In this lesson we learn to send a PC-prepared CNC program to the Mitsubishi M70 control and to run large programs directly from the computer. The topic splits in two: transferring the program from the computer to NC memory, and running the program directly from the computer in DNC/TAPE mode. These two methods are not the same.
1. The two methods of transferring a program from a computer
Method 1 – transfer to NC memory: the program is sent from the computer to the CNC’s internal memory; after the operation ends, the program can be run even if the computer connection is broken. Flow: Computer → NC memory → AUTO/MEMORY → CYCLE START. This is the safer and easier method for daily use. Method 2 – running in DNC/TAPE mode: the program is not fully saved to memory; the computer sends it piece by piece / block by block during operation. Flow: Computer → communication link → TAPE/DNC mode → the program runs directly. This method is usually used for large mold and CAM programs that do not fit in NC memory.
2. Connection types that can be used
Between the Mitsubishi M70 and a computer, one of these connections may exist: RS-232 serial, Ethernet, host connection, Computer Link or the builder’s special data-transfer system. Not all connections are on every M70 machine; the connection type depends on the machine builder, the control panel, the installed options and the communication parameters. In the M700 Handbook there are separate connection parameters for serial communication and Computer Link (control code, parity, start code, host settings); these settings make the machine and the computer use the same communication scheme.
3. What is the RS-232 connection?
RS-232 is the serial communication method widely used on older CNC machines; a special serial cable is used between the computer and the machine. For a connection, the settings on both sides must be the same. The basic settings checked are: baud rate, data bit, stop bit, parity, flow control, control codes and the communication port used. For example if the computer is 9600 baud and the CNC is 4800 baud, communication cannot be established.
4. Why do communication settings matter?
The computer and the CNC must speak the same language. If the settings are the same, transfer is possible; if different, the program does not come, corrupt characters appear, the transfer is cut off, a communication alarm appears, or only part of the file comes. The M700 Handbook states that there are parameters for parity and control-code selection for Computer Link communication; these values must be set to the connected device’s characteristics.
| Setting | Computer | CNC |
|---|---|---|
| Baud rate | 9600 | 9600 |
| Data bit | 7 | 7 |
| Stop bit | 2 | 2 |
| Parity | Even | Even |
5. Who should set the communication parameters?
A beginner operator must not change the communication parameters at random; because a previously working connection can break, DNC communication can stop, program transfer can be done incorrectly, and the machine’s other computer connections can be affected. If the connection is being set up for the first time, the settings should be checked by the machine builder, an authorized service or a CNC expert. In this lesson we learn the correct usage sequence rather than changing parameter values.
6. Preparing the computer program
Before sending, the program must be checked: is the correct O number at the start, is M30 at the end, are the lines separated properly, is it text-only, are there special characters/unreadable symbols, may it have been prepared for another control, does it have subprograms? The file extension may be .NC, .TXT or .PRG; the content matters more than the extension.
%
O1500
N10 G21 G17 G90
N20 G40 G49 G80
N30 G54
N40 T1 M6
N50 S2000 M3
N60 G0 X0 Y0
N70 M30
%7. Transferring a program from the computer to NC memory
This is the safest transfer form. CNC side: check the machine is not running → set mode to EDIT → open the PROGRAM/FILE/DATA I/O screen → select the appropriate communication port as the input device → select the INPUT/READ/RECEIVE command → put the CNC into a data-wait state (RECEIVING, INPUT WAIT, DATA INPUT, READ READY may appear). Computer side: open the DNC/communication program → select the correct COM port → check the communication settings → select the file to send → check it is the correct program → prepare the SEND/TRANSMIT command.
8. Sending order
On some systems the CNC is prepared to receive first, then sending is started from the computer. The generally safe order: (1) Set the CNC to EDIT mode. (2) Select INPUT/RECEIVE on the CNC. (3) Check the CNC is waiting for data. (4) Select the correct file on the computer. (5) Give SEND from the computer. (6) Wait for the transfer to complete. On some software and machines the order may differ; the machine builder’s instruction must be taken as the basis.
9. What not to do during transfer
While the program is being sent: do not unplug the RS-232 cable, do not turn off the computer, do not close the DNC program, do not press RESET unnecessarily on the CNC, do not change the mode, do not do another file operation at the same time, do not cut power to the machine. If the connection breaks, the program may come incomplete; an incomplete program must never be run.
10. Checking the program came completely
After the transfer completes: wait for the completed message on the CNC, open the NC memory program list, find the sent O number, open the program, check the first and last line, compare the file size if possible, and look for corrupt characters in the middle. If only the beginning of the program came, the transfer is not complete; especially check that M30 or a program-end mark is present on the last line.
11. Common problems in transfer from a computer
- No data comes: wrong COM port, unsuitable cable, CNC not put into receive mode, different baud rate, or wrong input device selected.
- Corrupt characters come: different baud rate/data bit/parity, or unsuitable file encoding.
- Transfer cuts off: flow control mismatch, weak cable, computer went to sleep, NC memory full, or the communication program stopped.
