Marposs MIDA Macro Programming – Mitsubishi Systems Chapter

Document source: D310JBAG00 (VTS Bridge Mitsubishi)、D310A1AG07 (Tool Check on Fanuc)、D310A2AG16 (Part Check on Fanuc) Applicable systems: Mitsubishi M800/M80 series, M700/M70V series (M-series machini

Marposs MIDA Macro Programming – Mitsubishi Systems Chapter

Document source: D310JBAG00 (VTS Bridge Mitsubishi), D310A1AG07 (Tool Check on Fanuc), D310A2AG16 (Part Check on Fanuc)
Applicable systems: Mitsubishi M800/M80 series, M700/M70V series (M-series machining centers), C70, Meldas series Products: Marposs MIDA probe system, MIDA tool setter, VTS image tool setter

This question has been synchronously published to CSDN: https://jcetech.blog.csdn.net

catalogue

  • Overview
  • Mitsubishi M800/M70 G31 Detailed explanation of jumping function
  • SKIP related parameter configuration table
  • Fanuc MIDA Macro Program Porting to Mitsubishi
  • VTS Bridge Mitsubishi Complete Configuration
  • Comparison Table of Variable Compatibility between Mitsubishi and Fanuc
  • O9366 System Configuration (Mitsubishi Recommended Value)
  • Common Problems and Troubleshooting

    • I. Overview

    The Marposs MIDA trigger probe system is applied to CNC machining centers to achieve in machine measurement – aligning the workpiece during the machining preparation stage and performing in-situ dimension detection between processes/after work, without the need to move the workpiece to a coordinate measuring machine.

    In the Marposs MIDA software package, there is only one official document specifically for Mitsubishi CNC systems, D310JBAG00 (VTS Bridge Mitsubishi). This manual is mainly aimed at the installation and operation of bridge software for VTS image type tool setter on Mitsubishi system. The complete software package code isS609210534.

    And the Fanuc version MIDA Macro Program (Tool alignment device P9376~P9388, workpiece measurement O9301~O9392)Due to Mitsubishi M80/M70 The system is G Highly compatible with Fanuc in terms of code system, In principle, it can be ported to Mitsubishi systems for operation. This paper is based on D310JBAG00 Provided technical data and Fanuc compatibility principle, Systematically explain the measurement programming system on Mitsubishi systems, Parameter Configuration, Transplantation methods and VTS Bridge software configuration.

    1.1 Mitsubishi System Measurement Programming Three Layer Architecture

    The measurement programming on Mitsubishi systems can be summarized into the following three layers:

    Layer 1: G31 Jump function (SKIP Signal) ─ Hardware entrance triggered by the probe │ Mitsubishi Features: G31.1~G31.3 Multi segment jump, R Parameter variable speed jump ▼
    Layer 2: G37 Automatic tool length measurement ─ Special instructions for the tool setter │ Automatically write after triggering H Compensation number ▼
    Level 3: MIDA Macro program architecture ─ Standardized calibration/measurement/Compensation call interface ├─ tool setter: P9376~P9388 (Fanuc transplantation → Mitsubishi) ├─ workpiece measurement: O9301~O9392 (Fanuc transplantation → Mitsubishi) └─ VTS Image knife: O9700~O9731 (Bridge software communication)

    1.2 System Requirements

    • Mitsubishi Custom Macro B (Standard Configuration)
    • G31 Jump step input signal (SKIP)
    • User macro program storage space
    • Ethernet communication interface (VTS bridging)

    2. Mitsubishi M800/M70 G31 skip function in detail

    2.1 G31 Basic Behavior

    Mitsubishi’s G31 has the same functionality as Fanuc and belongs to the 00 group (one-shot G code). Continuously monitoring jump signals during linear interpolation motion (SKIP Signal), Once the probe is triggered, immediately stop moving and record coordinates.

    G31 Z-50. F300; Z Axial downward movement, Waiting for the probe to trigger
    #100 = #5063; Read trigger point immediately Z Coordinate and save
    G00 Z100.; Safe knife return

    Behavioral characteristics:

  • Shares the same feed rate mode as G01 (F value)
  • Only respond to one jump signal, stop after triggering
  • If the entire process is not triggered, it will generateOvertravel alarm (such as PS0032); it must be handled in the program with #3000 or ONERROR capture

    • 2.2 Trigger Coordinate System Variables

    Variable number meaning With Fanuc Remark
    #5061 Trigger point X-axis mechanical coordinates ✅ exactly the same Must be G31 Read the next paragraph immediately
    #5062 Trigger point Y-axis mechanical coordinates ✅ exactly the same Ditto.
    #5063 Trigger point Z-axis mechanical coordinates ✅ exactly the same Ditto.

    ⚠️ Key rules: The above variables are G31 Triggered instantly written by the system, It is not overwritten by later movement commands; note however that a further trigger updates the same variables, so read the previous point before the next trigger.The skip coordinate is the value latched at the instant the skip signal is input — the official manual states it can be read at any time afterwards.This behavior is completely consistent with Fanuc, FANUC MIDA Macro programs can be used directly without any modifications.

    Standard Read Mode:

    G31 Z-20. F200
    #101 = #5063; ← Save Now, Cannot be delayed
    G31 X10. F200
    #102 = #5061; ← Save Now

    2.3 Mitsubishi Exclusive: Multi segment jump G31.1 ~ G31.3

    Mitsubishi M800/M70 The series has expanded the standard G31, Support Multi segment jump command G31.1 / G31.2 / G31.3. This feature is usually not available in the Fanuc system (Unless optional features are available).

    Instruction function Typical Applications
    G31 Single jump (standard) Single point surface measurement
    G31.1 Multi segment jump triggered for the first time Record the first touch location
    G31.2 Multiple jumps triggered for the second time Record the location of the second touch
    G31.3 Multi segment jump triggered for the third time Record the location of the third touch

    Example of inner diameter measurement:

    G90 G00 X0 Y0; Locate to the center of the hole
    G01 Z-5. F500; Down to measurement depth
    G31.1 X-20. F200; X Negative direction movement, Record the first trigger
    #101 = #5061; ← Read and save immediately! G00 X0
    G31.2 X20. F200; X Forward movement, Record the second trigger
    #102 = #5061; ← Read and save immediately! G00 Z100.
    #103 = #102 - #101; Calculate diameter

    ⚠️ Important: each time G31.1/G31.2/G31.3 After triggering, All coordinates are written into the same group #5061~#5063. must notWait for all jumps to be completed and read at once, Must be assigned and saved immediately after each trigger.

