📷 IMAGE AREA — Mitsubishi M70 MONITOR → RESEARCH → TYPE 2 restart, program selection with Top Search and File Set
Suggested alt text: Mitsubishi M70 program restart type 2 top search file set and entering a line number
In this lesson we learn to restart an interrupted program, or one to be re-run from a specific section, with the Program Restart Type 2 method. In Type 1 the control found where the program stopped by itself; in Type 2 the operator selects the program and the line/block to start from. So Type 2 requires more care and program knowledge. The source document explains that Type 2 is used to restart a specific program from a line or block chosen by the user.
1. When is Type 2 used?
Type 2 can generally be used when: Type 1 cannot find where the program stopped, you will start from a specific operation of the program, the operator knows the N number to start from, you do not want to re-run the whole long program, you will skip machined sections and continue from a specific section, or a specific tool operation will be re-run. But Type 2 can create a serious risk if the wrong line is selected; because the commands that should run before the selected line may not have been applied.
2. Difference between Type 1 and Type 2
| Type 1 | Type 2 |
|---|---|
| The control finds where it stopped itself | The operator sets the start point |
| No need to enter a line or block | Line and block info is entered |
| Easier to use | Needs more program knowledge |
| Suitable for normal interruptions | Suitable for starting from a specific point |
| Low risk of selecting the wrong line | High risk of selecting the wrong line |
If Type 1 can be used, Type 1 should generally be preferred first.
3. Checks before Type 2
Before entering the menu: determine why the program stopped, identify the correct program number, determine the N number/block to start from, check the workpiece has not moved, verify the workpiece zeros have not changed, make sure the correct tool will be used, check the tool length/radius offsets, move the tool to a safe Z position, check the spindle and coolant, lower Feed and Rapid Override. The start point must not be selected by guessing.
4. How is the start line determined?
The program below may have stopped around N90; but starting directly from N90 may not be correct. Because before N90, T1 was called, S1500 was given, the spindle was started with M3, G54 was selected, the G43 H1 tool length offset was activated, and the tool was lowered to cutting depth. So in Type 2 the question is not only “where did it stop?” but “where can it safely be restarted from?”
O2000
N10 G21 G17 G90;
N20 G40 G49 G80;
N30 G54;
N40 T1 M6;
N50 S1500 M3;
N60 G0 X0 Y0;
N70 G43 H1 Z50.;
N80 G1 Z-5. F100;
N90 X100. F300;
N100 G0 Z100.;
N110 M5;
N120 M30;5. Entering the Type 2 screen (MONITOR → RESEARCH → TYPE 2)
Per the source document, the sequence is: Step 1 – MONITOR press the MONITOR key. Step 2 – RESEARCH select the RESEARCH soft key. Step 3 – TYPE 2 select TYPE 2 from the submenu. The source shows the entry sequence to Type 2 this way.
6. Finding the program with Top Search
On the Type 2 screen the program to run is selected first; for this the TOP SEARCH key is pressed. Top Search is used to search for the program start from the program list or the relevant device. If the program is in NC memory, check the correct device is MEMORY; if it is on a CF card or another external device, the correct device must be selected separately.
7. Selecting the program with File Set
Per the source document, after Top Search, FILE SET is used. General sequence: open the program list → move onto the program to run with the arrow keys → press FILE SET → press INPUT if needed → the selected program name is automatically written into the relevant field. For example if O2000 is selected, O2000 should appear in the program field on the Type 2 screen.
8. Re-check the program number
After File Set, do not rely only on the program being selected. Check: is the program number correct, is the device the program is on correct, was a main program or a subprogram selected, may another program with a similar number have been selected? For example O2000, O2001, O2010 look similar and can be confused. Doing a restart with the wrong program creates a serious collision risk.
