth is reached following steps 3 and 4.
6.- Withdrawal to the safety position "Z SAF".
Chapter: 4
AUTOMATIC OPERATIONS
Section:
SURFACE MILLING
Page
39
5.
MACHINING OPERATIONS
This CNC offers the following machining operations:
* Center punching
* Drilling
* Tapping
* Boring / Reaming
Each one of these operations may be executed when operating in "DRO Mode" or may be associated to any automatic positioning operations.
When operating in "DRO Mode", the axes must be moved to the point where the machining will take place and proceed as follows:
* Press
* Press operation.
to access the machining operations.
or as many times as necessary to select the desired machining
* Properly define all the data corresponding to the selected operation.
* Press to start machining.
Proceed as follows in order to associate a machining operation to a positioning operation:
* Select and define the automatic positioning operation (point-to-point, in a straight line, in arc, in a rectangular pattern or in a grid pattern).
* Press
* Press operation.
to access the machining operations.
or as many times as necessary to select the desired machining
* Properly define all the data corresponding to the selected operation.
* The CNC associates the machining operation to the automatic positioning in such a way that it is possible to define "Positioning in a straight line + Drilling", "Positioning in an arc + Reaming", etc.
The machining conditions must be set in the automatic operation.
Chapter: 5
MACHINING OPERATIONS
Section: Page
1
Every time a machining operation is selected, the CNC shows:
* A graphic representation of the selected automatic operation in the main display area.
* The data pertinent to the selected operation at the bottom of the screen..
5.1 GENERAL CONCEPTS
Once the machining operation has been selected, press one of the following keys:
To quit the machining operation and return to the automatic positioning operation. No machining is associated to the positioning.
For the machining data to be assumed by the CNC and it returns to the automatic positioning operation. The machining operation is associated to the positioning operation.
To access the data entry mode.
The CNC highlights the first data on the graphic representation and in the data editing area.
Key in the desired value for that data and press [ENTER]. The CNC assumes the new value and highlights the next data.
To select any other data, use the keys.
Once all the data has been set, press [DATA] to quit the data entry mode.
The CNC takes the machining data and returns to the automatic positioning operation. The machining operation is associated to the positioning operation.
Page
2
Chapter: 5
MACHINING OPERATIONS
Section:
GENERAL CONCEPTS
5.1.1
MISCELLANEOUS FUNCTIONS "M" EXECUTED BEFORE
AND AFTER THE OPERATION
It is possible to associate two "M" functions to each operation. One of them will be executed before the operation and the other one afterwards.
The help screens show, to the right of the operation defining data, the "M" functions selected for each operation.
The top "M" indicates the one executed before the operation and the bottom "M" the one executed after the operation.
If any of them shows "M--", it means that no "M" function has been associated
To select the "M" function to be executed before the operation, proceed as follows:
- Press the keystroke sequence: [F] [BEGIN]
- Key in the desired "M" function number.
- Press [ENTER]
To select the "M" function to be executed after the operation, proceed as follows:
- Press the keystroke sequence: [F] [END]
- Key in the desired "M" function number.
- Press [ENTER]
To delete any of the selected "M" functions, do the following:
- Press the keystroke sequence: : [F] [BEGIN] or [F] [END]
- Press [ENTER]
The CNC will show: "M--"
Atention:
When storing an automatic operation, the CNC stores the selected "M" functions together with the data and parameters defining the automatic operation.
This way, every time a previously stored part is executed, the CNC executes each operation with the machining conditions previously set for it.
On power-up or after RESET, the CNC initializes all the operations (not the ones stored) setting the associated "M" functions to "M--" (no associated "M" function).
Chapter: 5
MACHINING OPERATIONS
Section:
M FUNCTIONS BEFORE AND
AFTER OPERATION
Page
3
5.2 CENTER PUNCHING
To define the amount of penetration of the center punch into the part, one of the following methods must be used:
* Set the punching depth (P)
* Set the angle "A" of the punch and the diameter of the point to make.
The following data must also be set in either case:
"Z" Position (coordinate) where the machining will take place.
"K" Dwell, in seconds, between punching and withdrawing the tool.
Basic operation:
1.- Punching at selected feedrate "F" and data.
2.- Dwell if "K" has been programmed.
3.- Withdrawal in rapid up to the safety position "Z SAF".
Page
4
Chapter: 5
MACHINING OPERATIONS
Section:
CENTER PUNCHING
5.2.1 PROGRAMMING EXAMPLE
Definition of "Positioning in a straight line"
X1 = 20
L = 50
N = 6
Z SAF = 1
Y1 = 10
A = 25
Definition of "Center Punching":
Z = 0
P = 1.5
K = 0
Chapter: 5
MACHINING OPERATIONS
Section:
CENTER PUNCHING
Page
5
5.3 DRILLING
The following data must be set:
"Z"
"P"
Position (coordinate) where the machining will take place
Drilling depth.
"I"
"K"
Drilling step
Dwell, in seconds, between drilling and withdrawing the tool.
Basic operation:
1.- First drilling move down to "Z-I" at feedrate "F".
2.- Withdrawal in rapid up to Z.
3.- Rapid approach up to 1mm from the previous peck.
4.- New drilling move (peck), "I" distance and at feedrate "F".
5.- Repeat steps 2, 3, 4, until the programmed total depth is reached.
6.- Dwell if "K" has been programmed.
7.- Rapid withdrawal to safety position "Z SAF".
Page
6
Chapter: 5
MACHINING OPERATIONS
Section:
DRILLING
5.3.1 PROGRAMMING EXAMPLE
Definition of "Positioning in a straight line":
X1 = 20
L = 50
N = 6
Z SAF = 1
Y1 = 10
A = 25
Definition of "Drilling":
Z = 0
P = 12
I = 5
K = 1
Chapter: 5
MACHINING OPERATIONS
Section:
DRILLING
Page
7
5.4 TAPPING
The following data must be set:
"Z" Position (coordinate) where the machining will take place.
"P"
"K"
Depth of the tap.
Dwell, in seconds between tap-in and tap-out
Basic operation
1.- Tap in all the way to the bottom at 100 % of the selected feedrate "F" (it cannot be overridden).
2.- If "K" has not be programmed, the spindle changes its rotating direction.
If "K" has been programmed, it behaves as follows:
* It stops the spindle.
* It waits for a "K" time period (dwell).
* Reverses the spindle rotating direction.
3.- Withdrawal up to the safety position "Z SAF" at the programmed "F".
4.- If "K" has not been programmed, reverses the spindle rotation again, thus recovering its initial rotating direction.
If "K" has been programmed, it behaves as follows:
* It stops the spindle.
* It waits for a "K" time period (dwell).
* Reverses the spindle rotation, thus recovering its initial rotating direction.
Page
8
Chapter: 5
MACHINING OPERATIONS
Section:
TAPPING
5.4.1 PROGRAMMING EXAMPLE
Definition of "Positioning in a straight line"
X1 = 20
L = 50
N = 6
Z SAF = 1
Y1 = 10
A = 25
Definition of "Tapping"
Z = 0
P = 12
K = 1
Chapter: 5
MACHINING OPERATIONS
Section:
TAPPING
Page
9
5.5 BORING / REAMING
The following data must be set:
"Z" Position (coordinate) where the machining will take place.
"P"
"K"
Boring depth.
Dwell, in seconds, between punching and withdrawing the tool.
Basic operation:
1.- Punching at selected feedrate "F" and data.
2.- Dwell if "K" has been programmed.
3.- Withdrawal to the safety position "Z SAF" at the programmed "F".
Page
10
Chapter: 5
MACHINING OPERATIONS
Section:
BORING
REAMING
5.5.1 PROGRAMMING EXAMPLES
Boring example
"Bolt-hole positioning" (in an arc):
Xc = 70
R = 40
N = 8
Z SAF = 1
Yc = 20
A = -15
B = 30
Definition of "Boring":
Z = 0
P = 12
K = 1
Reaming example
"Grid pattern positioning ":
X1 = 20
A = 0
LX = 90
LY = 40
Z SAF = 1
Y1 = 10
B = 90
NX = 4
NY = 3
Definition of "Reaming":
Z = 0
P = 12
K = 1
Chapter: 5
MACHINING OPERATIONS
Section:
BORING
REAMING
Page
11
6.
WORKING WITH PART-PROGRAMS
The 800M CNC can store up to 7 part-programs.
Each of these programs may have up to 20 basic operations.
Each of these operations will have been edited by the operator in the "AUTOMATIC" mode (CYCLE) and in the manner described in the chapter about "AUTOMATIC
OPERATIONS".
6.1 ACCESS TO THE PART-PROGRAM TABLE
To access this table, press [RECALL].
The upper right-hand side of the screen will show a directory of up to 7 part-programs of the 10 that may be stored, always numbered with 5 digits and comprised between
"00000" and "99995". To see the rest, use
The dashes indicate that there is no part-program. The symbols displayed to the right of the corresponding part number mean the following:
PART
01435 [*]
47632 [*]
32540 [*]
----[ ]
----[ ]
----[ ]
----[ ]
EXIT
[*] Indicates that the part-program has been previously edited and it contains data.
[ ] Indicates that the part-program contains no data.
To assign a number to the desired part, proceed as follows:
.
Position the cursor over it using the knowing that the selection rolls over.
keys and
.
Press [P]. The selected line will appear in reverse video blinking the number "00000".
. Press the digits of the number to be assigned and then press [ENTER]. If after pressing this key, this number keeps blinking, it means that this number has already been assigned to another part.
. If [CLEAR] is pressed, the selected line will return to its previous number if it had one.
To quit the part-program table, position the cursor over "EXIT" and press [ENTER].
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
ACCESS TO THE
PART-PROGRAM TABLE
Page
1
6.2 PART-PROGRAM SELECTION
To analyze the contents of a part-program in order to edit it or modify it, select it at the part-program table and press [RECALL].
Each part may consist of up to 20 basic operations. However, the upper right-hand side of the screen will show a set of 7 operations.
Whenever a part-program is accessed, the cursor appears at its first free position.
The free positions are indicated by means of the "?" character and the occupied positions indicate the type of operation that has been edited in them. Although the profiles are treated as a single operations, they occupy two positions.
PART 01346
1 - RECT.POCK
2 - CIRC.POCK
3 - ARCPO+DRI
4 - ROUNDBOSS
5 ?
Each one of these operations will have been previously edited by the operator in the "AUTOMATIC" mode
(CYCLE) and in the manner described in the chapter about "AUTOMATIC OPERATIONS".
To select one of these operations, position the cursor over it by using the keys.
6 -
7 -
?
?
EXIT
To quit the part-program option, position the cursor over
"EXIT" and press [ENTER].
To return to the part-program directory (previous menu), press the key until the cursor is positioned over
"PART 01346" and, then, press the key once more
Page
2
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
SELECTION
6.3 PART-PROGRAM EDITING
A part-program consists of various operations. Therefore, to edit it, we must edit its different operations.
Each operation will be edited as any normal operation and in the manner described in the section about "AUTOMATIC OPERATIONS".
Once defined, the operation may be simulated or executed to check that it works properly.
To store the operation as part-program, position the cursor over the operation number to be assigned to it and press [ENTER].
The CNC requests confirmation of the command. The following cases are possible:
* The selected operation number was free.
Once the command to store in memory is confirmed, the CNC will include the new operation in the indicated position and the operation listing will be updated.
* The selected operation number was occupied.
When the CNC requests confirmation of this command, it asks whether it is desired to:
Replace by pressing [ENTER].
Insert
The new operation will occupy the selected position and the previous operation will disappear. The rest of the operations will keep their original positions.
by pressing [1].
The new operation will occupy the selected position and the one which was there before as well as the following ones (including the free ones) will be shifted back one position.
If position number 20 is already occupied, the CNC will display a message indicating that this command cannot be executed.
Ignore
Atention:
(do nothing) by pressing [CLEAR].
When editing several operations of a part-program, it is recommended to start from operation "1" and use consecutive positions.
When executing a part-program, the CNC always starts from operation
"1" and ends the execution when a free position is found, even when the program has other operations.
Each one of the operations of the part-program is stored in memory with all the data which was edited with, including the machining conditions:
F, S, T, spindle rotating direction, etc.
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM EDITING
Page
3
6.4 PART-PROGRAM SIMULATION
With this CNC, it is possible to check a part-program in dry-run before executing it.
5 -
6 -
7 -
PART 01346
1 - RECT.POCK
2 - CIRC.POCK
3 - ARCPO+DRI
4 - ROUNDBOSS
?
?
?
EXIT
When simulating a part, the CNC always starts out from operation "1" and ends when it encounters a free position, even if the part contains more operations.
To do this, position the cursor over the part number (PART
01346) and press
The CNC will show a graphic representation.
The lower left-hand side of the screen shows the plane being represented (XY, YZ or YZ) or three-dimensional XYZ.
To have any other plane displayed, press its corresponding key:
[0] XY Plane
[1] XZ Plane
[2] YZ Plane
[3] Three-dimensional XYZ
This CNC can show up the graphics on up to 3 planes. Therefore, it will only show the selected ones. To select other planes, proceed as follows:
Press and the CNC will ask whether each one of the possible planes is to be selected or not.
To select the plane press [Y] and, if not, press [ENTER].
Once the planes have been defined, the display area must be set by indicating the XYZ coordinates of the center of the screen and the width of the display area. After keying in each value, press [ENTER].
Page
4
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
SIMULATION
To check the part, press . This will start the corresponding graphic simulation.
While simulating, it is possible to access any other plane (keys: 0, 1, 2 and 3) but it is not possible to set them. To set other planes or modify the display area, it is necessary to interrupt the simulation of the program by pressing .
Press [CLEAR] to clear the screen, and [END] to quit the simulation mode.
6.4.1 ZOOM FUNCTION
With the ZOOM function, it is possible to enlarge or reduce the whole graphic representation or part of it. To do this, the simulation of the program must be either interrupted or finished.
Once the drawing plane to be enlarged or reduced has been selected, press [Z]. The screen will show a rectangle over the original drawing. This rectangle is the zoom window which represents the new display area for the part to be enlarged or reduced.
To change the dimensions of the rectangle, use these keys:
Reduces the size of the rectangle (zoom in)
Use
Increases the size of the rectangle (zoom out) to move the zoom window around.
To set the area selected with the zoom window as the new display area, press [ENTER]
To see the selected area enlarged or reduced while keeping the previous display area values, press
The area contained in the zoom window will now fill out the whole screen.
To return to the previous display area (prior to the zoom), press [END].
To use the zoom again, just press [Z] and proceed as before.
To quit the ZOOM function and return to the graphic representation, press [END].
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
SIMULATION
Page
5
6.5 PART-PROGRAM EXECUTION
When executing a part-program, the CNC always starts from operation "1" and ends when a free position is found, even when the program has other operations.
PART 01346
1 - RECT.POCK
2 - CIRC.POCK
3 - ARCPO+DRI
4 - ROUNDBOSS
5 ?
6 ?
7 ?
EXIT
To execute a part-program, select it by positioning the cursor over its corresponding header (PART 01346) and press
Once the part-program is selected, it is executed operation after operation starting from the first one.
Every time the CNC selects an operation, it will highlight it and it will make a copy into the editing area (bottom of the screen) displaying the selected operation with all its parameters.
Once the operation has concluded, the tool is positioned at the safety point "Z SAF". The tool movement to the first point of the next operation is made in a straight line maintaining the "Z SAF" coordinate.
Before executing each operation, the CNC assumes the machining conditions F, S, T defined for the operation.
At the end of each operation, the tool returns to the safety position "Z SAF" for that operation.
If the next operation requires a tool change, the CNC moves the tool to the Z coordinate at the beginning of the program (where it was before pressing ), it stops the spindle and displays the tool change message.
Before starting the next operation, the tool positions at the "Z SAF" point of that operation.
The execution of the part-program ends when a free position is found even if there are more operations defined in later blocks.
The tool will return to the Z coordinate where the execution of the part-program began (where it was when was pressed.
To interrupt the program, press enabled:
. Once interrupted, the following keys are
To resume execution, press
Atention:
It must be borne in mind that the CNC always executes what is defined in the editing area, bottom of the screen. Therefore, the cursor must be positioned over the part's header (PART 01346) before pressing
If when pressing the cursor is positioned over an automatic operation, the CNC only executes that operation.
Page
6
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
EXECUTION
6.5.1 EXECUTION OF AN OPERATION PREVIOUSLY STORED IN A
PART-PROGRAM
To do this, select the corresponding part-program, position the cursor over the desired operation and press [RECALL].
The CNC recovers all the values that the operation was stored with and it shows them at the bottom of the screen.
* Data specific to the operation:
* Machining conditions: F, S, T, spindle turning direction, etc.
Then, press to execute the selected operation.
It is possible to modify any data before pressing if so desired.
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
EXECUTION
Page
7
6.5.2. TOOL INSPECTION
With this option it is possible to interrupt the execution of a part-program and inspect the tool to check its status and change it if necessary.
To do this, follow these steps: a) Press to interrupt the program.
b) Press [TOOL]
At this time, the CNC executes the miscellaneous function M05 to stop the spindle and it displays the following message on the screen:
JOG KEYS AVAILABLE
OUT c) Move the tool to the desired position by using the JOG keys.
Once the tool is "out of the way", the spindle may be started and stopped again by its corresponding keys at the Operator Panel.
d) Once the tool inspection or replacement is completed, press [END].
The CNC will execute an M03 or M04 function to start the spindle in the direction it was turning when the program was interrupted.
the screen will display the following message:
RETURN
AXES OUT OF POSITION
"Axes out of position" means that they are not at the position where the program was interrupted.
e) Jog the axes to the program interruption position by means the corresponding jog keys. The CNC will not allow to move them passed (overtravel) this position.
When the axes are in position, the screen will display: f) Press
RETURN
AXES OUT OF POSITION
NONE to resume the execution of the part-program.
Page
8
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
EXECUTION
6.6 PART-PROGRAM MODIFICATION
To modify an operation, select the corresponding part-program, position the cursor over the desired operation and press [RECALL].
The CNC recovers all the values stored with that operation and it displays them at the bottom of the screen.
From this moment, the operation may be modified as any normal operation and in the manner described in the section about "AUTOMATIC OPERATIONS".
Once all the modifications have been made, it is possible to simulate or execute the operation to verify that it works properly before storing it in memory.
Once [ENTER] has been pressed, the CNC requests the confirmation of the command. Press [ENTER] again to confirm it (replace option).
To delete an operation, select the corresponding part-program, position the cursor over the desired operation and press [CLEAR].
The CNC will request confirmation of the command.
When deleting an operation, the CNC compresses the part-program shifting all the following operations one position forward.
To insert a new operation, follow the same procedure as for editing a part-program.
Once the operation has been defined, position the cursor over the operation number to be assigned to it and press [ENTER] to store it in memory.
The CNC requests confirmation of the command. Press [1] to insert this new one or [ENTER] to replace the current (old) one.
To copy an already existing operation into another position, move the cursor over the operation to be copied and press [RECALL].
The CNC recovers all the values stored with that operation and it displays them at the bottom of the screen.
Then, select the operation number where it is to be copied and press [ENTER].
The CNC will request confirmation of the command.
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM
MODIFICATION
Page
9
6.7 PART-PROGRAM DELETION
To delete a part-program, choose one of the following methods:
Select the desired part-program on the part-program directory and press [CLEAR] or select the desired part-program, position the cursor over its header (PART01435) and press [CLEAR]. In either case, the CNC will request confirmation of the command.
PART
01435 [*]
47632 [*]
32540 [*]
----[ ]
----[ ]
----[ ]
----[ ]
EXIT
1 - RECT.POCK
2 - CIRC.POCK
3 - ARCPO+DRI
4 - ROUNDBOSS
5 -
6 -
7 -
PART 01346
?
?
?
EXIT
Page
10
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PART-PROGRAM DELETION
6.8 PERIPHERALS
With this CNC it is possible to communicate with the FAGOR Floppy Disk Unit, with a general peripheral device or with a computer in order to transfer programs from and to one another. This communication may be managed either from the CNC when in the "Peripheral mode" or from the computer by means of FAGOR's DNC protocol in which case the CNC may be in any of its operating modes.
6.8.1 PERIPHERAL MODE
In this mode, the CNC may communicate with the FAGOR Floppy Disk Unit, with a general peripheral device or with a computer having a standard off-the-shelf communications program.
To access this mode, press [AUX] and select the "Peripherals" option of the
"Auxiliary modes" menu.
The upper left-hand side of The CNC screen will show the following menu:
0 - RECEIVE FROM (Fagor) FLOPPY DISK UNIT
1 - SEND TO (Fagor) FLOPPY DISK UNIT
2 - RECEIVE FROM GENERAL DEVICE
3 - SEND TO GENERAL DEVICE
4 - (Fagor) FLOPPY DISK UNIT DIRECTORY
5 - (Fagor) DELETE FLOPPY DISK UNIT PROGRAM
6 - DNC ON/OFF
In order to use any of these options, the DNC mode must be inactive. If it is active
(the upper right-hand side of the screen shows: DNC), press [6] (DNC ON/OFF) to deactivate it (the DNC letters disappear).
With options 0, 1, 2 and 3 it is possible to transfer machine parameters, the decoded
M function table and the leadscrew error compensation table to a peripheral device.
The lower right-hand side of the CNC screen will show a directory of up to 7 partprograms of the CNC.
To do this, key in the desired number when the CNC requests the number of the program to be transferred and press [ENTER].
