FAGOR 800T CNC

SELF-TEACHING Manual

Ref. 9804 (ing)

INDEX
Chapter 1
Theory on CNC machines
1.1.- Machine axes .....3
1.2.- Machine reference zero and part zero .......4
1.3.- Home Search .........5
1.4.- Travel limits .......... 6
1.5.- Part zero preset ..........7
1.6.- Programming units ....8
1.7.- Spindle speed ........ 9
1.8.- Axis feedrate ....11
Chapter 2
Theory on tools
2.1.- The tool turret ....3
2.2.- Tool table .......... 4
2.3.- Tool calibration ....11
Chapter 3
Hands-on training
3.1.- Screen and keyboard description ...3
3.1.1.- Power-up ..........3
3.1.2.- Keyboard description .......4
3.1.3.- Description of the screen .........6
3.2.- Home Search .....7
3.3.- Spindle .......8
3.3.1.- Speed ranges (gears) ........8
3.3.2.- Work in RPM (Revolutions per minute) ....... 10
3.3.3.- Work at Constant Surface Speed (CSS) .... 11
3.4.- Axis jog ... 13
3.4.1.- Handwheels ........14
3.4.2.- Incremental JOG ....15
3.4.3.- Continuous JOG mm/min ......16
3.4.4.- Continous JOG mm/rev .....17
3.4.5.- Rapid jog key .....19
3.4.6.- Move the axes with keystroke sequence: BEGIN+start or END+start .. 20
3.5.- Tools ........22
3.5.1.- Tool selection .....22
3.5.2.- Tool calibration ......24
3.5.3.- How to complete the tool table ..27
3.6.- Checking for proper calibration ..28

Chapter 4
Automatic operations
4.1.- Operating modes ....... 3
4.2.- Example of turning in Semiautomatic mode .........7
4.3.- Example of turning in Automatic mode ......10
4.3.1.- Programming ..... 10
4.3.2.- Simulate an operation ............13
4.3.3.- Executing an operation ......16
Chapter 5
Summary of work cycles
5.1.- Facing. Automatic ..... 2
5.2.- Taper turning. Automatic ...... 3
5.3.- Rounding. Automatic 1 ..........4
5.4.- Rounding. Automatic 2 ......5
5.5.- Profile rounding .....6
5.6.- Threading. Automatic ........8
5.7.- Grooving ... 9
5.8.- Simple drilling .....10
5.9.- Tapping ....11
5.10.- Profiles ...... 12
Chapter 6
Part-programs
6.1.- Conversational part-programs .......3
6.1.1.- What is a conversational part-program? ..........3
6.1.2.- Edit a part-program ......4
6.1.3.- Modify a part-program ........ 7
6.1.4.- Simulate an operation of a part-program ...10
6.1.5.- Simulate a part-program ....11
6.1.6.- Execute an operation of a part-program ....12
6.1.7.- Execute a part-program from a particular operation on .....13
6.1.8.- Execute a part-program ......14
6.1.9.- Delete a part-program ........17
6.2.- Program P99996 ......18
6.2.1.- What is it? ......18
6.2.2.- How is it edited? ........19
6.2.3.- Execute/simulate program P99996 ............22

Appendix I
Other machining operations on a lathe
I.1.- Introduction ........2
I.2.- Spindle orientation .........3
I.3.- Live tool .4
I.4.- Multiple drilling .....5
I.5.- Slot milling .... 6
Appendix II
Peripherals
II.1.- Peripherals ....2
II.1.1.- Peripheral mode ...... 2
II.2.- Lock/Unlock .........4

1.- Theory on CNC machines

800T CNC
This chapter describes:
How to name the axes of the machine.
What machine reference zero and part zero are.
What Home Search is.
What travel limits are.
How to preset a part zero.
Which are the programming units.
> millimeters/inches.
> radius/diameter.
Ways to operate with the spindle.
> RPM/CSS. (Revolutions Per Minute/Constant Surface Speed).
Ways to move the axes.
> mm/min or mm/rev.

Self-teaching Manual

Chapter 1 Page 2

800T CNC
1.1 Machine Axes.

Z axis: Along the machine.

X axis: Across the machine.
Self-teaching Manual

Chapter 1 Page 3

800T CNC
1.2 Machine reference zero and part zero.
They are the references the machine needs in order to work:
Machine ref. zero (OM): Is set by the manufacturer and it is the origin point
for the axes.
Part zero (OP): Is set by the operator. It is the parts origin or datum point
with respect to which the movements are programmed. It could be set
anywhere on the part.

Home

Self-teaching Manual

Chapter 1 Page 4

800T CNC
1.3 Home Search.
When the CNC is off, the axes may be moved by hand or by accident.
In these situations, the CNC no longer keeps track of the real position of the axes. That is
why a Home Search should be carried out on power-up.
When searching home, the axes move to the home point set by the manufacturer and the
CNC assumes the value of the coordinates set by the manufacturer for that point. When
searching home, the part zero is lost.
Home
Home
Turrent Ref.
Real X

Real Z

Home: Set by the manufacturer. It is the point where the axes move during Home
Search.
Turret Ref.: Set by the manufacturer. Point moving with the turret. It is the point
that moves during Home Search.
Self-teaching Manual

Chapter 1 Page 5

800T CNC
1.4 Travel limits.
There are two types of limits:
Hard limits: Mechanical limits set on the machine to prevent the carriage
from moving beyond the ways.
Software limits: Software limits set at the CNC by the manufacturer to
prevent the carriage from running into the machines hard limits.

Home

Self-teaching Manual

Hard limits
Software limits

Chapter 1 Page 6

800T CNC
1.5 Part zero preset.
It is easier to program movements from a part zero.
The part zero is only set on the Z axis.

OM: Machine Ref. zero.

OP: Part zero.

Self-teaching Manual

Chapter 1 Page 7

800T CNC
1.6 Programming units.
The movement units of the CNC can be millimeters or inches.

millimeters

inches

The X axis movements may also be programmed in radius or in diameter.

Radius

Diameter

X=0 Z=0

X=0 Z=0

X=12 Z=-12

X=24 Z=-12

X=12 Z=-42

X=24 Z=-42

X=22 Z=-52

X=44 Z=-52

Self-teaching Manual

Chapter 1 Page 8

800T CNC
1.7 Spindle speed.
It could be defined in two ways:
Cutting speed (V):
It is the linear speed between the part and the tool at the
contact point.
Turning speed (N):
It is the angular speed of the part.
The relationship between them is: V=2**R*N/1000
The CNC offers two ways to operate with the spindle:
CSS: Constant Surface Speed.

RPM: Revolutions per minute.

V1=V2
N1<N2

N1=N2
V1>V2

The CNC maintains the cutting speed (V)

constant while varying the turning speed (N).

The CNC maintains the turning speed (N)

constant while varying the cutting speed (V).

Self-teaching Manual

Chapter 1 Page 9

800T CNC
To work at CSS, two things must be borne in mind:
The part zero must be at the parts turning
axis so that the calculated turning speed is the
same as the best cutting speed.

