Siemens SLOT1 and SLOT2 Slot Milling Cycles Programming Guide

Introduction

Dragging a milling cutter directly across the center axis of a turning machine during slot transitions will result in a violent, high-speed collision with the metal spigot or chuck left standing in the middle of the circular pattern. This critical setup issue arises from standard straight-line rapid traverse movements that do not account for the central physical spigot. When programmers utilize automated slot milling operations, they must govern coordinate positioning paths and tooling variables to prevent mechanical destruction. Uncut center pillars and tool fracture from vertical plunging represent significant risks if cutter geometry, active offsets, and safety clearances are incorrectly calculated. Proper cycle configuration ensures automated slot clearing without scrap parts or machine downtime.

Technical Summary

Feature / Constraint	Specification Details
Command Codes	SLOT1 (Longitudinal slot milling), SLOT2 (Circumferential slot milling)
Modal Group	Non-modal cycles (must be called explicitly or through MCALL)
Supported Brands	Siemens (Sinumerik)
Critical Parameters	WID (Slot width), VARI (Machining type/insertion mode), _FFCP (Circumferential position feedrate)
Main Constraint	Active tool radius compensation (D number) is mandatory prior to execution. Center-cutting cutter (DIN844) required for G1 vertical insertion.

Quick Read

• Select SLOT1 to mill straight slots oriented radially toward a central coordinate point.
• Select SLOT2 to mill curved, circumferential slots that conform to the layout circle radius.
• Use a milling cutter diameter greater than half of the slot width to prevent uncut center pillars that scrap the workpiece.
• Program tool radius compensation with G41, G42, or an active D number before calling the cycle to prevent Alarm 61000.
• Set the VARI parameter tens digit to 1 to force the tool to position circumferentially using safety feedrate _FFCP and avoid central spigots.
• Employ a DIN844 center-cutting endmill to survive the vertical plunging phase when G1 insertion is defined in the cycle parameters.
• Combine slot cycles with MCALL and HOLES2 position patterns in newer Siemens software where array variables are hidden.

Basic Concepts

The practical programming effect of the SLOT1 and SLOT2 cycles is the automated clearing of complex slot arrangements on circular paths. When invoking SLOT1, the machine radially aligns the longitudinal axis of the slots toward the center of the coordinate pattern, while SLOT2 shapes the slots along the curvature of the circle itself.

Programmers must carefully manage their tooling dimensions: while the control throws alarm code 61105 if the cutter diameter exceeds the slot width, it does not check if the cutter is too small. If the milling cutter diameter is less than half of the slot width, a tall pillar of residual material will remain standing in the center of the slot, rendering it a scrap part.

Operators must also watch out for tool geometry constraints; unless pre-drilled or helical insertion is used, the programmed tool must be center-cutting (DIN844) to survive the perpendicular plunge.

Command Structure

The SLOT1 and SLOT2 cycle syntax comprises a detailed sequence of coordinates, dimensions, and feeding rates. The control evaluates these arguments to generate toolpath loops without requiring manual G02 or G03 coordinate calculations. In addition to basic geometric dimensions, the cycle accepts safety parameters, finishing allowances, and insertion mode codes that adapt to different workpiece configurations.

A crucial aspect of these cycles is how they handle coordinate systems. The machining plane must be active before the cycle call. The values for the reference plane, safety clearance, and final machining depth are interpreted based on active coordinate offsets and global machine data settings.

Syntax

SLOT1 (RTP, RFP, SDIS, _DP, _DPR, NUM, LENG, WID, _CPA, _CPO, RAD, STA1, INDA, FFD, FFP1, _MID, CDIR, _FAL, VARI, _MIDF, FFP2, SSF, _FALD, _STA2, _DP1, _UMODE, _FS, _ZFS, _GMODE, _DMODE, _AMODE)

SLOT2 (RTP, RFP, SDIS, _DP, _DPR, NUM, AFSL, WID, _CPA, _CPO, RAD, STA1, INDA, FFD, FFP1, _MID, CDIR, _FAL, VARI, _MIDF, FFP2, SSF, _FFCP, _UMODE, _FS, _ZFS, _GMODE, _DMODE, _AMODE)

Parameters

Parameter	Type	Description	Value Range
NUM	Integer	Number of slots to be machined	Integer > 0
WID	Real	Slot width	Real, entered without a sign
LENG	Real	Slot length (used in SLOT1 only)	Real
AFSL	Real	Opening angle of the slot (used in SLOT2 only)	Real
CDIR	Integer	Milling direction setting	0 = Down-cut, 1 = Up-cut, 2 = G2 direction, 3 = G3 direction
VARI	Integer	Machining type code. Units digit represents process type. Tens digit represents tool insertion method.	Units: 0 = complete, 1 = roughing, 2 = finishing. Tens: 0 = G0 perpendicular, 1 = G1 perpendicular, 2 = helical, 3 = oscillation. (For SLOT2, tens = 1 positions on circular path)
_FFCP	Real	Feedrate for intermediate positioning on a circular path (used in SLOT2 only)	mm/min

