Sinumerik Programming Basics (828D)

Why Siemens Feels Different

If you grew up on Fanuc, the Sinumerik 828D looks familiar at first glance—G0, G1, G54, G41 all exist—then gets weird fast: programs have names instead of O-numbers, tools are called by name, canned cycles are function calls with parameter lists, and coordinate shifting is done with words like TRANS and AROT instead of G52 and G68. This page is the bridge: the minimum a Fanuc programmer needs to read, edit, and write 828D programs confidently.

Everything here applies to the Sinumerik 828D and its big brother the 840D sl—they share the same programming language.

Program Structure & File Types

Siemens programs are named files, not O-numbers. There are two file types, and workpieces can be grouped into workpiece directories (.WPD) that hold a part's main program, subprograms, and tool data together.

Block format is looser than Fanuc: N-numbers are optional, leading zeros are not required (G0 not G00), and decimal points are not needed on whole numbers. Comments start with a semicolon and run to the end of the line:

;**************** Tool change ****************
T="MILLER20" D1 M6        ; this is a comment
G95 FZ=0.14 S3900 M3 M8   ; feed per tooth, spindle on, coolant on

Operator messages: where Fanuc needs #3006 macro trickery, Siemens has MSG() built in. The text displays on the operator panel until cleared or overwritten:

MSG ("FLIP PART - OP20 FIXTURE")
M0                        ; hold for the operator
MSG ("")                  ; clear the message

The Fanuc-to-Siemens Translation Table

This is the heart of it. Most of what you know transfers—you just need the new vocabulary.

The biggest mental shifts: D is a cutting edge, not a comp register (one tool can carry several D edges, each with its own length and radius), and cycles are subroutine calls, not modal G-codes.

Frames: TRANS, ROT, SCALE, MIRROR

Siemens handles all programmable coordinate shifting through frames. Where Fanuc gives you G52 (local shift) and G68 (rotation) as separate features, Siemens gives you one consistent family of commands that stack on top of the active work offset. The plain form replaces any previous programmable frame; the A-prefixed form is additive to it.

Example — drill the same 3-hole pattern at two fixture locations, the second one rotated 30 degrees:

G54 G710
T="DRILL10" D1 M6
G94 F500 S1600 M3 M8

TRANS X100 Y50            ; shift origin to pocket 1
HOLES                     ; subprogram drills pattern at local 0,0

TRANS X250 Y50            ; REPLACES the first shift (not added)
AROT RPL=30               ; then rotate the pattern 30 deg
HOLES

TRANS                     ; cancel all frames - back to plain G54
G0 Z200 M9
M30

Suppression, from mildest to strongest: G500 deselects the settable work offset (G54–G599), G53 suppresses offsets for one block, and SUPA suppresses everything including programmable frames—use SUPA for tool-change and home moves.

Modal Groups & Key M-Codes

Like Fanuc, one code per G-group can be active at a time, and the control displays active groups in the G-function window. The groups you will actually look at:

M-codes are mostly home turf. Reserved system M-functions on the 828D: M0/M1 stop/optional stop, M2/M17/M30 program end, M3/M4/M5 spindle, M6 tool change, M40–M45 gear ranges. Coolant is machine-dependent but typically M7/M8 on, M9 off.

Cycles Instead of Canned Cycles

Drilling, pocketing, and contour work are done with named cycles—CYCLE81 (center/spot), CYCLE82 (drill), CYCLE83 (peck), CYCLE84 (rigid tap), CYCLE61 (face mill), POCKET3/POCKET4 (rectangular/circular pockets), CYCLE62/63/64 (contour milling). You almost never type the parameter lists by hand: the editor's cycle input screens fill them in graphically, and the resulting call is one line of code you can re-open in the same screen later.

To repeat a cycle at multiple positions, make it modal with MCALL—the cycle then executes at every subsequent position block until a bare MCALL cancels it:

T="DRILL10" D1 M6
G94 F500 S1600 M3 M8
MCALL CYCLE82(50,-10,1,-25,,0,0,1,12)   ; drill cycle now modal (like G81)
X15 Y15                                  ; drills here
X165 Y15                                 ; and here
X165 Y165                                ; and here
MCALL                                    ; cancel (like G80)
G0 Z200 M9

Position patterns can also be defined once with a label and replayed for the next tool using REPEATB—center-drill the pattern, then repeat the identical positions with the drill.

Subprograms

Subprograms are called by name, with an optional P repeat count, and end with M17 or RET. No M98, no P-number lookups:

; main program (PART1.MPF)
G54 G710
T="MILLER10" D1 M6
S8500 M3 M8
HOLES P2        ; call HOLES.SPF, run it twice
M30

; subprogram (HOLES.SPF)
G0 X0 Y0
G1 Z-5 F300
G0 Z5
X20
G1 Z-5
G0 Z50
M17             ; return to caller (Fanuc M99)

Subprograms stored outside NC memory (network drive, USB, CF card) are executed with EXTCALL "NAME.SPF"—the Siemens answer to drip-feeding a subprogram.

ShopMill vs G-Code Programs

The 828D editor can hold two kinds of programs, and both live side by side on the control. A G-code program is what everything above describes—DIN/Siemens code, typically posted from CAM. A ShopMill program (requires the ShopMill/ShopTurn option) is a conversational machining step program built entirely through graphic input screens: a work plan of steps rather than lines of code.

A ShopMill program has three parts: a program header (blank dimensions, retraction planes, and other parameters that affect the whole program), program blocks (the individual machining steps with technology data and positions—technology blocks and position blocks are automatically linked by the control), and an end of program block that can also set repeats. Tool changes, spindle direction, and coolant come from the step screens—no M6 or M3 to type. Bad inputs are caught at entry time instead of at the machine.

You can also insert G-code blocks inside a ShopMill program when a step screen can't express what you need—a common pattern is a ShopMill work plan with a few raw G-code lines dropped in.

Worked Example: Face and Drill

A compact but complete 828D program in the style of the Siemens milling manual's own example—face the top, then center-drill and drill a pattern with modal cycles:

;PART_4.MPF
WORKPIECE(,,"","BOX",112,1,-20,-100,-2.5,-2.5,182.5,182.5)  ; blank for simulation
G54 G710 G90                 ; offset, metric (incl. feeds), absolute

;**************** Face ****************
T="FACING TOOL" D1 M6
G95 FZ=0.1 S3000 M3 M8       ; feed per tooth
CYCLE61(50,1,1,0,-2.5,-2.5,185,185,2,80,0,0.1,31,0,1,10)
G0 Z200 M9

;**************** Spot drill ****************
T="CENTERING TOOL10" D1 M6
G94 F1000 S12000 M3 M8
MCALL CYCLE81(50,-10,1,5,,0,10,1,11)
POS_1: CYCLE802(111111111,111111111,15,15,165,15,165,165,15,165,,,,,,,,,,,0,0,1)
MCALL                        ; POS_1 labels the position pattern for reuse
G0 Z200 M9

;**************** Drill ****************
T="DRILL10" D1 M6
G94 F500 S1600 M3 M8
MCALL CYCLE82(50,-10,1,-25,,0,0,1,12)
REPEATB POS_1                ; repeat the labeled position pattern
MCALL
G0 Z200 M9
M30

References

• Siemens, SINUMERIK 840D sl / 828D Universal Operating Manual, 08/2018, 6FC5398-6AP41-0BA0.
• Siemens, SINUMERIK 840D sl / 828D Milling Operating Manual, 08/2018, 6FC5398-7CP41-0BA0.