Mitsubishi M70/M700 Program Transfer and Running Programs from External Memory

📷 IMAGE AREA — M70/M700 EDIT → I/O screen: A/B device selection (USB / CF Card / MEMORY) and A→B TRANSFER
Recommended size: 1200×630 px (16:9, hero) · WebP/JPG · <150 KB · filename: mitsubishi-m70-io-program-transfer.webp · alt: Mitsubishi M70 EDIT I/O screen USB CF card MEMORY program transfer A B

On the Mitsubishi M70 control, machining programs are not held only in the CNC’s internal memory. Depending on the machine hardware, the options enabled by the manufacturer and the connected peripherals, these sources can be used: CNC internal memory (MEMORY), USB memory, CF card / Memory Card, RS-232C serial connection, computer connection, Data Server or network connection, and on M700 models extra storage areas such as HD, FD and DS. Not all of these methods do the same job; some are used only to copy the program into CNC memory, while others allow the program to be run directly from an external source. The menus and available devices on the M70 and M700 screens vary by the manufacturer’s PLC layout and the purchased options. The Mitsubishi manual also states that not all functions may be present on every machine and that the machine tool builder’s manual takes priority.

1. First, separate the basic concepts

Program transfer is copying a machining file from one source to another destination (USB → CNC MEMORY, CF Card → CNC MEMORY, CNC MEMORY → CF Card, Computer ↔ CNC MEMORY). After the transfer, the program is usually run from the CNC’s internal memory. In direct running from an external source, for long die programs the file is not fully loaded into CNC memory; the lines are read from the external source and processed. This can appear under the names Tape mode, DNC operation, Drip feed, Computer Link, Host operation, Memory Card operation or Data Server operation. However, the direct-run feature over USB, CF card or serial is not enabled on every M70 machine. In running from CNC memory, the program is first transferred to the MEMORY area, then selected and run in AUTO mode; this is the most common and most reliable method.

2. Memory and device names used on the M70

On M70/M700 screens you may encounter terms such as MEMORY (internal memory), MEMORY CARD (CF card), USB, SERIAL / RS-232C, DS/Data Server, HD and FD (mostly M700). M70 usage notes state that the I/O screen is used for wired connection and for card-to-machine and machine-to-card transfer operations.

3. Running the program in CNC internal memory

This method is used when the program has already been loaded into the MEMORY area.

1. Put the machine in AUTO mode.
2. Press the MONITOR key.
3. Enter SEARCH from the sub-menu.
4. Select MEMORY as the source.
5. Find the file to run in the program list and move onto it.
6. Press INPUT and check that the program opens correctly on the monitor screen.
7. Check the tool, work zero, offsets and the start line.
8. After the required safety checks, press CYCLE START.

The M70 usage document explains that a registered program can be opened from MEMORY or MEMORY CARD, and that the MONITOR → SEARCH → MEMORY path can be used for AUTO operation.

4. Transferring a program from USB memory to CNC memory

The safest way to load a program from USB is to first copy it into the CNC’s MEMORY area. The program on the USB stick should be in plain text format, use a program structure the control accepts, contain a valid program number, have no special characters the control does not recognize in the file name, and have line endings in a suitable format. According to the Mitsubishi programming manual, programs created on the NC edit screen can be stored in CR/LF format; files created with RS-232C or other external devices may have only LF line endings. Therefore format differences can appear in files created on a computer.

1. Insert the USB stick into the USB port on the control panel.
2. Put the machine in EDIT mode and enter the EDIT page.
3. Open the I/O option from the sub-menu.
4. If there are A and B device areas: select USB for side A, MEMORY for side B.
5. Open the USB file list, move onto the program to transfer and select the file with INPUT.
6. If needed, verify the file name in the FILE SETTING area.
7. Press A → B TRANSFER; if a “Continue transfer?” prompt appears, confirm.
8. Wait for “TRANSFER COMPLETE” and check from the MEMORY list that the file arrived.

