Mach3 Z rises to zero with G42

[tack1000]

Hi

I have a small bench mill. Been using it fine to learn about the programing side.

I started with drawing everything by the cutter rad bigger to get me started, worked fine.

Now I am getting to grips with things I would like to use the tool cut compensator.

I can get the tool to move left or right of the line fine G41/42, BUT the tool will always rise to ZERO after it starts the offset. WHY?

The only way I have found to get over it is to add Z-5 (say) on every line to keep the cut at Z-5 level.

Sample of the sort of thing I mean.

G0 G49 G40 G17 G80 G50 G90
M6 T0(TOOL DIA. 4)
G64
G21 (mm)
M04 S10
G00 G43 H0 Z1
G0 X-10.35 Y2
G0 Z0
F20.000 G0 Z-6.000
G42
F800 G1 X-8.35 Y0.0000 Z-6
G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6
G1 X9.9818 Y-9.7748 Z-6
G3 X12.2182 Y6.7748 I11.1000 J-1.5000 Z-6
G1 X8.8263 Y7.2331 Z-6
G2 X8.3500 Y7.7782 I8.9000 J7.7782 Z-6
G40
G42
G1 X8.3500 Y21.0000 Z-6
G3 X-8.3500 Y21.0000 I0.0000 J21.0000 Z-6
G40
G42
G1 X-8.3500 Y0.0000 Z-6
G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6
G1 X9.9818 Y-9.9 Z-6
G40

G0 Z6
G0 X0 Y0

M30



Any help.

Thanks

Tack1000

[tack1000]

I have added these pics.

The second one showns the tool path as it would be without the z-6 and the two arc should be straight line cuts but i have to G40 then G42 at the start of each straight line. Is this right.


I hope this helps.

Tack1000

[cnccustom]

Tack ..you need to do a prep move 1st like this example to get cutter comp to work correctly....Do your prep move above the part

G54 G90 G40 G49 G80
G0 X-.35 Y-.5
G43 T1 H1 (.125 em)
G00 Z.1
G41 D1 G03 X-.25 I-.1 F50.
G1 Z-.0625 F2.
G1 Y0 X-.25 F5.
G3 Y1.3 X1. R3.
G3 Y2.4 X6. R8.
G1 Y0
X-.35
G0Z.1
G40
X0Y0
M30

[cnccustom]

Hi

I have a small bench mill. Been using it fine to learn about the programing side.

I started with drawing everything by the cutter rad bigger to get me started, worked fine.

Now I am getting to grips with things I would like to use the tool cut compensator.

I can get the tool to move left or right of the line fine G41/42, BUT the tool will always rise to ZERO after it starts the offset. WHY?

The only way I have found to get over it is to add Z-5 (say) on every line to keep the cut at Z-5 level.

Sample of the sort of thing I mean.

G0 G49 G40 G17 G80 G50 G90
M6 T0(TOOL DIA. 4)
G64
G21 (mm)
M04 S10
G00 G43 H0 Z1
G0 X-10.35 Y2
G0 Z0
F20.000 G0 Z-6.000
G42
F800 G1 X-8.35 Y0.0000 Z-6
G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6
G1 X9.9818 Y-9.7748 Z-6
G3 X12.2182 Y6.7748 I11.1000 J-1.5000 Z-6
G1 X8.8263 Y7.2331 Z-6
G2 X8.3500 Y7.7782 I8.9000 J7.7782 Z-6
G40
G42
G1 X8.3500 Y21.0000 Z-6
G3 X-8.3500 Y21.0000 I0.0000 J21.0000 Z-6
G40
G42
G1 X-8.3500 Y0.0000 Z-6
G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6
G1 X9.9818 Y-9.9 Z-6
G40

G0 Z6
G0 X0 Y0

M30



Any help.

Thanks

Tack1000

be carefull here ..you are rapiding into the part

[cnccustom]

Hi

I have a small bench mill. Been using it fine to learn about the programing side.

I started with drawing everything by the cutter rad bigger to get me started, worked fine.

Now I am getting to grips with things I would like to use the tool cut compensator.

I can get the tool to move left or right of the line fine G41/42, BUT the tool will always rise to ZERO after it starts the offset. WHY?

The only way I have found to get over it is to add Z-5 (say) on every line to keep the cut at Z-5 level.

Sample of the sort of thing I mean.

G0 G49 G40 G17 G80 G50 G90
M6 T0(TOOL DIA. 4)
G64
G21 (mm)
M04 S10
G00 G43 H0 Z1
G0 X-10.35 Y2
G0 Z0
F20.000 G0 Z-6.000
G42
F800 G1 X-8.35 Y0.0000 Z-6
G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6
G1 X9.9818 Y-9.7748 Z-6
G3 X12.2182 Y6.7748 I11.1000 J-1.5000 Z-6
G1 X8.8263 Y7.2331 Z-6
G2 X8.3500 Y7.7782 I8.9000 J7.7782 Z-6
G40
G42
G1 X8.3500 Y21.0000 Z-6
G3 X-8.3500 Y21.0000 I0.0000 J21.0000 Z-6
G40
G42
G1 X-8.3500 Y0.0000 Z-6
G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6
G1 X9.9818 Y-9.9 Z-6
G40

G0 Z6
G0 X0 Y0

M30



Any help.

