[adidoro]

I don't understand this error, can you help?

Attachment 491236

Is because is in line with G80 or M09? Should I modify my post processor?

O0001
N1 G21 G17 G40 G49 G90 G94
N2 (2.0mm JOBBER DRILL)
N3 T01 M01
N4 S15474 M03
N5 M08
N6 G43 H01
N7 G00 G90 X30. Y28.75
N8 G43 Z25. H01
N9 G83 G98 R3. Z-21. Q2. F628.897
N10 Y10.25
N11 X70.
N12 Y28.75
N13 X110.
N14 Y10.25
N15 X150.
N16 Y28.75
N17 X190.
N18 Y10.25
N19 X230.
N20 Y28.75
N21 X270.
N22 Y10.25
N23 G80 Z25. M09
N24 G53 Z0
N25 M05
N26 X0 Y0
N27 M30

[servtech]

I don't understand this error, can you help?

Attachment 491236

Is because is in line with G80 or M09? Should I modify my post processor?

O0001
N1 G21 G17 G40 G49 G90 G94
N2 (2.0mm JOBBER DRILL)
N3 T01 M01
N4 S15474 M03
N5 M08
N6 G43 H01
N7 G00 G90 X30. Y28.75
N8 G43 Z25. H01
N9 G83 G98 R3. Z-21. Q2. F628.897
N10 Y10.25
N11 X70.
N12 Y28.75
N13 X110.
N14 Y10.25
N15 X150.
N16 Y28.75
N17 X190.
N18 Y10.25
N19 X230.
N20 Y28.75
N21 X270.
N22 Y10.25
N23 G80 Z25. M09
N24 G53 Z0
N25 M05
N26 X0 Y0
N27 M30

You don't appear to have a feedrate programmed, G00 is blockwise I think so won't work in next line.
ie.

Z25. G01 F1000 G43 H01 ?

[adidoro]

You don't appear to have a feedrate programmed, G00 is blockwise I think so won't work in next line.
ie.

Z25. G01 F1000 G43 H01 ?

If I add G00 or G01 before Z in that line it works without F.
Also if I only cut Z25. from that line and paste it on new line underneath, it works without G00, G01 or F.
So I guess I need to modify my post processor.

[adidoro]

Or, it is safe to delete that Z on line N93 completely because at the end of peck drilling it is exactly on that Z height at witch is starting? (N8 G43 Z25. H01)

[adidoro]

To answer myself, yes it is safe.

The question is why PlanetCNC is bothered by that Z there, if it is standard on Fanuc?

We don't need to reinvent the wheel.

[PlanetCNC]

Because NIST RS274/NGC G-code standard clearly says that "It is an error if axis words are programmed when G80 is active".

[mactec54]

I don't understand this error, can you help?

Attachment 491236

Is because is in line with G80 or M09? Should I modify my post processor?

O0001
N1 G21 G17 G40 G49 G90 G94
N2 (2.0mm JOBBER DRILL)
N3 T01 M01
N4 S15474 M03
N5 M08
N6 G43 H01
N7 G00 G90 X30. Y28.75
N8 G43 Z25. H01
N9 G83 G98 R3. Z-21. Q2. F628.897
N10 Y10.25
N11 X70.
N12 Y28.75
N13 X110.
N14 Y10.25
N15 X150.
N16 Y28.75
N17 X190.
N18 Y10.25
N19 X230.
N20 Y28.75
N21 X270.
N22 Y10.25
N23 G80 Z25. M09
N24 G53 Z0
N25 M05
N26 X0 Y0
N27 M30

Did it move to the Z25. position then to the Z0 position, ??? if it did then G98 is moving it to that Z25. position and the G53Z0 is moving it to the Z0 position.

Put the G80 on a line below the Z25. and it should work.

[mactec54]

To answer myself, yes it is safe.

The question is why PlanetCNC is bothered by that Z there, if it is standard on Fanuc?

We don't need to reinvent the wheel.

This is not standard for Fanuc format; this has just been made by a postprocessor that someone has created.

Use Single Block and see if it does move the Z25. if it does then the G80 has not canceled the canned cycle until that line is complete which then it is ok for it to be there, it's not normal to be formatted like this but if it works then there is no problem with how it is formatted.

[adidoro]

Did it move to the Z25. position then to the Z0 position, ??? if it did then G98 is moving it to that Z25. position and the G53Z0 is moving it to the Z0 position.

Put the G80 on a line below the Z25. and it should work.

Yes, it move to Z25, the next Z0 you refer is G53 Z0 so it will be in machine coordinate. (upper Z position)

This is not standard for Fanuc format; this has just been made by a postprocessor that someone has created.

Use Single Block and see if it does move the Z25. if it does then the G80 has not canceled the canned cycle until that line is complete which then it is ok for it to be there, it's not normal to be formatted like this but if it works then there is no problem with how it is formatted.

I understand that. I just deleted the Z move from drilling cycle end and is gone, since the cycle start at Z 25 it will end at that height without that Z after G80. If it would not, I could insert a new line after or drop a G01 in front of Z.
Problem solved.
I was just curious why it is not allowed to have that Z move, and PlanetCNC already answered to that.

[mactec54]

Yes, it move to Z25, the next Z0 you refer is G53 Z0 so it will be in machine coordinate. (upper Z position)

Yes, that is the best thing to do, the Z25. was a redundant any way.

N8 G43 Z25. H01
N9 G83 G98 R3. Z-21. Q2. F628.897


N22 Y10.25 ( After this last move had finished it would move to Z25. because of the ( G98 ) in the first line of the canned cycle.)

[Superman]

.