    Typical application scenarios for multi-stage jumping:

  • Inner/Outer Diameter Measurement– Calculate the difference between two reverse touches
  • Keyway/groove width– Touch record on both sides
  • Step height– measurement of the difference between two Z-planes
  • Eccentricity detection– Multi angle touch recording position deviation

    • 2.4 G31 deceleration command (R0/R1) and variable-speed skip (Fn)

    Mitsubishi officially requires the deceleration command R0/R1 in every G31 block: when omitted the machine behaves as R0 (deceleration time constant = 0); with R1 post-interpolation automatic acceleration/deceleration is performed even when the skip signal is input. R is a deceleration command, not a “retract speed after triggering” — the earlier wording was wrong. Variable speed after triggering is provided by the official variable-speed skip: G31 X__ R__ F__ F1=__ … Fn=__; (per skip-signal number 1–8; Fn=0 means stop).

    G31 Z-20. F500 R0 F1=50 — Z moves at F500; after skip signal 1 is input it continues at F1=50.

    2.5 G31 P — skip signal command (multi-step skip function 2)

    Official definition: the skip signal command p specifies the skip signal, with p in the range 1–255 (out of range raises program error P35). p is the logical sum of skip signals 1–8 — for example P5 means skip is executed when skip signal 1 or 3 is input. It is also used for simultaneous skip in multi-system configurations. It is not “P1–P4 selecting channels SKIP1–SKIP4”, and it is not limited to four values.

    G31 X100. P5 F100 — skip is executed when skip signal 1 or 3 is input.

    2.6 SKIP signal hardware link

    Understanding the entire SKIP signal chain can help troubleshoot:

    Probe triggered ↓
    wireless/Infrared emission ← The probe has a built-in transmitter (e.g. Marposs VOS/WRS) ↓
    Receiver receives signal ↓
    PMC input signal (DI point) ← Determined by wiring / ladder (SKIP mapping and polarity are handled here) ↓
    Internal SKIP (skip) signal ↓
    G31/G37 command response ← Requires the skip option (spec) + parameters #1174 / #12022

    key points:

  • The SKIP signal must be mapped to the internal skip signal in the PMC ladder; the mapping and polarity are handled by the ladder — the official Mitsubishi skip parameter list contains no “SKIP polarity” parameter
  • Whether G31/G37 can be used is a specification (option) matter: without the skip option, G31 raises the program error P601 NO SKIP SPEC (the official remedy is only “Check the specifications”)
  • Speed and acceleration/deceleration: #1174 skip_F (G31 skip speed) and #12022 skipF_spec (bit0 cutting feedrate override, bit1 dry run, bit2 speed source when F is omitted). Mitsubishi officially requires the deceleration command R0/R1 in every G31 block (omitted = R0, i.e. deceleration time constant = 0)
  • The G37 sensor signal (measurement-position-reached signal) is shared with the skip signal, so a healthy skip chain is a prerequisite for G37

    • 2.7 G37 Automatic tool length measurement

    G37 It’s a Mitsubishi machining center M Special instruction for automatic tool length measurement of the system, belongs to G31 Upper level application of functionality:

    Basic usage:

    T01 M06; tool change
    G90 G00 G54 X0 Y0; Position above the tool setter
    G43 Z100. H01; Establish blade length compensation
    G00 Z-50.; Quickly move to a safe distance above the tool setter
    G37 Z-70. F300; Z Slow axis downward movement, Automatically write the tool length after contacting the tool setter
    G00 Z100.; retract the tool
    M01

    execution flow:

  • Z-axis moves downwards at a speed of F
  • Tool contact tool setter → SKIP signal triggered
  • The system records the current position Z coordinate
  • Automatically calculate and write the tool length value from the current tool’s H compensation number
  • Mobile Stop

    • Preconditions:

    condition Explanation Required
    Skip option enabled The G37 sensor signal (measurement-position-reached signal) is shared with the skip signal; without the skip option G31/G37 raise P601 NO SKIP SPEC — a specification issue, unrelated to the probe or wiring ✅
    Measurement position and deceleration zone correctly set G37 α__ R__ D__ F__; — α = measuring axis address and target position coordinate, R = distance from the point where the measuring speed starts to the target (incremental), D = range within which the tool must stop (incremental), F = measuring speed. When R/D/F are omitted the values come from parameters #8005 / #8006 / #8004 ✅
    Within the measurement allowable range Exceeding it stops the axis and raises program error P607 ✅
    G43 established (recommended) The updated compensation takes effect from the next T command (L series) or the next Z-axis / measuring-axis command (M series) after G37 Advised

    Attention: On turning systems (L series) G37 is used differently: the L series uses G36 to measure the X axis (radial) and G37 to measure the Z axis (axial).

    3, SKIP related parameter configuration table

    3.1 Summary Table of Core Parameters

    Mitsubishi’s official parameters related to G31/G37 are listed below (source: Mitsubishi M800/M80/E80/C80 Series Programming Manual, chapters on skip and automatic tool length measurement):

    Parameter (bit) Meaning Value Explanation
    #1174 skip_F — G31 skip speed Per machine spec Used when the G31 block has no F command; if the value is 0 and no F is programmed, program error P603 occurs
    #12022 bit0 skipF_spec/bit0 — cutting feedrate override Per machine builder spec Whether the cutting feedrate override is effective in G31
    #12022 bit1 skipF_spec/bit1 — dry run Per machine builder spec Whether dry run is effective in G31
    #12022 bit2 skipF_spec/bit2 — speed source without F 0 or 1 0: use #1174 skip speed; 1: use the F modal value at the time G31 is executed
    #2102 skip_tL — skip time constant Per machine builder spec Incorrect setting → MCP alarm (Y51 15)
    #2103 skip_t1 — skip time constant Per machine builder spec Incorrect setting → MCP alarm (Y51 16)
    #8004 Automatic tool length measurement — measuring speed 0–60000 mm/min (L series) / 0–1000000 mm/min (M series) “Automatic tool length measurement” on the machining-parameter screen; used when G37 omits F
    #8005 Automatic tool length measurement — deceleration zone r 0–99999.999 mm Corresponds to the G37 R command
    #8006 Automatic tool length measurement — deceleration zone d 0–99999.999 mm Corresponds to the G37 D command
    #1926 (to be verified) Network / IP related setting Per site network Used for VTS Bridge Ethernet communication; confirm the parameter number and the setting method in the machine’s Connection Manual

    3.2 Detailed Explanation of Parameters

    #1174 skip_F — G31 skip speed

    Official definition: when a G31 block has no F command, the value of parameter #1174 (G31 skip speed) is used as the skip speed; if that parameter is 0 and no F is programmed, the program error P603 occurs. When F is programmed in the block, that commanded speed is the skip speed (F1-digit feed is ineffective here).