Source notes give the order EDIT → I/O → A/B device selection → program selection → FILE SETTING → A-to-B TRANSFER for transferring from USB or flash memory to MEMORY. If the same program number exists in CNC memory, an overwrite confirmation may appear, the transfer may be rejected, the file may be saved under a different name, or the old program may need to be deleted first. Always back up the old program before deleting it.

5. Backing up a program from CNC memory to USB

The operation is the reverse of the previous one: insert the USB stick, open EDIT → I/O, select MEMORY for side A and USB for side B, choose the program to back up from the MEMORY list, check the FILE SETTING area and use the A → B TRANSFER command. When done, check the USB contents. If several programs are to be backed up, the machine may have a batch selection function; if there is no batch transfer, the programs must be selected one by one.

6. Running a program directly from USB memory

There is an important distinction here: the USB appearing on the I/O screen does not mean machining can be done directly from USB. On some M70 machines USB is used only to transfer files. For direct automatic operation, one of the following may be required: the USB appearing as a run device on the AUTO/SEARCH screen, the external-device operation option being enabled, the manufacturer’s PLC program supporting USB run mode, and the file size and folder structure of the program being supported.

If direct USB running is available, the general procedure is: insert the USB stick, go to AUTO mode, enter MONITOR → SEARCH, select USB from the device list, select the program, make it active with INPUT, verify the run source is USB, check the program first with SINGLE BLOCK and a low feed percentage, then give CYCLE START. If USB does not appear in the AUTO/SEARCH device list, the program must first be transferred to MEMORY. In direct running, removing the USB, poor contact, slow memory, a file-read error, a power cut, called subprograms not being found, or the file name/folder path not being supported can stop machining. Therefore, for long jobs use industrial-grade memory and never remove the USB during operation.

7. Transferring a program from a CF card to CNC memory

On M70 systems the term “Memory Card” usually means the CF card or the memory card the panel recognizes. From CF card to MEMORY: insert a suitable CF card into the slot, open EDIT → I/O, select MEMORY CARD for side A and MEMORY for side B, select the program to transfer from the card’s program list with INPUT, check the FILE SETTING area, give the A → B TRANSFER command, accept the confirmation and wait for “TRANSFER COMPLETE”. From CNC MEMORY to CF card: in EDIT → I/O select MEMORY for side A and MEMORY CARD for side B, select the program and transfer from A to B. Do not remove the card before the transfer finishes.

8. Running a program directly from a CF card

One of the external-run methods the M70 supports can be running from the Memory Card; this feature can be used for long programs. General order: insert the CF card, go to AUTO mode, enter MONITOR → SEARCH, select MEMORY CARD as the source, move onto the program to run, press INPUT, check the program path and number, give CYCLE START. The M70 usage document states that MEMORY or MEMORY CARD can be selected on the program-open screen and that memory and the memory card are among the supported run sources during automatic operation.

If a subprogram is used: if the main program runs from the card and contains M98 or M198, the device where the subprogram is searched must be defined correctly. In particular M198 can be used to call a subprogram on an external device, but its availability depends on the control option and the manufacturer settings. If the main program is on the card and the subprogram is in MEMORY, or vice versa, a program-call error can occur.

9. Formatting the CF card

Source notes give the M70 card formatting operation as: press MAINTE, open the INPUT/OUTPUT screen, if it is not visible in the sub-menu advance with the right arrow key, find the MEMORY CARD FORMAT option, type Y and press INPUT. This operation can erase all files on the card; before formatting, copy the data on the card to a computer. If the control does not recognize the card, check: the card capacity may not be supported, the file system may be unsuitable, a CF–SD adapter may be incompatible, the card slot may be faulty, the card may be write-protected, or the card may have been removed incorrectly while the machine was running.

