heidenhain TNC 430 User Manual

Pilot
TNC 426
TN C 42 6B TNC 4 30
TNC 43 0
NC-Software 280 476-xx 280 477-xx
8/2000
The Pilot
Contents
... is your concise programming guide for the HEIDENHAIN TNC 426 and TNC 430 contouring controls. For more comprehensive information on programming and operating, refer to the TNC User's Manual. There you will find com­plete information on:
 Q-parameter programming  The central tool file  3-D tool compensation  Tool measurement
Certain symbols are used in the Pilot to denote specific types of information:
Important note
WARNING: danger for the user or the machine!
The TNC and the machine tool must be prepared by the machine tool builder to perform these functions!
Chapter in User's Manual where you will find more detailed information on the current topic.
The information in this Pilot applies to TNCs with the following software numbers:
Control NC Software Number
TNC 426, TNC 430 280 476-xx TNC 426*, TNC 430* 280 477-xx
Fundamentals ................................................................... 4
Contour Approach and Departure .................................... 13
Path Functions .................................................................. 18
FK Free Contour Programming ........................................ 25
Subprograms and Program Section Repeats ................... 33
Working with Cycles ........................................................ 36
Cycles for Machining Holes and Threads ........................ 39
Pockets, Studs, and Slots ................................................. 56
Point Patterns ................................................................... 65
SL Cycles .......................................................................... 67
Multipass Milling .............................................................. 75
Coordinate Transformation Cycles................................... 78
Special Cycles ................................................................... 85
Digitizing 3-D Surfaces ..................................................... 88
Graphics and Status Displays ........................................... 94
ISO Programming ............................................................. 97
Miscellaneous Functions M ............................................. 103
Contents
*) Export version
Fundamentals
Files in the TNC
File type
Programs/Files
See Programming, File Management
The TNC keeps its programs, tables and texts in files. A file designation consists of two components:
THREAD2.H
File name File type
Maximum length: see table at right 16 characters
Fundamentals
Creating a New Part Program
Select the directory in which the program is stored Enter a new file name with file type Select unit of measure for dimensions (mm or inches) Define the blank form (BLK) for graphics:
Enter the spindle axis Enter coordinates of the MIN point:
the smallest X, Y and Z coordinates Enter coordinates of the MAX point:
the greatest X, Y and Z coordinates
1 BLK FORM 0.1 Z X+0 Y+0 Z-50 2 BLK FORM 0.2 X+100 Y+100 Z+0
Programs
 in HEIDENHAIN format  in ISO format
Tables for  Tools  Datums  Pallets  Cutting data  Positions
Texts as  ASCII files
.H .I
.T .D .P .CDT .PNT
.A
Choosing the Screen Layout
See Introduction, the TNC 426, TNC 430
Show soft keys for setting the screen layout
Mode of operation Screen contents
Manual operation Electronic handwheel
Positioning with manual data input
Program run, full sequence
Program run, single block test run
Positions
Positions at left Status at right
Program
Program at left Status at right
Program
Program at left Program structure at right
Program at left Status at right
Program at left Graphics at right
Graphics
Positions at left, status at right Program at left, graphics at right
Fundamentals
Continued
Mode of operation Screen contents
Programming and editing
Program
Program at left Program structure at right
Program at left Programming graphics at right
Fundamentals
Program at left, program structure at right
Absolute Cartesian Coordinates
The dimensions are measured from the current datum. The tool moves to the absolute coordinates.
Programmable axes in an NC block
Linear motion: 5 axes Circular motion: 2 linear axes in a plane or
3 linear axes with cycle 19 WORKING PLANE
Incremental Cartesian Coordinates
The dimensions are measured from the last programmed position of the tool. The tool moves by the incremental coordinates.
Fundamentals
Circle Center and Pole: CC
The circle center (CC) must be entered to program circular tool movements with the path function C (see page 21). CC is also needed to define the pole for polar coordinates.
CC is entered in Cartesian coordinates*.
An absolutely defined circle center or pole is always measured from the workpiece datum.
An incrementally defined circle center or pole is always measured from the last programmed position of the workpiece.
