Define the overcut before changing parameters
A DIXI machining center with a GE Fanuc 15 MB control produced an external circular feature marked D 4.8 more than 0.1 mm below the programmed contour. The job used aluminum, a solid-carbide cutter recorded as 6/2, 12000 r/min, and an initial feed of 1200 mm/min. The same contour-smearing behavior appeared during chamfering with a 90-degree cutter.
| Observation | Engineering significance |
|---|---|
| Reducing feed from 1200 to 500 mm/min moved the result toward the target, but it remained undersize. | Contour error is sensitive to feed, supporting a dynamic-following diagnosis. |
| G61 was active on critical radii. | Exact-stop behavior did not eliminate the circular contour error. |
| Changing the postprocessor from radius-defined arcs to I/J center-defined arcs improved contour entries and removed or reduced entry marks. | Arc representation affects the observed entry behavior, but the evidence does not show that it removes the radius error. |
| The feature is recorded as D 4.8. | Confirm whether this means a 4.8 mm diameter or another drawing convention before calculating compensation. |
Separate circular following error from corner rounding
The supported working diagnosis is axis-following error while the machine traverses a circular arc. Each interpolated axis continuously changes velocity and acceleration around the circle. If the feed drives and control cannot follow those commands closely enough, the executed path can depart from the programmed radius.
G61 addresses unwanted blending or rounding at block transitions. It does not directly remove the continuously changing acceleration demand within an arc, which explains why it can improve corner behavior without correcting this small-radius overcut. This remains a diagnosis supported by the feed-response test, not a completed servo measurement.
Servo-amplifier adjustment was suggested as another possible influence, particularly on an older machine. Treat that as a manufacturer-service investigation: the evidence supplies no parameter numbers, target values, or approved adjustment procedure.
Choose the next test from the observed behavior
| Finding | Next decision |
|---|---|
| Error decreases when arc feed decreases | Use a lower feed only on dimension-critical arcs, then measure the result. |
| Entry marks change when arcs switch from radius notation to I/J notation | Retain the verified I/J postprocessor output and inspect every arc center and direction. |
| G61 corrects corners but not the circular feature | Do not treat exact stop as the primary radius-error correction. |
| Error remains after feed reduction | Investigate control look-ahead availability and feed-drive following performance. |
| A fixed, repeatable residual remains | Consider geometric program compensation only after establishing repeatability for the same toolpath and cutting conditions. |
Run a controlled correction procedure
- Preserve the original program and record the commanded feature definition, tool, spindle speed, feed, G61 placement, arc format, and measured error.
- Confirm the drawing interpretation of
D 4.8and the sign of the error. Do not calculate compensation until diameter-versus-radius meaning and measured feature size are unambiguous. - Generate critical arcs with I and J center coordinates because that postprocessor change improved the observed contour entries. Verify the generated centers, endpoints, and clockwise or counterclockwise direction before machining.
- Repeat the critical arc at
500 mm/minwhile holding the remaining conditions constant. The existing test showed improvement at this feed, although the result remained below target. - Check the applicable GE Fanuc documentation for the multiple-block look-ahead function. The evidence associates it with
G05.1, an increase from 15 to 100 previewed blocks, manualB-63324GE/03beginning at page 678, and a requirement that the related G-code commands occupy separate blocks. The reported descriptions ofG05.1andG05.1 P1conflict about which command enables or disables the mode; verify the exact syntax for this control before executing either command. - If feed reduction and a verified look-ahead configuration do not produce an acceptable contour, request the machine manufacturer or qualified service organization to evaluate axis following and servo adjustment. Do not change undocumented amplifier settings from this evidence.
Verify the correction and control compensation risk
Machine the same feature under controlled conditions and measure it after every single-variable change. Compare the original 1200 mm/min result, the 500 mm/min result, and any verified look-ahead result. Also inspect the contour entry because the original evidence separates entry marks from the radius-size error.
A Fanuc manual appendix was reported to contain a radius-error formula using times T1 and T2. Those times, their definitions, and the formula are absent from the evidence, so no numerical error prediction is justified here. Obtain them from the exact manual applicable to the installed control.
Programming a compensating radius was suggested as a cycle-time workaround. Apply that only to a stable, measured residual and validate it on a test part. A compensation derived at one feed or machine condition is not established by the evidence as valid under another condition.
FAQ
Why does G61 not fix a small-radius overcut on a GE Fanuc 15 MB?
G61 addresses block-transition corner behavior, while the supported diagnosis for this arc is following error caused by changing axis acceleration throughout circular motion. The observed radius error therefore remained even with G61 active.
What feed should I test when a GE Fanuc 15 MB cuts the radius undersize?
The documented case improved when feed was reduced from 1200 to 500 mm/min, although the feature remained undersize. Use 500 mm/min as the controlled comparison for this case and measure the result rather than assuming correction.
Should I enable G05.1 look-ahead to improve the contour?
Check manual B-63324GE/03 from page 678 and confirm that the function applies to the installed control. The evidence conflicts on the enable/disable meaning of G05.1 and G05.1 P1, so verify the exact syntax before running either command.