9. Entering the line number and block number
Per the source document, after the program is selected, the line number and block number are entered according to the format on screen, then INPUT is pressed. Two concepts must be distinguished here. N number: the sequence number written in the program (e.g. N80 G1 Z-5. F100; → N80). Block/line number: the position the control counts internally within the program. Since not every line has an N number, the block number may be separate. For example in the sequence N80 ... / X50. / Y30. / N90 ..., X50. and Y30. have no separate N number; the control may distinguish them by an internal block/line number. So the input format on screen must be followed carefully.
10. Starting the search and the Completed message
After the program, line and block info are entered, press INPUT; the control starts searching for the selected position. During this, do not change the program, do not press RESET, do not give CYCLE START, do not change the mode, and wait for the search to complete. When the search completes, a Completed or similar completion message appears on screen; the program must not be started before this message. The source document states that in Type 2, after the line and block info are entered and INPUT is given, the Completed warning must be waited for.
11. Checking the selected start point
After the search completes, examine the program screen: is the cursor on the correct N line, is the selected line really the operation you want to start, was the tool called before this line, were the spindle speed/direction given earlier, was the coolant turned on earlier, was G54–G59 selected earlier, should G43 tool length compensation be active, is G41/G42 cutter compensation ongoing, is a canned cycle open, should it be G90 or G91? If these commands are not rewritten on the selected line, the control may assume them in the correct state; but after a reset or power failure the same modal state may not be preserved.
12. Why do modal commands matter?
Some G codes stay valid on later lines once written. For example in the sequence N10 G90; / N20 G0 X0 Y0; / N30 X100.;, G90 is not rewritten on N30 but is still valid. If you start directly from N30 with Type 2, whether the control is in G90 or G91 must be known. Especially check: G90/G91, G17/G18/G19, G20/G21, G40/G41/G42, G43/G44/G49, G54–G59, G80–G89, G94/G95, G98/G99. A wrong modal state can make the tool move in an unexpected direction or distance.
13. Tool length compensation (G43) check
If the program below is started from N70, G43 H1 was applied earlier (on N50). If you are not sure of the tool length compensation state after a reset, starting from N70 is risky. A safer start point may be N50 G43 H1 Z50.; or an earlier safe preparation block belonging to the operation.
N50 G43 H1 Z50.;
N60 G0 X0 Y0;
N70 G1 Z-5. F100;14. Cutter radius compensation (G41/G42) check
If the program stopped inside G41 or G42, do not start directly from a cutting line. If the program below stopped on N130, starting directly from N130 can be dangerous; because the G41 compensation vector was created in the lead-in move on N110. The safer method is to restart from the safe approach line where compensation begins.
N100 G0 X-10. Y0;
N110 G41 D1 G1 X0. F200;
N120 X100.;
N130 Y50.;
N140 G40 X110.;15. Canned cycle check
In the drilling program example, only the X position is written on N120; for this line to run, the G81 cycle must have been active earlier. If restarted directly from N120 after a reset, G81 may not be active, only the X axis may move, and the expected drilling may not happen. So in programs with canned cycles, you must start from the block where the cycle begins.
N100 G81 Z-20. R2. F150;
N110 X50.;
N120 X100.;
N130 G80;16. Preparing the M, S and T commands
After the Type 2 search completes, the following are checked to suit the operation where the program stopped: T tool number, S spindle speed, M3/M4 spindle direction, M8 coolant and machine-specific M commands. If needed, these are re-run in MDI mode, in MSTB History-like auxiliary screens or with the machine builder’s restart procedure. Since these operations vary by machine, commands must not be given at random.
17. Moving the axis to a safe position and CYCLE START
In Type 2 the machine may move to the selected program position. Before START: move the Z axis to a safe distance from the part, check the X and Y positions, make sure the tool will not hit the vise/clamping element, read the program’s first move, check the G90/G91 state, lower Rapid Override. Even if the program’s start line is correct, if the physical position is not safe a collision can occur. After all checks: verify AUTO/MEMORY mode, turn on SINGLE BLOCK, lower Feed and Rapid Override, close the door and press CYCLE START. Running the first blocks one by one is safer; after each move, the tool path, axis position, active tool, spindle speed and active compensations must be checked.