Fundamentals
Angle Reference Axis
Angles  such as a polar coordinate angle PA or an angle of rotation ROT  are measured from the angle reference axis.
Working plane Ref. axis and 0° direction
X/Y X Y/Z Y Z/X Z
*Circle center in polar coordinates: See FK programming
Polar Coordinates
Dimensions in polar coordinates are referenced to the pole (CC). A position in the working plane is defined by
 Polar coordinate radius PR = Distance of the position from the pole  Polar coordinate angle PA = Angle from the angle reference axis to
the straight line CC  PR
Incremental dimensions
Incremental dimensions in polar coordinates are measured from the last programmed position.
Programming polar coordinates
Select the path function
Press the P key Answer the dialog prompts
Defining Tools
Tool data
Every tool is designated by a tool number between 1 and 254 or, if you are using tool tables, by a tool name.
Entering tool data
You can enter the tool data (length L and radius R)
 in a tool table (centrally, Program TOOL.T)
or
 within the part program in TOOL DEF blocks (locally)
Fundamentals
Program the tool length as its difference DL to the zero tool: DL>0: The tool is longer than the zero tool
DL<0: The tool is shorter than the zero tool
With a tool presetter you can measure the actual tool length, then program that length.
Calling the tool data
Fundamentals
3 TOOL DEF 6 L+7.5 R+3 4 TOOL CALL 6 Z S2000 F650 DL+1 DR+0.5 5 L Z+100 R0 FMAX 6 L X-10 Y-10 R0 FMAX M6
Tool change
10
Tool number Tool length L Tool radius R
Tool number or name Working spindle axis: tool axis Spindle speed S Feed rate Tool length oversize DL (e.g. to compensate wear) Tool radius oversize DR (e.g. to compensate wear)
 Beware of tool collision when moving to the tool change
position!
 The direction of spindle rotation is defined by M function:
M3: Clockwise M4: Counterclockwise
 The maximum permissible oversize for tool radius or length
is ±99.999mm!
Oversizes on an end mill
Tool Compensation
The TNC compensates the length L and radius R of the tool during machining.
Length compensation Beginning of effect:
Tool movement in the spindle axis
End of effect:
Tool exchange or tool with the length L=0
Radius compensation Beginning of effect:
Tool movement in the working plane with RR or RL
End of effect:
Execution of a positioning block with R0
Working without radius compensation (e.g. drilling):
Tool movement with R0
S = Start; E = End
Fundamentals
11
Datum Setting without a 3-D Touch Probe
During datum setting you set the TNC display to the coordinates of a known position on the workpiece:
Insert a zero tool with known radius Select the manual operation or electronic handwheel mode Touch the reference surface in the tool axis with the tool and enter its length Touch the reference surface in the working plane with the tool and enter the position of the tool center
Fundamentals
Setup and Measurement with 3-D Touch Probes
A HEIDENHAIN 3-D touch probe enables you to setup the machine very quickly, simply and precisely.
Besides the probing functions for workpiece setup on the Manual and Electronic Handwheel modes, the Program Run modes provide a series of measuring cycles (see also the User's Manual for Touch Probe Cycles):
 Measuring cycles for measuring and compensating workpiece
misalignment  Measuring cycles for automatic datum setting  Measuring cycles for automatic workpiece measurement with
tolerance checking and automatic tool compensation
12
Contour Approach and Departure
Starting point P
PS lies outside of the contour and must be approached without radius
S
compensation.
Auxiliary point P
PH lies outside of the contour and is calculated by the TNC.
The tool moves from the starting point P P
at the feed rate last programmed feed rate!
H
First contour point P
The first contour point PA is programmed in the APPR (approach) block.
H
and last contour point P
A
to the auxiliary point
S
E
The last contour point is programmed as usual.
End point P
PN lies outside of the contour and results from the DEP (departure) block. P
N
is automatically approached with R0.
