G94/G95

[cormigu]

Can somebody tell me what means G94/G95, because I got an alarm on the machine, when i delete those g code (g94/g95)...it works fine......is it possible to modify my PST(mpmaster)....(Haas mill)

Thanks.

 

 

[Hardmill]

G94 is in per minute feed

 

G95 is feed per rev

 

Im sure someone else can give you a play by play

on the post mod. better than I can

 

Im more the hack and try type.

 

 

PEACE

[Philcott]

quote:

---

Yes, this is a new feature of the Haas control. G95 will interpret any feed value as Feed Per Rev. When G95 is active, a spindle revolution will result in a travel distance specified by the feed value. If Setting 9, DIMENSIONING, is set to INCH, then the feed value (F) will be taken as inches/rev. If Setting 9 is set to MM, then the feed will be taken as mm/rev. The G95 mode will stay effective until another feed mode, such as G94, Feed Per Minute, has been specified.

 

Note that the default at power-up is G94. Feed Override and Spindle Override will affect the behavior of the machine while G95 is active. When a spindle override is selected, any change in the spindle speed will result in a corresponding change in feed in order to keep the chip load uniform. However, if a feed override is selected, then any change in the feed override will only affect the feedrate and not the spindle. A command block that contains a tap cycle will ignore any feed and spindle overrides, and perform that block at 100%. Setting 56, RESTORE DEFAULT G, will determine whether or not an M30 should reset the Feed Per Rev mode. If this setting is enabled, then an M30 at the end of a program will reset this mode to its default G94, Feed Per Minute, mode. Alarm 309, EXCEEDED MAX FEEDRATE, will be generated if the combination of spindle speed and feed value (F) exceeds the limit specified by Parameter 59, MAX FEED IN/MIN.

 

Sincerely, Haas Applications

---

[Philcott]

If feeding the tap at F.05 you are going to want the G95 in there to give you feed per revolution. If you take it out you will need to put a feedrate calculated to the RPM you are running the tap at and recalculate the feed again of you change the RPM.

[lwells]

There is a switch in the post to switch from feed per rev to in per minute. This should switch yor f line from pitch to feed and get rid of g95. If I stop a program in the middle of a tapping cycle and try to restart without cancleing g95 my machine will not move. I stay in in per minute and and calculate my feed in tool library.

[cormigu]

hi Iwells,

 

Can you tell me where to change feed per rev to in per minute.?Below the G95 I have the M29 what does that mean?

thanks.

[Guest CNC Apps Guy 1]

IPM sucks for tapping. You gotta get your calculator out if you want to change a feed or speed. With IPR, your feed rate is ALWAYS the pitch of the tap, and you just adjust speed to go faster or slower.

 

M29 is Rigid Tapping active on some machines. Consult your Machine Tool Programming guide for specifics relative to your machine.

 

HTH

[lwells]

use_pitch : 0 #0 = Use feed for tapping, 1 = Use pitch for tapping

rigid_tap : 1 #0 = Floating tap output, 1 = Rigid tap output (suppress spindle output and output M29)

 

This is what I have in my post,(mpmaster). Once you set the pitch of your tool in tool parameters

feed will automaticly change when you change speed in your operation tool paremeter. IPR may be easier but I'm old and set in my ways.