The maximum turning speed must be

programmed because the turning speed increases
as the diameter decreases and a particular speed
should not be exceeded on parts with a large
diameter.
The CNC works at Constant Surface Speed
(Vc) and, starting at diameter Dc (when
N=Nmax), it works at constant turning speed
(N).

Self-teaching Manual

Chapter 1 Page 10

800T CNC
1.8 Axis feedrate.
The feedrate of the axes can be programmed in two ways:
mm/rev: The axis feedrate changes depending on spindle speed. If the
spindle is stopped, the axes do not move.
mm/min: The axis feedrate is independent of the spindle speed. The axes
move even when the spindle is stopped.

NOTE
It is recommended to work at Constant Surface Speed (CSS) and with the
feedrate in mm/rev. This way, the tool lasts longer and the resulting part finish is
better.

Self-teaching Manual

Chapter 1 Page 11

2.- Theory on tools

800T CNC
This chapter describes:
What the tool turret is.
What the tool table is and what information it contains.
What tool presetting is.
Defects due to errors in the tool table.
> Due to wrong tool calibration.
> Due to wrong tool location codes (tool shapes).
> Due to wrong tool radius values.

Self-teaching Manual

Chapter 2 Page 2

800T CNC
2.1 The tool turret.
The tools this CNC can use are placed on the tool turret. This turret may have
either a manual or automatic tool changer. When manual, the tool change is carried
out like on a conventional machine. When automatic, all the tools will be placed on
the turret and the CNC will rotate the whole turret to put the tool at the work
position.

Turret with manual tool change

Self-teaching Manual

Turret with automatic tool changer

Chapter 2 Page 3

800T CNC
2.2 Tool table.
The tool table contains tool information such as their position on the turret,
dimensions, etc.
When changing the tool, the CNC takes this tool information.
The information kept in the tool table refers to: T, X, Z, F, R, I, K:

T: Tool number.
X: Tool length (in radius) along the X axis
Z: Tool length along the Z axis.

Self-teaching Manual

Tool Ref.

Chapter 2 Page 4

800T CNC
R: Tool radius.

I: Tool wear along the X axis.

K: Tool wear along the Z axis.

Self-teaching Manual

Chapter 2 Page 5

800T CNC
F: Location code or tool shape as it has been calibrated.
Once the tool dimensions are known;

The CNC must know which is the calibration

point for that tool (location code) to compensate for
the shaded area (radius compensation).

The location code depends on the orientation of

the machine axes.

Self-teaching Manual

Chapter 2 Page 6

800T CNC
Table of location codes.

F7

F3

F6

F2

F5

F1

F4

F8

F0

Self-teaching Manual

Chapter 2 Page 7

800T CNC
Most common location codes.

Self-teaching Manual

Chapter 2 Page 8

800T CNC
Table of location codes

F1

F5

F2

F6

F3

F7

F4

F8

F0

Self-teaching Manual

Chapter 2 Page 9

800T CNC
Most common location codes.

Self-teaching Manual

Chapter 2 Page 10

800T CNC
2.3 Tool calibration.
By calibrating a tool, we indicate to the CNC the tool dimensions. It is essential
to carry this operation out properly for obtaining the parts with the right
dimensions and for controlling the same point after changing a tool.

Different tool dimensions, same point.

Self-teaching Manual

Chapter 2 Page 11

800T CNC
DEFECTS DUE TO WRONG LENGTH CALIBRATION

Part to be machined

X1: Real dim.

Z1: Real dim.

X2: Wrong dim.

X2<X1(Real dim.)

Tools

Right part dimensions

Wrong part dimensions

Wrong machining
Tools calibrated wrong

Self-teaching Manual

Right machining
Tools calibrated right

Chapter 2 Page 12

800T CNC
DEFECTS DUE TO WRONG LOCATION CODES
Real tool tip
The tool has a real tip
and another theoretical
tip.

Theoretical tool tip

To work with the theoretical tool tip, the

CNC needs to know which is the tool
calibration point (location code) in order to
compensate for the shaded area (radius
compensation).

When working with the theoretical tool tip, there

are machining ridges left. To avoid this, the CNC
works with the real tool tip.

Working with
theoretical tool tip

If the wrong location code is entered, the

error
increases
instead
of
being
compensated.

Working with real tool tip

Self-teaching Manual

Chapter 2 Page 13

800T CNC
DEFECTS DUE TO WRONG RADIUS VALUES

Rr

Rf

Rr: Real radius.

Rf: Wrong radius (false).
Machining ridges

Rr
Rf
There is residual stock due to the radius
difference.

Self-teaching Manual

Chapter 2 Page 14

3.- Hands-on training

800T CNC
This chapter describes:
The screen and the keyboard.
How to carry out a Home Search.
Ways to operate with the spindle.
> What the speed ranges (gears) are.
> Operate at CSS or in RPM.
Ways to move the axes.
> Selection of feedrate type. (mm/min or mm/rev)
> Jog modes. (Handwheels, incremental JOG, continuous JOG...)
Tool handling.
> Types of tool changer. (Manual or automatic).
> Tool calibration.
> Tool table.
Calibration verification.

Self-teaching Manual

Chapter 3 Page 2

800T CNC
3.1 Screen and keyboard description.
3.1.1 Power-up.

After the message:

PASSED
press any key to get into work
mode.

GENERAL TEST
PASSED

Welcome screen

Self-teaching Manual

Chapter 3 Page 3

800T CNC
3.1.2 Keyboard description.

Compact keyboard

Modular keyboard

1.- Screen. (On the modular, the CRT is separate from the keyboard).
2.- Keyboard to define special operations and their parameters.
3.- Alpha-numeric keyboard.
4.- Operator panel.
NOTE: Refer to the Operation Manual Chapter 1 Sections. 1.2/1.2.1/1.2.2
Self-teaching Manual

Chapter 3 Page 4

800T CNC
Description of the operator panel.

Compacts operator panel

Modulars operator panel

1. Axes jogging keys.

2. Work mode selector. (Continuous jog (FEED), incremental (JOG) or with
handwheel (
)).
3. Selection of the turning direction (
) and spindle start-up. Spindle speed
override (
) between 50% and 120%
4. Keyboard for CYCLE START (
) and CYCLE STOP (
).
5. Emergency stop.
NOTE: Refer to the Operation Manual Chapter 1 Section 1.2.3
Self-teaching Manual

Chapter 3 Page 5

800T CNC
3.1.3 Description of the screen.

1.- Work mode: Standard, Automatic, turning, threading...

Status during execution: In execution, interrupted or in position.
2.- Tool position in X and Z, spindle speed S and active tool.
Information on work units and active spindle speed range.
3.- Programmed cutting conditions and percentage being applied. Work mode: RPM or CSS
Active tool.
4.- BEGIN and END coordinates. When selecting an operation, it shows a drawing and the
associated parameters.
5.- Editing area and CNC messages.
6.- PLC messages.

NOTE: Refer to the Operation Manual Chapter 1 Section 1.1

Self-teaching Manual

Chapter 3 Page 6

800T CNC
3.2 Home Search.
After powering the machine up, carry out the Home Search just in case the
axes of the machine have moved while the CNC was off.
1st.- The CNC does not know the position of the
carriages. X?, Z? different from the X, Z displayed.