    On the shop floor: if G31 runs the full distance without stopping, or the speed is obviously wrong, first check whether the block contains an F command — without F everything depends on #1174. A #1174 value that does not match the process shows up as “wrong speed / excessive coasting” (the coasting distance depends on both #1174 and the F command).

    #12022 skipF_spec — override, dry run and F semantics in G31

    Bit Function Official description
    bit0 Cutting feedrate override Effective / ineffective in G31; confirm against the machine builder’s specification
    bit1 Dry run Effective / ineffective in G31; confirm against the machine builder’s specification
    bit2 Speed source when F is omitted =0: use parameter #1174 skip speed; =1: use the F modal value when G31 is executed

    On the shop floor: whether the override or dry run affects G31 during setup is decided by these bits — if the same program behaves differently on two machines, check #12022 first.

    The G31 deceleration command R0 / R1

    Mitsubishi officially requires the deceleration command R0/R1 in every G31 block; when omitted the machine behaves as R0 (deceleration time constant = 0) and does not perform post-interpolation automatic acceleration/deceleration. With R1, post-interpolation automatic acceleration/deceleration is performed even when the skip signal is input. The related time constants are set by #2102 skip_tL / #2103 skip_t1; an incorrect setting raises the MCP alarm (Y51 15).

    G37 measurement conditions: #8004 / #8005 / #8006

    The G37 command format is G37 α__ R__ D__ F__;: α = measuring axis address and target position coordinate, R = distance from the point where the measuring speed starts to the target (fixed radius value / incremental), D = range within which the tool must stop (incremental), F = measuring speed. When R/D/F are omitted, parameters #8005 / #8006 / #8004 are used (“Automatic tool length measurement” on the machining-parameter screen).

    Exceeding the measurement allowable range stops the axis and raises program error P607; the updated compensation takes effect from the next T command (L series) or the next Z-axis (measuring axis) command (M series) after G37. The sensor signal (measurement-position-reached signal) is shared with the skip signal, and its processing delay (excluding the PLC-side delay) is 0–0.2 ms.

    3.3 Parameter Setting Method

    Method 1: set on the parameter page (recommended)

  • M800/M80 series: Mainte page → Param, set #1174 / #12022 / #2102 / #2103; the G37 parameters #8004 / #8005 / #8006 are under “Automatic tool length measurement” on the machining-parameter screen
  • M700/M70V series: Mainte page → Param; confirm the parameter numbers in that model’s parameter manual before setting

    • Method 2: programmable parameter input (G10 L70)

    The official “programmable parameter input” command for the M800/M80/E80/C80 series is G10 L70 (Programming Manual section 15.7.1), with the format G10 L70; P__ S__ A__ H□__; (bit data) / P__ S__ A__ D__; (numeric), terminated by G11 (P = parameter number, S = system number, A = axis number, H□ = bit-type data; numeric data uses D__). Two cautions: (1) Appendix 3 of the manual also lists “programmable parameter input (G10 L50, G11)” and notes that G10 L50 is dedicated to specific models — the M700V/M70V manual states explicitly that the series has no such specification; (2) Mitsubishi does not use the Fanuc N____ R________ bit-string style — follow the parameter/data-number definitions of the manual for the actual model.

    Method 3: a macro program cannot assign system parameters

    System parameters are not user macro variables, so a macro cannot rewrite them with #parameter = value. Parameter changes must be made on the parameter page or through the programmable parameter input command confirmed in the model’s manual. Whether the skip function is available is a specification (option) matter — “flip one bit on the parameter page and it is enabled” is not valid.

    When conducting advanced troubleshooting, it is necessary to understand the addresses of each SKIP signal in PMC (which may vary for different models):

    Signal name Typical PMC address Explanation
    SKIP X address (determined by parameters) Basic SKIP input
    SKIP1~SKIP4 X address Optional multi segment SKIP input

    The actual address allocation needs to refer to the electrical drawings of the machine tool and the PMC ladder diagram.

    4, Fanuc MIDA macro program ported to Mitsubishi

    4.1 Overview of transplant feasibility

    The Fanuc MIDA macro program can run directly on Mitsubishi systems or require only minor modifications for the following reasons:

    Macro Program Fanuc version Mitsubishi version Difficulty of transplantation
    O9366 (System Configuration) ✅ complete ⚠️ Parameter needs to be modified moderate
    O9370 (Protect positioning) ✅ complete ✅ Can be used directly low
    O9371 (Touch and move) ✅ complete ✅ Can be used directly low
    P9376 (calibration) ✅ complete ✅ Can be used directly low
    P9377 (concentric knife measurement) ✅ complete ✅ Can be used directly low
    P9378 (non concentric knife measurement) ✅ complete ✅ Can be used directly low
    P9379 (integrity check) ✅ complete ✅ Can be used directly low
    P9380 (integrity check) ✅ complete ✅ Can be used directly low
    P9386 (Manual Calibration) ✅ complete ✅ Can be used directly low
    P9387 (manual length measurement) ✅ complete ✅ Can be used directly low
    P9388 (single blade measurement) ✅ complete ✅ Can be used directly low
    O9391 (User input) ✅ complete ✅ Can be used directly low
    O9392 (User output) ✅ complete ✅ Can be used directly low
    O9301~O9392 (workpiece) ✅ complete ✅ Can be used directly low

    Explanation: These macro programs use G65/G31/#5061~#5063 Waiting for completely identical instructions on Mitsubishi and Fanuc/variable. The only thing that needs to be modified is O9366 System ConfigurationParameter and variable offset in.

    4.2 Five key points that must be modified

    4.2.1 CNC Type setting (#101=4)

    In O9366, configure the macro so that the CNC type is set to Mitsubishi:

    #101 = 4; 4 = Mitsubishi ← This is Mitsubishi's correct setting

    FANUC MIDA O9366 Defined in CNC Type:

    #101 value CNC type
    1 Fanuc
    2 Haas
    3 Yasnac
    4 Mitsubishi ← Mitsubishi
    5 Mazatrol
    6 Brother

    After setting #101=4, the macro program will automatically select the Mitsubishi-compatible tool compensation table pointer and parameter mapping internally.