P00000 to P99990 Corresponding to part-programs
P99994 and P99996 Special user programs in ISO code
P99997 For internal use and CANNOT be transmitted back and
P99998
P99999 forth
Used to associate texts to PLCI messages
Machine parameters and tables
Atention:
The part-programs cannot be edited at the peripheral device or computer.
The CRT will show the message: "RECEIVING" or "SENDING" during the program transfer and the message: "PROGRAM NUM. P23256 (for example) RECEIVED" or "SENT" when the transmission is completed.
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PERIPHERALS
Page
11
When the transmission is not correct, it will display the message: "Transmission error" and when the data received by the CNC is not recognized (different format) by the CNC, it will issue the message: "Incorrect data received".
The CNC memory must be unlocked in order to perform any data transmission; if not so, the CNC will return to the menu of the peripheral mode.
When transmitting from a peripheral device other than a FAGOR Floppy Disk Unit, the following aspects must be considered:
* The program must begin with a "NULL" character (ASCII 00) followed by "%"
"program number" (for example %23256) and a "LINE FEED" character (LF).
* Blank spaces, the carriage-return key and the "+" sign are ignored.
* The program must end with either 20 "NULL" characters (ASCII 00) or with one "ESCAPE" character or with one "EOT" character.
* Press [CL] to cancel the transmission. The CNC will issue the message: PROCESS
ABORTED".
FLOPPY DISK UNIT DIRECTORY
This option displays the programs stored on the disk inserted in the FAGOR
Floppy Disk Unit and the number of characters (size) of each one of them.
It also shows the number of free characters available (free memory space) on the tape.
DELETE FLOPPY DISK UNIT PROGRAM
With this option it is possible to delete a program contained at the FAGOR Floppy
Disk Unit.
The CNC requests the number of the program to be deleted. After keying in the desired number, press [ENTER].
Once the program has been deleted, the CNC will display the message:
"PROGRAM NUM: P____ DELETED".
It also shows the number of free characters on the disk (free memory space).
6.8.2
DNC COMMUNICATIONS
To be able to use this feature, the DNC communication must be active (the upper right-hand side of the screen shows: DNC). To do this the corresponding parameters must be set accordingly by the manufacturer and option [6] of the
"Peripherals" mode selected if it was not active.
Once active and by using the FAGORDNC application software supplied, upon request, in floppy disks it is possible to perform the following operations from the computer:
. Obtain the CNC's part-program directory.
. Transfer part-programs and tables from and to the CNC.
. Delete part-programs at the CNC.
. Certain remote control of the machine.
Atention:
Any operating mode may be selected at the CNC.
Page
12
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
PERIPHERALS
6.9 LOCK/UNLOCK
With this option it is possible to lock/unlock the part-program memory in order to protect it against accidental manipulation.
To access this mode, press [AUX] and after selecting "Auxiliary Modes", press the key corresponding to the "LOCK/UNLOCK" option.
The codes used to do this are:
[BEG] 0000 [ENTER] Unlocks part-program memory.
[BEG] 1111 [ENTER] Locks part-program memory.
[P] F000 [ENTER] Erases the contents of all arithmetic parameters (data of the automatic operations) and sets them to "0".
Chapter: 6
WORKING WITH PART-PROGRAMS
Section:
LOCK/UNLOCK
Page
13
ERROR
CODES
008
009
010
011
012
004
005
006
007
001 This error occurs in the following cases:
* When the first character of the block to be executed is not an "N".
* When while BACKGROUND editing, the program in execution calls a subroutine located in the program being edited or in a later program.
The order in which the part-programs are stored in memory are shown in the part-program directory. If during the execution of a program, a new one is edited, this new one will be placed at the end of the list.
002
003
Too many digits when defining a function in general.
This error occurs in the following cases:
* When a negative value has been assigned to a function which does not accept the "-" sign.
* When an incorrect value has been assigned to an automatic operation:
Positioning in line: ..................................... If L=0, Xn=X1, Yn=Y1, I=0
If L=0, Xn=X1, Yn=Y1, N=0
If I=0, N=0
If I>0, L/I fraction
Positioning in arc: ...................................... If N=0
If R=0, Xc=X1, Yc=Y1
Positioning in rectangle or grid pattern: If
If
LX=0, IX=0
LX=0, NX=0 or LY=0, IY=0 or LY=0, NY=0
If LX>0, IX=0, NX<2 or LY>0, IY=0, NY<2
If LX>0, IX>0, LX/IX fraction
If LY>0, IY>0, LY/IY fraction
Rectangular pocket .................................... If L=0 or H=0
If r>(L/2) or r>(H/2)
Circular pocket .......................................... If Tool radius > R
Corner roughing ........................................ If L=0
If r>L
Surface milling .......................................... If L=0 or H=0 or r>H or H=0
Not being used at this time.
Parametric block programmed wrong.
There are more than 10 parameters affected in a block.
Division by zero.
Square root of a negative number.
Parameter value too large.
M41, M42, M43 or M44 has been programmed.
More than 7 "M" functions in a block.
This error occurs in the following cases:
- Function G50 is programmed wrong
- Tool dimension values too large.
- Zero offset values ( G53/G59 ) too large.
013
014
015
016
017
018
Not being used at this time.
A block has been programmed which is incorrect either by itself or in relation with the program history up to that instant.
Functions G20, G21, G22, G23, G24, G25, G26, G27, G28, G29, G30, G31, G32, G50, G52, G53, G54, G55,
G56, G57, G58, G59, G72, G73, G74, G92 and G93 must be programmed alone in a block.
The called subroutine or block does not exist or the block searched by means of special function F17 does not exist.
Negative or too large thread pitch value.
Error in blocks where the points are defined by means of angle-angle or angle-coordinate.
019
020
021
022
023
025
026
027
028
029
030
031
This error is issued in the following cases:
- After defining G20, G21, G22 or G23, the number of the subroutine it refers to is missing.
- The "N" character has not been programmed after function G25, G26, G27, G28 or G29.
- Too many nesting levels.
The axes of the circular interpolation are not programmed correctly.
There is no block at the address defined by the parameter assigned to F18, F19, F20, F21, F22.
An axis is repeated when programming G74.
K has not been programmed after G04.
Error in a definition block or subroutine call, or when defining either conditional or unconditional jumps.
This error is issued in the following cases:
- Memory overflow.
- Not enough free tape or CNC memory to store the part-program.
I/J/K has not been defined for a circular interpolation or thread.
An attempt has been made to select a tool offset at the tool table or a non-existent external tool (the number of tools is set by machine parameter).
Too large a value assigned to a function.
This error is often issued when programming an F value in mm/min (inch/min) and, then, switching to work in mm/rev (inch/rev) without changing the F value.
The programmed G function does not exist.
Tool radius value too large.
032 Tool radius value too large.
033 A movement of over 8388 mm or 330.26 inches has been programmed.
Example: Being the X axis position X-5000, if we want to move it to point X5000, the CNC will issue error
33 when programming the block N10 X5000 since the programmed move will be:
5000 - (-5000) = 10000 mm.
In order to make this move without issuing this error, it must be carried out in two stages as indicated below:
N10 X0
N10 X5000
; 5000 mm move
; 5000 mm move
034
035
036
037
038
039
040
041
S or F value too large.
Not enough information for corner rounding, chamfering or compensation.
Repeated subroutine.
Function M19 programmed incorrectly.
Function G72 or G73 programmed incorrectly.
It must be borne in mind that if G72 is applied only to one axis, this axis must be positioned at part zero (0 value) at the time the scaling factor is applied.
This error occurs in the following cases:
- More than 15 nesting levels when calling subroutines.
- A block has been programmed which contains a jump to itself. Example: N120 G25 N120.
The programmed arc does not go through the defined end point (tolerance 0.01mm) or there is no arc that goes through the points defined by G08 or G09.
This error is issued when programming a tangential entry as in the following cases:
- There is no room to perform the tangential entry. A clearance of twice the rounding radius or greater is required.
042
- If the tangential entry is to be applied to an arc (G02, G03), The tangential entry must be defined in a linear block.
This error is issued when programming a tangential exit as in the following cases:
- There is no room to perform the tangential exit. A clearance of twice the rounding radius or greater is required.
043
044
045
046
047
048
049
- If the tangential exit is to be applied to an arc (G02, G03), The tangential exit must be defined in a linear block.
Polar origin coordinates (G93) defined incorrectly.
Not being used at this time.
Function G36, G37, G38 or G39 programmed incorrectly.
Polar coordinates defined incorrectly.
A zero movement has been programmed during radius compensation or corner rounding.
Not being used at this time.
Chamfer programmed incorrectly in a rectangular pocket or corner roughing operation in such way that:
* The tool cannot machine it because the chamfer is too small.
* A chamfer that big cannot be machined with those L, H, E parameter values
050 Functions M06, M22, M23, M24, M25 must be programmed alone in a block.
051 * A tool change cannot be performed without being in the change position.
052 * The requested tool is not in the magazine.
057
058
059
060
061
053
054
055
056
Not being used at this time.
There is no tape in the cassette reader or the reader head cover is open.
Parity error when reading or recording a cassette.
Not being used at this time.
Write-protected tape.
Sluggish tape transport.
Communication error between the CNC and the cassette reader.
Internal CNC hardware error. Consult with the Technical Service Department.
Battery error.
The memory contents will be kept for 10 more days (with the CNC off) from the moment this error occurs. The whole battery module located on the back must be replaced. Consult with the Technical Service Department.
Atention:
Due to danger of explosion or combustion, do not try to recharge the battery, do not expose it to temperatures higher than 100°C (232°F) and do not short the battery leads.
064 * External emergency input (pin 14 of connector I/O1) is activated.
065 Not being used at this time.
066 * X axis travel limit overrun.
It is generated either because the machine is beyond limit or because a block has been programmed which would force the machine to go beyond limits.
067 * Y axis travel limit overrun.
It is generated either because the machine is beyond limit or because a block has been programmed which would force the machine to go beyond limits.
068 * Z axis travel limit overrun.
It is generated either because the machine is beyond limit or because a block has been programmed which would force the machine to go beyond limits.
069 Not being used at this time.
070 ** X axis following error.
071 ** Y axis following error.
072 ** Z axis following error.
073 Not being used at this time.
074 ** Spindle speed value too large.
075 ** Feedback error at connector A1.
076 ** Feedback error at connector A2.
077 ** Feedback error at connector A3.
078 ** Feedback error at connector A4.
079 ** Feedback error at connector A5.
080 This error occurs when using a tool smaller than the machining pass "G" in a rectangular/circular pocket or in a corner roughing operation.
081 This error occurs when the tool radius is greater than "(L/2)-E" or "H/2)-E".
082 ** Parity error in general parameters.
083 This error occurs when programming "r>0" or "C>0" in a rectangular pocket or corner roughing operation.
084
085
086
This error occurs when programming a tool radius greater than "R-E" in a circular pocket.
This error occurs when using a 0-radius tool (tool offset) having programmed "G=0" (machining pass) in a rectangular/circular pocket or in a corner roughing operation.
This error occurs when assigning an incorrect value to an automatic operation or to a machining operation:
- Rectangular pocket ................ If P=0 or I=0
- Circular pocket ...................... If P=0 or I=0
- Corner roughing ..................... If P=0 or I=0
- Surface milling ...................... If P=0 or I=0
- Center punching: ................... If P=0, =0
- Drilling: ................................. If P=0 or I=0
- Tapping: ................................. If P=0
- Boring, reaming: .................... If P=0
087 ** Internal CNC hardware error. Consult with the Technical Service Department.
088 ** Internal CNC hardware error. Consult with the Technical Service Department.
089 * All the axes have not been homed.
This error comes up when it is mandatory to search home on all axes after power-up. This requirement is set by machine parameter.
090 ** Internal CNC hardware error. Consult with the Technical Service Department.
091 ** Internal CNC hardware error. Consult with the Technical Service Department.
092 ** Internal CNC hardware error. Consult with the Technical Service Department.
093 ** Internal CNC hardware error. Consult with the Technical Service Department.
094
095
Parity error in tool table or zero offset table G53-G59.
This error occurs when the tool radius is larger than the rounding radius "r" in a rectangular pocket or corner roughing operation.
096 ** Parity error in Z axis parameters.
097 ** Parity error in Y axis parameters.
098 ** Parity error in X axis parameters.
099 ** Parity error in M table.
100 ** Internal CNC hardware error. Consult with the Technical Service Department.
101 ** Internal CNC hardware error. Consult with the Technical Service Department.
105 This error comes up in the following cases:
> A comment has more than 43 characters.
> A program has been defined with more than 5 characters.
> A block number has more than 4 characters.
> Strange characters in memory.
106 ** Inside temperature limit exceeded.
107 Not being used at this time.
108 ** Error in Z axis leadscrew error compensation parameters.
109 ** Error in Y axis leadscrew error compensation parameters.
110 ** Error in X axis leadscrew error compensation parameters.
111
112
113
Not being used at this time.
Not being used at this time.
Not being used at this time.
114 Not being used at this time.
115 * Watch-dog error in the periodic module.
This error occurs when the periodic module takes longer than 5 milliseconds.
116 * Watch-dog error in the main module.
This error occurs when the main module takes longer than half the time indicated in machine parameter "P729".
117 * The internal CNC information requested by activating marks M1901 thru M1949 is not available.
118 * An attempt has been made to modify an unavailable internal CNC variable by means of marks M1950 thru
M1964.
119 Error when writing machine parameters, the decoded M function table and the leadscrew error compensation tables into the EEPROM memory.
120
This error may occur when after locking the machine parameters, the decoded M function table and the leadscrew error compensation tables, one tries to save this information into the EEPROM memory.
Checksum error when recovering (restoring) the machine parameters, the decoded M function table and leadscrew error compensation tables from the EEPROM memory.
Atention:
The ERRORS indicated with "*" behave as follows:
They stop the axis feed and the spindle rotation by cancelling the Enable signals and the analog outputs of the CNC.
hey interrupt the execution of the part-program of the CNC if it was being executed.
The ERRORS indicated with "**" besides behaving as those with an "*", they activate the
INTERNAL EMERGENCY OUTPUT.
FAGOR 800M CNC
PROGRAMMING MANUAL
Ref. 9701 (ing)
ABOUT THE INFORMATION IN THIS MANUAL
This manual should be used when elaborating an ISO-coded program.
This CNC can store 2 user-defined ISO-coded programs:
P99994 Special ISO-coded user program to store subroutines.
P99996 ISO-coded user Part-program.
Both programs may be written at a PC and sent out to the CNC. The Peripherals section of the
Operating Manual describes how to transfer information between the CNC and a PC.
P99996 may be edited at the CNC; but P99994 cannot be accessed from the CNC. It must be edited at a PC or peripheral device.
This manual describes all the information on the ISO code used by the 800M CNC.
Notes: The information described in this manual may be subject to variations due to technical modifications.
FAGOR AUTOMATION, S.Coop. reserves the right to modify the contents of the manual without prior notice.
INDEX
Section Page
Chapter 2 COORDINATE PROGRAMMING
Section Page
Chapter 6 ADDITIONAL PREPARATORY FUNCTIONS
Selection and activation of tool radius compensation (G41, G42) ................................. 2
Section Page
Chapter 8 MACHINING CANNED CYCLES
Inside rectangular pocket machining (G67 N1 & P202=K0) .......................................... 7
Outside rectangular pocket machining (G67 N2 & P202=K0) ........................................ 11
Chapter 10 PARAMETRIC PROGRAMMING
COMPARISON TABLE
FOR FAGOR 800M
CNC MODELS
AVAILABLE 800M CNC MODELS
X, Y axes control
Z axis as DRO
Controlled Z axis
Spindle
Tools
Tool Radius Compensation
Tool Length Compensation
Electronic Handwheels
RS 232C Communications
Integrated PLC (PLCI)
ISO-coded program editing
(P99996)
Execution of ISO-coded program (P99996)
Graphics
800-MG 800-MGI l l l l l l l l l l
99 l l
3 l l l l
99 l l
3 l l l
NEW FEATURES
AND
MODIFICATIONS
Date:
FEATURE them to "0".
July 1995
Clear all arithmetic parameter contents setting
ISO Programming.
Editing of program P99996 at the CNC.
When interrupting execution, the keys for the spindle, the coolant and for O1, O2, O3 and
TOOL are enabled.
Subroutine associated to the execution of a tool
(only when executing program P99996)
ISO codes of the 800T CNC
Software version: 2.1 and newer
AFFECTED MANUAL AND SECTION
Installation Manual
Operating Manual
Programming Manual
Section 3.9
Section 3.8&6.9
Installation Manual
Operating Manual
Installation Manual
Operating Manual
Operating Manual
Installation Manual
Programming Manual
Programming Manual
Section 3.10
Section 3.9
Section 3.5.1
Section 2.5.1
Section 6.5
Section 4.3
Chapter 9.
Date:
FEATURE
November 1995
Subroutines to be executed before and after the "T" function.
"M" functions associated with automatic operations.
"M" functions associated with machining operations.
Software version: 2.2 and newer
AFFECTED MANUAL AND SECTION
Installation Manual
Programming Manual
Operating Manual
Section 4.3
Chapter 9
Section 4.1.2
Operating Manual Section 5.1.1
INTRODUCTION
Introduction - 1
SAFETY CONDITIONS
Read the following safety measures in order to prevent damage to personnel, to this product and to those products connected to it.
This unit must only be repaired by personnel authorized by Fagor Automation.
Fagor Automation shall not be held responsible for any physical or material damage derived from the violation of these basic safety regulations.
Precautions against personal damage
Before powering the unit up, make sure that it is connected to ground
In order to avoid electrical discharges, make sure that all the grounding connections are properly made.
Do not work in humid environments
In order to avoid electrical discharges, always work under 90% of relative humidity
(non-condensing) and 45º C (113º F).
Do not work in explosive environments
In order to avoid risks, damage, do no work in explosive environments.
Precautions against product damage
Working environment
This unit is ready to be used in Industrial Environments complying with the directives and regulations effective in the European Community
Fagor Automation shall not be held responsible for any damage suffered or caused when installed in other environments (residential or homes).
Install the unit in the right place
It is recommended, whenever possible, to instal the CNC away from coolants, chemical product, blows, etc. that could damage it.
This unit complies with the European directives on electromagnetic compatibility.
Nevertheless, it is recommended to keep it away from sources of electromagnetic disturbance such as.
- Powerful loads connected to the same AC power line as this equipment.
- Nearby portable transmitters (Radio-telephones, Ham radio transmitters).
- Nearby radio / TC transmitters.
- Nearby arc welding machines
- Nearby High Voltage power lines
- Etc.
Ambient conditions
The working temperature must be between +5° C and +45° C (41ºF and 113º F)
The storage temperature must be between -25° C and 70° C. (-13º F and 158º F)
Introduction - 3
Protections of the unit itself
It carries two fast fuses of 3.15 Amp./ 250V. to protect the mains AC input
All the digital inputs and outputs are protected by an external fast fuse (F) of 3.15 Amp./
250V. against a voltage overload (greater than 33Vdc) and against reverse connection of the power supply.
Precautions during repair
Do not manipulate the inside of the unit
Only personnel authorized by Fagor Automation may manipulate the inside of this unit.
Do not manipulate the connectors with the unit connected to AC power.
Before manipulating the connectors (inputs/outputs, feedback, etc.) make sure that the unit is not connected to AC power.
Safety symbols
Symbols which may appear on the manual
WARNING. symbol
It has an associated text indicating those actions or operations may hurt people or damage products.
Symbols that may be carried on the product
WARNING. symbol
It has an associated text indicating those actions or operations may hurt people or damage products.
"Electrical Shock" symbol
It indicates that point may be under electrical voltage
"Ground Protection" symbol
It indicates that point must be connected to the main ground point of the machine as protection for people and units.
Introduction - 4
MATERIAL RETURNING TERMS
When returning the CNC, pack it in its original package and with its original packaging material. If not available, pack it as follows:
1.- Get a cardboard box whose three inside dimensions are at least 15 cm (6 inches) larger than those of the unit. The cardboard being used to make the box must have a resistance of 170 Kg (375 lb.).
2.- When sending it to a Fagor Automation office for repair, attach a label indicating the owner of the unit, person to contact, type of unit, serial number, symptom and a brief description of the problem.
3.- Wrap the unit in a polyethylene roll or similar material to protect it.
When sending the monitor, especially protect the CRT glass.
4.- Pad the unit inside the cardboard box with poly-utherane foam on all sides.
5.- Seal the cardboard box with packing tape or industrial staples.
Introduction - 5
FAGOR DOCUMENTATION
FOR THE 800M CNC
800M CNC OEM Manual Is directed to the machine builder or person in charge of installing and starting up the CNC.
It has the Installation manual inside. Sometimes, it may contain an additional manual describing New Software Features recently implemented.
800M CNC USER Manual Is directed to the end user or CNC operator.
It contains 2 manuals:
Operating Manual describing how to operate the CNC.
Programming Manual describing how to program the CNC.
Sometimes, it may contain an additional manual describing New Software
Features recently implemented.
DNC 25/30 Software Manual Is directed to people using the optional DNC communications software.
DNC 25/30 Protocol Manual Is directed to people wishing to design their own DNC communications software to communicate with the 800 without using the DNC25/30 software..
PLCI Manual To be used when the CNC has an integrated PLC.
DNC-PLC Manual
Is directed to the machine builder or person in charge of installing and starting up the PLCI.
