[mactec54]

Hi tobyaxis

Yes that is correct It can affect more than just cutter compensation But like I said is not always needed

The plane selection G17XY G18XZ G19YZ for coordinated motion By not having one of these, the mostly used being G17 can affect
G2 G3 G81___G89, G40____G42

I edited my above post to add this

[tobyaxis]

Hi tobyaxis

Yes that is correct It can affect more than just cutter compensation But like I said is not always needed

The plane selection G17XY G18XZ G19YZ for coordinated motion By not having one of these, the mostly used being G17 can affect
G2 G3 G81___G89, G40____G42

I edited my above post to add this

Please note that their was no pun intended. I only mentioned it because I constantly switch for 3 axis vmc's and swiss with live tooling.

LOL my usual cure is to get a company to either buy more memory or I run DNC from my Lap Top.

Programs are getting bigger and bigger these days. There is one guy in this area that is very good with Macros which can reduce program sizes. Also you can use a Sub-Program for repeat patterns and frequently used operations like Nesting Jaws.

Plenty of ways to skin a cat when it comes to machining & programming.

[JohnJW]

Hi Johnjw

The G0 should never be in the first line it serves no purpose

End
G0Z2.
M9
M5
G0Y3.5
M30

Thank Mectec54,

What do you recommend for ending a tool cycle?

I was using G28 G91 Z0. M05 because that was recommended when I took the training class for the machine. However, Geof mentioned G53 G90 Z0. M05 and I think his reason on avoiding the G28 G91 combination make sense so I switch to using G53 G90 Z0. M05. But now it seems I can just retract Z and the next tool change will take care of the rest.

Your 8 year old probably has me beat I'm still in beginner stage so there's still quite a bit of fat in my program, ie I rapid to Z1.0 and start my plunge from Z.125 so I can roughly visually check the tool position . . . even at 25% rapid it's still a little too fast for me. . ..

thanks again,

John

[Geof]

....What do you recommend for ending a tool cycle?

.... But now it seems I can just retract Z and the next tool change will take care of the rest.....

.. I rapid to Z1.0 and start my plunge from Z.125 so I can roughly visually check the tool position . . .

If you are going into a tool change you really do not have to retract Z any further than your Z1.0 clearance because the Tn M06 command does everything. Heck you can call a tool change from the bottom of a hole if you want to save a few milliseconds.

There is nothing wrong with going to Z1. then Z0.125 I tend to do that in many of my programs. Maybe I am abit moredaring because I tend to use Z0.1.

[extanker59]

I use:
G53 Y0 Z0 M5
M1

because I like to check my progress after each tool during set up. So it moves the spindle up out of the way and the table toward me so I don't get as wet. Keep in mind we aren't watching every second of cycle time here. Short runs only. If you are, then Geof has the way.
I dislike G28 etc... for the reasons already mentioned.

[Caue]

Hi, guys

I Know I'm just a beginner here, but at this pont of discussion, some settings can be useful for those who posted their coments:

29 - G91 Non-modal
This is for those who don't use G91 G28 due to the risk of forgetting to turn G91 off after use. It's almost useful to cycles with looping (i.e. increment Z axis each run), for die & mould roughing operations.

36 - Program Restart
This setting avois you to need to repeat all safety codes at each tool change.

56 - M30 Restore Default G
This is for those who are happy with machine defaults conditions and don't want to use any block specially to write the safety codes.

I hope it can be helpful. The descriptions were suppressed so that the post could be more clear. Any additional information can be found at Haas Mill Operators Manual.

Thank you all for using Haas Automation Machining Solutions!!