2nd.-Home the X axis.

Press [X]+
+
Home

Home

4th.-The CNC shows the coordinates referred

to machine ref. zero Home (OM) taking the
tools X, Z dimensions.

3rd.-Home the Z axis.

Press [Z]+
+

Home

Home

Home X

Home Z

NOTE: Refer to the Operation Manual Chapter 1 Section 1.4.1

Self-teaching Manual

Chapter 3 Page 7

800T CNC
3.3 Spindle.
The spindle of a machine can work in two modes:
RPM: At constant turning speed. (Section 1.7)
CSS: At constant surface speed.(Section 1.7)
Press [CSS] to select the work mode.
3.3.1 Speed ranges (gears).
With this CNC the machine can have a gear box. By means of RANGES, we
can choose the best gear ratio for the programmed spindle speed.
P

Constant Power

Constant Power

RANGE 2

RANGE 1

If the work speed is between N1 and N2, RANGE 1 should be used and if between
N2 and N3, RANGE 2. Always try to work at constant power.
Self-teaching Manual

Chapter 3 Page 8

800T CNC
There are two types of gear changers:
Automatic.
If the machine has an automatic gear changer, the CNC selects the right range
when it has to be changed.
Manual.
If the machine does not have an automatic gear changer, when a gear change is
required, the CNC acts as follows:
The editing window of the CNC (last row) shows the range to be selected.
Make the change and press [ENTER].
The CNC considers the range change completed and starts the spindle.

NOTE: Refer to the Operation Manual Chapter 4 Section 4.4/4.4.1/4.4.2

Self-teaching Manual

Chapter 3 Page 9

800T CNC
3.3.2 Work in RPM mode. (Revolutions per minute)
To select the work speed (in rpm), press:
[S] + (turning speed) +
If the machine has a manual gear changer, the CNC will ask the user to change gears if
so required.
If the machine has an automatic gear changer, the CNC will assume the new range.
The CNC shows the following information:
F 0000.000

100%

RPM 1250

Selected
speed

100%

T2

Applied
override

Use the JOG keys of the operator panel to start the spindle.
Spindle clockwise.
Stop the spindle.
Spindle counter-clockwise.
Increase or decrease the applied override % in increments of 5% (between 50% &
120%).

NOTE: Refer to the Operation Manual Chapter 4 Section 4.2/4.5/4.6/4.7

Self-teaching Manual

Chapter 3 Page 10

800T CNC
3.3.3 Work at Constant Surface Speed. (CSS)
Before programming the cutting speed, the working speed range must be
selected. The CNC assumes the current range by default. To change the range,
select a turning speed in RPM within the range to be used. Once the change is
completed, enter the CSS mode and press [CSS].
To select the cutting speed (m/min) , press:
[S] + (cutting speed) +
To select the maximum turning speed (in rpm), press:
[S] +
+ (maximum speed) + [ENTER]
The CNC shows the following information:
F 0000.000

100%

CSS 250
Selected
cutting
speed

100%

SMAX 1500 T2

Applied
override

Maximum turning
speed selected

Self-teaching Manual

Chapter 3 Page 11

800T CNC
Start the spindle using the JOG keys of the operator panel.
Spindle clockwise.
Stop the spindle.
Spindle counter-clockwise.
Increases or decreases the applied override % in increments of 5%
(between 50% and 120%).
Depending on the position of the axes, the turning speed will be different:
If X decreases, the RPM increase.
If X increases, the RPM decrease.
NOTE
While machining an operation, NO range change will take place.
To work at constant surface speed, the tools MUST BE calibrated.
NOTE: Refer to the Operation Manual Chapter 4 Section 4.3/4.3.1
Self-teaching Manual

Chapter 3 Page 12

800T CNC
3.4 Axis jog.
To jog the axes, we will use:
Each key is used for
moving the axis in one
direction according to
the axes of the
machine.
(Section 1.1)
JOG keys

It can have one or

two handwheels.
The axes move in
the turning direction
of the handwheels.
Handwheel

To select the jog mode, use the selector switch:

Incremental jog

Continuous jog

Handwheel jog

Self-teaching Manual

Chapter 3 Page 13

800T CNC
The axes may be moved in mm/min or mm/rev. To select the type of feedrate, press:

[AUX] + [2] < F mm(inches)/min <---> F mm(inches)/rev >

To quit this option, press [AUX], [END] or [CLEAR].
3.4.1 Handwheels.
Select the feedrate of the carriages with the selector switch. (
It does not matter if it is in mm/min. mode or in mm/rev. mode.

position)

POSITION

1
10
100

Handwheel

Selector switch

D istance per
increment on the
handwheel dial
1 m icron.
10 m icrons
100 m icrons

Jogging distance table

Jog the axes with the handwheels.

If the machine has 1 handwheel:
Select an axis with the JOG keys.
The machine moves the axis as the handwheel is being turned.
If the machine has 2 handwheels:
The machine moves an axis with each handwheel.

NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.3

Self-teaching Manual

Chapter 3 Page 14

800T CNC
3.4.2 Incremental JOG .
Every time a JOG key is pressed, the axis will move the selected increment.
Select the distance to move at the selector (JOG position).
Move the axes with the JOG keys.
Only in mm/min. mode.

Actual displacement: 0.001 mm

JOG keys
Actual displacement: 1 mm

NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.2

Self-teaching Manual

Chapter 3 Page 15

800T CNC
3.4.3 Continuous JOG. mm/min.
Select the type of feedrate: mm/min .
Enter the feedrate value:
[F] + 120 <feedrate value> + [ENTER]
Change the % override of the axes with the selector switch in FEED position.
Jog the axis with JOG keys.

Actual displacement: 60 mm/min (50%)

Actual displacement: 120 mm/min (100%)

JOG keys

Selector Switch

NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.1

Self-teaching Manual

Chapter 3 Page 16

800T CNC
3.4.4 Continuous JOG. mm/rev.
In this mode, the feedrate is a function of the spindle rpm. Thus, the spindle must
be turning in order for the axes to be able to move.
Select the type of feedrate: mm/rev.
Enter the feedrate value:
[F] + 0.1 <Feedrate value> + [ENTER]
Try to jog the axes with JOG keys.
The axes will not move because the spindle is stopped.
Start the spindle in RPM mode.
Change the % override for the axes with the selector switch in FEED position.
Jog the axes with JOG keys.
Actual displacement: 0.05 mm/rev. (50%)

JOG keys

Selector Switch

Actual displacement: 0.1 mm/rev. (100%)

Self-teaching Manual

Chapter 3 Page 17

800T CNC

Stop the spindle.

Change the spindle work mode to Constant Surface Speed (CSS),
Start the spindle.
Check how the spindle speed varies while moving the X axis.
If X decreases, the spindle speed increases.
If X increases, the spindle speed decreases.
Stop the spindle.

NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.1

Self-teaching Manual

Chapter 3 Page 18

800T CNC
3.4.5 Rapid jog key.
Jog the axes with the JOG keys and press the Rapid jog key at the same
time.
It does not matter if it is in mm/min. or mm/rev. mode, the axes will move as fast
as possible. (Set by the manufacturer).