Is directed to people using the optional communications software: DNC-PLC.
FLOPPY DISK Manual Is directed to people using the Fagor Floppy Disk Unit and it shows how to use it.
Introduction - 6
MANUAL CONTENTS
The programming manual consists of the following sections:
Index
Comparative Table for Fagor 800M CNC models
New Features and modifications
Introduction Safety Conditions
Material returning conditions
Fagor documents for the 800M CNC
Manual Contents
Chapter 1 Program writing
Structure of the part-program and of all its blocks
It shows the available preparatory G functions.
Chapter 2 Coordinate programming
It shows how to select the work planes, work units, type of programming (absolute / incremental)
It describes the coordinate systems for coordinate programming (Cartesian, polar, cylindrical, by means of angles, by means of an angle and a Cartesian coordinate).
Chapter 3 Reference systems
It shows how to program machine reference search and coordinate preset as well as the zero offsets and polar origin preset.
It indicates how to save the current coordinate origin and retrieve it later on.
Chapter 4 Other functions:
It shows how to program the preparatory functions regarding axis feedrate and spindle speed.
It indicates how to program the spindle turning speed.
It shows how to program the tool and how to modify the table values via user program.
It indicates how to program the auxiliary "M" functions.
Chapter 5 Path control
It describes how to program the part in square and round corner.
It shows how to program fast positioning, linear and circular interpolations.
It indicates how to program tangential entries and exits as well as corner rounding and chamfering.
Chapter 6 Additional Preparatory Functions
It shows how to program a dwell.
How to apply mirror image functions.
How to display an error code.
How to work with jumps and unconditional jumps.
How to apply the scaling factor.
How to apply pattern rotation.
How to program the single-block treatment.
Chapter 7 Tool compensation
It shows how to program tool radius and length compensation.
Chapter 8 Machining canned cycles
It shows how to program the different machining canned cycles.
Chapter 9 Subroutines.
Special user program for subroutines: P99994
It shows how to identify a standard and a parametric subroutine.
How to program a call to a standard or to a parametric subroutine.
It shows the subroutine nesting levels.
Chapter 10 Parametric programming
It shows how to use parametric programming (assignments, operators, jump functions, etc.)
Error codes
Introduction - 7
1.
PROGRAM WRITING
A CNC program consists of a series of blocks or instructions.
These blocks or instructions consist of words formed by capital letters, signs and numbers
The signs and numbers for this CNC are:
. + -
0 1 2 3 4 5 6 7 8 9
It is possible to program without a number when the value is zero and without the sign when it is positive.
When programming, the numbers of a word may be replaced with an arithmetic parameter.
Later on, during basic execution, the CNC will replace the arithmetic parameter with its value. For example:
If XP3 has been programmed, the CNC will replace P3 with its numeric value when executing this instruction obtaining a result such as X20, X20.567, X-0.003, etc.
1.1 CNC PROGRAM STRUCTURE
All program blocks (lines) of the program will have the following structure:
Block number + Block contents
Chapter: 1
PROGRAM WRITING
Section: Page
1
1.2 BLOCK NUMBER
The block number serves to identify each one of the program blocks.
It is expressed by the letter "N" followed by up to 4 digits (0-9999).
These program blocks must be in numerical order (N10, N15, N37, N46, etc.). It is recommended not to assign them sequential numbers (N10, N11, N12, N13, etc.) in order to be able to insert future blocks between them if so required.
Atention:
All throughout this manual, we will indicate an "N4" format when referring to a block number meaning that the "N" letter must be followed by up to 4digits (without decimals),
1.2.1 CONDITIONAL BLOCK (BLOCK SKIP)
There are two types of conditional blocks: a) REGULAR BLOCK SKIP: N4.
If the block number N4 is followed by a period (.), the block is set as a regular block skip. This means that the CNC will execute it only if the corresponding conditional
(block skip) input is activated.
When executing any program, the CNC reads four blocks ahead (look ahead) of the one currently in execution.
In order for the conditional block to be executed, the conditional input must be activated 4 blocks ahead of the conditional block.
b) SPECIAL CONDITIONAL BLOCK (BLOCK SKIP): N4..
If the block number N4 is followed by two periods (..), the block is set as a special block skip. This means that the CNC will execute it only if the corresponding conditional (block skip) input is activated.
In this case, the conditional input may be activated while executing the block before the conditional one.
The special conditional block N4.., cancels tool radius compensation G41 and G42.
Page
2
Chapter: 1
PROGRAM WRITING
Section:
BLOCK NUMBER
1.3 BLOCK CONTENTS
It must be written with commands in ISO language, especially designed to control the movements of the axes, since it provides information and positioning conditions as well as feedrate data.
Each program block may contain the following functions:
G Preparatory functions
X, Y, Z Coordinates (position values) of the axes
F
S
Feedrate
Spindle turning speed
T
M
Tool number
Auxiliary (miscellaneous) functions
This order must be maintained in the block although all these functions need not be in each block.
Depending on the selected work units (mm or inches), the following programming format must be used:
Millimeter format: N4 G2 X±4.3 Y±4.3 Z±4.3 F4 S4 T2.2 M2
Inch format: N4 G2 X±3.4 Y±3.4 Z±3.4 F4 S4 T2.2 M2
Parametric format: N4 GP?? XP?? YP?? ZP?? SP?? TP?? MP??
Throughout this manual the following formats will be mentioned and their meanings are:
"N4" Block (program line) number indicating that the letter "N" must be followed by up to 4 digits (N0 through N9999).
"G2"
± 4.3
Referring to a preparatory function indicating that the letter "G" must be followed by up to 2 digits (G0 through G99).
Meaning that a positive or negative number may follow the letter (X, Y or Z) by up to 4 integers and up to 3 decimals.
± 3.4
Meaning that a positive or negative number may follow the letter (X, Y or Z) by up to 3 integers and up to 4 decimals.
"F5.4" Axis feedrate in mm/min, indicating that the letter "F" must be followed by up to 5 integers and up to 4 decimals.
"F4.5" Axis feedrate in inches/min, indicating that the letter "F" must be followed by up to 4 integers and up to 5 decimals.
"S4" Referring to spindle speed, indicating that the letter "S" must be followed by up to 4 digits (S0 through S9999).
T2.2
Referring to the work tool, indicating that the letter "T" must be followed by up to 2 integers and two decimals.
"M2" Referring to the miscellaneous functions, indicating that the letter "M" must be followed by up to 2 digits (M0 through M99).
Chapter: 1
PROGRAM WRITING
Section:
BLOCK CONTENTS
Page
3
1.4 PREPARATORY FUNCTIONS (G)
These functions are programmed by means of the letter "G" followed by two digits (G2).
They are always programmed at the beginning of the block and they are used to set the geometry and operating conditions of the CNC.
1.4.1 "G" FUNCTION TABLE FOR THIS CNC
G30
G31
G32
G36
G37
G38
G39
G25
G26
G27
G28
G29
G20
G21
G22
G23
G24
G12
G13
G17
G18
G19
G07
G08
G09
G10
G11
Function M D
G00 * * Rapid positioning
G01 * Linear interpolation
G02
G03
G04
G05
G06
*
*
* *
Meaning
Clockwise circular interpolation
Counter-clockwise circular interpolation
Dwell
Round corner
Circular interpolation with absolute center coordinates
*
*
*
*
*
*
*
*
Square corner
Arc tangent to previous path
Arc defined by three points
Cancellation of mirror image
Mirror image on X
Mirror image on Y
Mirror image on Z
* * XY plane selection
* XZ plane selection
YZ plane selection
Call to a standard subroutine
Call to a parametric subroutine
Identification of a standard subroutine
Identification of a parametric subroutine
End of subroutine
Unconditional jump/call
Jump/Call if equal to 0
Jump/Call if not equal to 0
Jump/Call if smaller than
Jump/Call if equal to or greater than
Display error code
Store coordinate origin
Recover coordinate origin previously stored with G31
Automatic radius blend
Tangential entry
Tangential exit
Chamfer
6.3
3.5
3.5
5.10
5.8
5.9
5.11
6.4
10.6
10.6
10.6
10.6
9.3
9.5
9.2
9.4
9.
6.2
6.2
2.1
2.1
2.1
5.2
5.6
5.7
6.2
6.2
Section
5.3
5.4
5.5
5.5
6.1
5.1
5.5.2
Page
4
Chapter: 1
PROGRAM WRITING
Section:
PREPARATORY
FUNCTIONS (G)
G67 N0 P202=K0
G67 N0 P202=K1
G67 N0 P202=K2
G67 N0 P202=K3
G67 N0 P202=K4
G67 N1 P202=K0
G67 N1 P202=K1
G67 N2 P202=K0
G67 N2 P202=K1
G67 N3
G67 N4
G67 N6
G67 N7
G67 N8
G67 N9
G70
G71
G72
G73
G74
G90
G91
G92
G93
Function
G40
G41
G42
G43
G44
G47
G48
G49
G50
G53/G59
M D Meaning
* * Cancelation of tool radius compensation
*
*
*
Left-hand tool radius compensation
Right-hand tool radius compensation
Tool length compensation
* * Cancellation of tool length compensation
* Single-Block treatment: ON
* * Single-Block treatment: OFF
* Programmable feedrate override %
*
Load tool dimensions into tool offset table
Zero offsets
Point to point positioning canned cycle
Linear positioning canned cycle
Rectangular positioning canned cycle
Grid pattern positioning canned cycle
Arc positioning canned cycle
Inside rectangular pocket milling canned cycle
Inside circular pocket milling canned cycle
Outside rectangular pocket milling canned cycle
Outside circular pocket milling canned cycle
Surface milling canned cycle
Corner roughing canned cycle
Drilling canned cycle
Tapping canned cycle
Boring and reaming canned cycle
Center punching canned cycle
*
*
*
*
Inch programming
Metric programming (in mm)
Scaling factor
Pattern rotation
Machine Reference (Home) search
* * Programming in absolute coordinates
* Programming in incremental coordinates
Coordinate preset
Polar origin preset
"M" means MODAL. In other words, that once the "G" function has been executed, it remains active until another incompatible "G" function, M02, M30, EMERGENCY, or
RESET is executed or the CNC is turned off and back on.
8.6
8.7
8.8
8.9
8.1
8.2
8.3
8.4
8.5
8.10
8.11
8.12
8.13
8.14
8.15
2.3
2.3
3.2
3.3
2.2
2.2
6.5
6.6
3.1
Section
7.1.3
7.1.1
7.1.1
7.2
7.2
6.7
6.7
4.1.1
4.3.1
3.4
"D" means BY DEFAULT. That is, that they will be assumed by the CNC on power-up, after executing an M02, M30 or after an EMERGENCY or RESET. Machine parameter
"P613(5)" indicates whether G05 or G07 is assumed on power-up.
One block may contain all the desired "G" functions and in any order except: G20, G21,
G22, G23, G24, G25, G26, G27, G28, G29, G30, G31, G32, G50, G51, G53/G59, G72,
G74 and G92 which must be programmed alone in a block for being special. If incompatible "G" functions are programmed in the same block, the CNC assumes the last one.
Chapter: 1
PROGRAM WRITING
Section:
PREPARATORY
FUNCTIONS (G)
Page
5
2.
COORDINATE PROGRAMMING
2.1 PLANE SELECTION (G17, G18, G19)
G17 : XY plane selection
G18 : XZ plane selection
G19 : YZ plane selection
Plane selection must be used when performing circular interpolations, corner rounding, tangential entries and exits, chamfering, machining canned cycles, pattern rotations or when applying tool length and radius compensation.
The CNC applies tool radius compensation to both axes of the selected plane and tool length compensation to the axis perpendicular to that plane.
Functions G17,G18,G19 are modal and incompatible with each other.
On power-up, after executing M02, M30 or after an EMERGENCY or RESET, the CNC assumes function G17.
Chapter: 2
COORDINATE PROGRAMMING
Section:
PLANE SELECTION
G17, G18, G19
Page
1
2.2 MEASURING UNITS. MILLIMETERS (G71) OR INCHES (G70)
The CNC has machine parameter "P13" to set the measuring units to be used.
However, these units may be changed along the program by means of the following "G" functions:
G70 Programming in inches
G71 Programming in millimeters
Depending on whether G70 or G71 has been programmed, the CNC assumes those units for all the following blocks.
Functions G70/G71 are modal and incompatible with each other.
On power-up, after executing M02, M30 or after an EMERGENCY or RESET, the CNC assumes the measuring units set by machine parameter "P13".
Page
2
Chapter: 2
COORDINATE PROGRAMMING
Section:
MILIMETROS (G71)
PULGADAS (G70)
2.3 ABSOLUTE (G90) OR INCREMENTAL (G91) PROGRAMMING
The coordinates of a point may be programmed either in absolute, G90, or in incremental,
G91.
When working in G90, the coordinates of the programmed point are referred to the coordinate origin point (Part Zero).
When working in G91, the coordinates od the programmed point are referred to the end point (target point) of the previous block.
On power-up, after executing M02, M30 or after an EMERGENCY or RESET, the CNC assumes G90.
Functions G90 and G91 are modal and incompatible with each other.
Programming example.
Initial point (P0)
X20 Y10.
Absolute programming G90
N20 G90 X50 Y40
N30 Y10
N40 X20
Incremental programming G91
P0 ==> P1
P1 ==> P2
P2 ==> P0
N20 G91 X30 Y30
N30 Y-30
N40 X-30
P0 ==> P1
P1 ==> P2
P2 ==> P0
Chapter: 2
COORDINATE PROGRAMMING
Section:
ABSOLUTO (G90)
INCREMENTAL (G91)
Page
3
2.4 COORDINATE PROGRAMMING
With this CNC, it is possible to program the axis coordinates in the following formats:
- Cartesian coordinates
- Polar coordinates
- Cylindrical coordinates
- By giving two angles
- By giving an angle and a cartesian coordinate
2.4.1 CARTESIAN COORDINATES
Their programming format is:
In mm
In inches
X+/-4.3 Y+/-4.3 Z+/-4.3
X+/-3.4 Y+/-3.4 Z+/-3.4
The values of the programmed coordinates will be either absolute or incremental depending on whether G90 or G91 has been programmed.
Positive coordinate values do not require the "+" sign. Leading zeros as well as trailing decimal zeros may also be omittted (0010.100 = 10.1).
Programming example being (X0 Y0) the starting point.
Page
4
Absolute coordinates:
N10 G90 G01 X150.5 Y200
N20 X300
N30 X0 Y0
Incremental coordinates:
N10 G91 G01 X150.5 Y200
N20 X149,5
N30 X-300 Y-200
Chapter: 2
COORDINATE PROGRAMMING
Section:
CARTESIAN COORDINATES
2.4.2 POLAR COORDINATES
When working with polar coordinates, only movements in the plane can be carried out
(two axes at the same time).
Either cartesian or cylindrical coordinates must be programmed to move three axes at the same time.
The format to define a point in the plane with polar coordinates is:
In mm
In inches
R+/-4.3 A+/-3.3
R+/-3.4 A+/-3.3
Where "R" is the radius of the arc and "A" is the angle (always in degrees) referred to the polar origin.
The "R" and "A" values will be either absolute or incremental depending on whether G90 or G91 is active.
For circular interpolations (G02 or G03), program the angle A±3.3 and the coordinates of the center referred to the starting point of the arc.
When the center of the arc is also the polar origin, the center coordinates need not be programmed, programming just the angle is enough.
Atention:
On power up, after M02, M30, EMERGENCY or RESET, the CNC assumes point X0 Y0 as the polar origin.
Every time a new main plane is selected during program execution, the origin point of the new plane becomes the polar origin
When programming G18, point X0 Y0 will be the polar origin point and with
G19 it will be point Y0 Z0.
When executing a circular interpolation with G02 or G03, the arc center becomes the new polar origin.
With function G93, it is possible to select any point in the plane as polar origin.
Chapter: 2
COORDINATE PROGRAMMING
Section:
POLAR COORDINATES
Page
5
DIRECTION AND SIGN OF THE ANGLES
XY Plane
XZ Plane
P605(4)=1
XZ Plane
P605(4)=0
YZ Plane
Page
6
Chapter: 2
COORDINATE PROGRAMMING
Section:
POLAR COORDINATES
Example:
The tool starts out at X0 Y0
N0 G93 I20 J20
N5 G01 G90 R5 A180 F150
N10 G02 A75
N15 G01 G91 R5
N20 G02 A-15
N25 G01 R10
N30 G03 A15
N35 G01 R10
N40 G02 A-50
N45 G01 R-10
N50 G03 A15
N55 G01 R-10
N60 G02 A-15
N65 G01 R-5
N70 G02 G90 A180
N75 G01 X0 Y0
Chapter: 2
COORDINATE PROGRAMMING
Section:
POLAR COORDINATES
Page
7
2.4.3 CYLINDRICAL COORDINATES
A point in the space can be defined by:
X Y Z cartesian coordinate values or in cylindrical coordinates.
The format to define cylindrical coordinates of a point is as follows:
Operating in G17 (plane XY): N10 G01 R.. A.. Z.
Where R,A define the projection of the point on the main plane in polar coordinates and
Z is the value of the coordinate Z at that point.
The format for G18 (plane XZ) is: N10 G01 R... A...Y
and for G19 (plane YZ) is: N10 G01 R...A...X
Page
8
Chapter: 2
COORDINATE PROGRAMMING
Section:
CYLINDRICAL
COORDINATES
2.4.4.
PROGRAMMING BY TWO ANGLES (A1,A2)
An intermediate point can also be identifieD by using: A1, A2 XY (YZ or XZ) where:
A1 is the esit angle from the starting point (P0).
A2 is the exit angle from the intermediate point (P1).
XY (YZ or XZ) are the coordinates of the end point P2, depending on the working plane.
The CNC calculates automatically the coordinates of P1.
Example:
Starting point is X0 Y0
N10 X20 Y10 (Coordinates of P0)
N20 A45 A30 (Exit angle of P0 and P1)
N30 X70 Y50 (Coordinates of P2)
Chapter: 2
COORDINATE PROGRAMMING
Section:
BY TWO ANGLES (A1, A2)
Page
9
2.4.5 BY ONE ANGLE AND ONE CARTESIAN COORDINATE
A point in the main plane can also be defined by the exit angle of the path in the previous point and one cartesian coordinate of the point which is to be defined.
Programming example being P0 (X10 Y20) the starting point:
N10 A45 X30 ; (Point P1)
N20 A90 Y60 ; (Point P2)
N30 A-45 X50 ; (Point P3)
N40 A-135 Y20 ; (Point P4)
N50 A180 X10 ; (Point P0)
When defining the points of a path, with two angles or one angle and one coordinate, roundings, tangential approaches and exists can be inserted.
Compensated path
Programmed path
Starting point X0 Y0 and tool’s radius T1=5 mm.
N100 T1.1
N110 G37 R10 G41 X20 Y20
N120 G39 R5 A90 A0
N130 X50 Y60
N140 G36 R7 A-45 X70
N150 G39 R10 A45 A-90
N160 G36 R10 X100 Y20
N170 G38 R10 X20
N180 G40 X0 Y0
N190 M30
Page
10
Chapter: 2
COORDINATE PROGRAMMING
Section:
ANGLE & ONE
CARTESIAN COORDINATE
3.
REFERENCE SYSTEMS
3.1 MACHINE REFERENCE (HOME) SEARCH (G74)
When programming G74 in a block, the CNC moves the axes to the machine reference point (home).
Two cases may occur: a) Search on all the axes.
If the block only contains G74, the CNC first moves the axis perpendicular to the selected plane, that is:
The Z axis when in G17, the Y axis when in G18 and the X axis when in G19.
It then moves the axis of the plane.
b) Search on one axis only or on both axes in a particular order.
To home only one axis, indicate the desired axis after function G74.
To home both axes; but in a particular order, other than the one described in a), program G74 followed by the axes in the desired order.
A block containing G74 cannot have any other function.
When the homing axis (or axes) reaches home, the screen displays the distance from that point to the last programmed part zero.
Chapter: 3
REFERENCE SYSTEMS
Section:
MACHINE REFERENCE
(HOME) SEARCH (G74)
Page
1
3.2 COORDINATE PRESET (G92)
By means of function G92, it is possible to preset any value for the CNC axes which translates into being able to apply any zero offset.
When programming function G92, the axes do not move and the CNC assumes the axis values programmed after G92 as the new coordinates for those axes.
Programming format: N4 G92 X Y Z .
Programming example with X0 Y0 as the starting point:
Without using function G92:
N10 G00 G90 X100 Y100
N20 X400
Using function G92:
N10 G92 X500 Y500
N20 G00 G90 X600 Y600
N30 X900
(Point P0 now becomes point X500 Y500)
The block containing G92 cannot have any other function.
The coordinate preset by G92 always refers to the current theoretical position of the axes.
Page
2
Chapter: 3
REFERENCE SYSTEMS
Section:
COORDINATE PRESET (G92)
3.3 POLAR ORIGIN PRESET (G93)
By means of function G93, it is possible to preset any point as the origin of polar coordinates.
There are two ways to preset a polar origin.
a) By setting the coordinates of the polar origin.
Format N4 G93 I±4.3 J±4.3 in mm
N4 G93 I±3.4 K±3.4 in inches
N Block number
I
G93 Polar origin presetting code
Abscissa value of the polar origin, X value (always an absolute value). That
J is, the X value for the XY and XZ planes and the Y value for the YZ plane.
Ordinate value of the polar origin, Z value (always an absolute value). That is, the Y value for the XY plane and the Z value for the XZ and YZ planes.