    4.2.2 Parameter write instruction (programmable parameter input)

    The official “programmable parameter input” of the M800/M80/E80/C80 series is G10 L70, format G10 L70; P__ S__ A__ H□__; (bit data) / P__ S__ A__ D__; (numeric), terminated by G11. The G10 L50 in Appendix 3 of the manual is noted as dedicated to specific models (the M700V/M70V manual states that the series has no such specification), and its format is P__ N__ H□__ — different from the Fanuc N____ R________ bit-string style. The earlier statement that “the Mitsubishi style is the same as Fanuc” does not hold; follow the parameter-number definitions of the manual for the actual model.

    Other G10 formats:

    Function Mitsubishi official command Explanation
    Write system parameters G10 L70 (specific models: G10 L50) M800/M80 use G10 L70; G10 L50 is dedicated to specific models, M700V/M70V have no such specification; the syntax differs from Fanuc
    Write workpiece offset G10 L2 / L20 Programmable compensation input (workpiece offset)
    Write tool compensation G10 L10 / L11 / L12 Programmable compensation input (tool compensation)
    Write blank shape G10 L101 Programmable blank-shape input

    according to D310A1AG07 Document, Mitsubishi CNC (#136=4)The pointer of the tool compensation table is as follows:

    variable Purpose Memory Type 1 Memory Type 2
    #145 Radius/diameter pointer 2000 / 10000 2400 / 16000
    #146 Length pointer 2000 / 10000 2000 / 10000
    #147 Length wear pointer — 2200 / 11000
    #149 Wear pointer for radius/diameter — 2600 / 17000

    Slash marks (such as 2000/10000) indicate different memory configuration options. Type 1 is the basic configuration, and Type 2 is the separated H/D configuration. It depends on the parameter settings of the Mitsubishi system (similar to Fanuc’s PM4029 configuration).

    Differences in Fanuc:

  • Fanuc length compensation is usually held in #2000~#2999 or #10000~#10999 (depending on the H/D separation configuration)
  • Mitsubishi’s compensation table storage area is different, But the macro program passes through #145/#146 Indirect access to pointer variables, Therefore, it is only necessary to O9366 Set the correct pointer value in the middle

    • Confirmation method: Execute the following command in MDI mode and check the tool compensation page to confirm the mapping relationship:

    #146 = 2000; Then check the knife repair page, Confirm correspondence H01 position

    4.2.4 Calibration data storage variable migration

    Fanuc defaults to using #530~#533 As a calibration data storage (Through #115 Pointer access). In the Mitsubishi system, #500~#599 Part of the scope is occupied by the system, Suggest migration:

    ; Fanuc default (May not be safe)
    #115 = 530; point to #530~#533
    #530 = Probe Center X
    #531 = Probe Center Y
    #532 = Z Axis distance
    #533 = Diameter calibration value; Mitsubishi's proposed solution
    #115 = 550; point to #550~#553 (Confirm that the scope is free)
    #550 = Probe Center X
    #551 = Probe Center Y
    #552 = Z Axis distance
    #553 = Diameter calibration value

    Mitsubishi public variable occupancy situation:

    Variable Scope Mitsubishi occupancy situation Suggestion
    #500~#509 Backup (recommended) ✅ Can be safely used for calibrating data
    #510~#549 Partial system occupancy ⚠️ To be confirmed
    #550~#599 Interface variables ⚠️ Partially occupied by PMC
    #600~#699 Internal use of the system ❌ avoid using
    #700~#799 Tool life management ⚠️ If enabled, avoid
    #800~#999 User macro area ✅ Can be used for intermediate operations

    Recommended strategy: Prefer to use #800~#999 As an intermediate operational variable, Use #500~#509 (Or confirm availability #550~#553)As a calibration data storage area.

    4.2.5 Macro Program Number and Protected Area Settings

    Fanuc Series Macro (O9000~O9999)The rules for protected areas in Mitsubishi systems are different, Need to manually set protection parameters:

    Program number range Mitsubishi default protection Explanation
    O0000~O0999 — Routine Procedures
    O7000~O7999 ⚠️ Some systems are navigation macros Possible conflict
    O9000~O9999 Parameter setting protection is required Set the protection range on the system parameter page
    O9800~O9899 If installing NAVI MILL, it will occupy Be careful not to conflict with the NAVI MILL macro

    Parameter settings for protected areas:

    The protection range of macro programs needs to be manually set with the start number, end number, and protection mode on the system parameter page (Mainte → Param). Please refer to the Mitsubishi parameter manual for the corresponding version of the machine tool.

    4.3 Migration workflow

    Step 1: Upload macro program to CNC └─ Upload P9376~P9388, O9301~O9392 and O9366 to the user macro area ↓
    Step 2: modify O9366 System Configuration ├─ #101 = 4 (CNC Type → Mitsubishi) ├─ #115 = 550 (Calibration data pointer → safety zone) └─ Setting #145/#146/#149 Compensation table pointer ↓
    Step 3: Set Mitsubishi system parameters ├─ Confirm the skip option is installed on this model (otherwise G31 raises P601) ├─ Parameter #1174 (G31 skip speed) ├─ Parameter #12022 (skipF_spec: override / dry run / speed source without F) ├─ For G37 confirm #8004/#8005/#8006 (measuring speed / deceleration zones) ↓
    Step 4: check G31 Is the function normal └─ Execute G91 G31 Z-20. F5. And manually trigger probe verification ↓
    Step 5: Install calibration reference knife, run P9376 Calibration └─ G65 P9376 H1. (H=Reference knife number) ↓
    Step 6: Run measurement cycle verification └─ G65 P9377 H3. (Measure the tool and write it into the tool patch)

    Explanation: Set the above parameters on the system parameter page (for #8004–#8006, on the “Automatic tool length measurement” screen). Whether the skip function is available is a machine specification (option) matter — confirm the specification before troubleshooting the probe and wiring.

    4.4 Key points for macro transplantation of workpiece measurement

    Workpiece measurement macro (O9301~O9392)Transplanting on Mitsubishi is simpler than using the tool alignment macro:

  • ✅ Use G31 Jump function — Mitsubishi and Fanuc have consistent grammar
  • ✅ Use #5061~#5063 Read trigger coordinates — Same variable number
  • ✅ Use G65 call — The grammar is completely identical
  • ✅ Not dependent on tool compensation table pointer – unless involving automatic write offset

    • The only thing to pay attention to: If the macro contains G10 Instruction to write the offset of the workpiece coordinate system, Mitsubishi’s G10 Grammar is consistent with Fanuc:

    ; FANUC G10 Set workpiece offset (G54)
    G10 L2 P1 X0 Y0 Z0; Mitsubishi G10 Set workpiece offset → Same grammar
    G10 L2 P1 X0 Y0 Z0

    G10 L2 (Offset writing of workpiece)The grammar is completely consistent between Mitsubishi and Fanuc, No need to modify.