Brand Applications

Siemens

Siemens significantly distinguishes its slot milling backend from other standard ISO control brands through several advanced behaviors. First is its dynamic obstacle-avoidance routing: Unlike basic macros that only support straight-line rapid returns between pattern features, Siemens natively integrates the _FFCP circular-path intermediate positioning directly into the SLOT2 cycle, mathematically conforming the transition path to the part's radius to avoid central spigots.

Second is its spindle-dependent direction logic: Rather than forcing the programmer to calculate cut direction mathematically, Siemens automatically reads the active spindle state (M3 or M4) prior to the cycle call and internally translates the programmer's request for "down-cut" or "up-cut" into the correct G2 or G3 toolpath direction.

Finally, Siemens features evolutionary pattern separation: In modern iterations, Siemens detaches the array logic (like hole counts and angles) from the slot cycle itself, allowing SLOT1 and SLOT2 to be effortlessly coupled with dedicated position pattern cycles like HOLES2 via MCALL, providing vastly superior coordinate flexibility.

Brand Comparison

Model / Version	Parameter Hiding & Array Logic	Depth Calculation Behavior	Programming Practice
Sinumerik 840D sl / 828D (Newer Software)	Array parameters such as NUM, RAD, and INDA are hidden on the cycle screen form.	Depth calculation can be altered globally using machine data parameter MD55214 $SCS_FUNCTION_MASK_MILL_SET.	Programmers define a single-slot cycle, then pair it with MCALL and pattern cycles like HOLES2.
Sinumerik 810D / 840D Powerline (Older Software)	All array parameters (NUM, RAD, INDA) are displayed and entered directly inside SLOT1 or SLOT2 parameters.	Follows legacy depth calculation, measuring depth strictly from the reference plane (RFP) down.	The cycles are executed directly with all spacing and quantity parameters defined in a single block.
Sinumerik 808D (Basic CNC)	Direct entry of slot array coordinates is supported on basic screens without advanced menu separation.	Standard depth calculation with fixed safety distance (SDIS) inclusion based on standard model configuration.	Called directly in the main G-code program block, often without advanced coordinate pattern cycle links.

Technical Analysis

Analyzing the behavior of Siemens slot cycles reveals that tool movement optimization is highly dependent on software version configurations. On older Powerline controllers, executing SLOT1 or SLOT2 required specifying the center points, radii, and counts directly. This unified parameterization made program modification tedious when changing pattern layouts. Modern Siemens Operate environments solve this by hiding array-specific parameters from the cycle screens, shifting coordinate array generation to independent position templates. This allows programmers to modalize the cycle via MCALL, executing it over varying layout coordinates defined in subsequent program lines.

Another crucial variable is the machine data parameter MD55214 $SCS_FUNCTION_MASK_MILL_SET. This parameter alters the depth calculation logic. Depending on its setting, the machine may or may not include the safety clearance SDIS in the final depth calculation. Failure to verify this parameter on a new machine setup can result in slots being milled either too deep or too shallow, leading to scrapped parts. Spindle state detection is also handled dynamically; the control reads the active M3 or M4 rotation before generating the climb or conventional toolpath (G2 or G3), ensuring proper chip evacuation and finish quality.

Program Examples

Siemens Example

N420 SLOT2( 50.00000, 0.00000, 2.00000, -5.00000, 2.00000, 3, 30.000, 6.00000, 38.00000, 70.00000, 20.00000, 165.00000, 90.00000, 300.00000, 300.00000, 3.00000, 3, 0.20000, 0, 5.00000, 250.00000, 3000.00000, 0.00000)