When using this polar origin presetting method, the CNC does not admit any other information in the same block.
b) By assuming the current point as the new polar origin.
If in any block, a G93 is also programmed, it will mean that the new origin point will be the current position before moving the axes to the position programmed in that block.
Atention:
When programming a circular interpolation with G02, G03, the CNC assumes the center of the arc as the new polar origin.
When switching main planes, the CNC assumes the cartesian coordinate origin of the new main plane as the new polar origin. That is, X0 Y0 with
G17, X0 Z0 with G18 and Y0 Z0 with G19.
On power-up or after an M02, M30, EMERGENCY or RESET, the CNC assumes the X0,Y0 point as the polar origin.
Next, two programming examples are being shown.
Chapter: 3
REFERENCE SYSTEMS
Section:
POLAR ORIGIN PRESET
(G93)
Page
3
Programming example being X0 Y0 the starting point:
P o l a r origin
N0 G93 I200 J0
N5 G01 R150 A90 F500
Point X200 Y0 has been defined as polar origin.
Linear interpolation (G01) up to point X200 Y150
Programming example being X0 Y0 the starting point:
P1
P2
Polar origin
N0 G93 G01 R200 A135 F500 Point X0 Y0 is now the polar origin and move to P1
N5 R100 A90 Move in G01 to P2.
Page
4
Chapter: 3
REFERENCE SYSTEMS
Section:
POLAR ORIGIN PRESET
(G93)
3.4 ZERO OFFSETS (G53...G59)
By means of functions G53, G54, G55, G56, G57, G58 and G59, it is possible to operate with 7 different zero offsets. These offset values are stored in the CNC memory and are referred to machine reference zero (home).
To access the zero offset table (G53-G59), press
Once the table is displayed, it is possible to clear all the offsets by pressing:
Functions G53-G59 must be used to load a zero offset into the table or to apply one of them on the running program.
Loading a zero offset into the table.
Absolute value loading. To load the values set by X, Y, Z into the desired table address
(G53-G59).
Format: N4 G53-G59 X±4.3 Y ±4.3 Z±4.3 in mm,
N4 G53-G59 X±3.4 Y ±3.4 Z±3.4 in inches.
N Block number
G Zero offset code (G53 through G59)
X X axis zero offset value, referred to home.
Y Y axis zero offset value, referred to home.
Z Z axis zero offset value, referred to home.
Incremental value loading. To increment the existing zero offset values (G53/G59) by a set amount (I, J, K).
Format: N4 G53-G59 I±4.3 J±4.3 K±4.3 in mm,
N4 G53-G59 I±3.4 J±3.4 K±3.4 in inches.
N Block number
G Zero offset code (G53 through G59)
I Amount to be added to the previously stored X axis zero offset value
I Amount to be added to the previously stored Y axis zero offset value
K Amount to be added to the previously stored Z axis zero offset value
Apply a particular pre-defined zero offset onto the running program.
Format: N4 G53-G59
It applies a zero offset, according to the values stored at the indicated table address
(G53-G59) onto the program currently in execution.
Chapter: 3
REFERENCE SYSTEMS
Section:
ZERO OFFSET (G53...G59)
Page
5
Programming example where the starting point X0 Y0 is also part zero.
N1 G53 X0 Y0 ..................................... Load G53 zero offset into the table
N2 G54 X-40 Y-40 .............................. Load G54 zero offset into the table
N3 G55 X-30 Y10 ............................... Load G55 zero offset into the table
N10 G0 G90 X70 Y20
N20 G1 Y35 F200
N30 X60
N40 G03 X60 Y20 I0 J-7,5
N50 G01 X70 Y20
N60 G54 ................................................ Applies G54
N70 G25 N10.50.1
N80 G55 ................................................ Applies G55
N90 G25 N10.50.1
N100 G53 ................................................ Applies G53 recovering the first part zero.
N110 X0 Y0
N120 M30
Page
6
Chapter: 3
REFERENCE SYSTEMS
Section:
ZERO OFFSET (G53...G59)
3.5 STORE AND RETRIEVE CURRENT PART ZERO (G31, G32)
G31 : Store current Part Zero.
G32 : Retrieve Part Zero previously stored by means of G31.
With G31, it is possible to store the current part zero at any time and retrieve it later on by using function G32.
This feature may prove useful whenever it is necessary to utilize several part zeros in the same program since it allows to dimension part of the program with respect to one zero, store it with G31, change the part zero with G92 or G53-G59, dimension it with respect to the new part zero and, finally, recover the initial part zero with G32.
Functions G31 and G32 must be programmed alone in the block. Their format is:
N4 G31 Store current Part Zero
N4 G32 Retrieve Part Zero previously stored by means of G31.
Programming example assuming that the tool is at X0 Y0 Z5:
N10 G00 G90 X-50 Y50
N20 G20 N1.1
N30 X60 Y110
N40 G20 N1.1
N50 X35 Y-90
N60 G20 N1.1
N70 M30
Position at the center of operation Nr.1
Run basic operation (subroutine N1)
Position at the center of operation Nr. 2
Run basic operation (subroutine N1)
Position at the center of operation Nr. 3
Run basic operation (subroutine N1)
End of program.
Chapter: 3
REFERENCE SYSTEMS
Section:
STORE AND RETRIEVE
PART ZERO (G31, G32)
Page
7
N100 G22 N1
N110 G31
N120 G92 X0 YO
N130 G1 Z-20 F350
N140 X— Y—
N—-
N—-
N—-
N—-
N—-
N200 G0 Z5
N210 G32
N220 G24
Basic operation (define subroutine N1)
Store current origin point (part zero)
Recover pre-stored part zero.
End of basic operation. End of subroutine.
Page
8
Chapter: 3
REFERENCE SYSTEMS
Section:
STORE AND RETRIEVE
PART ZERO (G31, G32)
4.
OTHER FUNCTIONS
4.1 FEEDRATE PROGRAMMING (F)
The axis feedrate is programmed with the letter "F" and its value depends on the currently selected work units, millimeters or inches, and type of feedrate, G94 or
G95.
Metric programming:
Format
Programming units
Minimum value Maximum value
F 5.4
F1= 1mm/min F0.0001 (0.0001 mm/min) F65535.000 (63535 mm/min)
Inch programming:
When operating in inches, we recommend setting machine parameter P615(6) to "1" so the programming units in G94 are in inches/minute.
P615(6) = 0 Programming format F1 = 0.1 inch/min.
Maintaining compatibility with older versions which did not accept decimal feedrate values.
P615(6) = 1 Programming format F1 = 1 inch/min.
P615(6)
P615(6)=0
P615(6)=1
Format
F 5.4
F 5.4
Programming units
Minimum value Maximum value
F1= 0.1 inch/min
F1= 1 inch/min
F0.001
(0.0001 inch/min)
F0.0001
(0.0001 inch/min)
F25801.1810
(2580.1181 inch/min)
F25801.1810
(25801.1810 inch/min)
The machine’s actual maximum feedrate may be limited to a lower value (see instruction book of the machine).
The machine’s maximum working feedrate can be programmed directly or by using code
F0.
Example: On a machine with a maximum programmable working feedrate of 10,000 mm/ min. it makes no difference whether F10.000 or F0 is programmed.
The programmed feedrate F is effective when operating on linear interpolation (G01) or circular interpolation (G02/G03). When not programming an F value, the CNC will assume F0. When in rapid positioning (G00), the machine will move in rapid regardless of the F programmed.
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
FEEDRATE PROGRAMMING
(F)
Page
1
The rapid traverse is set for each axis during the final adjustment of the machine, the maximum possible value being 65.535 m/min. (See instruction book of the machine).
The programmed feedrate can be varied between 0% and 120% or between 0% and 100% according to P606(2) by means of the knob on the front panel of the CNC. When G47 is active, this knob is cancelled and the operation is carried out at 100% of the programmed
F.
4.1.1 PROGRAMMABLE FEEDRATE OVERRIDE (G49)
By means of function G49, it is possible to indicate the override % to be applied on to the programmed feedrate.
When G49 is active, the Manual Feedrate Override switch of the operator panel has no effect. The programming format is: G49 K (1/120)
"G49 K" is followed by the % amount to be applied as feedrate override which must be an integer between 1 and 120.
Function G49 is modal; that is, once the % has been programmed, it is maintained until another % value is programmed or this function is cancelled.
To cancel this function, program either "G49 K" or G49 alone.
This function is also cancelled when executing an M02, M30, RESET or EMERGENCY.
Function G49 K must be programmed alone in the block.
Page
2
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
FEEDRATE PROGRAMMING
(F)
4.2 SPINDLE SPEED (S)
The spindle speed is programmed directly in rpm by means of the "S4" code.
Any integer value (non-decimal) between S0 and S9999 may be programmed. This maximum value is limited by the actual maximum value set for each particular machine by the corresponding machine parameter.
Consult the instructions manual for your particular machine.
The programmed spindle speed may be varied between 50% and 120% by the corresponding keys of the CNC front panel.
When tapping or while function G47 is active, these keys are ignored (being the override value set at 100% of the programmed spindle speed S)
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
SPINDLE SPEED (S)
Page
3
4.3 TOOL PROGRAMMING (T)
This CNC offers a table of up to 100 tools (00-99) for tool radius and tool length compensation.
The tool to be used is programmed by means of code: T2.2
The two digits to the left of the decimal point indicate the tool number to be selected.
The two decimals indicate the tool offset number to be applied.
Up to 100 tools (T0 through T99) and 100 tool offsets (Txx.0 through Txx.99) may be programmed.
The "T" function may be programmed in the following ways:
T2.2
The CNC selects the indicated tool and assumes the values of the indicated tool offset.
T2 The CNC selects the indicated tool and assumes the values of the same offset number as the indicated tool number. For example, "T19.19" may also be programmed as "T19".
T.2
The CNC does not change the tool but assumes the values of the indicated tool offset number.
When programming G41 or G42, the CNC applies, as radius compensation, the corresponding "R+I" value stored in the tool offset table (T00-T99).
When programming G43, the CNC applies, as tool length compensation, the corresponding
"L+K" value stored in the tool offset table (T00-T99).
If no "T" has been programmed, the CNC applies the "T00" values corresponding to a tool with zero dimensions.
Each address of the tool offset table contains the following fields:
R Tool radius
L Tool length
±1000.000 mm (±39.3700 inches).
±1000.000 mm (±39.3700 inches).
I Tool radius wear ±32.766 mm
K Tool length wear ±32.766 mm
(±1.2900 inches).
(±1.2900 inches).
Atention:
If the manufacturer has associated a subroutine with the T function, nothing must be programmed after the T function; otherwise, the CNC will issue the corresponding error.
If the manufacturer has not associated any subroutine to the T function, every time a new tool is selected, the CNC outputs the code of the new tool, displays the message "TOOL CHANGE" (in English for all languages) and interrupts the execution of the program.
Page
4
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
TOOL PROGRAMMING (T)
4.3.1 LOADING TOOL DIMENSIONS INTO TOOL OFFSET TABLE
(G50)
The different tool values can be entered in the table by using G50. There are two possibilities: a) Loading all the values.
It is possible to load the tool dimensions without having to do it by hand.
Metric format: N4 G50 T2 R±4.3 L±4.3 I±2.3 K±2.3.
Inch format: N4 G50 T2 R±2.4 L±2.4 I±1.4 K±1.4.
The values defined by R, L, I, K are loaded in the tool offset table address identified by T2.
I
N4 - Block number
G50 - Tool offsets loading code
T
R
- Tool offset table address (position)
- Tool radius
- Tool radius wear
L
K
- Tool length
- Tool length wear
The values of R, L, I, K replace the values previously existing in the T2 address
(position). If R and L are programmed and I, K are not, previous R and L values are replaced by the new ones. The correction values I, K are set to zero.
b) Incremental modification of the I, K values.
It is possible to compensate for tool wear as they occur.
In metric:
In inches:
N4 G50 T2 I±2.3 K±2.3.
N4 G50 T2 I±1.4 K±1.4.
The I,K values of the T2 address are modified.
N4 - Block number
G50 - Tool offsets loading code
I
T2 - Tool offset table address
- Value to be added to or subtracted from the I value previously recorded.
K - Value to be added to or subtracted from the K value previously recorded.
Atention:
A block containing the G50 code may not have any other type of information.
The tool radius compensation value will be R+I.
The tool length compensation value will be L+K.
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
TOOL PROGRAMMING (T)
Page
5
4.4 MISCELLANEOUS FUNCTIONS (M)
The miscellaneous functions are programmed by means of the "M2" code.
Up to 96 different miscellaneous functions (M00 through M99) may be programmed except for M41, M42, M43, M44 implicit with the "S" code
The miscellaneous functions will be output either in BCD code (M00/M99) or in binary code (M00/M254) depending on the setting of machine parameter P617(8).
The CNC also has 15 decoded outputs for miscellaneous functions. These outputs will be assigned to the required functions during the final adjustment of the CNC to the machine.
The miscellaneous functions which are not assigned a decoded output are always performed at the beginning of the block in which they are programmed.
In assigning a decoded output to a miscellaneous functions, a decision is also made as to whether it is to be performed at the beginning or at the end of the block in which it is programmed. Up to a maximum of seven miscellaneous functions may be programmed in one block.
When more than one miscellaneous function is programmed in a block, the CNC executes them consecutively in the order in which they are programmed.
Some of these miscellaneous functions have an internal meaning assigned to them in the
CNC.
M00. PROGRAM STOP
When the CNC reads code M00 in a block, it halts the program. Press the Cycle Start key to continue.
It is recommended that this function be set in the table of decoded M functions so that it is executed at the end of the block in which it is programmed (see Installation and Start up Manual).
M01. CONDITIONAL PROGRAM STOP
Same as M00 except that the CNC only takes it into account if the conditional stop input
(block skip) is activated.
M02. END OF PROGRAM
This code indicates end of program and performs a general reset function of the CNC (reset to initial conditions). It also acts as an M05.
As in the case of M00, it is recommended that this function be set so that it is executed at the end of the block in which it is programmed.
M30. END OF PROGRAM WITH RETURN TO THE BEGINNING
Same as M02 except that the CNC goes back to the first block at the beginning of the program. It also acts as an M05.
If machine parameter P609(3)=0, the CNC will output an M30 every time a RESET is carried out.
Page
6
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
MISCELLANEOUS
FUNCTIONS (M)
M03. CLOCKWISE START OF THE SPINDLE
It is recommended that this function be set so that it is executed at the beginning of the block in which it is programmed.
M04. COUNTER-CLOCKWISE START OF THE SPINDLE
Same as M03 except that the spindle rotates in the opposite direction.
M05. SPINDLE STOP
It is recommended that this be set so that the CNC executes it at the end of the block in which it is programmed.
M10, M11.
ASSOCIATED TO EXTERNAL DEVICE O1.
M12, M13.
ASSOCIATED TO EXTERNAL DEVICE O2.
M14, M15.
ASSOCIATED TO EXTERNAL DEVICE O3.
Codes associated to the keys corresponding to the external devices "O1", "O2" and "O3".
Codes M10, M12 and M14 activate their corresponding outputs and codes M11, M13 and
M15 deactivate them.
Chapter: 4
ADDITIONAL FUNCTIONS
Section:
MISCELLANEOUS
FUNCTIONS (M)
Page
7
5.
PATH CONTROL
5.1 ROUND CORNER (G05)
When operating in G05, the CNC starts executing the next block of the program as soon as the axes start decelerating to reach the target position programmed in the previous block.
Therefore, the movements programmed in the next block are executed before the axes reach their target position programmed in the previous block.
Programming example being X50,Y30 the starting point.:
N100 G91 G01 G05 Y70 F100
N110 X90
As seen in the example, the corners appear rounded.
The difference between the theoretical path and the real one depends on the actual axis feedrate.
The greater the feedrate, the greater the difference is between the theoretical and real paths
(greater radius).
Function G05 is modal and incompatible with G07. Function G05 may also be programmed as G5.
5.2 SQUARE CORNER (G07)
When operating in G07, the CNC starts executing the next block of the program once the axes have reached their target position programmed in the previous block.
Programming example being X50,Y30 the starting point.:
N100 G91 G01 G05 Y70 F100
N110 X90
The theoretical and real path are the same.
Function G07 is modal and incompatible with
G05. Function G07 may also be programmed as
G7.
On power-up, after executing M02, M30, an EMERGENCY or RESET, the CNC assumes
G07 if machine parameter P613(5)=1 and G05 if P613(5)=0.
Chapter: 5
PATH CONTROL
Section:
ROUND CORNER (G05)
SQUARE CORNER (G07)
Page
1
5.3 RAPID POSITIONING (G00)
Movements programmed after G00 are carried out at the maximum speed set by the corresponding machine parameters.
When two axes move simultaneously, the resulting path is a straight line from the beginning point to the end point at the feedrate of the slower axis.
When programming G00, the last programmed F is not canceled. Therefore, when programming G01, G02 or G03 afterwards, the CNC recovers that F and applies it.
Machine parameter P4 determines whether the Manual Feedrate Override (MFO) is ignored being fixed at 100% or not, thus being able to apply between 0% and 100% override.
"G00" is modal and incompatible with G01, G02, G03 and G33.
"G00" may also be programmed as "G" or "G0".
On power-up, after executing M02, M30, an EMERGENCY or RESET, the CNC assumes
G00.
Page
2
Chapter: 5
PATH CONTROL
Section:
RAPID POSITIONING (G00)
5.4 LINEAR INTERPOLATION (G01)
When executing a G01, the programmed axes move in a straight line from the starting point to the end point at the programmed Feedrate "F".
The CNC calculates the feedrate for each axis so the resulting straight path is carried out at the programmed "F".
Programming example with X150 Y150 as the starting point:
N100 G90 G01 X650 Y400 F150
By means of the "MFO" on the CNC keyboard, it is possible to override the programmed
"F" between 0% and 120% or between 0% and 100% depending on the setting of machine parameter P606(2).
If machine parameter "P606(2)=0", while keeping the rapid jog key: the CNC applies 200% of the programmed "F" to a G01 move.
p r e s s e d ,
The same thing occurs when activating the external CYCLE START input if machine parameter P609(7)=1.
"G01" is modal and incompatible with G00, G02 and G03.
"G01" may also be programmed as "G1".
On CNC power-up, after executing an M02/M30, after an EMERGENCY or RESET, the
CNC assumes "G00".
Chapter: 5
PATH CONTROL
Section:
LINEAR INTERPOLATION
(G01)
Page
3
5.5 CIRCULAR INTERPOLATION (G02, G03)
G02: Clockwise circular interpolation.
G03: Counter-clockwise circular interpolation.
Movements programmed after a G02 or G03 follow a circular path at the programmed feedrate.
The clockwise (G02) and counter-clockwise (G03) directions have been defined according to the following coordinate system:
This coordinate system is referred to the movement of the tool over the part.
The direction of G02 and G03 on the XZ plane can be changed by means of parameter
P605(4).
If the direction of the axes is changed, the directions of G02 and G03 are reversed.
Page
4
Chapter: 5
PATH CONTROL
Section:
CIRCULAR
INTERPOLATION (G02, G03)
The programming format for a circular interpolation in cartesian coordinates is:
XY plane
XZ plane
YZ plane
G17 G02 (G03) X±4.3 Y±4.3 I±4.3 J±4.3 F5.4
G18 G02 (G03) X±4.3 Z±4.3 I±4.3 K±4.3 F5.4
G19 G02 (G03) Y±4.3 Z±4.3 J±4.3 K±4.3 F5.4
Where: X X coordinate of the arc's end point..
Y Y coordinate of the arc's end point..
Z Z coordinate of the arc's end point..
I Distance, along X, from the starting point to the arc center.
J Distance, along Y, from the starting point to the arc center.
K Distance, along Z, from the starting point to the arc center.
Parameters I, J, K must always be defined, even when their values are 0.
The programming format for a circular interpolation in polar coordinates is:
XY plane
XZ plane
XZ plane
G17 G02 (G03) A±3.3 I±4.3 J±4.3 F5.4
G18 G02 (G03) A±3.3 I±4.3 K±4.3 F5.4
G19 G02 (G03) A±3.3 J±4.3 K±4.3 F5.4
Where: A Angle of the arc's end point with respect to the its center.
I Distance, along X, from the starting point to the arc center.
J Distance, along Y, from the starting point to the arc center.
K Distance, along Z, from the starting point to the arc center.
Parameters I, J, K must always be defined, even when their values are 0.
The CNC takes the arc’s center as the new polar origin when carrying out a G02,G03 circular interpolation.
The knob on the front panel of the CNC (M.F.O.) can be used to vary the programmed feedrate F between 0% and 120% or between 0% and 100%, according to parameter
P606(2).
If during a G02/G03 movement a Rapid Feed key is pressed, the movement will be performed at twice the programmed feedrate if P606(2) is zero. The same thing will happen when the external START input is activated if P609(7) is one.