    5, VTS Bridge Mitsubishi Complete Configuration

    5.1 Overview

    VTS (Vision Tool Setting) is Marposs’ image-based non-contact tool setting system. On the Mitsubishi system, communication between CNC and VTS systems is achieved through the VTS Bridge Mitsubishi (S609210534) bridge software. This is the core content of the D310JBAG00 document.

    Component Explanation
    Software Name VTS Bridge Mitsubishi
    Document Number D310JBAG00
    software code S609210534
    Knife macro code S609210535 (VTS CNC Macro)
    Communication Library FCSB1224W000 (Mitsubishi CNC Communication Library)
    Compatible Systems M700/M70V/E70, M800/M80, C70, Meldas series

    5.2 System Architecture

    The VTS system consists of three main components connected via Ethernet:

    ┌─────────────────────┐ Ethernet ┌──────────────┐ Ethernet ┌────────────────┐
    │ Mitsubishi CNC │ ◄──────────────► │ VTS Bridge │ ◄──────────────► │ VTS-EU │
    │ (M80/M70 etc.) │ │ (Windows PC) │ │ (processing unit) │
    │ │ │ │ │ │
    │ Communication variables: #149 │ │ config.txt │ │ IP: 192.168.1.8│
    │ (Default, configurable) │ │ Set variable number │ │ port: 22375 │
    └─────────────────────┘ └──────────────┘ └────────────────┘ │ │ ┌─────┴──────┐ │ VTS-SU │ │ (Optical sensor) │ └────────────┘

    workflow:

  • CNC Macro program communicates with variables (default #149)Write instruction data
  • VTS Bridge periodically polls this variable and parses instructions upon reading changes
  • Bridge forwards instructions to VTS-EU (processing unit) via Ethernet
  • VTS-EU controls VTS-SU (optical sensor) to perform image measurement
  • Measurement results passed VTS Bridge Write back #149 variable
  • CNC macro program reads the variable to obtain measurement results

    • 5.3 config. txt configuration file

    The communication variable number of VTS Bridge Mitsubishi is set through theconfig. txtconfiguration file. This file is located in the installation directory of Bridge software.

    config. txt file format (set variable number on line 5):

    ; VTS Bridge Mitsubishi Configuration; Line 1: CNC type = Mitsubishi M80
    Line 2: CNC IP address = 192.168.1.100
    Line 3: Port number = 22375
    Line 4: Polling interval (ms) = 100
    Line 5: Communication variable number ← ★ Key line = 149
    Line 6: Debugging mode (0 = off, 1 = on) = 0

    Variable number configuration rules:

    configuration value Communication variables Explanation
    149 (default) #149 D310JBAG00 default settings
    Other values (such as 150) #150 Customizable, but requires synchronous modification of CNC macros
    scope #100~#999 Public variables that need to be read and written using Mitsubishi macro programs

    ⚠️ Attention: If modified config.txt Variable number in, All modifications must be synchronized with the VTS CNC macro programs (O9700~O9731 etc.) and their variable references.

    5.4 #149 Detailed explanation of communication variables

    #149 is the default communication variable of VTS Bridge Mitsubishi, used for bidirectional data exchange between the CNC and the VTS system.

    Data format:

  • CNC write #149 → Send instructions to VTS (Instruction code + parameter)
  • VTS write #149 → Return the result to CNC (status code + measurement data)

    • Instruction Format Example:

    ; CNC Example of sending measurement instructions
    #149 = 1001; Instruction code: Execute standard measurement
    G04 X1.; Wait VTS Processing (Delay)
    IF [#149 EQ 9999] GOTO 100; check VTS Is it ready
    #100 = #149; Read measurement results

    • Instruction code range: 1000~9999 (defined by the D310A9AG07 macro program)
    • Response format: status code + data (Please refer to the specific code for details VTS Macro program code)
    • Synchronization mechanism: CNC Writing in #149 Wait later VTS Read the results after completing the processing

    Example of Communication Process:

    timeline: ① CNC: #149 = 1001 (Initiate measurement request) ② CNC: G04 X0.5 (wait 500 ms to let VTS process it) ③ VTS: read #149, Parse command ④ VTS: control VTS-EU Perform image measurement ⑤ VTS: #149 = 123.456 (Write back the measurement results) ⑥ CNC: #100 = #149 (Read the result)

    5.5 IP Address configuration

    CNC-side IP address

    The IP address of the Mitsubishi CNC is set through parameter #1926:

    parameter function typical value
    #1926 CNC IP address 192.168.1.100

    Read the current CNC IP address:

  • M800/M80 Series: Diagn page → H/W config → read CNC model → Mainte page → Param → Ethernet param → Read parameters #1926
  • M700/M70V Series: Diagn page → H/W S/W config → H/W config → read CNC model → Mainte page → Param → Ethernet param → Read parameters #1926

    • Set CNC IP address:

    Set the IP address on the CNC network-setting screen (confirm the parameter number and the writing method in the machine’s Connection Manual). System parameters cannot be assigned directly by a macro program or by the Fanuc bit-string style.

    VTS Bridge end configuration

    In the configuration interface of VTS Bridge software:

  • Input CNC IP address (consistent with #1926)
  • Select CNC type (Mitsubishi M80/M70)
  • Set communication port (default 22375)

    • VTS-EU default address

    parameter default value
    IP address 192.168.1.8
    port 22375
    OEM password erm82af6

    5.6 VTS Macro Program List

    The VTS complete macro package (S609210535) includes the following programs, all of which need to be uploaded to the CNC user macro program area:

    Macro Number Name function
    O9700 VTS_PRES Standard measurement cycle (rotating tool)
    O9701 VTS_CALIBRATION Auto-calibration
    O9702 VTS_MOVEG1 Linear motion
    O9703 VTS_MOVETOUCH Measure movement
    O9704 VTS_FASTCHECK Initial check of operating status
    O9706 VTS_FOCUS Focus state acquisition
    O9709 VTS_ROICALC ROI and corner step size calculation
    O9712 VTS_SKIP Jump function
    O9717 VTS_GEOMAN Measurement and calculation
    O9719 VTS_SHUTDOWN VTS shutdown program
    O9721 VTS_INIV Initialize configuration parameters
    O9722 VTS_INTCHECK Integrity detection frame setting
    O9723 VTS_SPINDLEINDEX Spindle indexing
    O9725 VTS_ERR Error status management
    O9727 VTS_SETTOOLINFO Write tool data to VTS EU
    O9728 VTS_GETTOOLINFO Read tool data from VTS EU
    O9730 VTS_SINGLEC_PRES Static mode measurement
    O9731 VTS_SINGLEC_INTCHECK Static mode contour/surface integrity inspection
    O9736 VTS_SINGLEC_CUTTINGEDGE Static mode cutting edge wear inspection
    O9760 VTS_TURN_PRES Tool presetting (tool measurement)
    O9761 VTS_TURN_INTCHECK Tool integrity inspection
    O9768 VTS_RDTOOL Read data from CNC tool table
    O9769 VTS_WRTOOL Write data to CNC tool table

    These macro programs are defined as part of the VTS CNC Macro (S609210535) software package in the D310A9AG07 (VTS Software for Fanuc CNC) manual. Communication is achieved through VTS Bridge Mitsubishi (D310JBAG00) bridging software on the Mitsubishi system. During installation, it is necessary to upload all SPF files toDHCUS.DIRand activate GUD.

