[extanker59]

mactec54 you threw me for a loop. I read what you first wrote and began feverishly looking for documentation. I thought I was missing some setting.
Then you edited.
Oh well. I learn til I die (hopefully).

[HayreAss]

Many of us prefer more granular control.
I certainly don’t want to wait for a tool change to stop my spindle, nor do I want the spindle and coolant to come on with one.

I could see occasions where that could be handy.
But far more often it would piss me off.

[mactec54]

Many of us prefer more granular control.
I certainly don’t want to wait for a tool change to stop my spindle, nor do I want the spindle and coolant to come on with one.

I could see occasions where that could be handy.
But far more often it would piss me off.

It' turns the spindle 0ff before the Tool change and is doing it whether you use it or not, coolant is good to turn 0ff before the spindle though, with what you are doing with having Stops in your program, you would have to do a M5 and M9 anyway

When you run a program without Stops in it, it runs very smooth without any problems

[HayreAss]

Yeah. I was responding to your pre edited post.
About M6 turning in the spindle and coolant.

[metalmayhem]

The M6 turns off the Spindle and the Coolant before a Tool Change so other code for this is not needed as programed by Haas

I was referring to this statement

The M6 will turn the spindle on with your Haas control so it does not matter where the M3 is or placed as it is redundant

,

A guy can replace a 53 or g28 move , and a spindle stop by using m6 but why thats just sloppy . The other codes aren't redundant they are commonly used in properly formatted programs , which is the way most post processors post code

[HayreAss]

So, if your machine is set to have M6 turn on the spindle, I imagine you put your speed on that line as well?
What happens if you don’t?
Does it come on at the last speed like the spindle forward button does?
That could be catastrophic.
I’m picturing a face mill or probe firing up at 15k…
I’m really ok with having to enter SxxxM3.

[mactec54]

I was referring to this statement

Sorry, that is incorrect, it should have been M6 only turns the spindle 0FF not 0N that would be an imposable task for it to turn it 0n

[mactec54]

I was referring to this statement




A guy can replace a 53 or g28 move , and a spindle stop by using m6 but why thats just sloppy . The other codes aren't redundant they are commonly used in properly formatted programs , which is the way most post processors post code

A Post Processor is whatever flavor you want it to be, that is adjustable for the customer needs or how the user wants the G-Code Program to work for them, that is why there are so many different Post Processors that different Cam software suppliers have most are what someone has had custom to their needs, there is no real generic Post Processors, what most do is pick (1) and adjust it to suit your needs.

[mactec54]

So, if your machine is set to have M6 turn on the spindle, I imagine you put your speed on that line as well?
What happens if you don’t?
Does it come on at the last speed like the spindle forward button does?
That could be catastrophic.
I’m picturing a face mill or probe firing up at 15k…
I’m really ok with having to enter SxxxM3.

No that is incorrect I posted that incorrectly the M6 only turns the Spindle 0FF It should have read that is turns the Spindle / Coolant 0FF

[metalmayhem]

you also said it made m3 redundant


out of the box most post processors tend to follow the same format , except the odd machine company that run outside the norm . Custom posts are a common thing and I have some myself but they still fall withing a normal format

you can make things up as you go along and have it work for you , but it doesn't mean everyone needs to follow your way of thinking
this is straight out of the haas manual which is the format most follow , you'll notice g54 is not on a line of it's own , and an m6 isn't being used to end a tool operation
personally I find g49 unnecessary but at the same time some people use it which doesn't hurt anything . And I always have my g54 on the fist move line vs having it along with the safety codes(like most people) . You can also put a g54 on a line of it's own and it's ok but it's not a must

%
O40001 (Basic program) ;
(G54 X0 Y0 is top right corner of part) ;
(Z0 is on top of the part) ;
(T1 is a 1/2" end mill) ;
(BEGIN PREPARATION BLOCKS) ;
T1 M06 (Select tool 1) ;
G00 G90 G17 G40 G49 G54 (Safe startup) ;
X0 Y0 (Rapid to 1st position) ;
S1000 M03 (Spindle on CW) ;
G43 H01 Z0.1 (Tool offset 1 on) ;
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G01 F20. Z-0.1 (Feed to cutting depth) ;
X-4. Y-4. (linear motion) ;
(BEGIN COMPLETION BLOCKS) ;
G00 Z0.1 M09 (Rapid retract, Coolant off) ;
G53 G49 Z0 M05 (Z home, Spindle off) ;
G53 Y0 (Y home) ;
M30 (End program) ;
%