18. Safe start approach for Type 2
The program must be started from the operation’s preparation section, not from the exact cutting line. In the program below, even if it stopped on N170, a safer restart may be from N100, or from around N110 after a suitable check. This way the tool, zero, speed, spindle, tool length compensation and coolant are prepared again in the correct order. But since the previously machined region will be cut again, the tool path must be examined separately.
N100 T2 M6;
N110 G54 G90;
N120 S2500 M3;
N130 G0 X50. Y20.;
N140 G43 H2 Z50.;
N150 M8;
N160 G1 Z-10. F100;
N170 X100. F300;19. Common mistakes in Type 2
- Selecting the wrong program: re-check the number after File Set.
- Confusing the N number with the block number: follow the input format on screen.
- Starting from the exact cutting line: the preparation commands may not have run.
- Not checking the G90/G91 state: the tool may move an unexpected distance.
- Forgetting G43 tool length compensation: serious Z-axis collision risk.
- Starting inside G41/G42: the cutter compensation path may be miscalculated.
- Starting in the middle of a canned cycle: the drilling cycle may not run.
- Starting without turning on the spindle and coolant: the tool or part may be damaged.
20. When must Type 2 not be used?
Type 2 must not be used when: the start line is not clearly known, the program content is not understood, the CAM program is very long and complex, there are five-axis moves, the workpiece or zero changed, the tool offsets are not verified, the program was changed afterward, the correct version of the external file is not clear, or the operator is not familiar with modal G codes. In these cases the program should be run from the beginning or support obtained from an authorized CNC expert.
21. The method known as Type 3
In the source document there is a separate method that does not appear as Type 3 in the menu but is described by that name. In this method the operator opens the program, moves to the wanted line with the arrow keys, and gives START from that line. Per the source, for this to be usable, parameter number 11031 = 1. General sequence: MONITOR → MODE AUTO → EDIT → move to the wanted line → START. But this method is not a real Program Restart; it only starts the program from the line the cursor is on.
22. Why is Type 3 riskier?
In Type 3-like start-from-a-line, the control may not safely prepare, on the operator’s behalf, the previous M commands, tool calls, spindle speed, G54–G59 selection, tool offsets, canned cycles and the G90/G91 state. So just going to a line and giving START is not safe in most cases. Also, parameter 11031 must not be changed without the machine builder’s approval.
23. Short Type 2 application sequence
(1) Determine the stop reason. (2) Determine the correct program and a safe start line. (3) Check the tool, zero and offsets. (4) Move the Z axis to a safe position. (5) Press MONITOR. (6) Select RESEARCH. (7) Select TYPE 2. (8) Find the program with TOP SEARCH. (9) Select the correct program with FILE SET. (10) Re-check the program number. (11) Enter the line and block info per the format. (12) Press INPUT. (13) Wait for the Completed message. (14) Check the cursor is on the correct line. (15) Check the modal G codes. (16) Prepare the tool, speed, spindle and coolant. (17) Lower Feed and Rapid Override. (18) Turn on SINGLE BLOCK. (19) Give CYCLE START. (20) Watch the first moves carefully.
24. Lesson summary
In this lesson we learned when Type 2 is used, its difference from Type 1, the MONITOR → RESEARCH → TYPE 2 sequence, using Top Search and File Set, entering line and block info, waiting for the Completed message, checking the modal commands before the selected line, the risks in G43/G41/G42 and canned cycles, and the start-from-a-line method known as Type 3.
Next lesson — Lesson 11: Warnings encountered after a Program Restart and how to solve them (restart search not complete, Restart position return incomplete, Program restart machine lock, Rapid/Feed Override zero, wrong tool and spindle state, the machine not moving after restart, safe cancel and starting over).
📷 IMAGE AREA — In Type 2, restarting from a safe preparation block (tool/zero/G43) instead of the cutting line
Suggested alt text: Mitsubishi M70 type 2 restart from a safe preparation block