Actual movement: Rapid feedrate

Rapid jog key
JOG keys

Any position

NOTE: Refer to the Operation Manual Chapter 2 Section 2.3.1

Self-teaching Manual

Chapter 3 Page 19

800T CNC
3.4.6 Move the axes with keystroke sequence: BEGIN + start and END + start.
1.- Select the feedrate value.
2.- Select the BEGIN and END points.
Moving the machine by hand:
BEGIN
or END

[BEGIN] or [END]
[ENTER]

BEGIN
or END

BEGIN
or END

[BEGIN] or [END]
[X]
[ENTER]

At the keyboard:
1. Press [BEGIN] or [END]
2. [X]
3. (X value)

[BEGIN] or [END]
[Z]
[ENTER]

4. [Z]
5. (Z value)
6. [ENTER]

Self-teaching Manual

Chapter 3 Page 20

800T CNC
3.- Moving to the BEGIN or END points.
Moving two axes:
1.[BEGIN] +
2.[END] +

Moving one axis:

1.[BEGIN] + [X] +
2.[BEGIN] + [Z] +
3.[END] + [X] +
4.[END] + [Z] +

:Interrupts the movements.

: Resumes execution.
[RESET]+[RESET]: Cancels the execution.
NOTE: Refer to the Operation Chapter 2 Section 2.4
Self-teaching Manual

Chapter 3 Page 21

800T CNC
3.5 Tools.
3.5.1 Tool selection.
Depending on the machine, there are two possibilities:
Machine with manual tool changer.
The tool change is carried out like on a conventional machine:
Change the tool on the machine.

Remove the old tool

Put the new tool in

Press [TOOL].
Enter the tool number so the CNC assumes the values of the corresponding
tool table.
Press
NOTE: If when executing a part, a tool change is necessary, the CNC stops the spindle
and shows a message requesting the number of the required tool.
Self-teaching Manual

Chapter 3 Page 22

800T CNC

Machine with automatic tool changer.

No tool has to be removed.
Press [TOOL].
Enter the tool number.
Press
The CNC rotates the turret until the new tool is in work position.

NOTE: If while making a part, a tool change is necessary, the CNC makes the change
automatically, takes the turret to the change position and makes the change.

NOTE: Refer to the Operation Manual Chapter 2 Section 2.2

Self-teaching Manual

Chapter 3 Page 23

800T CNC
3.5.2 Tool calibration.
Just before calibrating the tools,a Home Search must be carried out on all axes.
Homing the X axis.
[X]+
+

Homing the Z axis.

[Z]+
+
Home

Home

To calibrate a tool, a part previously turned and faced is needed.

Use continuous JOG or handwheels

Self-teaching Manual

Chapter 3 Page 24

800T CNC
Measure the part.
Enter in calibration mode
[AUX] + [3]<Tool> + [2]<Tool calibration >
To calibrate, start the spindle.
Answer the questions asked by the CNC.
1.- Parts X dimension.
(radius or diameter) + [ENTER]
2.- Parts Z dimension.
(Length) + [ENTER]
3.- Tool number.
[TOOL] + (tool number) +

Self-teaching Manual

Part dimensions

Chapter 3 Page 25

800T CNC
4.- Move the axes in JOG and touch the part along the X axis. Press:
[X] + [ENTER]
The CNC shows the X coordinate.
5.- Move the axes in JOG and touch the part along the Z axis. Press:
[Z] + [ENTER]
The CNC shows the Z coordinate.

[X] + [ENTER]

[Z] + [ENTER]

To calibrate another tool, repeat steps 3, 4, and 5.

Stop the spindle.
To exit this mode, press [END].
NOTE: Refer to the Operation Manual Chapter 3 Section 3.4.2
Self-teaching Manual

Chapter 3 Page 26

800T CNC
3.5.3 How to complete the tool table.
The I, K values are set to zero when calibrating.
To enter the other values (F, R), press:
[AUX] + [3]< Tools > + [1]<Tool table>
Select the tool data to be changed:
(Tool number) + [RECALL]
Use the
keys to place the cursor over the value to be changed.
Key in the new value.
Press [ENTER].
To change another value, place the cursor over it and change it.
To quit this option, press [END].

NOTE: Refer to the Operation Manual Chapter 3 Section 3.4.1

Self-teaching Manual

Chapter 3 Page 27

800T CNC
3.6 Checking for proper calibration.
Preset the part zero.

Select a tool.
e.g. Location code 3

Approach the tool along Z.

Press [Z]+[0]+[ENTER]

Withdraw the tool.

Part zero position.

Start the spindle and touch the part diameter with several tools while
checking the value on the screen.
The tools are different but the value on the screen must be the same.

Self-teaching Manual

Chapter 3 Page 28

4.- Automatic Operations

800T CNC
This chapter describes:
Which are the keys associated with the automatic operations.
How to execute an operation.
> In Semiautomatic mode.
> In Automatic mode (cycle level).
Turning example in Semiautomatic mode.
Turning example in Automatic mode.
> Define the specific parameters for the operation.
> Other parameters. (Safety distance, finishing conditions).
> Simulate an operation.
ZOOM function.
> Execute an operation.
Tool inspection.
Tool wear compensation.

Self-teaching Manual

Chapter 4 Page 2

800T CNC
4.1 Operating modes.
Compact keyboard

Modular keyboard

Layout of the automatic function keys

Self-teaching Manual

Chapter 4 Page 3

800T CNC
Operation keys

Grooving.
Threading.
Rounding.
Taper turning.
Facing.
Turning.
Profiling.
Compact

Modular

Access to simple drilling, tapping.

Semiautomatic / Automatic.
Self-teaching Manual

Chapter 4 Page 4

800T CNC
It is possible to work in Semiautomatic or Automatic mode. The choice is
made as follows:
Automatic operations in Semiautomatic mode.
In this mode, the operator controls the machine with the JOG keys and the
handwheels.
The BEGIN and END points of the section to be machined, chamfer angles,
rounding radius, etc. must be defined.
The CNC does not apply tool radius compensation.

Turning

Taper turning

Rounding

Examples of Semiautomatic mode

NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.1

Self-teaching Manual

Chapter 4 Page 5

800T CNC
Automatic operations in automatic mode.
In this mode, the operation is defined and it is run automatically.
Besides the BEGIN and END points, the operation data must also be defined.
The keys for defining this data are:
: Depth of cut.

: Rounding radius.

: Angles.

: Thread pitch.

: Diameters.

: Number of passes.

In this mode, the following parameters must also be defined: Finishing pass,
finishing feedrate, finishing tool, safety distances in X and Z. Press [AUX].
For a good finish, the tool nose radius and location code must be defined in the
tool table. (Section 2.2 of this manual).

NOTE: Refer to the Operation Manual

Chapter 5 Section 5.1.2

Self-teaching Manual

Chapter 4 Page 6

800T CNC
4.2 Example of turning in Semiautomatic mode.
Select the turning operation. Press
Select the Semiautomatic mode. Press

Diagram for Semiautomatic mode

Set the BEGIN and END values.

[BEGIN] + [Z] + (Value) + [ENTER]
[END] + [Z] + (Value) + [ENTER]
Set the cutting conditions (feedrate, spindle speed and tool).
Start the spindle.