N
Path Functions for Approach and Departure
Press the soft key with the desired path function:
Straight line with tangential connection
Straight line perpendicular to the contour point
Circular arc with tangential connection
Straight line segment tangentially con­nected to the contour through an arc
Contour Approach
and Departure
 Program a radius compensation in the APPR block!  DEP blocks set the radius compensation to 0!
13
Approaching on a Straight Line with Tangential Connection
Coordinates for the first contour point P Distance Len (length) from PH to P Enter a length Len > 0 Tool radius compensation RR/RL
A
7 L X+40 Y+10 R0 FMAX M3 8 APPR LT X+20 Y+20 LEN 15 RR F100 9 L X+35 Y+35
Contour Approach
and Departure
Approaching on a Straight Line Perpendicular to the First Contour Element
Coordinates for the first contour point P Distance Len (length) from PH to P Enter a length Len > 0 Tool radius compensation RR/RL
7 L X+40 Y+10 R0 FMAX M3 8 APPR LN X+10 Y+20 LEN 15 RR F100 9 L X+20 Y+35
A
A
A
14
Approaching Tangentially on an Arc
Coordinates for the first contour point P Radius R Enter a radius R > 0 Circle center angle (CCA) Enter a CCA > 0 Tool radius compensation RR/RL
A
7 L X+40 Y+10 R0 FMAX M3 8 APPR CT X+10 Y+20 CCA 180 R10 RR F100 9 L X+20 Y+35
Approaching Tangentially on an Arc and a Straight Line
Coordinates for the first contour point P Radius R Enter a radius R > 0 Tool radius compensation RR/RL
7 L X+40 Y+10 R0 FMAX M3 8 APPR LCT X+10 Y+20 R10 RR F100 9 L X+20 Y+35
A
Contour Approach
and Departure
15
Departing Tangentially on a Straight Line
Distance Len (length) from PE to P Enter a length Len > 0
N
23 L X+30 Y+35 RR F100 24 L Y+20 RR F100 25 DEP LT LEN 12.5 F100 M2
Contour Approach
and Departure
Departing on a Straight Line Perpendicular to the Last Contour Element
Distance Len (length) from PE to P Enter a length Len > 0
23 L X+30 Y+35 RR F100 24 L Y+20 RR F100 25 DEP LN LEN+20 F100 M2
N
16
Departing Tangentially on an Arc
Radius R Enter a radius R > 0
Circle center angle (CCA)
23 L X+30 Y+35 RR F100 24 L Y+20 RR F10 25 DEP CT CCA 180 R+8 F100 M2
Departing on an Arc Tangentially Connecting the Contour and a Straight Line
Coordinates of the end point P Radius R Enter a radius R > 0
23 L X+30 Y+35 RR F100 24 L Y+20 RR F100 25 DEP LCT X+10 Y+12 R8 F100 M2
N
Contour Approach
and Departure
17
Path Functions for Positioning Blocks
Path functions
See Programming: Programming contours.
Programming the Direction of Traverse
Regardless of whether the tool or the workpiece is actually moving, you always program as if the tool is moving and the workpiece is stationary.
Entering the Target Positions
Target positions can be entered in Cartesian or polar coordinates  either as absolute or incremental values, or with both absolute and incremental values in the same block.
Entries in the Positioning Block
Path Functions
A complete positioning block contains the following data:  Path function  Coordinates of the contour element end points (target position)  Radius compensation RR/RL/R0  Feed rate F  Miscellaneous function M
Before you execute a part program, always pre-position the tool to prevent the possibility of damaging the tool or workpiece!
Straight line
Chamfer between two
straight lines
Corner rounding
Circle center or pole for polar coordinates
Circular path aroundthe
circle center CC
Circular path with known radius
Circular path with tangential connection to
previous contour
Page 19
Page 20
Page 20
Page 21
Page 21
Page 22
Page 23
18
FK Free Contour Programming
Page 25
Straight Line
Coordinates of the straight line end point Tool radius compensation RR/RL/R0 Feed rate F Miscellaneous function M
With Cartesian coordinates:
7 L X+10 Y+40 RL F200 M3 8 L IX+20 IY-15 9 L X+60 IY-10
With polar coordinates:
12 CC X+45 Y+25 13 LP PR+30 PA+0 RR F300 M3 14 LP PA+60 15 LP IPA+60 16 LP PA+180
 You must first define the pole CC before you can program
polar coordinates!  Program the pole CC only in Cartesian coordinates!  The pole CC remains effective until you define a new one!