[mactec54]

you also said it made m3 redundant


out of the box most post processors tend to follow the same format , except the odd machine company that run outside the norm . Custom posts are a common thing and I have some myself but they still fall withing a normal format

you can make things up as you go along and have it work for you , but it doesn't mean everyone needs to follow your way of thinking
this is straight out of the haas manual which is the format most follow , you'll notice g54 is not on a line of it's own , and an m6 isn't being used to end a tool operation
personally I find g49 unnecessary but at the same time some people use it which doesn't hurt anything . And I always have my g54 on the fist move line vs having it along with the safety codes(like most people) . You can also put a g54 on a line of it's own and it's ok but it's not a must

%
O40001 (Basic program) ;
(G54 X0 Y0 is top right corner of part) ;
(Z0 is on top of the part) ;
(T1 is a 1/2" end mill) ;
(BEGIN PREPARATION BLOCKS) ;
T1 M06 (Select tool 1) ;
G00 G90 G17 G40 G49 G54 (Safe startup) ;
X0 Y0 (Rapid to 1st position) ;
S1000 M03 (Spindle on CW) ;
G43 H01 Z0.1 (Tool offset 1 on) ;
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G01 F20. Z-0.1 (Feed to cutting depth) ;
X-4. Y-4. (linear motion) ;
(BEGIN COMPLETION BLOCKS) ;
G00 Z0.1 M09 (Rapid retract, Coolant off) ;
G53 G49 Z0 M05 (Z home, Spindle off) ;
G53 Y0 (Y home) ;
M30 (End program) ;
%

M3 that was part of the incorrect posting, when using an M6 you don't need M5 /M9 you would need it only at the end of a Program unless you were staging the next tool

I Just did a Test try and this works nothing else needed at the end of the program if you are staging a Tool, if not staging a Tool, then you would need the M5 / M9 and wherever you want to move the spindle and Axis Too

M6 by itself will turn 0ff the Spindle / Coolant but won't move the Z axis to the tool change position it needs a T command and a different tool call from the courant one in the spindle for the Z axis to go to Home

%
O1502
N1G17G40G80
T3M6
M9
G54
S3450M3
G90G0X.7533Y.4558
G43Z.1H3
G81G98X.7533Y.4558Z-.06R.1F8.
X3.4853
X6.2173
X8.9493
X13.0522Y-4.2529
X9.9437Y-4.9706
X6.8351Y-5.6882
X3.7266Y-6.4059
X3.1641Y-3.97
X2.1172Y-3.2604
X.2262Y-2.6092
X.0399Y-1.6144
G80G0Z.1
T2M6 (Moves Z axis up to Home (Tool Change Position) turns spindle / Coolant 0ff)
M30 (Cancels Tool 0ffset the same as using a G49 this is why a G49 is not needed in any basic 3 axis program)
%

[HayreAss]

M89
M5
G0 G53 Z0.
M1
For the win in my shop.
No time lost.
The next tool is staged right after the earlier tool change, so not a concern.
Tool is still in the spindle if I need to run it again
Program pauses if I want it to. .

[mactec54]

M89
M5
G0 G53 Z0.
M1
For the win in my shop.
No time lost.
The next tool is staged right after the earlier tool change, so not a concern.
Tool is still in the spindle if I need to run it again
Program pauses if I want it to. .

You would have had a G0Z move before the M89 so the G0 is not needed with the G53Z0. is all that is needed

Having a M1 in any program is time lost.

Having the next tool loaded is a time saver. staging does very little unless you take advantage of it.

Running the same Tool and program on the same part without any change, would not make any sense

[metalmayhem]

An m1 is not lost time at all if optional stop is not turned on , if anything it just uses space on haas floppy sized memories . During a proper setup it's usually important to verify part dimensions between tools , and often it is important to rerun a tool . Thats why most people have an m1 between tools . Under those circumstances it is time wasted to have the next tool loaded , and since an m6 does not act as an m1 then m1 is actually an important little piece of code . It could be argued that an m1 can be put after a tool change but that becomes a break in the next operation

There are 2 kinds of production shops . One that runs all the tools , measures the parts in the end , make needed changes and often scrap the first set of parts . Then there are the shops that make proper adjustments as they go which means stopping at an m1 or stopping after a critical cut . Both have their time and place depending on the situation , after all time is money .
Except , the second shows less professional integrity and it is a method that wouldn't fly in a jobbing shop where a guy only has one chance to get it right . Safe coding and lots of stops is common place , and reckless short cuts that result in scrap is the difference between having a job and not