Chapter: 5
PATH CONTROL
Section:
CIRCULAR
INTERPOLATION (G02, G03)
Page
5
Example 1:
CARTESIAN COORDINATES
G17 G02 G91 X26 Y26 I18 J8 G17 G02 G91 X26 Y-26 I8 J-18
POLAR COORDINATES
G17 G02 G91 A-138 I18 J8 G17 G02 G91 A- 138 I8 J-18
Example 2:
Cartesian coordinates:
N5 G90 G17 G03 X110 Y90 I0 J50 F150
N10 X160 Y40 I50 J0
Page
6
Chapter: 5
PATH CONTROL
Section:
CIRCULAR
INTERPOLATION (G02, G03)
Polar coordinate values: N5 G90 G17 G03 A0 I0 J50 F150
N10 A-90 I50 J0 or N5 G91 G17 G03 A90 I0 J50 F150
N10 A90 I50 J0 or or
N5 G93 I60 J90
N10 G90 G17 G03 A0 F150
N15 G93 I160 J90
N20 A-90
N5 G93 I60 J90
N10 G91 G17 G03 A90 F150
N15 G93 I160 J90
N20 A90
Example 3: Single block programming of a full circle.
Assuming that the starting point is X170 Y80
Cartesian coordinate values: N5 G90 G17 G02 X170 Y80 I-50 J0 F150
Polar coordinate values: or
N5 G90 G17 G02 A360 I-50 J0 F150
N5 G93 I120 J80 (Definition of polar centre)
N10 G17 G02 A360
Chapter: 5
PATH CONTROL
Section:
CIRCULAR
INTERPOLATION (G02, G03)
Page
7
5.5.1 CIRCULAR INTERPOLATION BY PROGRAMMING THE ARC
RADIUS
Format in mm: XY plane: G17 G02 (G03) X+/-4.3 Y+/-4.3 R+/-4.3 F5.4
XZ plane: G18 G02 (G03) X+/-4.3 Z+/-4.3 R+/-4.3 F5.4
YZ plane: G19 G02 (G03) Y+/-4.3 Z+/-4.3 R+/-4.3 F5.4
Format in inches: XY plane: G17 G02 (G03) X+/-3.4 Y+/-3.4 R+/-4.3 F4.5
XZ plane: G18 G02 (G03) X+/-3.4 Z+/-3.4 R+/-4.3 F4.5
YZ plane: G19 G02 (G03) Y+/-3.4 Z+/-3.4 R+/-4.3 F4.5
Where: G02(G03) Circular interpolation code
X X coordinate of the end point
Y
Z
R
Y coordinate of the end point
Z coordinate of the end point
Radius of the arc
This means that the circular interpolation may be programmed by means of the end point and the arc radius instead of the arc center coordinates (I, K).
When the arc is smaller than 180º, the radius must be programmed with a positive sign and with negative sign if otherwise.
Considering P0 as the starting point of the arc and P1 as the end point, four different arcs may be defined with the same radius.
Depending on the direction of the circular interpolation G02 or G03 and the sign of the radius, the resulting arc programming formats are:
Arc 1 G02 X Y R -
Arc 2 G02 X Y R +
Arc 3 G03 X Y R +
Arc 4 G03 X Y R -
Atention:
If a complete circle is programmed using any of these four formats, the CNC will issue error 47 indicating that there are infinite solutions.
Page
8
Chapter: 5
PATH CONTROL
Section:
CIRCULAR
INTERPOLATION (G02, G03)
5.5.2 CIRCULAR INTERPOLATION WITH ABSOLUTE CENTER
COORDINATES (G06)
By adding function G06 to a block containing a circular interpolation, it is possible to use absolute coordinates for the arc center (I, J, K); that is, with respect to the part zero and not referred to the arc's starting point.
"G06" is NOT MODAL. Therefore, it must be programmed every time the arc center coordinates are to be absolute.
Programming example where X60 Y40 is the starting point:
Circular interpolation by programming the radius.
N5 G90 G17 G03 X110 Y90 R50 F150
N10 X160 Y40 R50
Circular interpolation by programming the center in absolute coordinates:
N5 G90 G17 G06 G03 X110 Y90 I60 J90 F150
N10 G06 X160 Y40 I160 J90
Chapter: 5
PATH CONTROL
Section:
CIRCULAR
INTERPOLATION (G02, G03)
Page
9
5.5.3 HELICAL INTERPOLATION
Helical interpolations can be programmed by using G02/G03. Helical interpolation is defined as a circular interpolation on the main plane plus a simultaneous synchronized linear movement on the third axis. It is programmed as follows:
Cartesian coordinates
XY plane G02 (G03) X+/-4.3 Y+/-4.3 I+/-4.3 J+/-4.3 Z+/-4.3 K4.3 F5.4
XZ plane G02 (G03) X+/-4.3 Z+/-4.3 I+/-4.3 K+/-4.3 Y+/-4.3 J4.3 F5.4
YZ plane G02 (G03) Y+/-4.3 Z+/-4.3 J+/-4.3 K+/-4.3 X+/-4.3 I4.3 F5.4
In the XY plane: XY. Coordinate values of the arc’s final point.
IJ.
Center coordinates referred to the arc’s initial point.
Z.
Final position on the Z axis.
K.
Helical pitch on the Z axis.
Polar coordinates
XY plane G02 (G03) A+/-3.3 I+/-4.3 J+/-4.3 Z+/-4.3 K4.3 F5.4
XZ plane G02 (G03) A+/-3.3 I+/-4.3 K+/-4.3 Y+/-4.3 J4.3 F5.4
YZ plane G02 (G03) A+/-3.3 J+/-4.3 K+/-4.3 X+/-4.3 I4.3 F5.4
Programming example where X0, Y0, Z0 is the starting point:
Cartesian coordinates
N10 G03 X0 Y0 I15 J0 Z50 K5 F150.
Polar coordinates
N10 G03 A180 I15 J0 Z50 K5 F150.
Atention:
When the program is executed in DRY RUN operation mode (4), with no real machine movement, the tool path in a helical interpolation will be displayed neither on the graphic simulation nor when a ZOOM function is used.
Page
10
Chapter: 5
PATH CONTROL
Section:
HELICAL INTERPOLATION
In helical movements where the final position on the axis perpendicular to the main plane is reached before the circular interpolation on the main plane (Z on the XY plane) is finished, the arc will end at the programmed coordinate value. From there to the programmed final point, the CNC will move the axes describing a straight line on a plane parallel to the main plane.
Programming example where X0, Y0, Z0 is the starting point:
N10 G03 X0 Y0 I15 J0 Z35 K10 F250
Atention:
When a circular (helical) interpolation is programmed with G02,G03, the
CNC takes the arc’s center as the new polar origin.
Chapter: 5
PATH CONTROL
Section:
HELICAL INTERPOLATION
Page
11
5.6 ARC TANGENT TO PREVIOUS PATH (G08)
By means of function G08, it is possible to program an arc tangent to the previous path without having to program its center coordinates (I, J, K).
The cartesian coordinate format is:
N4 G08 X±4.3 Y±4.3 in mm
N4 G08 X±3.4 Y±3.4 in inches
N4 Block number.
G08 Code for the arc tangent to previous path.
X X coordinate of the end point of the arc.
Y Y coordinate of the end point of the arc.
The polar coordinate format is:
N4 G08 R±4.3 A±4.3 in mm
N4 G08 R±3.4 A±4.3 in inches
N4 Block number
G08 Code for the arc tangent to previous path.
R
A
Radius (with respect to the polar origin) of the arc's end point.
Angle (with respect to the polar origin) of the arc's end point.
Example:
Being X0 Y40 the starting point, program a straight line joined to an arc tangent to it and ending with another arc tangent to the previous arc.
N0 G90 G01 X70 F100
N5 G08 X90 Y60
N10 G08 X110 Y60
Since both arcs are tangent to each other, the programming of their center coordinates (I,J) is not required.
If G08 is not used:
N100 G90 G01 X70 F100
N105 G03 X90 Y60 I0 J20
N110 G02 X110 Y60 I10 J0
"G08" is not modal, it only replaces G02 and G03 in the block containing it. It may be programmed whenever a tangential arc is desired. The previous path may be a straight line or another arc.
Atention:
G08 cannot be used to draw a complete circle since there are infinite solutions. The CNC will issue error 47 when attempting to do so.
Page
12
Chapter: 5
PATH CONTROL
Section:
ARC TANGENT TO
PREVIOUS PATH (G08)
5.7 ARC DEFINED BY THREE POINTS (G09)
By means of function G09, it is possible to program an arc by defining the end point and an intermediate point (the starting point is the end point of the previous block or the current position of the axes).
In other words, any intermediate point may be programmed instead of the center coordinates (I, K).
The cartesian coordinate format for the XY plane is:
N4 G09 X±4.3 Y±4.3 I±4.3 J±4.3
I
Y
J
N4 Block number
G09 Code for arc defined by three points
X X coordinate of the arc's end point
Y coordinate of the arc's end point
X coordinate of an intermediate point of the arc
Y coordinate of an intermediate point of the arc
The polar coordinate format for the XY plane is:
N4 G09 R±4.3 A±4.3 I±4.3 J±4.3
I
J
N4 Block number
G09 Code for arc defined by three points
R
A
Radius of the arc's end point (with respect to the polar origin)
Angle of the arc's end point (with respect to the polar origin)
X coordinate of an intermediate point of the arc
Y coordinate of an intermediate point of the arc
As can be observed here, the intermediate point must always be expressed in cartesian coordinates.
Programming example where X-50 Y0 is the starting point:
N10 G09 X35 Y20 I15 J25
"G09" is not modal. The direction of the arc (G02 or G03) is not required when programming G09.
"G09" only replaces "G02" and "G03" in the block containing it.
Atention:
A complete circle cannot be drawn by using "G09" since all three points must be different. The CNC will issue error 40 when attempting to do so.
Chapter: 5
PATH CONTROL
Section:
ARC DEFINED BY 3 POINTS
(G09)
Page
13
5.8 TANGENTIAL ENTRY (G37)
By means of function "G37", it is possible to link two paths tangentially without having to calculate the intersection points.
"G37" is not modal and, therefore, must be programmed every time the tangential link between two paths is desired. These paths may be: straight-to-straight or straight-tocurve. "G37" must be followed by the radius of the entry arc (R4.3 in mm or R3.4 in inches).
The radius value must always be positive.
"G37 R" must be programmed in the linear movement to be affected by it (either a G00 or a G01).
If "G37 R" is programmed in a circular interpolation (G02 or G03), the CNC will issue error 41.
Example:
N0 G90 G01 X40 Z40 F100
N5 G02 X60 Y10 I20 J0
Same example applying a tangential entry with a 5mm radius:
N0 G90 G01 G37 R5 X40 F100
N5 G02 X60 Y10 I20 J0
As can be seen in the diagram, the CNC modifies the path of block N0 so that the tool starts machining with a tangential entry to the part.
Page
14
Chapter: 5
PATH CONTROL
Section:
TANGENTIAL ENTRY (G37)
5.9 TANGENTIAL EXIT (G38)
By means of function "G38", it is possible to link two paths tangentially without having to calculate the intersection points.
"G38" is not modal and, therefore, must be programmed every time the tangential link between two paths is desired. These paths may be: straight-to-straight or curve-to-
straight. "G38" must be followed by the radius of the entry arc (R4.3 in mm or R3.4 in inches).
The radius value must always be positive.
"G38 R" must be programmed in the block prior to the linear one (either a G00 or a G01) being affected by it .
If the next programmed path, after the one containing "G38 R", is an arc (G02 or G03), the CNC will issue error 42.
Example:
N0 G90 G01 X40 F100
N5 G02 X80 Y30 I20 J0
N10 G00 X120
Same example applying a tangential exit with a 5mm radius:
N0 G90 G01 X40 F100
N5 G90 G02 G38 R5 X80 Y30 I20 J0
N10 G00 X120
Chapter: 5
PATH CONTROL
Section:
TANGENTIAL EXIT (G38)
Page
15
5.10 AUTOMATIC RADIUS BLEND (G36)
On turning operations, it is possible to round corners (blend paths) with a particular radius without the need to calculate the center of the arc or its starting and end points, simply by using function G36.
"G36" is not modal and, therefore, must be programmed every time this feature is desired.
The blending radius is programmed by R4.3 in mm or R3.4 in inches and it must be a positive value.
Example 1:
Starting point: X20 Y20
N50 G90 G01 G36 R5 X35 Y60 F100
N60 X50 Y0
Example 2:
Starting point: X20 Y20
N50 G90 G03 G36 R5 X50 Y50 I0 J30 F100
N60 G01 X50 Y0
Page
16
Chapter: 5
PATH CONTROL
Section:
AUTOMATIC RADIUS
BLEND (G36)
5.11 CHAMFER (G39)
On turning operations, it is possible to chamfer the intersection of two straight lines by using function G39 without having to calculate the intersection point.
"G39" is not modal and, therefore, must be programmed every time a chamfer is desired.
This function must be programmed in the block whose end is to be chamfered.
A positive value of R4.3 in mm or R3.4 in inches, sets the chamfer distance from the intersection point.
Example:
Starting point: X20 Y20
N0 G90 G01 G39 R15 X35 Y60 F100
N10 X50 Y0
Chapter: 5
PATH CONTROL
Section:
CHAMFER (G39)
Page
17
6.
ADDITIONAL PREPARATORY FUNCTIONS
6.1 DWELL (G04)
By means of function "G04", it is possible to program a dwell (delay).
The amount of dwell time is indicated by the letter "K".
Example: G04 K0.05 => 0.05 second dwell
G04 K2.5 => 2.5 second dwell
When "K" is followed by a figure, it can be a value between 0 and 99.99 seconds whereas when followed by an arithmetic parameter (KP3) this parameter value may be between 0 and 655.35 seconds.
The dwell is executed at the beginning of the block containing it. "G04" may also be programmed as "G4".
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
DWELL (G04)
Page
1
6.2. MIRROR IMAGE
G10: Cancellation of mirror image
G11: Mirror image on the X axis
G12: Mirror image on the Y axis
G13: Mirror image on the Z axis
When the CNC operates on G11,G12,G13 it executes the movements programmed on
X,Y,Z with the sign reversed.
Functions G11,G12,G13 are modal; i.e. once programmed they remain active until G10 is programmed.
Functions G11,G12,G13 can all be programmed in the same block, since they are not incompatible with each other.
Example: a) N5 G91 G01 X30 Y30 F100
N10 Y60
N12 X20 Y-20
N15 X40
N20 G02 X 0 Y-40 I 0 J-20
N25 G01 X-60
N30 X-30 Y-30 b) N35 G11
N40 G25 N5.30
c) N45 G10 G12
N50 G25 N5,30
Page
2
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
MIRROR IMAGE
G10, G11, G12, G13
d) N55 G11 G12
N60 G25 N5.30
N65 M30
Example 2:
N10 X— Y—
N20 ' '
N30 ' '
N40 ' '
N50 ' '
N60 G11 G12
N70 G25 N10.50
N80 M30
If mirror imaging is programmed while G73 (pattern rotation) is active the CNC will apply mirror image first and then the rotation.
The CNC assumes G10 on being turned ON, after executing M02,M30 or after an
EMERGENCY or RESET.
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
MIRROR IMAGE
G10, G11, G12, G13
Page
3
6.3 DISPLAY AN ERROR CODE (G30)
As soon as the CNC reads a block containing the "G30" code, interrupts the running program and displays the indicated error.
Programming format: N4 G30 K2
N4
G30
Block number
Error programming code
K2(0-99) Error code number to be displayed
The error code may also be programmed by an arithmetic parameter between P0 and P255.
For example: N4 G30 KP123.
This code, in combination with G26, G27, G28 and G29, permits interrupting the program and detecting possible measuring errors, etc.
A block containing "G30" cannot have any other information.
Atention:
When wishing the CNC's own error code comments NOT to appear on the screen, the error code number to be displayed by "G30" must be greater than those used by the CNC.
Remember that the operator may write comments in the program and the
CNC will display them when executing the corresponding block.
Page
4
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
DISPLAY AN ERROR CODE
(G30)
6.4 UNCONDITIONAL JUMP / CALL (G25)
Function "G25" may be used to jump from one block to another within the same program.
The block containing "G25" may not contain any other information. There are two programming formats.
Format a) N4 G25 N4
N4 Block number
G25 Unconditional jump code
N4 Block number jumping to
When the CNC reads this block, the program "jumps" to the indicated block and continues its execution from there on.
Example: N0 G00 X100
N5 Z50
N10 G25 N50
N15 X50
N20 Z70
N50 G01 X20
When reaching block N10, the CNC skips blocks N15 and N20 continuing from N50 to the end of the program.
Format b) N4 G25 N4.4.2
N4
G25
N4.4.2
Block number
Unconditional jump code
Number of repetitions
Number of the last block to be executed
Number of the block jumping to
When the CNC reads a block of this type, jumps to the block defined between "N" and the first period.
Executes the program portion between this block and the one defined between the two periods as many times as indicated by the last figure.
This last figure may be between 0 and 99. However, if an arithmetic parameter is used to define it, its value may be between 0 and 255.
When writing only N4.4, the CNC will execute this program section only once (same as for: N4.4.1)
Once the CNC has completed the last repetition of the section, it returns to the block following the one containing "G25 N4.4.2 "
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
UNCONDITIONAL
JUMP/CALL (G25)
Page
5
Example: N0 G00 X10
N5 Z20
N10 G01 X50 M3
N15 G00 Z0
N20 X0
N25 G25 N0.20.8
N30 M30
When reaching "N25", the CNC jumps to "N0" and executes the section "N0 through
N20" eight times. It, then, returns to "N30".
The preparatory functions corresponding to the conditional jumps/calls (G26, G27, G28,
G29 and G30) will be described in the section regarding PARAMETRIC
PROGRAMMING, OPERATIONS WITH PARAMETERS later on in this manual.
Page
6
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
UNCONDITIONAL
JUMP/CALL (G25)
6.5 SCALING FACTOR (G72)
G72 allows the machining of parts of similar shape but different size using the same program.
G72 must be programmed alone in a block. There are two different methods of programming G72.
6.5.1
SCALING FACTOR APPLIED ONTO ALL AXES
Programming format: N4 G72 K2.4
N4 Block number
G72 Scaling code
K2.4 Value of the scaling factor
Min. value K0.0001 (x 0.0001)
Max. value K100 (x 100)
Tool radius and length compensation are possible with this scaling mode.
All coordinate values programmed after G72 will be multiplied by K until the scaling is cancelled by K=1, or after M02,M30, EMERGENCY or RESET.
Example:
Starting point is X-30 Y10
N10 G00 G90 X-19 Y0
N20 G01 X0 Y10 F150
N30 G02 X0 Y-10 I0 J-10
N40 G01 -19 Y0
N45 G31...................................................(Store datum point)
N50 G92 X-79 Y-30 .............................. (Change datum point)
N60 G72 K2 .......................................... (Apply Scaling factor 2)
N70 G25 N10.40.1
N80 G72 K1............................................ (Cancel scaling factor)
N85 G32 ................................................. (Retrieve original datum point)
N90 G0 X-30 Y10 ................................ (Return to initial point)
N100 M30 ...............................................(End of program)
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
SCALING FACTOR (G72)
Page
7
6.5.2 SCALING FACTOR APPLIED ONLY ONTO ONE AXIS
Programming format:
N4 G72 V,W,X,Y,Z 2.4
N4: Block number
G72: Function which defines the scale factor
X,Y,Z: Axis to which the scale factor is applied.
2.4: Scaling factor value (betweem 0.0001 and 15.9999)
In this case the axis to which the scale factor is applied must be at the zero point (value
0) when the factor is applied or cancelled.
The coordinate value of the axis affected must be zero when G72 is applied. When the scaling factor affects only one axis, the coordinate values of the datum point cannot be altered by functions such as G32, G92 or G53 through G59.
Tool radius compensation will also be affected by the scaling factor applied to the axis.
If, within the same program, both scaling methods are used, the CNC will apply to the axis affected by both methods a factor equal to the multiplication of both values.
When checking a program in graphic mode, the graphic being displayed is not affected by any scaling factor. Therefore, when the scaling factor is applied to one axis only, the values and graphics displayed will represent the programmed values.
The scaling function is cancelled by applying a factor of 1, after M02,M30, EMER-
GENCY or RESET. If an scaling factor is entered, any preceding factor is automatically cancelled, regardless of the axis affected.
Page
8
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
SCALING FACTOR (G72)
6.6 PATTERN ROTATION (G73)
This feature allows the rotation of the coordinate axes around the part program’s datum point on the main plane.
Programming format: N4 G73 A+/-3.3
N4
G73
- Block number
- Pattern rotation code
A+/-3.3
- Rotation angle (between 0º and 360º)
G73 is incremental, i.e., if more than one G73 is programmed. Their respective "A" values will be added together.
G73 must be programmed alone in a block.
Pattern rotation is cancelled with: G17, G18, G19, G73 (without an "A" value). An M02,
M30, EMERGENCY or RESET.
While G73 is active, blocks defining a point by one angle plus an absolute (G90) cartesian coordinate are not possible.
Programming example with X0 Y0 as the starting point:
N10 G01 X21 Y0 F300
N20 G02 A0 I5 J0
N30 G03 A0 I5 J0
N40 A180 I-10 J0
N50 G73 A45
N60 G25 N10.50.7
N70 M30
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
PATTERN ROTATION (G73)
Page
9
6.7 SINGLE-BLOCK TREATMENT. ON (G47), OFF (G48)
This CNC considers a "single block" the section of a program contained between a G47 and a G48.
After executing function G47, the CNC executes all the following blocks in a row until a G48 is detected.
When pressing the key while executing a "Single-Block" block, either in Automatic or block by block, the CNC goes on executing all the following blocks until a G48 is executed.
While function G47 is active, the Manual Feedrate Override switch as well as the spindle speed override keys are ignored, thus that section of the program is executed at 100% of the programmed "F" and "S".