Path Functions
19
Inserting a Chamfer Between Two Straight Lines
Chamfer side length Feed rate F for the chamfer
7 L X+0 Y+30 RL F300 M3 8 L X+40 IY+5 9 CHF 12 F250 10 L IX+5 Y+0
 You cannot start a contour with a CHF block!  The radius compensation before and after the CHF block must
be the same!
 An inside chamfer must be large enough to accommodate
the current tool!
Path Functions
Corner Rounding
The beginning and end of the arc extend tangentially from the previous and subsequent contour elements.
Radius R of the circular arc Feed rate F for corner rounding
5 L X+10 Y+40 RL F300 M3 6 L X+40 Y+25 7 RND R5 F100 8 L X+10 Y+5
20
An inside arc must be large enough to accommodate the current tool!
Circular Path Around the Circle Center CC
Coordinates of the circle center CC
Coordinates of the arc end point Direction of rotation DR
C and CP enable you to program a complete circle in one block.
With cartesian coordinates:
5 CC X+25 Y+25 6 L X+45 Y+25 RR F200 M3 7 C X+45 Y+25 DR+
With polar coordinates:
18 CC X+25 Y+25 19 LP PR+20 PA+0 RR F250 M3 20 CP PA+180 DR+
 Define the pole CC before programming polar coordinates!  Program the pole CC only in Cartesian coordinates!  The pole CC remains effective until you define a new one!  The arc end point can be defined only with the polar
coordinate angle (PA)!
Path Functions
21
Circular Path with Known Radius (CR)
Coordinates of the arc end point Radius R If the central angle ZW > 180, R is negative. If the central angle ZW < 180, R is positive. Direction of rotation DR
10 L X+40 Y+40 RL F200 M3 Arc starting point 11 CR X+70 Y+40 R+20 DR- Arc
11 CR X+70 Y+40 R+20 DR+ Arc
1
2
or
Path Functions
10 L X+40 Y+40 RL F200 M3 Arc starting point 11 CR X+70 Y+40 R-20 DR- Arc
11 CR X+70 Y+40 R-20 DR+ Arc
22
3
4
or
Arcs
and
1
2
Arcs 3 and
4
Circular Path CT with Tangential Connection
Coordinates of the arc end point Radius compensation RR/RL/R0 Feed rate F Miscellaneous function M
With cartesian coordinates:
5 L X+0 Y+25 RL F250 M3 6 L X+25 Y+30 7 CT X+45 Y+20 8 L Y+0
With polar coordinates:
12 CC X+40 Y+35 13 L X+0 Y+35 RL F250 M3 14 LP PR+25 PA+120 15 CTP PR+30 PA+30 16 L Y+0
 Define the pole CC before programming polar coordinates!  Program the pole CC only in Cartesian coordinates!  The pole CC remains effective until you define a new one!
Path Functions
23
Helix (Only in Polar Coordinates)
Calculations (upward milling direction)
Path revolutions: n = Thread revolutions + overrun at start and
end of thread Total height: h = Pitch P x path revolutions n Incr. coord. angle: IPA = Path revolutions n x 360° Start angle: PA = Angle at start of thread + angle for
overrun Start coordinate: Z = Pitch P x (thread revolutions + thread
overrun at start of thread)
Shape of helix
Internal thread Work direction Direction Radius comp.
Right-hand Z+ DR+ RL Left-hand Z+ DR RR
Path Functions
Right-hand Z DR RR Left-hand Z DR+ RL
External thread
Right-hand Z+ DR+ RR Left-hand Z+ DR RL
Right-hand Z DR RL Left-hand Z DR+ RR
24
M6 x 1 mm thread with 5 revolutions
12 CC X+40 Y+25 13 L Z+0 F100 M3 14 LP PR+3 PA+270 RL 15 CP IPA-1800 IZ+5 DR- RL F50
:
FK Free Contour Programming
See Programming Tool Movements  FK Free Contour Programming
If the end point coordinates are not given in the workpiece drawing or if the drawing gives dimensions that cannot be entered with the gray path function keys, you can still program the part by using the FK Free Contour Programming.