10. Backing up SRAM and system to a CF card

A machining program backup and an SRAM backup are not the same thing. Depending on the machine, an SRAM backup can contain parameters, tool data, workpiece coordinates, macro variables, PLC data, programs, tool magazine information and system settings. General SRAM backup path: insert the CF card, press MAINTE, advance with the right arrow in the sub-menu, find the SRAM BACKUP option, select the data groups to back up, choose MEMORY CARD as the target, start the A-to-B transfer, wait for the completion message and remove the card in a controlled way. The #8919 parameter shows that the automatic backup target can be the Memory Card for the M70, while for the M700 the options DS, HD or Memory Card can exist.

📷 IMAGE AREA — RS-232C connection diagram (9-pin PC ↔ 25-pin CNC) and serial communication settings (baud, parity, stop bit)
Recommended size: 1000×750 px (4:3, in-content) · WebP/JPG · <150 KB · filename: mitsubishi-m70-rs232c-connection.webp · alt: Mitsubishi M70 RS-232C serial connection diagram 9 pin 25 pin baud parity

11. Transferring a program from a computer to the CNC via RS-232C

A connection referred to as “RS-832” is most likely RS-232C serial communication; RS-832 is not a standard program-transfer connection for this control. RS-232C can be used for three purposes: sending a program from the computer to CNC MEMORY, receiving a program from CNC MEMORY to the computer, and running a program directly from the computer via the DNC/drip-feed method.

Cable connection: in a typical diagram the computer side is a 9-pin female and the CNC side a 25-pin male. But in practice, whether the TX and RX connections are straight or crossed can depend on the computer adapter used and the serial-port structure on the machine side. Therefore, before making a cable just from the pin numbers, check the existing machine cable or the manufacturer’s wiring diagram.

Serial communication settings must be identical on the computer and the CNC: baud rate, data bits, stop bits, parity, flow control, ISO/EIA code selection, EOB/line-end format, device number, I/O channel and serial-port selection. A commonly used example setting: baud 9600, data bits 7 or 8, parity Even, stop bits 2, flow control RTS/CTS or XON/XOFF, code ISO. This is only an example; the computer software must not be set to these values without seeing the values present on the machine.

Sending from the computer to CNC MEMORY: connect the serial cable; on the CNC select SERIAL / RS-232C as the input device and MEMORY as the destination in EDIT → I/O; prepare the program-receive function, enter the program number if needed and put the CNC in receive-wait state. On the computer, open the serial software, select the correct COM port, set baud/parity/stop bit and flow control the same as the CNC, select the NC program and start SEND while the CNC is in receive state. Do not interfere with the cable or program until the transfer completes. At the end, check the file in the program list, the start/end characters, the program number, that lines have not merged, and that the program end contains M30 and the required end characters.

12. Receiving a program from the CNC to the computer via RS-232C

On the computer, select the correct COM port, match the communication settings to the CNC and put the software in RECEIVE state. On the CNC, enter EDIT → I/O, select MEMORY for side A and SERIAL / RS-232C for side B, select the program to send and start the OUTPUT or TRANSFER command. Check the data flow on the computer; when done, save the file and check the first/last lines of the program.

13. Running a program directly from a computer via RS-232C (DNC / drip feed)

This method is used when long programs do not fit in CNC memory. The computer sends the program line by line to the CNC; the CNC takes the received lines into a buffer and processes them. Required conditions: the machine must have a Tape/DNC operation mode, the RS-232C port must be enabled for DNC, the communication settings must be identical, the DNC software must support flow control, the machine PLC must support serial automatic operation, and the program lines must be sent at a speed the control can read.

General procedure: connect the serial cable, open the DNC software on the computer, set the communication values, select the program, put the machine in TAPE/DNC/SERIAL AUTO or the manufacturer’s equivalent mode, put the CNC in data-wait state, give SEND/DNC START on the computer, wait for data to reach the CNC buffer and give CYCLE START. The computer, cable and software must stay on throughout machining. Because the program is not fully copied to the CNC, if the computer or DNC software closes, the USB–serial converter disconnects, the cable loses contact, or Windows goes to sleep, the machine can stop the program.