    5.7 Summary of Installation Steps

  • Install VTS Bridge software: Install S609210534 on a Windows PC
  • Configure config. txt: Set CNC type, IP address, and communication variable number
  • Configuration CNC Ethernet: Through #1926 setting CNC IP address
  • Upload Macro: Upload VTS CNC Macro (S609210535) to the CNC user macro program area
  • Network Connection Test: Confirm CNC ↔ Bridge PC ↔ VTS-EU network connectivity
  • Run initial configuration: call O9721 (VTS_INIV)Initialize parameters
  • Calibration: run O9701 (VTS_CALIBRATION)Complete system calibration

    • 6, Mitsubishi and Fanuc Variable Compatibility Comparison Table

    6.1 System Variable Comparison

    function Fanuc variable Mitsubishi variable compatibility
    Jump triggers X coordinate #5061 #5061 ✅ exactly the same
    Jump triggers Y coordinate #5062 #5062 ✅ exactly the same
    Jump triggers Z coordinate #5063 #5063 ✅ exactly the same
    Mechanical coordinate X #5021 #5021 ✅ same
    Mechanical coordinate Y #5022 #5022 ✅ same
    Mechanical coordinate Z #5023 #5023 ✅ same
    Absolute coordinate X #5041 #5041 ✅ same
    Absolute coordinate Y #5042 #5042 ✅ same
    Absolute coordinate Z #5043 #5043 ✅ same
    Current tool number #4120 #4120 ✅ Same (possible)
    Current spindle speed #4119 #4119 ✅ possibly the same
    Program pause/wait G04 G04 ✅ same
    Macro call G65/G66 G65/G66 ✅ exactly the same

    6.2 G Code Compatibility Comparison

    G code function FANUC Mitsubishi Attention
    G31 Jump function ✅ ✅ compatible, Mitsubishi Duo G31.1~G31.3
    G31 Pp Skip signal command (multi-step skip 2) — ✅ p=1~255 Different semantics: P is the logical sum of skip signals 1~8
    G31 R0/R1 Deceleration command — ✅ officially required R is not a speed parameter; use F1=~Fn= for post-trigger speed
    G37 Automatic knife length measurement ✅ ✅ Functional compatibility, different parameter mappings
    G65/G66 Macro call ✅ ✅ fully compatible
    G43 Blade length compensation ✅ ✅ Grammatical Concord
    G10 L70 (write parameters) Write system parameters Fanuc uses G10 L50 ✅ M800/M80 use G10 L70 Syntax differs; G10 L50 is model-specific on Mitsubishi
    G10 L2 Write workpiece offset ✅ ✅ compatible
    G10 L10/L12 Writing knife repair ✅ ✅ compatible

    6.3 M code compatibility

    function Fanuc Typical Value Mitsubishi Typical Value Explanation
    Probe turned on M173 M173 (or custom) Usually consistent, PMC mapping needs to be confirmed
    Probe closed M174 M174 (or custom) Usually consistent
    Turn on the knife setting device M173 (or mapping) To be confirmed Different machine tools may be different
    Turn off the knife setting device M174 (or mapping) To be confirmed Different machine tools may be different
    Main axis orientation M19 M19 Usually compatible

    The M code for operating the probe and tool setter needs to be confirmed based on the PMC ladder diagram of the specific machine tool, and it is not recommended to directly use the default values of Fanuc.

    6.4 Comparison of Public Variable Occupancy

    Variable Scope FANUC Mitsubishi Transplantation suggestions
    #500~#509 User available Backup (recommended) ✅ Can be used to calibrate data
    #510~#549 User available Partial system occupancy ⚠️ Confirmation is required on a case by case basis
    #550~#599 User available Interface variables/PMC ⚠️ Possible conflict
    #600~#699 User available system internal ❌ avoid using
    #700~#799 User available Tool life management ⚠️ Enable to avoid
    #800~#999 User available User macro area ✅ Recommended for intermediate operations
    #100~#149 Local variables (non nested) local variable ✅ Only for use within macros

    6.5 Calibration Data Variable Mapping (Recommended Solution)

    variable Purpose Fanuc default Mitsubishi Recommended
    #115 Calibration data pointer 530 550 (or confirm the available area)
    #[#115] Probe center X coordinate #530 #550
    #[#115+1] Probe center Y coordinate #531 #551
    #[#115+2] Z-axis distance/0 #532 #552
    #[#115+3] Diameter calibration value #533 #553

    6.6 Tool Compensation Table Address Comparison

    Compensation type Fanuc Typical Value Mitsubishi Type 1 Mitsubishi Type 2
    Length H #2000~ #2000 / #10000 #2000 / #10000
    Radius/diameter D #2000~ #2000 / #10000 #2400 / #16000
    Length wear and tear #2200~ — #2200 / #11000
    Radius wear #2400~ — #2600 / #17000

    Mitsubishi Type 1 is the basic configuration (H/D merging), and Type 2 is the separated H/D configuration. It depends on the system parameter settings.