Self-teaching Manual

Chapter 4 Page 7

800T CNC
Carry out the turning operation.
Move the X axis with the JOG keys and the handwheel up to the
desired depth.
Move the Z axis by pressing [BEGIN]+start or [END]+start.
Only the Z axis moves.

1. Approach manually.

2. Turn with [END]+

3. Move away manually.

4. Withdraw with [BEGIN]+

NOTE: Refer to the Operation Manual Chapter 5 Section 5.2.1

Self-teaching Manual

Chapter 4 Page 8

800T CNC
NOTE: Remember that in Semiautomatic mode and depending on which
operation has been selected, the [BEGIN]+start or [END]+start will execute it
differently.
When turning or threading, movements parallel to the Z axis.
When facing, movements parallel to the X axis.
If no operation has been selected, when doing [BEGIN]+start or
[END]+start both axes move.
Semiautomatic mode

DRO mode

[BEGIN]+

Self-teaching Manual

[END]+

Chapter 4 Page 9

800T CNC
4.3 Example of turning in automatic mode.
4.3.1 Programming.
Select the turning operation. Press
Select the Automatic mode. Press

Diagram for the Automatic mode

Define these parameters:

:(
): Final turning diameter.
:(
): Pass (depth of cut).
N:(
): Total number of passes for the turning operation.
The N value is only taken into account when =0.
Self-teaching Manual

Chapter 4 Page 10

800T CNC
Other parameters:
With this CNC it is possible to change the finishing feedrate, the depth of the
pass and finishing tool. To access this option, press [AUX].
The screen will show the following menu:
1.- % CYCLE FINISHING PASS

(% of pass for the finishing pass)

2.- % CYCLE FINISHING PASS.

3.- T CYCLE FINISHING PASS.
4.- SAFETY DISTANCE X.
5.- SAFETY DISTANCE Z.

(% of feedrate for the finishing pass)

(Finishing tool)

With options [4] and [5], we set the safety distances along the X and Z axes.
These safety distances are programmed to prevent the tool from running into
the part when approaching in rapid.

Example of how to apply safety distances.

NOTE: Refer to the Operation Manual Chapter 5 Section 5.2.2

Self-teaching Manual

Chapter 4 Page 11

800T CNC
With option [1], we select the finishing pass.
If =2mm and %D=50, the finishing pass will be 1mm (50%).
If =2mm and %D=100, the finishing pass will be 2mm (100%).
If =2mm and %D=0, the finishing pass will be 2mm (100%).
With option [2], we select the feedrate for the finishing pass.
If %F=50, the finishing feedrate will be 50% of the programmed F.
If %F=100, the finishing feedrate will be100% of the programmed F.
With option [3], we select the tool for the finishing pass. If T=0, the
roughing tool will be used for the finishing pass.

Self-teaching Manual

Chapter 4 Page 12

800T CNC
4.3.2 Simulate an operation.
It is used for checking the tool path on the screen.
Press [SIMUL] (at the compact) or [AUX]+[S] (at the modular). The CNC will
display the graphics menu.
To define the display area, press [AUX].

X,Z: Point on the part that will appear at the center

of the screen.
WIDTH: Width of the graphics on the screen.
After setting the display area, to start the simulation, press
The simulation speed is controlled with the Feedrate Override Switch.
Other useful keys are:
: Interrupt simulation. While interrupted:
: Resume simulation.
[CLEAR] : Delete the graphics on the screen.
[END] : Exit the simulation mode.
Once the simulation is over. Press [END].

NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.3

Self-teaching Manual

Chapter 4 Page 13

800T CNC
NOTE: When simulating the path, the screen only shows half the part. This is
because only the path of the tool tip is shown and not the part.

Graphics
The screen shows:
Rapid movement.
Movement at programmed F.

NOTE: To check the part dimensions on the simulation screen, the simulation has
to be made with a tool with a nose radius R=0.

Self-teaching Manual

Chapter 4 Page 14

800T CNC
ZOOM function:
Only when the simulation is interrupted or finished. It is used for enlarging or
decreasing the drawing or a section of it.
Press [Z]

MODULAR

COMPACT

[AUX]

[SIMUL]

Move the rectangle.

Increase the size of the rectangle.
Decrease the size of the rectangle.
Draw the selected section.
Draw the selected section and assume the new display area.
End of the ZOOM function.

[ENTER]
[END]

NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.3.1

Self-teaching Manual

Chapter 4 Page 15

800T CNC
4.3.3 Execute an operation.
The operations in Automatic mode may be executed from beginning to end
or a pass at a time. This choice is made by the
key.
To start the execution, press
Once the execution has started:
: Interrupts the execution. While interrupted:
: Resumes the execution.
[CLEAR] : Cancels the execution.
The execution can be interrupted at any time, except during a threading pass. In
that case, the execution will stop at the end of the pass.
When interrupting a program, the active keys are:

NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.4

Self-teaching Manual

Chapter 4 Page 16

800T CNC
Tool inspection.
With this option, the operation may be interrupted for inspecting and replacing the tool.
Press
+ [TOOL]. The CNC stops the spindle and displays the message:
JOG KEYS AVAILABLE
EXIT
Move the tool with the JOG keys or the handwheels.
Check the tool.
Press [END]. The CNC starts the spindle and displays the message:
RETURN
AXES OUT OF POSITION
With the JOG keys or handwheels, take the axes back to their position when the
execution was interrupted. The CNC will not let the axes go beyond this point. The
CNC displayes the message:
RETURN
AXES OUT OF POSITION
NONE
Press

NOTE: Refer to the Operation Manual Chapter 5 Section 5.1.4.1

Self-teaching Manual

Chapter 4 Page 17

800T CNC
Changing the tool wear values:
With this option, it is possible to change the I, K values while the program is
either running or interrupted. The entered values are incremental and will be added
to the ones stored before.
Press
. The CNC shows the message T.
Key in the tool number and press [RECALL].
The CNC shows the table for that tool and requests the I value.
Enter the I value and press
. The CNC requests the K value.
Enter the K value and press [ENTER].
To change the offset of another tool, press [TOOL].
To quit this option, press [END].

NOTE: Refer to the Operation Manual Chapter 3 Section 3.4.4

Self-teaching Manual

Chapter 4 Page 18

5.- Summary of work cycles

800T CNC
5.1 Automatic Facing.
Cycle parameters
BEGIN, END: First and last points of the cycle.

: Final facing diameter.

: Depth of each pass.
If =0, N will be taken into account.
N : Number of facing passes.
Finishing parameters.
Cutting conditions.
Execution
1. Approach to the BEGIN point
2. Roughing the part in several passes.
3. Finish the part in a single pass. If programmed.

Roughing

Finish

NOTE: The CNC starts and stops the spindle.

NOTE: Refer to the Operation Manual Chapter 5 Section 5.3.2

Self-teaching Manual

Chapter 5 Page 2

800T CNC
5.2 Automatic Taper Turning.
Cycle parameters
BEGIN: Theoretical positioning corner.
: Smaller final diameter.
: Depth of the Pass.
If =0, N will be taken into account.
N : Number of taper turning passes.
a : Taper angle with the Z axis.
% : Slope of the chamfer.
When entering a or %, another value is updated.
: Selection of the profile type.
Finishing parameters.
Cutting conditions.