14. Computer Link B and Host Link setting (#8109)

In the M700 Handbook, the #8109 HOST LINK parameter makes this distinction: #8109 = 0 normal RS-232C communication enabled; #8109 = 1 Computer Link B enabled, normal RS-232C communication disabled. So when Computer Link B is turned on, the classic RS-232C transfer can become disabled. The Handbook also states that during a Computer Link B operation, if Cycle Start is given before reset completes, or if operation is attempted from the second or later system in a multi-part system, the alarm M01 Computer Link B not possible 0123 can occur; as a solution it recommends completing the reset and, if needed, setting #8109 HOST LINK to 0 and back to 1. This parameter must not be changed without authorization; if HOST LINK is turned on while serial communication is running, the existing RS-232C transfer can be cut off.

15. Transferring a program from a computer over Ethernet or network

Depending on the M70 control hardware and the manufacturer’s installation, program transfer over Ethernet can be possible. Usable structures: NC Explorer, NCnet Lite, NC Link, SDNC, Data Server, FTP-like file transfer and manufacturer-specific DNC software. However, the existence of this software does not mean every M70 machine is directly compatible. Installation usually requires the CNC IP address, computer IP address, subnet mask, port number, CNC/host name, user authority, communication protocol, PLC/network option and Windows firewall permission.

Transfer from computer to MEMORY: put the CNC and computer in the same network group, verify the CNC IP address is reachable, open the compatible Mitsubishi transfer software, select M70 or the supported series as the control model, test the connection, read the CNC program list, select the program on the computer, send it to the CNC MEMORY area and verify from the CNC screen that it arrived. Direct running over the network: if a Data Server or Computer Link configuration exists, long programs can be run from a networked computer or server; in this method the program’s network path must be fixed, the computer must not sleep, the network must be uninterrupted, the antivirus/firewall must not cut the connection, and the file must not be changed during operation. On M700 systems DS and HD run/storage areas can be more common, while on the M70 the hardware and options can be more limited; the M700 Handbook separates the automatic backup targets as DS, HD and Memory Card for the M700 and only Memory Card for the M70.

16. Which method should be chosen for large programs?

If the program fits in CNC memory, the safest method is USB or CF Card → MEMORY → AUTO run. Advantages: the program runs even if the external device disconnects, no serial communication error occurs, the computer need not stay on, and Program Restart can be applied more safely. If the program does not fit in CNC memory, the usual order of preference is: direct running from CF card, running over Data Server or Ethernet, RS-232C DNC/drip feed, direct running from USB (only if the machine supports it). For long die programs, the CF card or network-based method can be faster and more stable than RS-232C; but for this the machine must support automatic operation from an external device.

17. What to check if a program will not transfer

• File not visible: the extension may be unsupported, the file name too long, Turkish characters present, the file inside a folder, the USB/card format unsuitable, or the device capacity too high.
• Program not accepted into MEMORY: the same program number exists, the number is invalid, MEMORY is full, write protection is on, EDIT LOCK is active, or the EDIT-I/O menu is hidden due to #8923. The #8923 parameter can hide the EDIT input/output menu; however the input/output menu on the maintenance screen still works.
• No data over RS-232C: wrong COM port, different baud rate, mismatched parity/stop bit, wrong TX/RX connection, unsuitable RTS/CTS jumpers, #8109 HOST LINK having disabled normal RS-232C, the CNC not put in receive mode, or the computer sending before the CNC is ready.
• Lines arrive corrupted: CR/LF vs LF mismatch, wrong ISO/EIA selection, wrong parity, Turkish/non-control characters present, or the program saved incorrectly in Windows text format.
• Program will not run directly: no external-run option, wrong AUTO mode, the TAPE/DNC input not opened by the PLC, the program open only for editing from the device, subprograms on another device, or an EOR/program-end error during transfer.