    7. O9366 System Configuration (Mitsubishi Recommended Values)

    O9366 is the core configuration file of the MIDA tool-setting macro program, Must be edited before first use. The following are recommended configurations for Mitsubishi systems:

    O9366 (MIDA System Configuration - Mitsubishi version);; === CNC Type ===
    #101 = 4; CNC Type: 4 = Mitsubishi ← ★ Key modifications;; === Tool control ===
    #103 = M___; M code to turn on the tool setter (e.g. M173)
    #104 = M___; M code to turn off the tool setter (e.g. M174)
    #105 = 9; Probe selection M code (9 = do not use);; === Motion parameters ===
    #108 = 3000; Approaching moving speed (mm/min, 0 = G0)
    #109 = 2; Knife repair radius/Diameter pointer mode (1=radius, 2=diameter)
    #110 = 1; Knife repair gauge length pointer mode;; === Calibration and Measurement ===
    #112 = 0; Are there dimensions in the tool table (0 = yes, 1 = no)
    #113 = 500; Maximum measured contact speed (mm/min)
    #114 = 0.02; Measurement tolerance (mm);; === Calibration data pointer ===
    #115 = 550; → #550~#553 (Mitsubishi Safety Zone) ← ★ Key modifications;; === Axis number ===
    #116 = 1; X Axis number
    #117 = 2; Y Axis number
    #118 = 3; Z Axis number;; === Probe parameters ===
    #119 = 1; radius/diameter: 1=radius, 2=diameter
    #120 = ___; Radius/diameter of the measuring tip ball (consistent with #119);; === Function Selection ===
    #126 = 1; Calibration Type: 0=unilateral, 1=Four sides
    #127 = ___; Minimum measuring tool length
    #128 = 1; SKIP Input number (1-4)
    #131 = 0; Wear pointer (0=do not use)
    #132 = 0; Length wear pointer (0=do not use)
    #133 = 1; Diameter measurement direction (1=X+, 2=Y+, 3=X-, 4=Y-)
    #134 = ___; Maximum tool length
    #135 = ___; Maximum tool radius/diameter;
    M30

    O9366 Mitsubishi Chemical Modification Summary:

    modification items Fanuc Value Mitsubishi Value Explanation
    #101 1 4 CNC type → Mitsubishi
    #115 530 550 Calibration data pointer → Mitsubishi safety zone
    #145 2000 (Fanuc) 2000/2400 Radius pointer (system related)
    #146 2000 (Fanuc) 2000 Length pointer (system related)
    Parameter write instruction G10 L50 (N__ R________) G10 L70 (P__ S__ A__ H□__, S = system number) Syntax differs; G10 L50 is model-specific

    8, Common problems and troubleshooting

    8.1 G31 No trigger

    phenomenon Possible reasons Solution
    G31 runs the full distance without stopping The model’s specification does not include the skip function (option not installed), or the SKIP signal is not mapped into the system Check the specification first (without the option G31 raises P601 NO SKIP SPEC), then verify the SKIP input mapping in the ladder
    G31 does not respond to the probe trigger The SKIP signal chain (probe → receiver → PMC input → system) is broken somewhere Measure stage by stage: does the receiver output toggle, does the PMC input point change; mapping and polarity are handled in the ladder
    G31 triggers only occasionally Low probe battery Replace the battery
    G31 triggers but with large error Pre-travel not consistent Use the same F value for calibration and measurement; keep R0/R1 deceleration settings consistent
    G31 slow to trigger / large delay PMC scan time / signal filtering Check the PMC scan time; verify #2102 / #2103 skip time constants

    8.2 G37 not working

    phenomenon Possible reasons Solution
    G37 does not respond Skip option not enabled, or α / R / D / F and #8004–#8006 set incorrectly Check the specification first (P601); then verify position and deceleration zone against G37 α__ R__ D__ F__;
    G37 overtravel alarm (P607) Beyond the measurement allowable range Check the target position, R (deceleration start distance), D (stop range) and #8005 / #8006
    G37 triggers but the tool length is written incorrectly Compensation direction / datum wrong Confirm the G43 direction; compensation takes effect from the next T command (L series) or the next Z-axis / measuring-axis command (M series) after G37

    8.3 MIDA Macro Program Issues

    phenomenon Possible reasons Solution
    Abnormal calibration data #115 The pointed variable is occupied by the system replace #115 Pointer to free area
    Error in writing tool compensation value #145/#146 Pointer value does not correspond to Mitsubishi format Set the correct pointer based on the system type
    Macro programs cannot be edited Macro area is protected but not set correctly Check the protection range settings on the system parameter page
    Variable values are overwritten during execution Used common variables occupied by the system Confirm the free range of variables

    8.4 Common problems after transplantation

    Question Reason Solve
    Writing system parameters from a macro with #parameter = value System parameters are not macro variables and cannot be assigned that way Set them on the parameter page, or follow the model manual for programmable parameter input (G10 L70 on M800/M80)
    variable #500~#599 Abnormal value Mitsubishi’s partial variables are occupied by the system switch to #800~#899 region
    Program number O9xxx cannot be saved Macro protection zone not set up Set the protection range on the system parameter page
    VTS Bridge communication failure IP/variable number mismatch in config. txt Confirm that the CNC IP, config. txt, and variable numbers in the macro are consistent
    The M code of the tool setter is invalid Different mapping of M code in PMC Refer to PMC ladder diagram for confirmation

    8.5 Troubleshooting flowchart

    G31/The probe does not trigger ↓ ┌─── ┌──────────────────────────────┐ │ ① │ Skip option installed on this model? │ │ ├─ No → G31 raises P601 without it │ │ │ → check the spec / add the option │ │ └─ Yes → continue │ │ ↓ │ ┌──────────────────────────────┐ │ ② │ SKIP signal reaching the system (PMC input)?│ │ ├─ No → check receiver output / wiring │ │ │ Yes → continue │ │ └──────────────────────────────┘ │ ↓ │ ┌──────────────────────────────┐ │ ③ │ Probe battery/Receiver status is normal? │ │ ├─ No → Replace the battery/Check the receiver │ │ │ Yes → Continue │ │ └──────────────────────────────┘
    Check direction │ ↓
    top-down │ ┌──────────────────────────────┐ │ ④ │ PMC Ladder diagram SKIP Signal mapping is correct? │ │ ├─ No → Correction PMC Ladder diagram │ │ │ Yes → Check the hardware link: │ │ │ Probe→transmitter→receiver→PMC→system│ │ └──────────────────────────────┘ │ ↓ │ Issue resolved? │ ├─ Yes → End │ └─ No → Contact Marposs Technical Support └─── G37/The knife alignment device is not working ↓ ┌─── ┌──────────────────────────────┐ │ ① │ G37 position / R / D / F set correctly? │ │ ├─ No → reset per G37 α R D F │ │ │ or change #8004–#8006 │ │ └─ Yes → continue │ │ ↓ │ ┌──────────────────────────────┐ │ ② │ Within the measurement range (no P607)? │ │ ├─ No → increase R/D or stroke margin │ │ │ Yes → continue │ │ └──────────────────────────────┘ │ ↓ │ ┌──────────────────────────────┐ │ ③ │ The hardware connection of the tool setter is normal? │ │ ├─ No → Check the wiring/power supply │ │ │ Yes → Continue │ │ └──────────────────────────────┘ │ ↓ │ ┌──────────────────────────────┐ │ ④ │ manual testing: G91 G31 X-20. F5. │ │ ├─ No trigger → check SKIP Signal Link │ │ │ Triggered → check G37 Parameter Configuration │ │ └──────────────────────────────┘ │ ↓ │ Issue resolved? │ ├─ Yes → End │ └─ No → check G43 Blade length compensation direction └─── VTS Bridge communication failure ↓ ┌─── ┌──────────────────────────────┐ │ ① │ CNC IP address (#1926) Correctly configured? │ │ ├─ No → reset #1926 │ │ │ Yes → Continue │ │ └──────────────────────────────┘ │ ↓ │ ┌──────────────────────────────┐ │ ② │ VTS Bridge config.txt Correct? │ │ ├─ No → Correction config.txt │ │ │ Confirm CNCType/IP/Variable number │ │ │ Yes → Continue │ │ └──────────────────────────────┘ │ ↓ │ ┌──────────────────────────────┐ │ ③ │ #149 Communication variables can be read and written? │ │ ├─ No → check CNC↔Bridge communication link │ │ │ Yes → Continue │ │ └──────────────────────────────┘ │ ↓ │ ┌──────────────────────────────┐ │ ④ │ Network connectivity testing (ping)? │ │ ├─ impassable → Check the network cable/IP/port │ │ │ OK → check Bridge Software operating status │ │ └──────────────────────────────┘ │ ↓ │ Issue resolved? │ ├─ Yes → End │ └─ No → Check the firewall/port 22375 └───

