Re: [CAD_CAM_EDM_DRO] EMC error

Assuming you're programming for a Mill or Router, perhaps you're using
a tool with a diameter of less than 3/16" (0.094" radius). The G41 in
line N21 generates a tool offset, and most systems need at least the
tool radius to accomplish this. The linear move for the G41 in line N14
is 0.3094" (due to X & Y components), but line N21, there is only a Y
component, of 0.0916". It may be doing a 'look-ahead', and seeing
trouble at line N21, and stops you at line N20. By the way, you move
the Z axis to 0.0 in line N13, and never retract it for the G00
moves... BAD practice. Also, why G0 in line N13, and G00 in line N14?
Also, you don't have a Txx M06 line to specify a tool dia. offset. Or
are you using a demo copy of VECTOR? Word has it that some demo
programs only run a few lines, then stop.

RayHex

----------

> From: reed_irion <Reed_Irion@...>
> To: CAD_CAM_EDM_DRO@yahoogroups.com
> Subject: [CAD_CAM_EDM_DRO] EMC error
> Date: Monday, June 03, 2002 8:00 PM
>
> So here is my G-code, it's just a few shapes:
>
> N10 (PROGRAM GENERATED BY VECTOR)
> N11 G90 G40 G20 G17
> N12 G49 G54
> N13 G0 X0.0 F4.0
> N13 G00 X0.517 Y0.1405 Z0.
> N14 G41 G01 X0.2991 Y-0.079
> N15 X0. Y0.
> N16 X-0.0811 Y0.2985
> N17 X0.1368 Y0.518
> N18 X0.4359 Y0.439
> N19 G40 X0.517 Y0.1405
> N20 G00 X0.4705 Y0.4084
> N21 G41 G01 Y-0.0916
> N22 X0.9705
> N23 Y0.4084
> N24 G40 X0.4705
> N25 G00 X0.6863 Y-0.3279
> N26 G41 G01 X1.0588 Y0.2195
> N27 X1.5384 Y-0.2658
> N28 G40 X0.6863 Y-0.3279
> N29 G00 X1.7418 Y0.2195
> N30 G03 X1.7418 Y0.2195 I-0.3162 J0.
> N31 M30
>
>
> When it gets to line N20 I get Error:axis 1 following error.
>
> I generated the code in vectorCAM. What gives ?
>