Functions G47 and G48 are modal and incompatible with each other.
On CNC power-up, after executing an M02/M30, after an EMERGENCY or RESET, the
CNC assumes G48.
Page
10
Chapter: 6
ADDITIONAL PREPARATORY FUNCTIONS
Section:
SINGLE-BLOCK
TREATMENT
(G47, G48)
7.
TOOL COMPENSATION
7.1 TOOL RADIUS COMPENSATION
In normal milling work the path of the tool has to be calculated and defined taking its radius into account so as to obtain the required dimensions of the part produced.
Tool radius compensation enables the contour of the part to be programmed directly without taking the dimensions of the tool into account.
The CNC automatically calculates the path to be followed by the tool, based on the contour of the part and the tool radius value stored in the tool table.
There are three preparatory functions for tool radius compensation:
G40 : Cancellation of tool radius compensation
G41 : Left hand tool radius compensation
G42 : Right hand tool radius compensation
G41. The tool is on the left of the part as seen from the direction of movement.
G42. The tool is on the right of the part as seen from the direction of movement.
The CNC has a table of up to 100 pairs of values for tool radius compensation. R identifies the tool radius and I the tool wear. The CNC will add (or subtract) the value of I to the value of R.
The maximum compensation values are: R ±1000 mm or ±39.3699 inches
I ±32.766 mm or ±1.2900 inches
The compensation values must be stored in the tool table (operating mode 8) before starting the machining or else at the beginning of a part program by means of G50.
The values of I,K can also be checked and modified without stopping the cycle’s execution (See Operation Manual).
Once the plane in which the compensation is to be applied has been determined by codes
G17,G18,G19 the compensation is made effective by means of G41 or G42 and acquires the table value selected by code Txx.xx (Txx.00-Txx.99).
Functions G41 and G42 are modal (maintained) and are cancelled by G40, G74, G81,
G82, G83, G84, G85, G86, G87, G88, G89, M02 and M30 and by EMERGENCY or
RESET.
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
G40, G41, G42
Page
1
7.1.1
SELECTION AND ACTIVATION OF RADIUS COMPENSATION
(G41, G42)
Once G17, G18 or G19 has been used to select the plane in which tool radius compensation is to be applied, the code G41 or G42 must be used to initiate compensation.
G41: The tool remains to the left of the part in the machining direction.
G42: The tool remains to the right of the part in the machining direction.
Either the block in which G41/G42 is programmed or a previous block must include programming of function Txx.xx (Txx.00-Txx.99) to select from the tool table the correction value to be applied. If no tool is selected, the CNC assumes the value T00.00.
Tool radius compensation selection (G41/G42) can only be carried out when G00 or G01
(rectilinear movements) is active. If the first call for compensation is made when G02 or
G03 are active, the CNC will display error code 40.
The next pages illustrate various cases of initiation of tool radius compensation.
Page
2
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
ON - G41, G42
STRAIGHT-STRAIGHT PATH
Compensated path
Programmed path
Path programmed in two blocks
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
ON - G41, G42
Page
3
STRAIGHT-CURVE PATH
Compensated path
Programmed path
Page
4
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
ON - G41, G42
Special cases to be considered
a). If compensation is programmed in a block in which there is no movement, the initiation of the compensation differs from the case explained above (compare with diagram in section on straight/straight path).
N0 G91 G41 G01 T00.00
N5 Y-100
N10 X+100
b). If compensation is entered with zero movement programming:
N0 G91 G01 X100 Y100
N5 G41 X0 T00.00
N10 Y-100
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
ON - G41, G42
Page
5
7.1.2
OPERATING WITH TOOL RADIUS COMPENSATION
The graphs below illustrate the various paths followed by a tool controlled by a CNC programmed with radius compensation.
Page
6
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
G41, G42
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
G41, G42
Page
7
When the CNC operates with tool radius compensation, it reads four blocks ahead of the block being executed so that it can calculate in advance the path to be followed.
There are certain cases in which particular care has to be taken.
For instance: Three or more blocks which do not include movement in the compensation plane, between blocks which do.
N0 G01 G91 G17 G41 X50 Y50 F100 T1.1
N5 Y100
N10 X200
N15 Z100
N20 M07
N25 Z200
N30 Y-100
Error 35 will be displayed at point (1). Only blocks containing G20, G21, G22, G23, G24,
G25,G26,G27,G28 or G29 can be programmed and they will not originate error 35 as they will not have a block without movement.
Page
8
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
G41, G42
7.1.3 CANCELLATION OF TOOL RADIUS COMPENSATION
Tool radius compensation is cancelled by function G40.
It should be borne in mind that tool radius compensation cancellation (G40) can only be carried out in a block in which a rectilinear movement is programmed (G00,G01).
If G40 is programmed in a block containing G02 or G03, the CNC will give alarm 40.
The following is series of various cases of cancellation of compensation.
CURVE - STRAIGHT PATH
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
OFF - G40
Page
9
STRAIGHT-STRAIGHT PATH
Compensated path
Programmed path
Path programmed in two blocks
Page
10
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
OFF - G40
7.1.4
MACHINING EXAMPLES WITH TOOL RADIUS
COMPENSATION
Example 1
Compensated path
Programmed path
(profile of the part)
Tool radius : 10 mm.
Tool number : T1.1
It is assumed that there are no movements on the Z axis.
N0 G92 X0 Y0 Z0
N5 G90 G17 S100 T1.1 M03
N10 G41 G01 X40 Y30 F125
N15 Y70
N20 X90
N25 Y30
N30 X40
N35 G40 G00 X0 Y0 M30
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
(Examples)
Page
11
Example 2
Compensated path
Programmed path
(profile of the part)
Tool radius: 10 mm.
Tool number: T1.1
It is assumed that there are no movements on the Z axis.
N0 G92 X0 Y0 Z0
N5 G90 G17 G01 F150 S100 T1.1 M03
N10 G42 X30 Y30
N15 X50
N20 Y60
N25 X80
N30 X100 Y40
N35 X140
N40 X120 Y70
N45 X30
N50 Y30
N55 G40 G00 X0 Y0 M30
Page
12
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
(Examples)
Example 3
Compensated path
Programmed path
(profile of the part)
Tool radius: 10 mm.
Tool number: T1.1
It is assumed that there are no movements on the Z axis.
N0 G92 X0 Y0 Z0
N5 G90 G01 G17 F150 S100 T1.1 M03
N10 G42 X20 Y20
N15 X50 Y30
N20 X70
N25 G03 X85 Y45 I0 J15
N30 G02 X100 Y60 I15 J0
N35 G01 Y70
N40 X55
N45 G02 X25 Y70 I-15 J0
N50 G01 X20 Y20
N55 G40 G00 X0 Y0 M05 M30
Chapter: 7
TOOL COMPENSATION
Section:
RADIUS COMPENSATION
(Examples)
Page
13
7.2 TOOL LENGTH COMPENSATION
This function makes it possible to compensate for possible differences in length between the tool programmed and the tool to be used.
As previously indicated in the section on tool radius compensation, the CNC has storage capacity for dimensions, radius and length of 100 tools (Txx.oo- Txx.99).
L identifies the tool length and K the tool wear. The CNC will add (or subtract) the value of K to the value of L.
The maximum length compensation values are:
L±1000 mm or ±39.3699 inches K±32.766 mm (1.2900 inches).
The call codes for length compensation are:
G43 : Length compensation
G44 : Cancellation of length compensation
When G43 is programmed, the CNC compensates the length according to the value selected from the tool table (Txx.00-Txx.99).
Length compensation is applied to the axis perpendicular to the principal plane.
G17 : Length compensation on the Z axis
G18 : Length compensation on the Y axis
G19 : Length compensation on the X axis
Function G43 is modal (persistent) and is cancelled by G44, G74, M02, M30,
EMERGENCY or RESET.
Length compensation can be used in conjunction with canned cycles, although in that case the precaution has to be taken of applying the compensation before the cycle starts.
Page
14
Chapter: 7
TOOL COMPENSATION
Section:
LENGTH COMPENSATION
(G43, G44)
Example of tool length compensation
It is supposed that the tool used is 4 mm shorter than the tool programmed.
The tool number is T1.1 (the value stored in the tool table is L-4).
N0 G92 X0 Y0 Z0
N5 G91 G00 G05 X50 Y35 S500 M03
N10 G43 Z-25 T1.1
N15 G01 G07 Z-12 F100
N20 G00 Z12
N25 X40
N30 G01 Z-17
N35 G00 G05 G44 Z42 M05
N40 G90 G07 X0 Y0
N45 M30
Chapter: 7
TOOL COMPENSATION
Section:
LENGTH COMPENSATION
(G43, G44)
Page
15
8.
MACHINING CANNED CYCLES
This CNC offers the following machining canned cycles:
G67 N0 & P202=K0 Point to point positioning canned cycle
G67 N0 & P202=K1 Straight-line positioning canned cycle
G67 N0 & P202=K2 Rectangular pattern positioning canned cycle
G67 N0 & P202=K3 Grid pattern positioning canned cycle
G67 N0 & P202=K4 Bolt-hole pattern (arc pattern) positioning canned cycle
G67 N1 & P202=K0 Inside milling canned cycle for a rectangular pocket
G67 N1 & P202=K1 Inside milling canned cycle for a circular pocket
G67 N2 & P202=K0 Outside milling canned cycle for a rectangular pocket
G67 N2 & P202=K1 Outside milling canned cycle for a circular pocket
G67 N3 Surface milling canned cycle
G67 N4 Corner roughing canned cycle
G67 N6 Drilling canned cycle
G67 N7 Tapping canned cycle
G67 N8 Boring / Reaming canned cycle
G67 N9 Center-punching canned cycle
Parameters related to the canned cycles:
The canned cycle can alter the contents of parameters P0 through P99.
Parameters P200 through P209 are reserved for the CNC and some of them, as described next, have a special meaning.
On power-up, after a Reset and when quitting the execution of program P99996, the
CNC updates the following arithmetic parameters:
P200 The Z axis is set as being controlled by the CNC (0) or as a DRO axis (1)
P201 Work units (0=mm, 1=inches)
P209 Z axis interpolations are possible (0) or not (1)
When programming the canned cycles, if the parameter value is a constant, press K after the "=" sign. For example: P0 = K25 ......
Chapter: 8
MACHINING CANNED CYCLES
Section: Page
1
8.1 POINT TO POINT POSITIONING (G67 N0 & P202=K0)
Basic canned cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinate of 1st point
P112, P113 X, Y coordinate of 2nd point
P114, P115 X, Y coordinate of 3rd point
P116, P117 X, Y coordinate of 4th point
P118, P119 X, Y coordinate of 5th point
P120, P121 X, Y coordinate of 6th point
P122, P123 X, Y coordinate of 7th point
P124, P125 X, Y coordinate of 8th point
Feedrate (F) related parameters:
P205 Currently selected machining feedrate value (F) .
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected.
Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Programming example:
N10 P205=K100 .................................... Set the machining feedrate
N20 FP205
N30 P106=K1 ........................................ Parameters for straight-line positioning
P110=K10 P111=K10 .................... Coordinates of the 1st point
P112=K60 P113=K15 .................... Coordinates of the 2nd point
P114=K25 P115=K30 .................... Coordinates of the 3rd point
P116=K25 P117=K30 .................... No more points
N40 P202=K0 ........................................ Indicative of "point-to-point positioning"
N50 G67 N0 ........................................... Call a canned cycle
N60 M30 ................................................ End of program
Page
2
Chapter: 8
MACHINING CANNED CYCLES
Section:
POINT-TO-POINT
POSITIONING
8.2 STRAIGHT-LINE POSITIONING (G67 N0 & P202=K1)
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinates of starting point (X1, Y1). It must always be defined
P112, P113 X, Y coordinates of the end point (Xn, Yn)
P130
P131
P132
P133
Length (L)
Steps between points (I)
Number of points (N)
Path angle (A)
Use one of the methods below to define the desired path:
Set (L, A, N) ....................................... Parameters P130, P133, P132.
Set (L, A, I) ........................................ Parameters P130, P133, P131.
Set (Xn, Yn, L=0, N) ......................... Parameters P112, P113, P130=K0, P132.
Set (Xn, Yn, L=0, I)........................... Parameters P112, P113, P130=K0, P131.
Set (I, N, A) ....................................... Parameters P131, P132, P133
In the latter, set: L=0, Xn=X1, Yn=Y1.
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Definition example:
Either one of the following formats may be used:
P110=K P111=K P130=K60
P110=K P111=K P130=K60
P110=K P111=K P112=K51.961
P110=K P111=K P112=K51.961
P133=K30
P133=K30
P113=K30
P113=K30
P110=K P111=K P112=K P113=K P130=K
P132=K4
P131=K20
P130=K
P130=K
P132=K4
P131=K20
P131=K20 P132=K4 P133=K30
Chapter: 8
MACHINING CANNED CYCLES
Section:
STRAIGHT-LINE
POSITIONING
Page
3
8.3 RECTANGULAR PATTERN POSITIONING (G67 N0 & P202=K2)
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinate of the first point (X1, Y1). It must always be set
P130 Length along X (Lx)
P131
P132
P134
P135
P136
P133
P137
Step between points along X (Ix)
Number of points along X (Nx)
Length along Y (Ly)
Step between points along Y (Iy)
Number of points along Y(Ny)
Path angle (A). It must always be set
Angle between paths (B). It must always be set
For both movements to be parallel to X and Y, set:
P133=K0 ........... A=0
P137=K90 ......... B=90
To define each path, use one of the following methods:
Set (L, N) ............................................ Parameters P130, P132 & P134, P136
Set (L, I)............................................. Parameters P130, P131 & P134, P135
Set (I, N) ............................................ Parameters P131, P132 & P135, P136
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Page
4
Chapter: 8
MACHINING CANNED CYCLES
Section:
RECTANGULAR PATTERN
POSITIONING
8.4 GRID PATTERN POSITIONING (G67 N0 & P202=K3)
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinate of the first point (X1, Y1). It must always be set
P130 Length along X (Lx)
P131
P132
P134
P135
P136
P133
P137
Step between points along X (Ix)
Number of points along X (Nx)
Length along Y (Ly)
Step between points along Y (Iy)
Number of points along Y(Ny)
Path angle (A). It must always be set
Angle between paths (B). It must always be set
For both movements to be parallel to X and Y, set:
P133=K0 ........... A=0
P137=K90 ......... B=90
To define each path, use one of the following methods:
Set (L, N) ............................................ Parameters P130, P132 & P134, P136
Set (L, I)............................................. Parameters P130, P131 & P134, P135
Set (I, N) ............................................ Parameters P131, P132 & P135, P136
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Chapter: 8
MACHINING CANNED CYCLES
Section:
GRID PATTERN
POSITIONING
Page
5
8.5 BOLT-HOLE (ARC) PATTERN POSITIONING (G67 N0 & P202=K4)
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinates of the first point (X1, Y1)
P138, P139 X, Y coordinates of the center (Xc, Yc). It must always be set
P141
P140
P132
P142
Arc radius (R)
Angle of the first point (A)
Number of points (N). It must always be set
Angular step between points (B). It must always be set
The angular step "B" is always given in degrees and indicates the moving direction.
With a negative value for clockwise and positive for counter-clockwise.
For a full circle, program B0. The moving direction will be counter-clockwise.
To set the starting point, use one of the following methods:
Set (R, A) ............................................ Parameters P141, P140
Set (X1, Y1, R=0) .............................. Parameters P110, P111, P141=K0
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Page
6
Chapter: 8
MACHINING CANNED CYCLES
Section:
BOLT-HOLE PATTERN
POSITIONING
8.6 INSIDE RECTANGULAR POCKET MACHINING (G67 N1 & P202=K0)
Z SAF
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinates of the first point (corner X1, Y1)
P146 Length of the pocket (L). The sign indicates the machining direction.
P147
P150
P151
Pocket width (H)
Rounding radius (r)
Chamfer (C)
For a pocket with rounded corners, set "C0" and assign to "r" the desired rounding radius.
For a pocket with chamfered corners, set "r0" and assign to "C" the distance from the theoretical corner.
P148
When making a regular pocket, without roundings or chamfers, program "r0" and "C0".
Machining pass (G). When programmed as 0, the CNC assumes a value 0.75 times the tool diameter.
Chapter: 8
MACHINING CANNED CYCLES
Section:
INSIDE RECTANGULAR
POCKET MILLING
Page
7
P149
P198
P133
Finishing pass (E). When programmed as 0, no finishing pass is carried out.
% of feedrate F used for the finishing pass (%F).
When set to 0, the finishing pass is carried out at the same feedrate as the one used for the roughing passes.
Pocket angle (A)
Parameters related to the Z axis:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P199
Z coordinate where the pocket is to be milled out
Pocket depth (P)
Penetration step (in-feed) (I)
% of the feedrate F used to in-feed the Z axis (%F Z)
When set to 0, The in-feed is performed at the selected feedrate.
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Page
8
Chapter: 8
MACHINING CANNED CYCLES
Section:
INSIDE RECTANGULAR
POCKET MILLING
8.7 INSIDE CIRCULAR POCKET MILLING (G67 N1 & P202=K1)
Z SAF
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinates of the pocket center (Xc, Yc)
P141 Radius of the pocket (R). The sign indicates the machining direction.
P148 Machining pass (G). When programmed as 0, the CNC assumes a value 0.75 times the tool diameter.
Chapter: 8
MACHINING CANNED CYCLES
Section:
INSIDE CIRCULAR POCKET
MILLING
Page
9
P149
P198
Finishing pass (E). When programmed as 0, no finishing pass is carried out.
% of feedrate F used for the finishing pass (%F).
When set to 0, the finishing pass is carried out at the same feedrate as the one used for the roughing passes.
Parameters related to the Z axis:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P199
Z coordinate where the pocket is to be milled out
Pocket depth (P)
Penetration step (in-feed) (I)
% of the feedrate F used to in-feed the Z axis (%F Z)
When set to 0, The in-feed is performed at the selected feedrate.
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Page
10
Chapter: 8
MACHINING CANNED CYCLES
Section:
INSIDE CIRCULAR POCKET
MILLING
8.8 OUTSIDE RECTANGULAR POCKET MILLING (G67 N2 & P202=K0)
Z SAF
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinates of the first point (corner X1, Y1)
P146 Length of the pocket (L). The sign indicates the machining direction.
P147
P150
P151
Pocket width (H)
Rounding radius (r)
Chamfer (C)
For a pocket with rounded corners, set "C0" and assign to "r" the desired rounding radius.
For a pocket with chamfered corners, set "r0" and assign to "C" the distance from the theoretical corner.
P148
When making a regular pocket, without roundings or chamfers, program "r0" and "C0".
Machining pass (G). When programmed as 0, the CNC assumes a value 0.75 times the tool diameter.
Chapter: 8
MACHINING CANNED CYCLES
Section:
OUTSIDE RECTANGULAR
POCKET MILLING
Page
11
P152
P149
P198
Excess material, both along X and along Y (Q).
Finishing pass (E). When programmed as 0, no finishing pass is carried out.
% of feedrate F used for the finishing pass (%F).
When set to 0, the finishing pass is carried out at the same feedrate as the one used for the roughing passes.
Pocket angle (A) P133
Parameters related to the Z axis:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P199
Z coordinate where the pocket is to be milled out
Pocket depth (P)
Penetration step (in-feed) (I)
% of the feedrate F used to in-feed the Z axis (%F Z)
When set to 0, The in-feed is performed at the selected feedrate.
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Page
12
Chapter: 8
MACHINING CANNED CYCLES
Section:
OUTSIDE RECTANGULAR
POCKET MILLING
8.9 OUTSIDE CIRCULAR POCKET MILLING (G67 N2 & P202=K1)
Z SAF
Basic cycle defining parameters:
P106 Safety distance along Z
P110, P111 X, Y coordinates of the pocket center (Xc, Yc)
P141 Radius of the pocket (R). The sign indicates the machining direction.
P148
P149
P152
P198
Machining pass (G). When programmed as 0, the CNC assumes a value 0.75 times the tool diameter.
Finishing pass (E). When programmed as 0, no finishing pass is carried out.
Excess material, both along X and Y (Q).
% of feedrate F used for the finishing pass (%F).
When set to 0, the finishing pass is carried out at the same feedrate as the one used for the roughing passes.
Parameters related to the Z axis:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P199
Z coordinate where the pocket is to be milled out
Pocket depth (P)
Penetration step (in-feed) (I)
% of the feedrate F used to in-feed the Z axis (%F Z)
When set to 0, The in-feed is performed at the selected feedrate.
Chapter: 8
MACHINING CANNED CYCLES
Section:
OUTSIDE CIRCULAR
POCKET MILLING
Page
13
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Page
14
Chapter: 8
MACHINING CANNED CYCLES
Section:
OUTSIDE CIRCULAR
POCKET MILLING
8.10 SURFACE MILLING (G67 N3)
This CNC offers 4 types of surface milling. Use arithmetic parameter P202 to choose a particular one.
These surface milling types are:
P202=K0 Bidirectional milling on X
Z SAF
P202=K1 Bidirectional milling on Y
Z SAF
P202=K2 Unidirectional milling on X
Chapter: 8
MACHINING CANNED CYCLES
Section:
SURFACE MILLING
Page
15
Z SAF
P202=K3 Unidirectional milling on Y
Basic cycle defining parameters
P106
P202
Safety distance along Z
Milling type
P110, P111 X, Y coordinate of the first point (corner X1, Y1)
P146 Length of the surface to be milled (L). In unidirectional milling, the
P147 sign indicates the machining direction.