    Reference Documentation

    Document Number Name Purpose
    D310JBAG00 VTS Bridge Mitsubishi 🔴 Mitsubishi VTS Image knife — The core source of this article
    S609210534 VTS Bridge Mitsubishi (software package) VTS Bridge software installation
    S609210535 VTS CNC Macro (software package) VTS Macro Program (O9700~O9769)
    FCSB1224W000 Mitsubishi CNC Communication Library Bridge ↔ CNC Communication
    D310A1AG07 Tool Check on Machining Centre (Fanuc) Macro program source for the tool setter (Fanuc Edition)
    D310A2AG16 Part Check on Machining Centre (Fanuc) Macro program source for workpiece measurement (Fanuc Edition)
    D310A9AG07 VTS Software for Fanuc CNC VTS Macro program source (General)
    IB-1501277 / IB-1501290 etc. Mitsubishi M800/M80/E80/C80 Series Programming Manual (L/M series) Official source for skip (G31 / G160), 22.1 automatic tool length measurement (G37) and 15.7 programmable parameter input
    IB-1501279 etc. Mitsubishi M800/M80/E80 Series Alarm/Parameter Manual Official source for program errors P601 / P603 / P607 and parameter numbers

    Attention: This article is based on Marposs D310JBAG00 (VTS Bridge Mitsubishi) Technical Documentation, D310A1AG07 (tool setter) and D310A2AG16 (workpiece measurement) Fanuc-compatibility data, as well as Mitsubishi M800/M80/M700/M70 System feature writing. The parameter numbers mentioned in the text, The variable mapping and configuration methods have been validated on the system, But there may be differences between different firmware versions. in application, Please make sure to use the manual of the corresponding version of the machine tool as the final basis. First-time use MIDA Before macro program, Suggest testing each section and confirming that all parameter mappings are correct.

    FAQ — Selected Q&A

    Q: How does the Marposs VTS imaging tool communicate with the CNC on Mitsubishi systems?
    A: Through VTS Bridge software plus Ethernet communication. The VTS imaging system writes the measurement results into#149variable (Default), CNCSide macro program (O9700~O9769Series)Read the variable to obtain the measurement value. The communication configuration is set in the config. txt file, Including CNC type, IPaddress, Port number 22375 and communication variable number.

    Q: What should I do if the VTS Bridge communication on the Mitsubishi system is not working?
    Answer: Follow the four steps in order to troubleshoot: ① Confirm that the VTS Bridge software is running (Windows taskbar); ② Check the config. txt configuration (CNC type, IP address, port number 22375, variable number 149); ③ Manually read # 149 variable on the CNC side to confirm readability and writing; ④ Ping CNC IP to confirm network connectivity. When the network is open but Bridge is not reading, check if the Windows firewall has allowed port 22375.

    Q: Is the Macroscope serial number used by Marposs VTS on Mitsubishi the same as on Fanuc?
    A: The macro program for the Marposs VTS image alignment tool is the same O9700 on Mitsubishi and Fanuc~O9769Series (23 programs in total), The calling format and parameter interface are completely consistent. The only difference between the two lies in the communication method: Mitsubishi uses VTS BridgeSoftware uses Ethernet bridging (config.txtConfiguration), Fanuc uses Focas2 communication library. If you are asking about a contact type tool setter (P9376/P9388)Or workpiece measurement macro program (O9301~O9392), Mitsubishi does not have an official release package, Need to port and use the Fanuc version.

    Related Reading

  • CNC machine internal measurement configuration scheme: Processing scenario x brand– View all brand recommended schemes by processing scenario
  • MIDA programming: FANUC system tool setter and workpiece measurement macro program
  • Mitsubishi M80 System Probe and Tool Alignment Programming Guide
  • Renishaw vs Marposs vs Blum: Comparison of mainstream CNC probe model parameters

    • Official Appointment:jcetech.cn/contact
    Consultation Hotline: 157-5780-7400/132-2194-1413
    Shipping address: A2-12B17, Yinzhou R&D Park, Ningbo

    Correction notice

    An earlier version of this article cited a set of “Mitsubishi SKIP / G37 system parameters” (#60001 bit 6 / bit 7, #60002 bit 7, #60010, #60011, #60025–#60026) together with a “G10 L50 + N____ R________” writing style. After checking the Mitsubishi official manuals item by item: #60001–#64700 are tool-life-management system variables (the L-series manual prints #60001–#63016) (#60001 = number of registered tools, #60002 = current life value), unrelated to skip / G31 / G37. The official Mitsubishi skip parameters are #1174 / #12022 / #2102 / #2103; the G37 measurement conditions come from the programmed R / D / F or from #8005 / #8006 / #8004; “programmable parameter input” on the M800/M80 is G10 L70, and the G10 L50 in Appendix 3 is noted as dedicated to specific models (the M700V/M70V series has no such specification) — neither is the Fanuc N____ R________ bit-string style. Those incorrect passages have been removed and corrected against the official manuals.