All the nit picking of the original code or individual codes is proving nothing . He's run this program numerous times without issue . The haas tech would have looked at the program and would have make recommendations as to any code changes needed . If he didn't recommend changes then the problem is with the machine and not the code , which is why he suggested it was a power surge that did the impossible and blew out g56

[HayreAss]

FWIW, I’m neither a job shop, or a production house.
I make and sell my own, boutique products.
Running 2 dozen of one particular program at a time is higher production for me.
I may run that program 20 times a year, but a dozen to two dozen parts per run.
X 60 SKU’s that all use the same base, but different engravings.
Couple time a year, that machine gets the 4th axis taken off, and a whole different product line run, because I want to use the 15k spindle.
I could be putting a $1000 piece of material in it.
I’m ok with an extra G0, an M1 that adds zero time when I don’t have it turned on, allowing me to measure, and adjust compensation and sometimes aesthetics before carrying on or adjusting and running again
My next tool is already staged, so no time lost there either.
All is good in my hood, except for the occasional ‘power surge’…

[mactec54]

FWIW, I’m neither a job shop, or a production house.
I make and sell my own, boutique products.
Running 2 dozen of one particular program at a time is higher production for me.
I may run that program 20 times a year, but a dozen to two dozen parts per run.
X 60 SKU’s that all use the same base, but different engravings.
Couple time a year, that machine gets the 4th axis taken off, and a whole different product line run, because I want to use the 15k spindle.
I could be putting a $1000 piece of material in it.
I’m ok with an extra G0, an M1 that adds zero time when I don’t have it turned on, allowing me to measure, and adjust compensation and sometimes aesthetics before carrying on or adjusting and running again
My next tool is already staged, so no time lost there either.
All is good in my hood, except for the occasional ‘power surge’…

Power Surge how are you powering your machine what is the supply Power

[HayreAss]

600 amp 3 phase panel.

Haas just likes to say power surge when they can’t explain an issue.

Now, we have dropped a phase twice in 5 years, due to trees falling and taking a line out upstream.

We shut down, and go home.
Same as the other machine shop next door, who has experienced none of the mysterious power surges as me even though we are fed from the same transmission lines.
We both have our own transformers, but are freed from the same lines.

- - - Updated - - -

600 amp 3 phase panel.

Haas just likes to say power surge when they can’t explain an issue.

Now, we have dropped a phase twice in 5 years, due to trees falling and taking a line out upstream.

We shut down, and go home.
Same as the other machine shop next door, who has experienced none of the mysterious power surges as me even though we are freed from the same transmission lines.
We both have our own transformers, but are fed from the same lines.

[mactec54]

600 amp 3 phase panel.

Haas just likes to say power surge when they can’t explain an issue.

Now, we have dropped a phase twice in 5 years, due to trees falling and taking a line out upstream.

We shut down, and go home.
Same as the other machine shop next door, who has experienced none of the mysterious power surges as me even though we are fed from the same transmission lines.
We both have our own transformers, but are freed from the same lines.

- - - Updated - - -

600 amp 3 phase panel.

Haas just likes to say power surge when they can’t explain an issue.

Now, we have dropped a phase twice in 5 years, due to trees falling and taking a line out upstream.

We shut down, and go home.
Same as the other machine shop next door, who has experienced none of the mysterious power surges as me even though we are freed from the same transmission lines.
We both have our own transformers, but are fed from the same lines.

Yes, I got the Haas Surge part, that's their easy fix, I wonder if they have a Part number for that fix

A Line Reactor would help, has to be sized correct though, this can help any machine that is using 3Ph power, you have a good supply, so that would be the only thing to add if you wanted to be sure, it would be good for the machines electronics as well

[HayreAss]

So, interestingly enough, and contrary to what you may have read earlier in this thread, not only CAN our work offsets be called out on the same line as our first X-Y move, as most of us already knew, but Haas themselves actually promote doing that way!
This screenshot is from an official Haas video that I ran into today.
Attachment 486466

[HayreAss]

Well, that led me down a short rabbit hole.
I downloaded some 'bonus content' from the Haas videos, and what do you know?
They actually teach folks to use an almost identical line to what my posts have always used.
The only difference being that my post opted to actually turn the spindle on in the next line...
But they teach G90, G17, Work offset, G0, XY movement, AND spindle commands, all in the same line!
So for those of you playing along at home and wondering WTF is going on in this thread, know that the original code posted is not only just fine according the manufacturers own publications, but a method they directly teach.