Types of profile
Execution

Roughing

Finishing

NOTE: Refer to the Operation Manual Chapter 5 Section 5.4.2

Self-teaching Manual

Chapter 5 Page 3

800T CNC
5.3 Automatic Rounding (Cycle Level 1).
Cycle parameters
BEGIN: Theoretical positioning corner.
: Defines the rounding radius.
: Depth of the pass.
If =0, N will be taken into account.
N : Number of rounding passes.
: Selection of the profile type.
: Type of rounding.(concave, convex).
Finishing parameters.
Cutting conditions.
Types of profile to be machined
Execution

Roughing

Finishing

NOTE: Refer to the Operation Manual Chapter 5 Section 5.5.2

Self-teaching Manual

Chapter 5 Page 4

800T CNC
5.4 Automatic Rounding (Cycle Level 2).
Cycle parameters
BEGIN: First rounding point.
END: Last rounding point.
R: Defines the rounding radius.
: Depth of the pass.
If =0, N will be taken into account.
N : Number of rounding passes.
: Selection of the profile type.
: Type of rounding.(concave, convex).
Types of profiles to be machined

Finishing parameters.
Cutting conditions.

Execution

Roughing

Finishing

NOTE: Refer to the Operation Manual Chapter 5 Section 5.5.2

Self-teaching Manual

Chapter 5 Page 5

800T CNC
5.5 Profile Rounding.
Cycle parameters
BEGIN: First rounding point.
END: Last rounding point.
R: Rounding radius.
: Distance between two passes.

: Angle with Z of the first rounding section.

1: Angle with Z of the second rounding section.
use the
key to select this data.
T: Cutter angle with the X axis. Use the
keys to select this data.
Setting the angles

Setting the angle of the tool

Self-teaching Manual

Chapter 5 Page 6

800T CNC
Cycle parameters
H: Amount of material to be removed (in radius).
use the
keys to select this data.
With the sign, we choose the roughing type.
H(+): Passes parallel to programmed profile.
H(-): Passes parallel to the Z axis or X axis
depending on the tool.
For the finishing pass, the CNC has to know how
the tool enters and exits the profile.
To select how it enters, press
Roughing passes

To select how it exits, press

Finishing parameters.
Cutting conditions.
Tool entry/exit

NOTE: Refer to the Operation Manual Chapter 5 Section 5.5.3

Self-teaching Manual

Chapter 5 Page 7

800T CNC
5.6 Automatic Threading.
Cycle parameters
BEGIN: First threading point.
END: Last threading point.
P : Thread pitch.
: Depth of the first pass (in radius).
H: Depth of the thread (in radius).
: Penetration angle.
:Inside or outside thread.

D: End of thread distance.

X, Z: Safety distances.

Finishing parameters.
Cutting conditions.
Penetration angle
Execution

Approach to the
BEGIN point.

Making the thread

in
consecutive
passes.

NOTE: Refer to the Operation Manual Chapter 5 Section 5.6.2

Self-teaching Manual

Chapter 5 Page 8

800T CNC
5.7 Grooving.
Cycle parameters
BEGIN: First grooving point.
END: Last grooving point or depth of the groove.
F : Last smaller diameter.
: Depth of the pass.
If =0, N will be taken into account.
N : Number of grooving passes.
TW: Tool width.
Finishing parameters.
Cutting conditions.
Execution

Roughing

Finishing

NOTE: Refer to the Operation Manual Chapter 5 Section 5.7

Self-teaching Manual

Chapter 5 Page 9

800T CNC
5.8 Simple drilling.
[AUX] + [6] + Simple drilling. Tapping
Cycle parameters
BEGIN: First drilling point.
END: Last drilling point.
P : maximum penetration in each drilling peck.
If P=0, tapping.
Finishing parameters.
Cutting conditions.
Execution

The tool penetrates P and withdraws

up to BEGIN+Z position to remove
material.
Rapid approach up to 1 mm off the
previous peck.
Repeat these steps until reaching the
total drilling depth.
Rapid Move.
The tool stays at the bottom of the
Move at programmed F. hole for 400 msec (dwell) for better part
finish.

NOTE: Refer to the Operation Manual Chapter 5 Section 5.8

Self-teaching Manual

Chapter 5 Page 10

800T CNC
5.9 Tapping.
[AUX] + [6] + Simple drilling. Tapping
Cycle parameters
BEGIN: First tapping point.
END: Last tapping point.
P=0, tapping.
Finishing parameters.
Cutting conditions.

Execution

Rapid move.
Move at programmed F.

The
tool
penetrates
at
the
programmed feedrate up to the END
point.
The spindle starts turning in the
opposite direction.
Withdrawal at programmed feedrate
to the BEGIN + Z position.

NOTE: Refer to the Operation Manual Chapter 5 Section 5.8

Self-teaching Manual

Chapter 5 Page 11

800T CNC
5.10 Profiles.
Cycle parameters

Roughing passes

Up to 9 points and 6 rounding operations may be

defined. If all the points are not used, the first unused
point will have the values of the last point used.
: Depth of the pass.
: Amount of material to be removed. Press
>0: Roughing passes parallel to the profile.
H=0: No roughing. Only finishing pass.
H<0: Roughing passes parallel to one axis.
T: Cutter angle with respect to the X axis.
For the finishing pass, the CNC needs to know how
the tool enters and exits the profile.
To select how it enters, press
To select how it exits, press

Setting tool angle

Finishing parameters and cutting conditions.

NOTE: Refer to the Operation Manual Chapter 6 Section 6.2

Self-teaching Manual

Chapter 5 Page 12

6.- Part programs

800T CNC
This chapter describes:
Conversational part-programs.
> What a conversational part-program is.
> How to edit it.
> How to change it (Insert or delete operations).
> How to simulate an operation or part-program.
> How to execute an operation.
> How to execute starting at a particular operation.
> How to execute a program.
> Delete a program.
Program P99996.
> What it is.
> How to edit it.
> How to simulate and execute it.

Self-teaching Manual

Chapter 6 Page 2

800T CNC
6.1 Conversational part-programs.
6.1.1 What is a conversational part-program?
It is a set of operations ordered secuentially. Each operation is defined separately (always
in automatic mode) and they are then stored one after the other in a program. Up to 20
operations.
The name of the part-program can be any integer between 00000 and 99990.
Besides these, the number 99996 corresponds to a part-program written in CNC
language, ISO code (Section 6.2 in this manual).
The CNC can store up to 10 part-programs. The rest of them must be stored at a PC.
Turning
Taper turning
Rounding
Profile

Facing

PART 32741
1 - FACING
2 - TURNING
3 - TAPER
4 - ROUNDING
567?
EXIT

NOTE: The profile occupies two memory positions.

Self-teaching Manual

Chapter 6 Page 3

800T CNC
6.1.2 Edit a part-program.
To edit a part-program, we first choose the operations needed to execute the
part. A part may be executed in various ways.
Taper turning
Rounding
Turning

Profile

Different solutions for the same part

Self-teaching Manual

Chapter 6 Page 4

800T CNC
Once the sequence of operations has been chosen (in our case we will make the
previous example), we are going to build the part program editing the operations
one by one in automatic mode.