- Program cannot be found: the file may have come but may not contain a suitable O number inside.
12. What is DNC?
DNC is running the program directly from the computer without fully loading it into CNC memory; it is used for large programs (3D mold programs, very long CAM programs, surface-machining programs that do not fit in NC memory). During DNC the computer and the CNC stay continuously connected.
13. Difference between DNC and normal memory running
| Running from NC memory | DNC running |
|---|---|
| The program is in CNC memory | The program is on the computer |
| A computer is not required | The computer stays connected |
| AUTO/MEMORY mode is used | TAPE/DNC/EXT mode is used |
| Connection loss does not affect it | Running can stop if the connection is lost |
| The program is easily recalled | Reconnection and search may be needed |
14. Preparation before DNC running
Before DNC running: the program is checked on the computer, the communication settings are verified, the cable connection is checked, the computer’s sleep mode is turned off, the screen saver/power saving is disabled, the sending software is kept open, the machine is checked to be at the correct start position, tools and zeros are checked, and whether the program uses subprograms is checked. During DNC, where subprograms are searched can vary by machine setting.
15. Selecting DNC or TAPE mode
The panel may have one of TAPE, DNC, EXT, EXTERNAL or REMOTE modes. General sequence: check no program is running → set the mode switch to TAPE/DNC → open the MONITOR screen → check the external device or host connection is selected → prepare the program on the computer for sending → set SINGLE BLOCK and low override. The mode name may not be the same on every panel.
16. Order to start a DNC program
The start order can vary by machine. A common order: (1) Open the correct program on the computer. (2) Set the CNC to TAPE/DNC mode. (3) Put the CNC screen into a program-wait state. (4) Give SEND/DNC START from the computer. (5) Check data is coming on the CNC. (6) Give CYCLE START on the machine. On some systems CYCLE START first, then sending from the computer, may be needed; so the machine’s previously used procedure must be followed.
17. What not to do while DNC runs
During DNC running: do not unplug the cable, do not turn off the computer, do not close the DNC software, do not put the computer to sleep, do not send another file, do not change the communication port, do not modify the program file, do not remove the USB-serial adapter. If the connection drops, which block the program stopped at must be determined carefully.
18. How to stop the program while DNC runs
Temporary stop: for a normal check, FEED HOLD is used; the program can stay active, and after the issue is fixed and if the connection is sound, it can be resumed with CYCLE START. Canceling the program: when RESET is used, DNC running can be canceled; in that case the sending on the computer must also be stopped, and to run again the program must be prepared from the start or from a safe restart point.
19. What to do if the connection drops
When the connection drops, START is not given again immediately. Sequence: apply FEED HOLD or RESET if needed → check the machine has fully stopped → stop the sending on the computer → check the cable and port connection → re-prepare the communication software → read the alarm on the CNC → determine the block where the program stopped → decide whether to continue from the start or with a Program Restart → check the tool, spindle, coolant and axis positions. After a connection drop, starting the program from a random line is not safe.
20. Important warning about Computer Link B
The M700 Handbook states that the “Computer link B not possible” warning can occur if Cycle Start is given before reset is complete or if Computer Link B is attempted on an unsuitable part system. The recommended actions: wait for the reset to complete, then give Cycle Start, and if needed turn the #8109 HOST LINK setting off and on again. In multi-part systems Computer Link B can only be used on the suitable part system; such setting changes must not be made by the operator at random.
21. Cycle Start block during host communication
While the control communicates with the host computer, Cycle Start may not be accepted in some cases. In that case: wait for the communication to finish, check the communication message on screen, verify the data transfer is complete, and then give Cycle Start. While the computer connection is ongoing, forcing a mode change or repeatedly giving START is not correct.
22. A safe first try for DNC
If the DNC connection is being tried for the first time, do not start with a real part program. A short, motion-limited test program can be used first — it applies a short dwell command without axis motion and ends. The aim: to check that communication has started, that the lines come correctly and that the program end is recognized. Real motion tests must be done under expert supervision.
%
O900
N10 G21 G17 G90
N20 G4 P2.
N30 M30
%23. Short application sequence and lesson summary
Sending the program to NC memory: set the CNC to EDIT mode → open the DATA I/O or FILE screen → select the correct communication device → start INPUT/RECEIVE on the CNC → select the correct COM port on the computer → check the settings → open the correct program → give SEND → wait for the transfer to finish → check the program in NC memory. Running directly with DNC: check the program on the computer → prepare the communication → set the CNC to TAPE/DNC mode → select SINGLE BLOCK and low override → start DNC sending → verify data is coming → give CYCLE START → keep watching the program and the connection. In this lesson we learned the two methods of transferring a program from a computer, the difference between NC memory transfer and DNC, the RS-232 logic, that the settings must be the same, sending to NC memory and direct running with DNC/TAPE, what to do when the connection drops, and the Computer Link/Host warnings.
Next lesson — Lesson 7: Deleting, copying and backing up programs (deleting a single/multiple program in NC memory, why the active program is not deleted, copying a program under a different O number, backing up to USB/CF card and preventing the wrong program from being deleted).