G91 G28 incremental???

[stan z]

N56 G80
N58 M09
N60 M5
N62 G91 G28 Z0.
N64 M01
( OP 1 PART POCKET )
N66 M8
N68 T3 M6 ( 3/8 FLAT ENDMILL STANDARD )
N70 G0 G90 G55 X2.1812 Y-.9275 S4000 M3

Will the N62 line put the machine in incremental mode and keep it there till another code changes it?

[jess fuqua]

Originally Posted by stan z N56 G80 N58 M09 N60 M5 N62 G91 G28 Z0. N64 M01 ( OP 1 PART POCKET ) N66 M8 N68 T3 M6 ( 3/8 FLAT ENDMILL STANDARD ) N70 G0 G90 G55 X2.1812 Y-.9275 S4000 M3 Will the N62 line put the machine in incremental mode and keep it there till another code changes it?

yes, thats why we cancel every thing out in our start up line.
Be careful of G91 its a powerful tool.
I use that same ending line always.

[WayneHill]

The G90 code will change it back

http://www.linuxcnc.org/docs/html/gcode_main.html

[stan z]

I was told that this will do the same thing...send the Z home

G49 G00 Z0


Have you ever tried this ?

[jess fuqua]

G91 G28 Z0
G28 Y0
M30

this is what i like at the end of my prog.


M5
M9
G91 G28 Z0
M01

is at the end of my tool change

[stan z]

Thats how I've been programmig at most places I've worked. My current employer is concerned with the G91,even though the G90 is the next line etc. Hes concerned that the g91 will keep the machine in INC mode with the possibility of crashinng.
They program all parts using sub programs and G52 for work shifts its a high volume production shop .

Although we program our fixtures using absolute mode hes concerned that the G91 will cause aproblem. The G49 G00 Z 0 is used in the "safe" macro M9998.
They also have in this program the following

M9998:
G17 G20 G40 G80 G90 M09 M05
M99

This way they just put this at the beginning and end of the program with no worries.

I come along (been here 2 months) and wanna change there perspective a bit but not make too many waves.

Anyways...just wondering if anyone does it any other way other than the G91 G28 Etc....

[jess fuqua]

I think its cool to program different it will make you a better machinist

[Machineit]

When I learned to program, many many moons ago, I was taught to start and stop each program with a safe line. That way nothing is left modal etc.

The start line is always: G00 G90 G80 G40 G54

This puts you in absolute mode, cancels any modals, and designates the work offset. Unless you machine a lot in other planes, I see no reason to always put a G17 in the line.

The end line is always: G00 G91 G28 Z0. Y0. M05

This returns the spindle to the tool change position, and moves the table to the front (Zero position for Y for part changing) and turns off the spindle.

The line just before the last one is always a simple clearance line;

G00 Z.1 M09

Always works well, for 18 years at least.

You example line, G17 G20 G40 G80 G90 M09 M05, will not work though, as you cannot have more than one M code in a line, but I'm sure you know that.


Cheers---Mike

Originally Posted by stan z Thats how I've been programmig at most places I've worked. My current employer is concerned with the G91,even though the G90 is the next line etc. Hes concerned that the g91 will keep the machine in INC mode with the possibility of crashinng. They program all parts using sub programs and G52 for work shifts its a high volume production shop . Although we program our fixtures using absolute mode hes concerned that the G91 will cause aproblem. The G49 G00 Z 0 is used in the "safe" macro M9998. They also have in this program the following M9998: G17 G20 G40 G80 G90 M09 M05 M99 This way they just put this at the beginning and end of the program with no worries. I come along (been here 2 months) and wanna change there perspective a bit but not make too many waves. Anyways...just wondering if anyone does it any other way other than the G91 G28 Etc....

[Pondo]

Setting 56 will reset the modal G codes at the M30.
You can also use G53 to home an axis
G0 G53 Z0.
The G53 is non-modal, so there is no worries at all like there is with a G91. It is only active in the line it is in. The G53 offset is the machine 0 point.

[Geof]

Originally Posted by stan z I was told that this will do the same thing...send the Z home G49 G00 Z0 Have you ever tried this ?

Yes this will send Z to zero in the active work coordinate system because G49 cancels length offsets.

This is fine if you have 0.0 as your Z work offset because then the Z axis goes to machine zero.

HOWEVER, many people choose to set the Z work zero at a reference point such as the table or the top of a vise. Now if you just cancel the work offset and the Z goes to the work coordinate zero you may get big crunching noises.

As Pondo suggests use G53.

[stan z]

thanks people..I like the G53 best