DRO
MODE

PART
01234 [*]
24832 [*]
12345 [ ]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

Press
[RECALL]

PART
01234 [*]
24832 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

Choose
position

PART
01234 [*]
24832 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

Press [P]

The dashes indicate that there is no part-program.

[*] : The part has been already edited. It contains data.
[ ] : The part contains no data.
[ENTER] EXIT: Exit the table.
If when pressing [P] no other program can be entered,
it means that there are already 10 programs in memory.

Self-teaching Manual

PART
01234 [*]
24832 [*]
00000 [ ]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

Enter
number

PART 12345
1?
2?
3?
4?
5?
6?
7?
EXIT

Chapter 6 Page 5

800T CNC
Choose the operation and define
the parameters.
Choose
position

NOTE: To go from the parameter table

to the operations table, press

PART 12345
1?
2?
3?
4?
5?
6?
7?
EXIT

[ENTER]
[ENTER]

PART 12345
1 - TAPER
2?
3?
4?
5?
6?
7?
EXIT

Repeat these steps with the other operations. In our case, the finished partprogram will be:
Program number
Operations

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

Self-teaching Manual

Chapter 6 Page 6

800T CNC
6.1.3 Modify a part-program.
The operations making up a part-program can be modified.

Choose
program

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

The CNC shows the cycle with

all its data.
Modify the operation parameters
like in the editing mode.

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

[ENTER]

Choose
operation

CNC requests
confirmation.

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

[ENTER]

[RECALL]

The new operation

replaces the old one.

7 Section 7.6
Self-teaching Manual

Chapter 6 Page 7

800T CNC
New operations can also be inserted into a part-program.

Choose
program

Choose
position

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

[ENTER]

Choose
operation

CNC requests
confirmation.

Define parameters and

cutting conditions of the
operation to be inserted.

Press [1]

PART 12345
1 - TAPER
2 - GROOVING
3 - ROUNDING
4 - TURNING
5?
6?
7?
EXIT

NOTE: Refer to the Operation Manual Chapter 7 Section 7.6

Self-teaching Manual

Chapter 6 Page 8

800T CNC
Operations can be deleted from a part-program.
PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

CNC requests
confirmation.

PART 12345
1 - TAPER
2 - GROOVING
3 - ROUNDING
4 - TURNING
5?
6?
7?
EXIT

[ENTER]

PART 12345
1 - TAPER
2 - GROOVING
3 - ROUNDING
4 - TURNING
5?
6?
7?
EXIT

[CLEAR]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

NOTE: Refer to the Operation Manual Chapter 7 Section 7.6

Self-teaching Manual

Chapter 6 Page 9

800T CNC
6.1.4 Simulate an operation of a part-program.
It is used to check the tool path on the screen.
PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT
PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

Choose
program

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

At the compact model, press [SIMUL]

[RECALL]+

At the modular model, press [AUX]+[S]

Graphics
screen.

To define a display area, press [AUX].

Self-teaching Manual

Chapter 6 Page 10

800T CNC
6.1.5 Simulate a part-program.
The simulation starts with the first operation and ends when finding a free
(empty) position.
PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

Choose
program

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

At the compact model, press [SIMUL]

At the modular model, press [AUX]+[S]

Graphics
screen

To define a display area, press [AUX].

Self-teaching Manual

Chapter 6 Page 11

800T CNC
6.1.6 Execute an operation of a part-program.
The operations of a part-program can be executed separately.

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
[RECALL]+
4?
5?
6?
7?
EXIT

NOTE: Refer to the Operation Manual Chapter 7 Section 7.5.1

Self-teaching Manual

Chapter 6 Page 12

800T CNC
6.1.7 Execute a part-program from a particular operation on.
The execution may begin at any operation.

DRO
MODE

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

Operations 2 and 3 will be executed.

Self-teaching Manual

Chapter 6 Page 13

800T CNC
6.1.8 Execute a part-program.
The execution begins with the first operation and ends when finding a free
(empty) position.
PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[RECALL]

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

PART 12345
1 - TAPER
2 - ROUNDING
3 - TURNING
4?
5?
6?
7?
EXIT

NOTE: Refer to the Operation Manual Chapter 7 Section 7.5

Self-teaching Manual

Chapter 6 Page 14

800T CNC
The execution begins with the first operation and ends when finding a free
(empty) position.
When the CNC executes an operation, the bottom of the screen shows the
operation with all its parameters.
Once the execution has started:
: Interrupts the execution. While being interrupted:
: Resumes the execution.
[RESET]+[RESET] : Cancels the execution.
The execution can be interrupted at any time, except during a threading pass. In
that case, the execution will stop at the end of the pass.
When interrupting a program, the active keys are:

NOTE: Refer to the Operation Manual Chapter 7 Section 7.5

Self-teaching Manual

Chapter 6 Page 15

800T CNC
How does the tool move?
After executing an operation, the tool goes to the BEGIN point maintaining the
safety distances.
When going from one operation to another, the tool moves in a straight line
from the BEGIN point of the current one to the BEGIN of the next one.
When ending the last operation, the tool goes back to the where the partprogram execution started.
If the manufacturer has not set a tool change position, it will be done where the
execution started.

Self-teaching Manual

Chapter 6 Page 16

800T CNC
6.1.9 Delete a part-program.
Select the program in the table and press [CLEAR].

[RECALL]

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

PART
01234 [*]
24832 [*]
12345 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

[CLEAR]

CNC requests
confirmation.

[ENTER]

PART
01234 [*]
24832 [*]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
----- [ ]
EXIT

NOTE: Refer to the Operation Manual Chapter 7 Section 7.7

Self-teaching Manual

Chapter 6 Page 17

800T CNC
6.2 Program P99996.
6.2.1 What is it?
It is a program written in CNC programming language. (ISO code).

...
N100 G01 X20 Z0
N110 G01 X20 Z-30
N120 G03 X34 Z-37 R7
N130 G01 X34 Z-60
N140 G02 X54 Z-70 R10
N150 G01 X54 Z-100
N160 G00 X70 Z20
...

Self-teaching Manual

Chapter 6 Page 18

800T CNC
6.2.2 How is it edited?
It can be edited at the CNC or at a PC. To edit it at the CNC, press:
[AUX]+[5]<Auxiliary modes>+[5]<Editing program 99996>

Blocks in memory

Block to be edited

Editing screen

Self-teaching Manual

Chapter 6 Page 19

800T CNC
When editing blocks:
Besides the alphanumeric keys [0]...[9], [F], [S], [T], [X], [Z] we will use:
as P.
as R.
as A.
The missing function keys (G, M, I, K) are displayed in the help [AUX].
(The CNC will only offer the right help possibilities).
[ENTER]: Save block.
[CL]: Delete character.
Example:
N40 G01 X10 Z-10_
[CL]
N40 G01 X10 Z-1_
Self-teaching Manual

Chapter 6 Page 20

800T CNC
When modifying blocks:
[RECALL] :Call a block.
Example:
N40
[RECALL]
N40 G01 X10 Z-10_
:Delete a block.
:To insert or overwrite .
:Search for previous or next blocks.
To move over a block:
N60
[RECALL]
N60 G01 G90 X30 Z-20 T2_
<Move the cursor>
N60 G01 G90_ X30 Z-20 T2

at the compact,

at the modular.

