Syntec CNC: Resolving G43 H Offsets, ATC Limits, Servo Alarms

1. Scope and confirmed evidence

This reference consolidates field procedures for Syntec-controlled Excitech routers, including SHM1325 and MAXI-C 1325 SE-T-V examples. Confirmed behaviors: the controller must know workpiece X/Y/Z zero relative to machine zero, the tool position called by the program, and each tool length difference from a reference tool. Tool changes can be commanded in MDI with M6 Tx where x is the tool-bar position; one machine had an empty MDIBLOCK file yet still changed tools correctly from MDI.

Unknowns that must not be guessed: BLU in parameters 2801-2803 and 2843 is not defined in the evidence; the exact tool-table capacity is not confirmed, only that one screen showed 30 MG/T entries with MG 1-6 populated and 7-30 at zero, while another screen listed 12 tools; the meaning of Turret No. 1 and Spindle No. 6 was observed but not established.

2. Establish workpiece zero with a reference tool

1. Choose a reference tool that stays constant in length; avoid a wear item such as a flycutter as the standard. One shop used a worn 5 mm boring bit in a dedicated holder, measured tip-to-collet-face, recorded it in the machine logbook, and rechecked it before use.
2. Flycut the spoilboard first, then vacuum it down. Place material later and expect Z to shift with material, spoilboard state, and vacuum pull-down; the evidence notes parts suck down further after material is loaded and pull-down changes as the spoilboard is milled away.
3. Press F1 Position, F5 Set Workpiece, then MPG mode. Stand facing the spindle; the lower-left spoilboard corner is the workpiece zero example. Jog the reference tool center over that corner.
4. Lower Z with the paper method: slide 20 lb bond copy paper between tool tip and spoilboard, use MPG increment 1 near contact, and stop when the paper begins to drag. The evidence gives paper thickness as 0.004 in = 0.1016 mm.
5. In the External Shift area, clear reference values to all zeros, highlight X, press F1 Latch Machine Coordinate, then repeat for Y and Z. Ignore C on a 3-axis machine because the zero logic calculates off Y1, not the Y2 servo.
6. Paper sign convention from the evidence: compensating by subtracting 0.1016 mm from the indicated Z requires adding 0.1016 mm to the tool compensation number. Treat this as a sign-convention warning and verify with a shallow test cut before production.

3. Measure and enter tool length compensation

Two equivalent manual procedures appear in the evidence. Both make the reference tool the zero standard and store only the length difference for every other tool.

Diameter practice supported by the evidence: enter measured tool diameter rather than relying on diameter wear, and leave tool length wear at zero. If programming is done in CAM such as Enroute, enter actual diameters there and let the CAM compensate the toolpath; wear values are otherwise ignored unless programming at the Syntec controller. When not using a tool sensor, keep the G54 Z value as set; for a new workpiece thickness, reset G54 and the other tools adjust through their offsets.

4. Audit G43 H after every M6 before cutting

The highest-risk defect in the evidence is a program that changes tools but never changes the H offset. A bad sample showed M6 T1, M6 T2, M6 T4, M6 T5, M6 T6, while every following compensation line remained G43 H1. The machine then applies tool 1 length compensation to all tools and can drive longer tools into the spoilboard or bed.

Bad pattern:
N9  M6 T1
N11 G43 H1
N24 M6 T2
N26 G43 H1
N39 M6 T4
N41 G43 H1

Required pattern:
N80  M6T1
N100 G43 H1
N1150 M6T2
N1170 G43 H2

A separate HSM Works sample used the same rule with explicit Z approach: T1 M06 later followed by G43 Z15. H01, then T2 M06 followed by G43 Z15. H02. If H is not changing while the program runs, inspect the live G-code first; the evidence points to CAM output or the post processor, and Type 3 was specifically called out as having this problem. A useful operator check is to print the G-code and check off each M6 T* while loading tools into matching tool-bar positions.

5. ATC Z-positive software-limit fault during tool change

Reported trigger: after gantry work, hard crashes, and limit-switch repair, ATC settings were disturbed and any tool change produced Z-Axis positive software limit exceded. The expanded alarm text was Motion 17 ZAxis Positive software limit exceed Coordinate 40 The 1NcProgramL1 Block end point exceed software limit when MDI M6T1 executed. The tool-holder coordinates in PLC line 200 were checked, safe Y zone was 3078, tool holder at 3203, and changing Z positive limits did not clear the fault.

Decision path: because 1NcProgramL1 Block end point exceed software limit occurs during M6T1, inspect the ATC macro target coordinates and the reference/frame it uses before changing more limits. Verify PLC line 200 holder positions, safe Y zone 3078 versus holder 3203, Z second reference 2803, Z fourth reference 2843, stroke #2 limits 2445/2446, and tool-measurement contact plane 3841 as a set. Do not assume 2405 is the only Z ceiling; the evidence shows changing 2405 alone failed, so the limiting coordinate is likely produced by the tool-change block from a reference, safe zone, or holder position.

6. Limit-switch, homing, and MOT 009 no-motion faults

Crash damage can bend the mechanical limit-switch mounting tabs inside the housing, pulling the switch off center so the dog does not fully depress it. The failure can be intermittent: voltage checks pass while manually pressing the wheel button, then the axis fails again after reassembly. The reported repair was to remove the plastic cover, remove the two screws holding the inner switch mechanism, straighten the tabs, verify switch continuity, reinstall, reset dogs if needed, and stop crashing the machine.

For a dead machine after shipping, the reported alarm set was MOT 009 for X, Y, Z, A, and 6th servo driver alarms, plus PLC 003 X not yet back home, PLC 011 Y not yet back home, and PLC 019 Z not yet back home. The pump ran and AUX1-AUX6 solenoids actuated, but MPG jog and homing produced no servo sound or motion. One machine had been delivered with the 4th-axis drive power connector disconnected; another loose green start-button screw prevented the first MDI run until tightened.

1. Use a meter to check whether current reaches the servo motors while rotating the MPG. If not, inspect the servo drives and the X/Y/Z limit switches for pressed or faulty states.
2. Check the Z upper-limit switch and the X/Y homing-area switches for continuity; a pressed switch was reported to stop the motors responding to instructions or pulses.
3. Check servo-cable continuity after transit, especially if a drive was delivered disconnected.
4. Use MDI isolation only after basic enable faults are cleared: S10000 with spindle start tests controller-to-machine communication; Z100 tests positive Z motion. The evidence explicitly says not to command negative Z during this check.
5. A confirmed minimal MDI recovery was M3 S10000, Y1000, X500, M5, which proved motion after the start-button repair.

7. Absolute-position, storage, and network observations

One controller homed to absolute coordinates X -1269.344, Y -482.480, Z 334.361, A 0.000 at the top-left looking at the Y axis. The evidence does not provide a validated absolute-reset procedure; do not edit parameters 2401-2408 merely to force a displayed position, because those values are software limits and the soft-limit set already has an ATC interaction.

Program transfer facts: one machine had no USB and used floppy; another could not read a USB stick even after reboot, so the second CF card was imaged and copied to a 1 GB CF card to gain program space. Backing up the original CF card was raised as advisable but no procedure is evidenced. Ethernet link LEDs were green at both ends and a network drive was exported, yet the Syntec could not be pinged; the evidence contains no working network configuration, so treat link-up as physical-layer only and keep file transfer on known-working media until addressing is verified.

FAQ