Width of the surface to be milled (H). In unidirectional milling, the sign indicates the machining direction.
Z SAF
Page
16
P148
P152
Step between two consecutive passes (G). When set to 0, the CNC assumes 0.75 times the tool diameter.
Tool overshoot distance on each side of the part for better part finish on the edges (E)
Chapter: 8
MACHINING CANNED CYCLES
Section:
SURFACE MILLING
Parameters related to the Z axis:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P199
Z coordinate where the part is to be milled off.
Milling depth (P)
Penetration step (in-feed) (I)
% of the feedrate F used to in-feed the Z axis (%F Z)
When set to 0, The in-feed is performed at the selected feedrate.
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Chapter: 8
MACHINING CANNED CYCLES
Section:
SURFACE MILLING
Page
17
8.11 CORNER ROUGHING (G67 N4)
With this CNC, it is possible to rough out sharp, rounded or chamfered corners as shown below:
Basic cycle defining parameters:
Z SAF
P154 Machining direction.
P106 Safety distance along Z
P110, P111 X, Y coordinate of the inside point of the corner (X1, Y1)
P146, 147 Length along X and Y respectively (L, H).
Depending on which corner is to be machined, these parameters will have either a positive or negative sign.
Page
18
Chapter: 8
MACHINING CANNED CYCLES
Section:
CORNER ROUGHING
P150
P151
Rounding radius (r)
Chamfer (C)
P148
P149
To round a corner, set C0 and assign to "r" the desired rounding radius.
To chamfer a corner, set R0 and assign to "C" the distance to the theoretical corner to be chamfered.
To machine a sharp corner (neither rounded nor chamfered), program r0 & C0.
Machining pass (G). When programmed as 0, the CNC assumes a value 0.75 times the tool diameter.
Finishing pass (E). When programmed as 0, no finishing pass will be carried out.
P198
P133
% of the feedrate F applied on the finishing pass (%F).
When set to 0, the finishing pass will be run at the same feedrate as the one used for roughing.
Angle of the corner with respect to the X axis (A)
Parameters related to the Z axis:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P199
Z coordinate where the corner is to be roughed out
Roughing depth (P)
Penetration step (in-feed) (I)
% of the feedrate F used to in-feed the Z axis (%F Z)
When set to 0, The in-feed is performed at the selected feedrate.
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Chapter: 8
MACHINING CANNED CYCLES
Section:
CORNER ROUGHING
Page
19
8.12 DRILLING (G67 N6)
Basic cycle defining parameters:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P109
P143
Z coordinate where the hole is to be drilled
Hole depth (P)
Drilling step (in-feed) (I)
Dwell at the bottom of the hole before withdrawing the drill bit (K).
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Drilling example:
N10 P205=K100 ........................................ Set machining feedrate
N20 FP205
N30 G01 X107 Y78 ................................... Move to drilling position
N40 P107=K0 P108=K12 P109=K5 .......... Drilling parameters
P143=K1
N50 G67 N6 ............................................... Call the drilling cycle
N60 M30 .................................................... End of program
Page
20
Chapter: 8
MACHINING CANNED CYCLES
Section:
DRILLING
Associate the Drilling operation with the Positioning canned cycle
To do this, proceed as follows:
1st Set the basic parameters to define the drilling operation.
2nd Set the basic parameters of the positioning canned cycle
3rd Set the drilling operation indicator. P203=K1
4th Set the indicator for type of positioning. P202=K*
5th Call the positioning canned cycle. G67 N0
(There is no need to call the drilling canned cycle. G67 N6)
Straight-line drilling example:
N10 P205=K100 ............................................. Set machining feedrate
N20 FP205
N30 P107=K0 P108=K12 P109=K5 .............. Drilling parameters
P143=K1
N40 P106=K1 P110=K20 P111=K10 ............ Parameters for straight line positioning
P130=K50 P133=K25 P132=K6
N50 P203=K1 ................................................. Indicator of drilling operation
P202=K1 ................................................. Indicator for positioning type
N60 G67 N0.................................................... Call the straight-line positioning cycle
N70 M30 ......................................................... End of program
Chapter: 8
MACHINING CANNED CYCLES
Section:
DRILLING
Page
21
8.13 TAPPING (G67 N7)
Basic cycle defining parameters:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P143
Z coordinate where the hole is to be tapped
Tap depth (P)
Dwell at the bottom of the hole before starting to tap-out (K)
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Tapping example:
N10 P205=K100 ........................................ Set machining feedrate
N20 FP205
N30 G01 X107 Y78 ................................... Move to tapping position
N40 P107=K0 P108=K12 P143=K1 .......... Tapping parameters
N50 G67 N7 ............................................... Call the tapping cycle
N60 M30 .................................................... End of program
Page
22
Chapter: 8
MACHINING CANNED CYCLES
Section:
TAPPING
Associate the Tapping operation with the Positioning canned cycle
To do this, proceed as follows:
1st Set the basic parameters to define the tapping operation.
2nd Set the basic parameters of the positioning canned cycle
3rd Set the tapping operation indicator. P203=K2
4th Set the indicator for type of positioning. P202=K*
5th Call the positioning canned cycle. G67 N0
(There is no need to call the tapping canned cycle. G67 N7)
Straight-line tapping example:
N10 P205=K100 ............................................. Set the machining feedrate
N20 FP205
N30 P107=K0 P108=K12 P143=K1 .............. Tapping parameters
N40 P106=K1 P110=K20 P111=K10 ............ Parameters for straight-line positioning
P130=K50 P133=K25 P132=K6
N50 P203=K2 ................................................. Indicator of tapping operation
P202=K1 ................................................. Indicator of straight-line positioning
N60 G67 N0.................................................... Call straight-line positioning cycle
N70 M30 ......................................................... End of program
Chapter: 8
MACHINING CANNED CYCLES
Section:
TAPPING
Page
23
8.14 BORING / REAMING (G67 N8)
Basic cycle defining parameters:
These parameters are to be set when the Z axis has been set as being controlled by the CNC.
Machine parameter "P617(4)=0".
P107
P108
P143
Z coordinate where the machining operation will take place
Boring / reaming depth (P)
Dwell at the bottom of the hole before pulling the tool out (K).
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Boring example:
N10 P205=K100 ........................................ Set machining feedrate
N20 FP205
N30 G01 X107 Y78 ................................... Move to boring position
N40 P107=K0 P108=K12 P143=K1 .......... Boring parameters
N50 G67 N8 ............................................... Call boring cycle
N60 M30 .................................................... End of program
Page
24
Chapter: 8
MACHINING CANNED CYCLES
Section:
BORING / REAMING
Associate the Boring / Reaming operation with the Positioning canned cycle
To do this, proceed as follows:
1st Set the basic parameters to define the Boring/Reaming operation.
2nd Set the basic parameters of the positioning canned cycle
3rd Set the Boring/reaming operation indicator. P203=K3
4th Set the indicator for type of positioning. P202=K*
5th Call the positioning canned cycle. G67 N0
(There is no need to call the Boring/Reaming canned cycle. G67 N8)
Example of a Bolt-hole pattern (in an arc) boring operation:
N10 P205=K100 ............................................. Set machining feedrate
N20 FP205
N30 P107=K0 P108=K12 P143=K1 .............. Boring parameters
N40 P106=K1 P138=K70 P139=K20 ............ Parameters for bolt-hole positioning
P141=K40 P140=K-15
P142=K30 P132=K8
N50 P203=K3 ................................................. Indicator of boring operation
P202=K4 ................................................. Indicator of bolt-hole positioning
N60 G67 N0.................................................... Call bolt-hole positioning
N70 M30 ......................................................... End of program
Chapter: 8
MACHINING CANNED CYCLES
Section:
BORING / REAMING
Page
25
8.15 CENTER PUNCHING (G67 N9)
Basic cycle defining parameters:
P107
P108
P144
P145
P143
Z coordinate where the center punching is to be carried out (Z)
Punch depth (P)
Punch diameter (F)
Punch angle (A)
Dwell after the punch until the tool starts withdrawing (K).
To set the punching depth, use one of the following methods:
Set the punching depth (P) ........................................... Parameter P108
Set P=0, Punch angle (A) &
Punch diameter (F) ........................................... Parameters P108=K, P144, P145
Feedrate (F) related parameters:
P205 Currently selected feedrate value (F).
When running a canned cycle, it is recommended to set this parameter whenever a new feedrate is selected. Example for setting a feedrate of F100:
P205 = K100 Sets parameter P205 to the desired feedrate value (100).
FP205 Selects the feedrate value indicated by P205
Center punching example:
N10 P205=K100 ........................................ Set machining feedrate
N20 FP205
N30 G01 X107 Y78 ................................... Move to punch position
N40 P107=K0 P108=K1.5 P143=K0 ......... Punch parameters
N50 G67 N9 ............................................... Call the center-punching cycle
N60 M30 .................................................... End of program
Page
26
Chapter: 8
MACHINING CANNED CYCLES
Section:
CENTER PUNCHING
Associate the Center-punching operation with the Positioning canned cycle
To do this, proceed as follows:
1st Set the basic parameters to define the center-punching operation.
2nd Set the basic parameters of the positioning canned cycle
3rd Set the center-punching operation indicator. P203=K4
4th Set the indicator for type of positioning. P202=K*
5th Call the positioning canned cycle. G67 N0
(There is no need to call the center-punching canned cycle. G67 N9)
Example of a grid pattern center-punching:
N10 P205=K100 ............................................. Set machining feedrate
N20 FP205
N30 P107=K0 P108=K1.5 P143=K0 ............. Center-punching parameters
N40 P106=K1 P110=K20 P111=K10 ............ Grid pattern positioning parameters
P130=K90 P132=K4 P134=K40
P136=K3 P133=K0 P137=K90
N50 P203=K4 ................................................. Indicator of center-punching operation
P202=K3 ................................................. Indicator of grid pattern positioning
N60 G67 N0.................................................... Call the grid pattern positioning cycle
N70 M30 ......................................................... End of program
Chapter: 8
MACHINING CANNED CYCLES
Section:
CENTER PUNCHING
Page
27
9.
SUBROUTINES
A subroutine is a section of a program which, properly identified, may be called upon to be executed from any position (block) of the program.
A subroutine may be called upon several times from different program positions or from different programs.
With a single call, the subroutine may be executed up to 255 times.
A subroutine may be included within the user-defined program P99996 or may be stored in the special program P99994 for user-defined subroutines.
Standard and parametric subroutines are basically identical. Their only difference being that the calling block for a parametric subroutine (G21 N2.2) may contain up to 15 definition parameters.
In the case of a standard subroutine, the parameters may not be defined in the calling block.
The maximum number of parameters of a standard or parametric subroutine is 255 (P0 through P254).
9.1 SPECIAL PROGRAM P99994 FOR USER SUBROUTINES
Program P99994 must be edited at a PC and sent out to the CNC. It cannot be modified at the CNC.
It must only contain the user-defined subroutines edited in ISO code.
When program P99996 calls upon a subroutine, the CNC looks for it in P99996 first and, then, if not found, in P99994.
Using P99994 is recommended when several user-defined programs P99996 are being utilized. This way, if P99994 contains all the usual subroutines, they will not have to be repeated in each P99996 program.
It is recommended to store the subroutines associated to the T function, machine parameters "P743" and "P745", in program P99994.
Chapter: 9
SUBROUTINES
Section: Page
1
9.2 IDENTIFICATION OF A STANDARD SUBROUTINE (G22)
A standard subroutine (not parametric), always starts with a block containing function
"G22". The structure of this block is:
N4 G22 N2 N4 Block number
G22 Defines the beginning of the subroutine
N2 Identifies the subroutine (number between "N0" and "N99").
This block cannot contain any additional information.
Program all the desired blocks after this first subroutine block and remember that a standard subroutine may also contain parametric blocks.
A subroutine must always end with a block of the type: N4 G24. This "G24" code indicates the end of the subroutine. This block cannot contain any other information.
Programming example: N0 G22 N25
N10 X20
N15 P0=P0 F1 P1
N20 G24
Atention:
Subroutines "N91" through "N99" may not be defined because they are utilized by the CNC.
The CNC memory may not contain two standard subroutines with identical
ID numbers even if they belong to different programs. However, it is possible to use the same number to identify a standard subroutine and a parametric one.
9.3 CALLING A STANDARD SUBROUTINE (G20)
A standard subroutine may be called upon from any program or other subroutine (standard or parametric). To do this, "G20" must be used. The structure of a calling block is:
N4 G20 N2.2
N4 Block number
G20 Calling a subroutine
N2.2 The two digits to the left of the period, identify the subroutine being called upon (00 through 99).
The two digits to the right of the period, indicate the number of times that subroutine is to be executed (00 through 99).
The number of times may also be programmed by an arithmetic parameter between P0 and
P255. For example: N4 G20 N10.P123
If the number of times is not programmed, the CNC will execute it only once.
The block calling the standard subroutine may not contain any other information.
Page
2
Chapter: 9
SUBROUTINES
Section:
STANDARD SUBROUTINE
(G20, G22)
9.4 IDENTIFICATION OF A PARAMETRIC SUBROUTINE (G23)
A parametric subroutine always starts with a block containing a "G23".
The structure of this first block is:
N4 G23 N2 N4 Block number
G23 Defines the beginning of a parametric subroutine
N2 Identifies the subroutine (number between "N0" and "N99").
This block cannot contain any additional information.
Program all the desired blocks after this first subroutine block and remember that a parametric subroutine may also contain parametric blocks.
A subroutine must always end with a block of the type: N4 G24. This "G24" code indicates the end of the subroutine. This block cannot contain any other information.
Atention:
Subroutines "N91" through "N99" may not be defined because they are utilized by the CNC.
The CNC memory may not contain two parametric subroutines with identical ID numbers even if they belong to different programs. However, it is possible to use the same number to identify a standard subroutine and a parametric one.
9.5 CALLING A PARAMETRIC SUBROUTINE (G21)
A parametric subroutine may be called upon from any program or other subroutine
(standard or parametric). To do this, "G21" must be used.
The structure of a calling block is:
N4 G21 N2.2 P3=K±5.5 P3=K±5.5
N4 Block number
G21 Calling a parametric subroutine
N2.2 The two digits to the left of the period, identify the subroutine being called upon
(00 through 99).
The two digits to the right of the period, indicate the number of times that subroutine is to be executed (00 through 99).
The number of times may also be programmed by an arithmetic parameter between P0 and
P255. For example: N4 G21 N10.P123
If the number of times is not programmed, the CNC will execute it only once.
P3 Number of the arithmetic parameter (P00-P254).
K Value assigned to the arithmetic parameter.
Atention:
When concluding the execution of the parametric subroutine (G24), the parameters recover the values assigned to them in the calling block even when they have been set to other values throughout the program.
Chapter: 9
SUBROUTINES
Section:
PARAMETRIC SUBROUTINE
(G21, G23)
Page
3
9.6 EXAMPLES
Example 1. Using standard subroutines without parameters
Drill four 15mm-deep holes.
N0 G90 G00 X35 Y35 M03
N5 G22 N1 ............................................... Define the standard subroutine
N10 Z-32
N15 G01 Z-50 F100
N20 G04 K1.0
N25 G00 Z0
N30 G24 .................................................... End of subroutine
N35 X60
N40 G20 N1.1 ........................................... Call subroutine N1
N45 X80 Y30
N50 G20 N1.1 ........................................... Call subroutine N1
N55 X100
N60 G20 N1.1 ........................................... Call subroutine N1
N65 X0 Y0 M05
N70 M30 ................................................... End of program
Page
4
Chapter: 9
SUBROUTINES
Section:
PROGRAMMING EXAMPLES
Example 2. Using standard subroutines with parameters
N10 P0=K48 P1=K24
N20 G1 X40 Y32 F0
N30 G22 N10 .................................. Define the standard subroutine
N40 G91 XP0 F500
N50 YP1
N60 X-P0
N70 Y-P1
N80 G24 .......................................... End of subroutine
N90 G90 X-6 Y72
N100 P0=K24 P1=K16
N110 G20 N10.1 .............................. Call the standard subroutine
N120 G01 G90 X0 Y0 F0
N130 M30 ........................................ End of program
Chapter: 9
SUBROUTINES
Section:
PROGRAMMING EXAMPLES
Page
5
Example 3. Using parametric subroutines with parameters
Perform the machining operations shown above using the same parametric subroutine.
The tool moves over the part to Z10 and the machining depth is Z-10.
N0 G90 G00 X20 Y20 Z10 S1500 M03
N10 G01 Z-10 F100
N15 G21 N1.1 P0=K20 P1=K30 P2=K-20 P3=K-10 P4=K-20 .............. Part 1
N20 G90 G00 Z10
N25 X60 Y20
N30 G01 Z-10
N35 G21 N1.1 P0=K30 P1=K10 P2=K-30 P3=K20 P4=K-30 ............... Part 2
N40 G90 G00 Z10
N45 X110 Y120
N50 G01 Z-10
N55 G21 N1.1 P0=K10 P1=K30 P2=K-10 P3=K0 P4=K-30 ................. Part 2
N60 G90 G00 Z10
N65 X0 Y0 M05
N70 M30
N100 G23 N1 ................................. Define subroutine
N105 G01 G91 YP0 F100
N110 XP1
N115 XP2 YP3
N120 XP4
N145 G24 ........................................ End of subroutine
Page
6
Chapter: 9
SUBROUTINES
Section:
PROGRAMMING EXAMPLES
Example 4. Using parametric subroutines without parameters
Starting point: X0 Y0
N10 G90 G01 X40 Y30 F0
N20 G23 N8 .............................................. Define parametric subroutine
N30 G01 G91 X50 F500
N40 Y30
N50 X-10
N60 G03 X-30 Y0 I-15 J0
N70 G01 X-10
N80 Y-30
N90 G24 .................................................... End of subroutine
N100 G01 G90 X0 Y0 F0
N110 X-70 Y50
N120 G21 N8.1 ......................................... Call subroutine
N130 G01 G90 X0 Y0 F0
N140 M30 ................................................. End of program
When the CNC reads block N120, it will execute subroutine N8 ( defined between N30 and N80) once.
Chapter: 9
SUBROUTINES
Section:
PROGRAMMING EXAMPLES
Page
7
9.7 NESTING LEVELS
It is possible to call upon a subroutine from the main program or from another subroutine
(standard or parametric) and upon another one from this one and so on up to 15 levels. Each one of these levels may be repeated 255 times.
Subroutine nesting diagram
M02 or M03
Page
8
Chapter: 9
SUBROUTINES
Section:
NESTING LEVELS
10.
PARAMETRIC PROGRAMMING
This CNC offers 255 arithmetic parameters (P0 through P254) which can be used to edit parametric blocks and perform math operations and jumps within a program. These parametric blocks may be written anywhere in the program.
The various operations to be performed with these parameters are:
F1 Addition
F2 Subtraction
F3 Multiplication
F4 Division
F5 Square root
F6 Square root of the sum of squares (Pythagorean formula)
F7 Sine
F8 Cosine
F9 Tangent
F10 Arc tangent
F11 Comparison
F12 Entire part (integer without decimals)
F13 Entire part plus one
F14 Entire part minus one
F15 Absolute value (without sign)
F16 Complement (invert sign)
F17 Memory address (location) of the indicated block
F18 X coordinate contained in the block located at the indicated address
F19 Y coordinate contained in the block located at the indicated address
F20 Z coordinate contained in the block located at the indicated address
F21 Not being used at this time.
F22 Memory address (location) of the block previous to the indicated one
F23 Selected tool offset number
F24 R value of the indicated tool
F25 L value of the indicated tool
F26 I value of the indicated tool
F27 K value of the indicated tool
F28 Not being used at this time.
F29 Number of the selected tool
F30 Logic AND function
F31 Logic OR function
F32 Logic XOR function
F33 Logic NOR function
Chapter: 10
PARAMETRIC PROGRAMMING
Section: Page
1
10.1 ASSIGNMENTS
Any value may be assigned to any parameter.
a) N4 P1 = P2
P1 takes the value of P2 while P2 keeps its original value b) N4 P1 = K1.5
P1 takes the value of 1.5
"K" indicates that it is a constant. Its value range is: ±99999.99999.
c) N4 P1= H (HEXADECIMAL value)
P1 takes the HEXADECIMAL value indicated after "H".
Possible "H" values: 0/FFFFFFFF.
d) N4 P1 = X
P1 takes the current theoretical coordinate value of the X axis.
e) N4 P1 = Y
P1 takes the current theoretical coordinate value of the Y axis.
f) N4 P1 = Z
P1 takes the current theoretical coordinate value of the Z axis.
g) N4 P1 = T
This CNC has an internal clock which keeps track of the program execution (running) time.
P1 takes the current value of this clock (always in hundredths of a second).
In order to find out the execution time required by some parts or operations, include this type of blocks at the beginning and end of the program section to be timed and then subtract the obtained values.
h) N4 P1= 0X
P1 takes the current theoretical X axis coordinate referred to Machine Reference Zero
(home).
i) N4 P1= 0Y
P1 takes the current theoretical Y axis coordinate referred to Machine Reference Zero
(home).
j) N4 P1= 0Z
Page
2
P1 takes the current theoretical Z axis coordinate referred to Machine Reference Zero
(home).