[CL]
N60 G01 G9_ X30 Z-20 T2
[1]
N60 G01 G91_ X30 Z-20 T2
[ENTER]

NOTE: Refer to the Operation Manual Chapter 3 Section 3.11

Self-teaching Manual

Chapter 6 Page 21

800T CNC
6.2.3 Ejecute/simulate program P99996.
To access this mode:
Press [AUX]+[5]<Auxiliary modes>+[4]<Program 99996 execution>
Steps to execute/simulate program P99996.
Choose execution mode AUTOMATIC/SINGLE BLOCK
Choose first block:
[N] + [RECALL] or [N]+ (block number) + [RECALL]
To simulate, press [SIMUL], (at the compact model), or [AUX]+[S], (at the
modular model). To define the display area, press [AUX].
To execute program P99996, press the START key
NOTE: While executing, press [4] to display the tool path or [0] to return to the
previous screen.

NOTE: Refer to the Operation Manual Chapter 3 Section 3.10

Self-teaching Manual

Chapter 6 Page 22

800T CNC
Screen for executing program P99996
Execution mode

Block in execution
and following ones

Cutting conditions

A: Actual
C: Command
R: To go

Active functions

COMMAND: Tools target point.

ACTUAL:
Current tool position.
TO GO:
Distance left to reach the target point.

Self-teaching Manual

Chapter 6 Page 23

Appendix I
Other machining
operations on a lathe

800T CNC
I.1 Introduction.
For this type of machining operations, the machine must have a spindle which can be
oriented and a live tool. If the machine has these features, the CNC menu will offer the
Multiple drilling and Slot milling choices when pressing [AUX]+[6].

Multiple drilling

Slot milling

Self-teaching manual

Appendix I Page 2

800T CNC
I.2 Spindle orientation.
With this feature the spindle can be oriented to the desired angular position for
drilling holes and milling slots both on the face of the part or on its turning
surface.
To orient the spindle, press:
[S]+ . The CNC shows the message: S POS= .
Enter the target angular position for the spindle.
Press
The spindle stops, (if it was turning) and it positions at the specified angle.
The CNC shows the angular position in degrees.
By pressing
or
, it will return to the conditions prior to orienting the
spindle.

Self-teaching manual

Appendix I Page 3

800T CNC
I.3 Live tool.
To select the speed of the live tool, press:
[TOOL] + [S]. The CNC shows the message: T RPM= .
Enter the speed of the live tool in rpm.
Press
The CNC shows the following information:
F 0000.000

100%

RPM 1250

100%

TRPM 800

T2

Live tool speed

To stop the live tool, press:
[TOOL] + [S] + [0] + [ENTER].

NOTE: Refer to the Operation manual Chapter 2 Section 2.2.1

Self-teaching manual

Appendix I Page 4

800T CNC
I.4 Multiple drilling.
[AUX] + [6] + Multiple drilling

Cycle parameters

Execution

BEGIN: First drilling point.

END: Last drilling point.
P : Maximum drilling depth.

: Angular position of the first hole.

D: Angular gap betwen holes.
N: Number of holes.
Finishing parameters.
Cutting conditions.

Rapid move.
Move at F.

NOTE: Refer to the Operation manual Chapter 5 Section 5.9

Self-teaching manual

Appendix I Page 5

800T CNC
I.5 Slot milling.
[AUX] + [6] + Slots

Cycle parameters

Execution

BEGIN: First point of the slot.

END: Last point of the slot.

: Angular position of the first slot.

D: Angular gap between slots.
N: Number of slots.
Finishing parameters.
Cutting conditions.
Rapid move.

Move at F.

NOTE: Refer to the Operation manual Chapter 5 Section 5.10

Self-teaching manual

Appendix I Page 6

Appendix II
Peripherals

800T CNC
II.1 Peripherals.
Peripherals are devices external to the CNC (FAGOR floppy disk unit, PC, etc.) which
could be used to store data. This data is transmitted from the CNC (while in Peripheral
mode) or by means of the DNC protocol.

II.1.1 Peripheral mode.

In this mode, part-programs can be transferred between the CNC and the FAGOR floppy
disk unit, a general peripheral device or a PC. To select this option, press:
DRO
MODE

[AUX] + [5]<Auxiliary modes> + [2]<Peripherals>

The CNC will show the following menu:

0 - RECEIVE FROM FLOPPY DISK UNIT (Fagor)

1 - SEND TO FLOPPY DISK UNIT (Fagor)
2 - RECEIVE FROM GENERAL DEVICE
3 - SEND TO GENERAL DEVICE
4 - FLOPPY DISK UNIT DIRECTORY (Fagor)
5 - DELETE FLOPPY DISK UNIT PROGRAM (Fagor)
6 - DNC ON/OFF
Self-teaching manual

Appendix II Page 2

800T CNC
In order to work with these options, the DNC option must be OFF. If ON, (the word DNC will appear at
the upper right-hand corner of the screen), press [6] to turn it OFF. The word DNC disappears.
0 - RECEIVE FROM FLOPPY DISK UNIT
1 - SEND TO FLOPPY DISK UNIT
2 - RECEIVE FROM GENERAL DEVICE
3 - SEND TO GENERAL DEVICE
Options 0, 1, 2 and 3 are used to exchange programs between the CNC and the peripheraldevices.
The numbers of the programs which can be exchanged are:
P00000 through P99990
Corresponding to part-programs.
P99994 and P99996
Special ISO-coded programs.
P99997
CANNOT be transmitted (internal use).
P99998
Used to associate texts with PLC messages.
P99999
Machine parameters and tables.
While working with these options, the screen will show: RECEIVING or SENDING and, when
the transmission is completed, PROGRAM NUM. P----- RECEIVED or SENT.
4 - FLOPPY DISK UNIT DIRECTORY
To see the list of the programs stored in the Fagor Floppy Disk Unit.
5 - DELETE FLOPPY DISK UNIT PROGRAM
To delete a program of the Fagor Floppy Disk Unit, key in the program number and press [ENTER].
6 - DNC ON/OFF
To turn the DNC mode ON or OFF.

NOTE: Refer to the Operation manual Chapter 3 Section. 3.8.1

Self-teaching manual

Appendix II Page 3

800T CNC
II.2 Lock/unlock.
With this option, it is possible to lock or unlock the machine parameters and
the part-program memory of the CNC.
When the part-program memory is locked, the existing programs cannot be
modified and new ones cannot be edited. They can only be displayed and
executed. To access this option, press:
[AUX] + [5]<Auxiliary modes> + [3] <Lock/Unlock>
The codes which can be used are:
N0000 [ENTER] to unlock part-program memory.
N1111 [ENTER] to lock part-program memory.

NOTE: Refer to the Operation manual Chapter 3 Section. 3.9

Self-teaching manual

Appendix II Page 4