18. Program end and file format

The basic structure of a machining program can be as follows:

%
O1001
G90 G54 G17
...
M30
%

On some M70 systems the file name and the program number can differ. The program number should usually be on an independent line at the start of the program; the Mitsubishi programming manual requires the program number to be used as an independent line in the first part of the program. If the program end is not written correctly, P36 Program End Error can appear; the Handbook cites the absence of a proper M02, M30 or M99 for a subprogram despite an EOR being read in tape or memory mode as a cause of the error.

19. Checking a transferred program safely

After a program is transferred it must not be run at full speed directly. In order: check the program number, the first lines, the M30/M99 at the last line, the G54–G59 zero used, the tool numbers, the tool length/diameter offsets, the subprogram calls and the absolute/incremental mode. On the first run use SINGLE BLOCK, reduce the rapid and feed override, and if possible use the graphic or program-check function first. The Mitsubishi manual recommends checking the program, tool offsets and workpiece offsets with a dry run before actual machining.

20. Restarting if an external program is interrupted

If a long program running from USB, CF card, MEMORY or another source stops, Program Restart can be used; but the program must be accessible and the same file unchanged. In the M70/M700 Program Restart function, TYPE 1 helps the control automatically find where it stopped, TYPE 2 lets you start from a specific point by entering program/line/block information, and the method referred to as TYPE 3 lets the user run from the desired line. During restart, the tool, speed, M codes and axis positions must be checked; since the machine can move automatically to the restart position when START is given, the Z axis and other axes must be in a safe position.

21. Which function is on the M70, which on the M700?

Commonly expected on the M70: MEMORY program running, program transfer from USB, Memory Card/CF card use, program transfer via RS-232C, DNC if the option exists, opening a program from the Memory Card, backup to the Memory Card, SRAM backup, and Ethernet/computer connection on some models. Additionally on the M700: HD, FD, DS/Data Server, extended network functions, more comprehensive storage and large-program editing on external storage. The #8921 parameter defines normal or mass-editing selection for large programs on HD, FD and Memory Card. However, there can be hardware and menu differences between M70 Type A, M70 Type B and M700.

22. Recommended usage layout

• Daily small/medium programs: Computer → USB → CNC MEMORY → AUTO
• Long die programs: Computer → CF Card → run from Memory Card, or Computer → Ethernet/Data Server → direct running
• Old/network-less machines: Computer → RS-232C → CNC MEMORY (if very large, RS-232C DNC → direct running)
• Setup and program backup: CNC SRAM/MEMORY → CF Card → Computer → second backup disk

Conclusion

On the Mitsubishi M70 there is no single method for program transfer; the best method should be chosen according to the program size and the machine hardware. USB and CF card are the easiest ways to copy a program into MEMORY. The CF card can be used to run long programs directly if the machine allows. RS-232C can be used for sending, receiving and DNC running. Ethernet and Data Server, with the right option, provide fast transfer and long-program running. CNC MEMORY is the most reliable run source for small and medium programs. Options such as HD and DS found on the M700 are not present on every M70 control.

⚠️ Mentor CNC disclaimer: This content is prepared for training and general information purposes. Mentor CNC is not responsible for wrong connections, faulty parameter changes, data loss, incorrect program operation, machine collision, hardware failure or any work accidents that may occur. Even with the same Mitsubishi M70 control panel, serial communication parameters, USB and CF card support, DNC mode, Ethernet connection, PLC layout, menu names and active options can vary from manufacturer to manufacturer. Before changing a parameter, making a cable or running a program directly from an external source, consult the machine manufacturer’s manual and get help from qualified service personnel.

Related content: for serial communication on FANUC controls see our RS-232 Program Transfer on CNC Machines: DB9–DB25 Cable Pinout and CNCCOM Settings guide.