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
ASSIGNMENTS
10.2 OPERATORS "F1" through "F16"
F1 Addition
Example: N4 P1 = P2 F1 P3
P1 takes the value resulting from adding P2 and P3. That is, P1 = P2 + P3.
It may also be programmed as: N4 P1 = P2 F1 K2 which means that P1 takes the value of P2 + 2. The letter "K" indicates that it is a constant.
When the same parameter appears as an addend and a result, N4 P1 = P1 F1 K2 , it indicates that, from this moment on, it increments its value by "2" (P1 = P1 + 2).
F2 Subtraction
N4 P10 = P2 F2 P3 ............... P10 = P2 - P3
N4 P10 = P2 F2 K3 .............. P10 = P2 - 3
N4 P10 = P10 F2 K1 ............ P10 = P10 - 1
F3 Multiplication
N4 P17 = P2 F3 P30 ............. P17 = P2 x P30
N4 P17 = P2 F3 K4 .............. P17 = P2 x 4
N4 P17 = P17 F3 K8 ............ P17 = P17x 8
F4 Division
N4 P8 = P7 F4 P35 ............... P8 = P7 : P35
N4 P8 = P2 F4 K5 ................ P8 = P2 : 5
N4 P8 = P8 F4 K2 ................ P8 = P8 : 2
F5 Square root
N4 P15 = F5 P23 .................. P15 = P23
N4 P14 = F5 K9 .................... P14 = 9
N4 P18 = F5 P18 .................. P18 = P18
F6 Square root of the sum of squares
N4 P60 = P2 F6 P3 .............. P60 = P2² + P3²
N4 P50 = P40 F6 K5 ............ P50 = P40² + 5 2
N4 P1 = P1 F6 K4 ............... P1 = P1² + 4²
F7 Sine
N4 P1 = F7 K5 ...................... P1 = Sine 5 degrees
N4 P1 = F7 P2 ...................... P1 = Sine P2
The angle (P2) must be given in degrees.
F8 Cosine
N4 P1 = F8 P2 ...................... P1 = Cosine P2
N4 P1 = F8 K75 .................... P1 = Cosine 75 degrees
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
OPERATORS
"F1" through "F16"
Page
3
F9 Tangent
N4 P1 = F9 P2 .................... P1 = tg P2
N5 P1 = F9 K30 .................. P1 = tg 30 degrees
F10 Arc tangent
N4 P1 = F10 P2 .................. P1 = arc. tg P2 (result in degrees)
N4 P1 = F10 K0.5 ............... P1 = arc. tg 0.5
F11 Comparison
It compares one parameter with another one or with a constant and it activates the conditional jump flags (its usefulness will be described in the section on conditional jumps G26, G27, G28, G29).
N4 P1 = F11 P2
If P1 = P2, the "if zero" flag is activated.
If P1 > P2, the "if equal to or greater than" flag is activated.
If P1 < P2, the "if smaller than" flag is activated.
It may also be programmed as: N4 P1 = F11 K6
F12 Entire Part (Integer without decimals)
N4 P1=F12 P2 .................... P1 takes the integer value of P2.
N4 P1=F12 K5.4 ................. P1 = 5
F13 Entire part plus one
N4 P1 = F13 P2 .................. P1 takes the integer value of P2 plus 1.
N4 P1 = F13 K5.4 ............... P1 = 5 + 1 = 6
F14 Entire part minus one
N4 P1 = F14 P27 ................ P1 takes the integer value of P27 minus 1.
N4 P5 = F14 K5.4 ............... P5 = 5 - 1 = 4
F15 Absolute value
N4 P1 = F15 P2 .................. P1 takes the absolute value of P2.
N4 P1 = F15 K-8 ................ P1 = 8
F16 Complement
N4 P7 = F16 P20 ................ P7 takes the value of P20 with the opposite sign. P7 = -
P20
N4 P7 = F16 K10 ................ P7 = -10
Page
4
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
OPERATORS
"F1" through "F16"
10.3 OPERATORS "F17" through "F29"
These functions do not affect the jump flags.
F17 N4 P1 = F17 P2
P1 takes the memory address value (location) of the block number indicated by P2.
Example N4 P1 = F17 K12. P1 takes the value of the memory address where block
N12 is located.
F18 N4 P1=F18 P2
P1 takes the X coordinate value contained in the block whose address is (located at)
P2.
F18 does not admit a constant operand. Example : P1 = F18 K2 IS WRONG.
F19 N4 P1=F19 P2
P1 takes the Y coordinate value contained in the block located at P2.
F19 does not admit a constant operand. Example: P1 = F19 K3 IS WRONG
F20 N4 P1 = F20 P2
P1 takes the Z coordinate value contained in the block located at P2.
F19 does not admit a constant operand. Example: P1 = F19 K3 IS WRONG
F20 does not admit a constant operand. Example: P1 = F20 K4. IS WRONG
F21 Not being used at this time
F22 N4 P1=F22 P2
P1 takes the memory address (location) of the block prior to the location indicated by
P2.
F22 does not admit a constant operand. Example: P1 = F22 K5. IS WRONG.
F23 N4 P1 = F23
P1 takes the number of the current active tool offset.
F24 This function may be programmed in two different ways:
N4 P9=F24 K2 P9 takes the R value appearing in position 2 of the tool table.
N4 P8=F24 P12 P8 takes the R value appearing in the tool table position indicated by the value of P12.
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
OPERATORS
"F17" through "F29"
Page
5
F25 This function may be programmed in two different ways:
N4 P15=F25 K16 P15 takes the L value appearing in position 16 of the tool table.
N4 P13=F25 P34 P13 takes the L value appearing in the tool table position indicated by the value of P34.
F26 This function may be programmed in two different ways:
N4 P6=F26 K32 P6 takes the I value appearing in position 32 of the tool table.
N4 P14=F26 P15 P14 takes the I value appearing in the tool table position indicated by the value of P15.
F27 This function may be programmed in two different ways:
N4 P90=F27 K13 P90 takes the K value appearing in position 13 of the tool table.
N4 P28=F27 P5 P28 takes the K value appearing in the tool table position indicated by the value of P5.
F28 Not being used at this time.
F29 N4 P1=F29
P1 takes the number of the current active tool.
One block may contain all the desired assignments and operations as long as they do not modify more than 15 parameters.
Page
6
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
OPERATORS
"F17" through "F29"
10.4 BINARY OPERATORS "F30" THROUGH "F33"
The available binary operations are:
F30
F31
F32
F33
Logic AND function
Logic OR function
Logic XOR function
Logic NOR function
These BINARY operations also activate the internal flags depending on the results of their operations for later use when programming CONDITIONAL JUMPS/CALLS (G26,
G27, G28, G29).
Binary operations may be performed between:
Parameters P1 = P2 F30 P3
Parameters and constants P11 = P25 F31 H(8)
Constants P19 = K2 F32 K5
The "H" value must be a positive hexadecimal number of up to 8 characters. In other words, it must be between "0" and "FFFFFFFF" and may not be the first operand.
F30 Logic AND function
Example: N4 P1= P2 F30 P3 Value of P2 Value of P3 Value of P1
A5C631F C883D C001D
F31 Logic OR function
Example: N4 P11= P25 F31 H35AF9D01
Value of P25 Value of H
48BE6 35AF9D01
F32 Logic XOR function
Value of P11
35AF9FE7
Example: N4 P19= P72 F32 H91C6EF
Value of P72 Value of H
AB456 91C6EF
F33 Logic NOT function
Value of P19
9B72B9
Example: N4 P154= F33 P88 P154 takes the "ones" complement of (inverts its bits )
P88
Value of P88 Value of P154
4A52D63F B5AD29C0
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
OPERATORS
"F30" through "F33" & "F36"
Page
7
10.5 CONDITIONAL JUMP FUNCTIONS (G26, G27, G28, G29)
They are similar to function G25 (unconditional jump) described in the chapter on
"Additional Preparatory Functions" in this manual.
Functions G26, G27, G28 and G29, before jumping to the indicated program block, verify that the required condition has been met.
G26 Jump if zero.
G27 Jump if not zero.
It requires the "Zero" condition to be met.
It requires the "Zero" condition NOT to be met.
G28 Jump if less than zero.
It requires the "Less than" condition to be met.
G29 Jump if equal/greater than "0". It requires the "Less than" condition NOT to be met.
The "Zero" condition also referred to as "Equal to" is activated in the following cases:
* When the result of an operation is equal to zero.
Example: N001 P1 P3 F2 K5 If P3 = 5
* If both sides of a comparison are identical
Example: N002 P1 F11 K8 If P1 = 8
The "Less than" condition is also referred to as "Negative" and it is activated in the following cases:
* When the result of an operation is less than zero (negative).
Example: N001 P1 = P3 F2 K5 If P3 < 5
* When the first operand in a comparison is smaller than second one.
Example: N002 P1 F11 K8 If P1 < 8
Atention:
Assignments and non-parametric functions do not alter the status of the condition flags.
Programming example: N060 P2 F11 K22
N065 G01 X10
N070 Y20
N071 G26 N100
N072 G28 N200
N073 G29 N300
Block N060 does a comparison
Blocks N65 and N70 do not change the condition flags.
Thus, If P2 = 22, the program continues at block N100
If P2 < 22, the program continues at block N200
If P2 > 22, the program continues at block N300
Care must be taken when programming functions G26 and G29. If, in the above example, the following were programmed instead: N071 G28 N200
N072 G29 N300
N073 G26 N100
The program would not execute N073. With P2 < 22, it would jump to N200 and, with
P2 > 22, it would jump to N300. Thus, skipping block N073.
Page
8
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
JUMP FUNCTIONS
(G26, G27, G28, G29)
Parametric programming example to calculate the various points forming a cardioid, its formula being: R = B |cos A/2|
Where: X0 Y0 is the starting point and
P0 = A (angle)
P1 = B
P2 = A/2
P3 = cos A/2
P4 = |cos A/2|
P5 = R = B |cos A/2|
N10 G93 G01 F500
N20 P0=K0 P1=K30 ............................................................. A=0, B=30
N30 P2=P0 F4 K2 P3=F8 P2 P4=F15 P3 P5=P1 F3 P4 ....... R = B |cos A/2|
N40 G01 G05 R P5 A P0 ...................................................... Motion block
N50 P0=P0 F1 K5 ................................................................. Angular step of 5°
N60 P0=F11 K365 ................................................................ If A=365° --> End
N70 G27 N30 ........................................................................ If not, calculate new point
N80 X0 Y0
N90 M30
Chapter: 10
PARAMETRIC PROGRAMMING
Section:
JUMP FUNCTIONS
(G26, G27, G28, G29)
Page
9
ERROR
CODES
008
009
010
011
012
004
005
006
007
001 This error occurs in the following cases:
* When the first character of the block to be executed is not an "N".
* When while BACKGROUND editing, the program in execution calls a subroutine located in the program being edited or in a later program.
The order in which the part-programs are stored in memory are shown in the part-program directory. If during the execution of a program, a new one is edited, this new one will be placed at the end of the list.
002
003
Too many digits when defining a function in general.
This error occurs in the following cases:
* When a negative value has been assigned to a function which does not accept the "-" sign.
* When an incorrect value has been assigned to an automatic operation:
Positioning in line: ..................................... If L=0, Xn=X1, Yn=Y1, I=0
If L=0, Xn=X1, Yn=Y1, N=0
If I=0, N=0
If I>0, L/I fraction
Positioning in arc: ...................................... If N=0
If R=0, Xc=X1, Yc=Y1
Positioning in rectangle or grid pattern: If
If
LX=0, IX=0
LX=0, NX=0 or LY=0, IY=0 or LY=0, NY=0
If LX>0, IX=0, NX<2 or LY>0, IY=0, NY<2
If LX>0, IX>0, LX/IX fraction
If LY>0, IY>0, LY/IY fraction
Rectangular pocket .................................... If L=0 or H=0
If r>(L/2) or r>(H/2)
Circular pocket .......................................... If Tool radius > R
Corner roughing ........................................ If L=0
If r>L
Surface milling .......................................... If L=0 or H=0 or r>H or H=0
Not being used at this time.
Parametric block programmed wrong.
There are more than 10 parameters affected in a block.
Division by zero.
Square root of a negative number.
Parameter value too large.
M41, M42, M43 or M44 has been programmed.
More than 7 "M" functions in a block.
This error occurs in the following cases:
- Function G50 is programmed wrong
- Tool dimension values too large.
- Zero offset values ( G53/G59 ) too large.
013
014
015
016
017
018
Not being used at this time.
A block has been programmed which is incorrect either by itself or in relation with the program history up to that instant.
Functions G20, G21, G22, G23, G24, G25, G26, G27, G28, G29, G30, G31, G32, G50, G52, G53, G54, G55,
G56, G57, G58, G59, G72, G73, G74, G92 and G93 must be programmed alone in a block.
The called subroutine or block does not exist or the block searched by means of special function F17 does not exist.
Negative or too large thread pitch value.
Error in blocks where the points are defined by means of angle-angle or angle-coordinate.
019
020
021
022
023
025
026
027
028
029
030
031
This error is issued in the following cases:
- After defining G20, G21, G22 or G23, the number of the subroutine it refers to is missing.
- The "N" character has not been programmed after function G25, G26, G27, G28 or G29.
- Too many nesting levels.
The axes of the circular interpolation are not programmed correctly.
There is no block at the address defined by the parameter assigned to F18, F19, F20, F21, F22.
An axis is repeated when programming G74.
K has not been programmed after G04.
Error in a definition block or subroutine call, or when defining either conditional or unconditional jumps.
This error is issued in the following cases:
- Memory overflow.
- Not enough free tape or CNC memory to store the part-program.
I/J/K has not been defined for a circular interpolation or thread.
An attempt has been made to select a tool offset at the tool table or a non-existent external tool (the number of tools is set by machine parameter).
Too large a value assigned to a function.
This error is often issued when programming an F value in mm/min (inch/min) and, then, switching to work in mm/rev (inch/rev) without changing the F value.
The programmed G function does not exist.
Tool radius value too large.
032 Tool radius value too large.
033 A movement of over 8388 mm or 330.26 inches has been programmed.
Example: Being the X axis position X-5000, if we want to move it to point X5000, the CNC will issue error
33 when programming the block N10 X5000 since the programmed move will be:
5000 - (-5000) = 10000 mm.
In order to make this move without issuing this error, it must be carried out in two stages as indicated below:
N10 X0
N10 X5000
; 5000 mm move
; 5000 mm move
034
035
036
037
038
039
040
041
S or F value too large.
Not enough information for corner rounding, chamfering or compensation.
Repeated subroutine.
Function M19 programmed incorrectly.
Function G72 or G73 programmed incorrectly.
It must be borne in mind that if G72 is applied only to one axis, this axis must be positioned at part zero (0 value) at the time the scaling factor is applied.
This error occurs in the following cases:
- More than 15 nesting levels when calling subroutines.
- A block has been programmed which contains a jump to itself. Example: N120 G25 N120.
The programmed arc does not go through the defined end point (tolerance 0.01mm) or there is no arc that goes through the points defined by G08 or G09.
This error is issued when programming a tangential entry as in the following cases:
- There is no room to perform the tangential entry. A clearance of twice the rounding radius or greater is required.
042
- If the tangential entry is to be applied to an arc (G02, G03), The tangential entry must be defined in a linear block.
This error is issued when programming a tangential exit as in the following cases:
- There is no room to perform the tangential exit. A clearance of twice the rounding radius or greater is required.
043
044
045
046
047
048
049
- If the tangential exit is to be applied to an arc (G02, G03), The tangential exit must be defined in a linear block.
Polar origin coordinates (G93) defined incorrectly.
Not being used at this time.
Function G36, G37, G38 or G39 programmed incorrectly.
Polar coordinates defined incorrectly.
A zero movement has been programmed during radius compensation or corner rounding.
Not being used at this time.
Chamfer programmed incorrectly in a rectangular pocket or corner roughing operation in such way that:
* The tool cannot machine it because the chamfer is too small.
* A chamfer that big cannot be machined with those L, H, E parameter values
050 Functions M06, M22, M23, M24, M25 must be programmed alone in a block.
051 * A tool change cannot be performed without being in the change position.
052 * The requested tool is not in the magazine.
057
058
059
060
061
053
054
055
056
Not being used at this time.
There is no tape in the cassette reader or the reader head cover is open.
Parity error when reading or recording a cassette.
Not being used at this time.
Write-protected tape.
Sluggish tape transport.
Communication error between the CNC and the cassette reader.
Internal CNC hardware error. Consult with the Technical Service Department.
Battery error.
The memory contents will be kept for 10 more days (with the CNC off) from the moment this error occurs. The whole battery module located on the back must be replaced. Consult with the Technical Service Department.
Atention:
Due to danger of explosion or combustion, do not try to recharge the battery, do not expose it to temperatures higher than 100°C (232°F) and do not short the battery leads.
064 * External emergency input (pin 14 of connector I/O1) is activated.
065 Not being used at this time.
066 * X axis travel limit overrun.
It is generated either because the machine is beyond limit or because a block has been programmed which would force the machine to go beyond limits.
067 * Y axis travel limit overrun.
It is generated either because the machine is beyond limit or because a block has been programmed which would force the machine to go beyond limits.
068 * Z axis travel limit overrun.
It is generated either because the machine is beyond limit or because a block has been programmed which would force the machine to go beyond limits.
069 Not being used at this time.
070 ** X axis following error.
071 ** Y axis following error.
072 ** Z axis following error.
073 Not being used at this time.
074 ** Spindle speed value too large.
075 ** Feedback error at connector A1.
076 ** Feedback error at connector A2.
077 ** Feedback error at connector A3.
078 ** Feedback error at connector A4.
079 ** Feedback error at connector A5.
080 This error occurs when using a tool smaller than the machining pass "G" in a rectangular/circular pocket or in a corner roughing operation.
081 This error occurs when the tool radius is greater than "(L/2)-E" or "H/2)-E".
082 ** Parity error in general parameters.
083 This error occurs when programming "r>0" or "C>0" in a rectangular pocket or corner roughing operation.
084
085
086
This error occurs when programming a tool radius greater than "R-E" in a circular pocket.
This error occurs when using a 0-radius tool (tool offset) having programmed "G=0" (machining pass) in a rectangular/circular pocket or in a corner roughing operation.
This error occurs when assigning an incorrect value to an automatic operation or to a machining operation:
- Rectangular pocket ................ If P=0 or I=0
- Circular pocket ...................... If P=0 or I=0
- Corner roughing ..................... If P=0 or I=0
- Surface milling ...................... If P=0 or I=0
- Center punching: ................... If P=0, =0
- Drilling: ................................. If P=0 or I=0
- Tapping: ................................. If P=0
- Boring, reaming: .................... If P=0
087 ** Internal CNC hardware error. Consult with the Technical Service Department.
088 ** Internal CNC hardware error. Consult with the Technical Service Department.
089 * All the axes have not been homed.
This error comes up when it is mandatory to search home on all axes after power-up. This requirement is set by machine parameter.
090 ** Internal CNC hardware error. Consult with the Technical Service Department.
091 ** Internal CNC hardware error. Consult with the Technical Service Department.
092 ** Internal CNC hardware error. Consult with the Technical Service Department.
093 ** Internal CNC hardware error. Consult with the Technical Service Department.
094
095
Parity error in tool table or zero offset table G53-G59.
This error occurs when the tool radius is larger than the rounding radius "r" in a rectangular pocket or corner roughing operation.
096 ** Parity error in Z axis parameters.
097 ** Parity error in Y axis parameters.
098 ** Parity error in X axis parameters.
099 ** Parity error in M table.
100 ** Internal CNC hardware error. Consult with the Technical Service Department.
101 ** Internal CNC hardware error. Consult with the Technical Service Department.
105 This error comes up in the following cases:
> A comment has more than 43 characters.
> A program has been defined with more than 5 characters.
> A block number has more than 4 characters.
> Strange characters in memory.
106 ** Inside temperature limit exceeded.
107 Not being used at this time.
108 ** Error in Z axis leadscrew error compensation parameters.
109 ** Error in Y axis leadscrew error compensation parameters.
110 ** Error in X axis leadscrew error compensation parameters.
111
112
113
Not being used at this time.
Not being used at this time.
Not being used at this time.
114 Not being used at this time.
115 * Watch-dog error in the periodic module.
This error occurs when the periodic module takes longer than 5 milliseconds.
116 * Watch-dog error in the main module.
This error occurs when the main module takes longer than half the time indicated in machine parameter "P729".
117 * The internal CNC information requested by activating marks M1901 thru M1949 is not available.
118 * An attempt has been made to modify an unavailable internal CNC variable by means of marks M1950 thru
M1964.
119 Error when writing machine parameters, the decoded M function table and the leadscrew error compensation tables into the EEPROM memory.
120
This error may occur when after locking the machine parameters, the decoded M function table and the leadscrew error compensation tables, one tries to save this information into the EEPROM memory.
Checksum error when recovering (restoring) the machine parameters, the decoded M function table and leadscrew error compensation tables from the EEPROM memory.
Atention:
The ERRORS indicated with "*" behave as follows:
They stop the axis feed and the spindle rotation by cancelling the Enable signals and the analog outputs of the CNC.
hey interrupt the execution of the part-program of the CNC if it was being executed.
The ERRORS indicated with "**" besides behaving as those with an "*", they activate the
INTERNAL EMERGENCY OUTPUT.
advertisement
* Your assessment is very important for improving the workof artificial intelligence, which forms the content of this project
Related manuals
advertisement