Thanks

Tack1000

also no radius values here

[tack1000]

Hi

I see the G0 on the Z feed line is a mistake. Its not over the work as it drops down the side then moves onto the job. The L shape is held down with two pre drilled holes not shown, and is a rough shape ready for a clean up cut on the outside.
The 0.0000 on the rad line is cose its on the x0 y0 of the machine. guess thats why it reads G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6 .

Can you see why the z would raise to 0 when it starts the cutand loops out on the straight cuts.

Tack1000

[cnccustom]

Hi

I see the G0 on the Z feed line is a mistake. Its not over the work as it drops down the side then moves onto the job. The L shape is held down with two pre drilled holes not shown, and is a rough shape ready for a clean up cut on the outside.
The 0.0000 on the rad line is cose its on the x0 y0 of the machine. guess thats why it reads G3 X-1.1182 Y-8.2748 I0.0000 J0.0000 Z-6 .

Can you see why the z would raise to 0 when it starts the cutand loops out on the straight cuts.

Tack1000

when I tried to run your program I got errors at those I and J lines saying no radius implemented....

it lifts because your cutter comp moves are not right....look at my example and try to program your part that way......


I will see if I can help you out with it tonight when I get some time

[ger21]

What version of Mach3 are you using? I can't get it to run. Is this in absolute or incremental IJ? Because I get errors both ways. Either zero radius arc with your 0.000 I and J, or a comp error about tool radius.

As custom said, you need to do a lead in move for cmp to work. You can't just turn it off and on like your doing.

Can you post a .dxf of what you're trying to do, and I'll see if I can give you correct code.

G40
G42

will not work.

[tack1000]

Hi

The program will run as shown but I have got around things in a way that I am sure an't nessasary.

I have moved the drawing away from the x0 y0. so its not how I started as you said your program does not like the x0 y0

[tack1000]

Hi

I have run this new g code and the green lin shows the tool path and the z stays at 5.1 depth.

(File arm as drawn 2 )
(Saturday, November 29, 2008)
G90G80G49
G0 Z1.0000
G90.1
S10
G0 Z1.0000
g42
g0 x11 y2
g40
G0 Z-5.1000
g41
G1 X9.1429 Y3.6576
g40
g41
F40.000 G2 X3.6000 Y10.0000 I10.0000 J10.0000 z-5.1
g40
g41
G1 X3.6000 Y31.0000 z-5.1
G2 X16.4000 Y31.0000 I10.0000 J31.0000 z-5.1
G1 X16.4000 Y17.7782 z-5.1
G3 X18.5652 Y15.3007 I18.9000 J17.7782 z-5.1
G1 X21.9571 Y14.8424 z-5.1
G2 X20.2429 Y2.1576 I21.1000 J8.5000 z-5.1
G1 X9.1429 Y3.6576 z-5.1
g1 x6.17 y4.059 z-5.1
g40
M5
G0 Z1.0000
M5
G53 X0 Y0
M5M30


Tack1000

[tack1000]

Hi

Captured this pic too, maybe it helps.

Tack1000

[ger21]

I had to use incremental IJ, but try this. It ramps in during the comp move and ramps out at the end.

G40G80G48
G21 G91.1
M3
G0 Z1.0000
G0 X13.9014 Y0.8332 Z1.0000
G1 X13.9014 Y0.8332 Z0.0000 F10
G41
G1 X11.5242 Y2.6640 Z-5.1000 F40
G3 X9.1429 Y3.6576 Z-5.1000 I-3.0509 J-3.9613
G2 X3.6000 Y10.0000 Z-5.1000 I0.8571 J6.3424
G1 X3.6000 Y31.0000 Z-5.1000
G2 X16.4000 Y31.0000 Z-5.1000 I6.4000 J0.0000
G1 X16.4000 Y17.7782 Z-5.1000
G3 X18.5652 Y15.3007 Z-5.1000 I2.5000 J0.0000
G1 X21.9571 Y14.8424 Z-5.1000
G2 X20.2429 Y2.1576 Z-5.1000 I-0.8571 J-6.3424
G1 X9.1429 Y3.6576 Z-5.1000
G3 X6.5529 Y3.3192 Z-5.1000 I-0.6696 J-4.9550
G40
G1 X4.4638 Y2.4501 Z0.0000
G0 X4.4638 Y2.4501 Z1.0000
G0 X0 Y0
M5
M30