dry run

• Step 1: Rapid positioning. The tool traverses at rapid speed (G0) to the safety retraction plane RTP of 50.0 mm.
• Step 2: Center and start alignment. The controller calculates the position of the first slot on the circle using center coordinates _CPA (38.0 mm) and _CPO (70.0 mm), radius RAD (20.0 mm), and starting angle STA1 (165.0 degrees). The tool moves to this position at rapid feed.
• Step 3: Depth positioning. The tool plunges to the safety clearance SDIS (2.0 mm above reference plane RFP).
• Step 4: Plunging execution. The tool feeds vertically down to the first cutting depth at the programmed feedrate FFD (300.0 mm/min). Since VARI is 0 (G0 perpendicular plunge), the tool descends directly.
• Step 5: Slot milling. The spindle runs at speed SSF (3000.0 rpm) in the programmed direction. The tool mills the first slot along the circumference corresponding to opening angle AFSL (30.0 degrees) at G3 (CDIR = 3) with feedrate FFP1 (300.0 mm/min), leaving a wall finishing allowance _FAL of 0.2 mm.
• Step 6: Pattern iteration. The tool retracts to safety clearance, positions for the second slot at an increment of INDA (90.0 degrees), and repeats the process until all 3 slots (NUM = 3) are rough-machined.
• Step 7: Finishing wall pass. The cycle automatically performs finishing passes along the slot walls at finishing feedrate FFP2 (250.0 mm/min) to clean the 0.2 mm finishing allowance.
• Step 8: Final retraction. The tool retracts to the retraction plane RTP (50.0 mm) at G0 upon completing all slots.

Error Analysis

Alarm Code	Trigger Condition	Operator Symptom	Root Cause / Fix
Alarm 61000	Slot cycle called before a tool radius compensation is programmed.	The machine cycle aborts execution immediately at the start of the block.	Program tool radius compensation (G41/G42 or active D number) before the cycle call.
Alarm 61105	Active milling cutter diameter exceeds the programmed slot width.	The control interrupts execution and throws a cutter radius too large error.	Change to a smaller milling cutter; the cutter diameter must be strictly less than slot width WID.
Alarm 61102	An unsupported value is programmed for the VARI parameter.	The program halts and displays a machining type defined incorrectly message.	Correct the value of the VARI parameter in the cycle call block.

Application Note

Scrapping a precision workpiece due to a tall pillar of residual metal remaining in the slot center occurs when the milling cutter diameter is programmed to be less than half of the slot width, because the control does not automatically verify the minimum tool diameter. To ensure clean clearing of the slot pocket, the operator must select a cutter whose diameter is greater than half of the width value (WID). Additionally, when machining circumferential slot configurations (SLOT2) on turning centers, a physical spigot is frequently left standing at the center of the circular pattern. Programmers must set the tens digit of the VARI parameter to 1 to command the control to position the tool circumferentially between slots at a controlled feedrate (_FFCP), avoiding G0 rapid transitions directly across the center axis which would drag the spindle into a hard collision with the spigot or chuck.

Related Command Network

• LONGHOLE: Machines elongated holes on a circle, serving as a simpler alternative to SLOT1 when no wall offset or finishing allowances are required.
• POCKET3: Invokes rectangular pocket milling, which uses similar parameter structures for defining finishing allowances and infeed steps on flat planes. Also compare with pocket cycle details in pocket3-pocket4-pocket-milling.
• POCKET4: Executes circular pocket clearing, sharing the unit-digit and tens-digit machining type definition system found in the VARI parameter.
• HOLES2: Generates a circular pattern of holes, which is coupled with slot cycles to distribute slots at specific coordinate points. Also check the centering cycle at siemens-cycle81-centering-drilling-cycle and deep hole drilling at cycle83-deep-hole-drilling.
• MCALL: Activates a modal cycle call, enabling the controller to execute SLOT1 or SLOT2 at every position programmed in a subsequent coordinate list or pattern cycle.

Conclusion

Successful slot milling using SLOT1 and SLOT2 requires exact tool radius compensation activation beforehand and precise matching of tool diameter to slot width. Correctly configuring the VARI parameter prevents collisions with central spigots and eliminates uncut residual pillars, guaranteeing dimensionally stable slot features on Sinumerik controls.

FAQ

How can I prevent a central spigot from causing a tool collision in SLOT2?

Spindle collisions with uncut center spigots during slot transitions are avoided by changing the positioning strategy. Proactively set the tens digit of the VARI parameter to 1, and define a controlled positioning feedrate in the _FFCP parameter to force the tool to travel along the slot circle circumference rather than moving in a straight G0 line across the center.

Why does the CNC abort with Alarm 61000 when invoking SLOT1?

The Sinumerik control requires tool radius information to calculate the offsets for slot boundaries before starting any path movement. Always activate a tool correction offset by programming G41, G42, or selecting an active tool offset number (D number activation) prior to calling the slot cycle.

How do I handle slot cycles on newer Siemens software where some parameters are hidden?

Modern Siemens Operate systems shift array layout logic out of the core cycle parameter screen. Program a single-slot cycle without array details, activate it modally using the MCALL command, and then call a coordinate pattern cycle like HOLES2 immediately after to locate each slot.