Possible data on a contour element:
 Known coordinates of the end point  Auxiliary points on the contour element  Auxiliary points near the contour element  A reference to another contour element  Directional data (angle) / position data  Data regarding the course of the contour
To use FK programming properly:
 All contour elements must lie in the working plane.  Enter all available data on each contour element.  If a program contains both FK and conventional blocks, the FK
contour must be fully defined before you can return to conventional programming.
These dimensions can be programmed with FK
FK Free Contour
Programming
25
Working with the Interactive Graphics
Select the PGM+GRAPHICS screen layout!
The interactive graphics show the contour as you are programming it. If the data you enter can apply to more than one solution, the following soft keys will appear:
To show the possible solutions
To enter the displayed solution in the part program
To enter data for subsequent contour elements
FK Free Contour
Programming
Standard colors of the interactive graphics
Fully defined contour element
The displayed element is one of a limited number of possible solutions
The element is one of an infinite number of solutions
Contour element from a subprogram
To graphically display the next programmed block
26
Initiating the FK Dialog
Initiate the FK dialog
Straight Circular
Contour element without tangential connection
Contour element with tangential connection
Pole for FK programming
End Point Coordinates X, Y or PA, PR
Cartesian coordinates X and Y
Polar coordinates referenced to FPOL
Incremental input
7 FPOL X+20 Y+30 8 FL IX+10 Y+20 RR F100 9 FCT PR+15 IPA+30 DR+ R15
FK Free Contour
Programming
27
Circle Center (CC) in an FC/ FCT block
Cartesian coordinates of the circle center
Polar coordinates of the circle center referenced to FPOL
Incremental input
10 FC CCX+20 CCY+15 DR+ R15 11 FPOL X+20 Y+15 ... 13 FC DR+ R15 CCPR+35 CCPA+40
FK Free Contour
Programming
Auxiliary Points
... P1, P2, P3 on a contour
:
For straight lines For circles: up to 3 auxiliary points
... next to a contour
Coordinates of the auxiliary points
Perpendicular distance
up to 2 auxiliary points
28
13 FC DR- R10 P1X+42.929 P1Y+60.071 14 FLT AN-70 PDX+50 PDY+53 D10
Direction and Length of the Contour Element
Data on a straight line
Gradient angle of a straight line
Length of a straight line
Data on a circular path
Gradient angle of the entry tangent
Length of an arc chord
27 FLT X+25 LEN 12.5 AN+35 RL F200 28 FC DR+ R6 LEN 10 AN-45 29 FCT DR- R15 LEN 15
Identifying a closed contour
Beginning: CLSD+ End: CLSD
12 L X+5 Y+35 RL F500 M3 13 FC DR- R15 CLSD+ CCX+20 CCY+35 ... 17 FCT DR- R+15 CLSD-
FK Free Contour
Programming
29
Values Relative to Block N: Entering Coordinates
Cartesian coordinates relative to block N
Polar coordinates relative to block N
 Relative data must be entered incrementally!  CC can also be programmed in relative values!
12 FPOL X+10 Y+10 13 FL PR+20 PA+20 14 FL AN+45
FK Free Contour
15 FCT IX+20 DR- R20 CCA+90 RX 13
Programming
16 FL IPR+35 PA+0 RPR 13
30
Values Relative to Block N: Direction and Distance of the Contour Element
Gradient angle
Parallel to a straight contour element Parallel to the entry tangent of an arc
Distance from a parallel element
Always enter relative values incrementally!
17 FL LEN 20 AN+15 18 FL AN+105 19 FL LEN 12.5 PAR 17 DP 12.5 20 FSELECT 2 21 FL LEN 20 IAN+95 22 FL IAN+220 RAN 18
FK Free Contour
Programming
31
Loading...
+ 74 hidden pages