The program runs, but the Toolpath display holds the physical Y axis at Y0.0, or the control stops with alarm 1802 ILLEGAL STARTUP CONDITION G12.1. These symptoms have different causes. A stationary Y display can be normal because cylindrical interpolation converts planar motion into coordinated X- and C-axis motion; alarm 1802 means the control has not accepted the startup state or plane selection.
Discard the usual quick fixes
Do not remove G12.1 just to make the Toolpath display move in Y. The program may then execute ordinary planar moves, but its X-coordinate interpretation can change between radial and diametral programming. The resulting path is not an equivalent test.
Changing every Y word to C is also not a universal correction. Some control dialects accept planar coordinates and transform the second coordinate internally, while other examples use C directly. Likewise, moving a plain G17 before G12.1 did not clear the problem on one Matrix-controlled machine; that control required G17UH.
| Quick fix | Why it fails | Useful check |
|---|---|---|
Delete G12.1
|
Leaves cylindrical interpolation and can change X-coordinate meaning. | Compare the commanded radius with the actual radial tool position. |
| Expect physical Y motion | The interpolation can generate X/C motion while Y stays at zero. | Watch the commanded and actual C-axis positions. |
Add plain G17
|
Matrix control may require the XC plane suffix. | Check whether G17UH is accepted before G12.1. |
| Copy parameters from another control | The documented values conflict between control families. | Identify the installed control before changing any bit. |
Check before continuing: Confirm whether the symptom is only a stationary Y display or an actual startup alarm.
Identify the control and coordinate convention
Treat T32-compatible, MT-Pro, and Matrix programs as separate dialects. Their plane-selection words, option checks, and radial-programming commands are not interchangeable.
An MT-Pro example required the cylindrical-interpolation option and P16 bit 3 = 1. A different T32-compatible setup was checked with P16 bit 3 = 0, P6 bit 2 = 1, and P10 bit 3 = 1. A Matrix installation showed option 38 CYLINDER, but the working correction was the XC plane command rather than a copied parameter change. This direct conflict is the reason to use the parameter manual for the installed control and software configuration.
Resolve X programming at the same time. The Matrix and MT-Pro samples use G122.1 to put X in radial programming. Do not infer that every control enters the same convention with G12.1 alone. Read the active coordinate convention on the position page or prove it with a non-cutting radial move.
- Record the control family shown by the machine.
- Check whether cylindrical interpolation is installed or enabled.
- Read the current values of the applicable parameter bits without changing them.
- Determine whether
G122.1is required for radial X input on that control.
Check before continuing: Stop if the control family, installed option, or radial/diametral convention remains unknown.
Establish milling mode and zero the C axis
Enter the machine-specific milling state before cylindrical interpolation. The T32-compatible correction added M201 as the milling-mode command, while the supplied Matrix sequence used its own head and mode preparation. Retain the proven preparation commands for the machine; do not transplant M codes between configurations.
Command C to zero before G12.1. Both the T32-compatible and Matrix sequences use G00 C0.0, and the MT-Pro notes explicitly require C at zero before entry. Homing or referencing C may be necessary when the displayed position is not based on a valid reference.
T3535.0
M201
G97 S3000 M203
G0 C0
G12.1Keep the tool clear of the stock during this test. Verify that the commanded C position reaches zero and that the control completes the mode transition without an axis or startup alarm.
Check before continuing: C must be referenced, at commanded zero, and stationary before the control reads G12.1.
Select the interpolation plane before startup
Plane selection tells the control which programmed coordinates belong to the transformed interpolation plane. On the Matrix-controlled Integrex, the sequence that cleared alarm 1802 placed G17UH before G12.1; UH selected XC. A plain G17 had not corrected that installation.
G00 C0.0
G17UH
G12.1
G122.1For a T32-compatible configuration, the working direction was to zero C, enter G12.1, select G17, and program the planar path while the machine generated X/C motion. Because the successful Matrix syntax is control-specific, check the control manual before attempting G19 or adding an unlisted plane suffix.
| Control case | Startup detail | X convention detail |
|---|---|---|
| Matrix |
G00 C0.0, then G17UH, then G12.1
|
G122.1 used for radial X |
| MT-Pro example | C at 0.0 before G12.1
|
G122.1 used for radial X |
| T32-compatible case | Milling mode, C zero, G12.1, and G17
|
Verify on the installed control |
Check before continuing: Run through the entry blocks in single block with the tool clear; the control must accept the plane and G12.1 without alarm 1802.
Prove the transformed path without cutting
A Y value that remains at Y0.0 does not prove that interpolation failed. Watch X and C instead. The control converts the programmed planar path into radial X displacement and spindle-angle motion, so the physical Y slide need not move.
- Raise Z to a clearance position.
- Reduce the program to one line or arc that cannot contact the workholding.
- Run in single block and compare programmed position, commanded X/C position, and actual X/C position.
- Confirm the radial X convention before allowing the tool near the part.
- Test rapid blocks separately because rapid legality inside interpolation depends on the control; the Matrix sample contains
G00moves, while another proposed sequence used feed moves.
Avoid a path through X0 Y0. At the interpolation center, the angular motion needed to maintain a finite Cartesian feed becomes singular; the required C-axis rate tends toward an unbounded value. Offset the path, change the strategy, or break the geometry before it crosses the center.
Check before continuing: The dry run must show the intended X/C direction, radius, and arc sense without approaching the interpolation center.
Exit the mode and verify the complete cycle
Cancel cylindrical interpolation with G13.1 before returning to ordinary positioning. Move the tool clear before cancellation, then perform the machine-specific return, spindle, coolant, and milling-mode exit commands.
- Dry-run the complete entry sequence from a known machine state.
- Verify C reaches zero before the plane and interpolation commands.
- Confirm the control accepts
G12.1and, where required,G122.1. - Confirm the commanded planar path produces the expected X/C motion even if Y remains at zero.
- Move clear, execute
G13.1, and verify subsequent ordinary moves use the expected coordinate convention.
Final check: Repeat the cycle from reset and from the normal preceding operation. A sequence that works only after manual mode changes is not ready for unattended production.
FAQ
Why does Y stay at 0.0 during G12.1 milling?
G12.1 can transform the programmed planar path into coordinated X- and C-axis motion, so the physical Y axis remains at zero. Monitor commanded and actual C movement before declaring the path inactive.
Why does a Mazak Integrex show alarm 1802 with G12.1?
On the Matrix case, G17UH had to precede G12.1 to select the XC plane; plain G17 did not clear 1802 ILLEGAL STARTUP CONDITION G12.1. C also had to be at 0.0 before startup.
Why does G12.1 work on one Integrex control but not another?
T32-compatible, MT-Pro, and Matrix controls use different plane syntax, option handling, and parameter values. Stop if the documented option, parameter map, or radial X convention does not match the installed control; do not change parameter bits by trial. Escalate to official Mazak support with the control family, alarm text, option list, current parameter values, and the shortest program that reproduces the failure.