can you "G93" with a Haas VF3

[Toolfab]

On my Maho mills if we need to adjust for something we simply put in a G93 x x.xx I am being told be the operators that you cant do that in a Haas. Is there a way to just "offset" a toolpath rather than having them find me, change the geo, and repost it?

 

I have very limited knowledge of the Haas so any info would be greatly helpful. Thank you.

[Guest]

G93 on a HAAS I believe is for Inverse feedrates.

 

quote:

---

nverse Time Feed Mode (G93)

This VMC/HMC feature specifies that all F (feedrate) values are to be interpreted as “strokes per minute.” This is equivalent to saying that the F code value, when DIVIDED INTO 60, is the number of seconds that the motion should take to complete. G93 is generally used in 5-axis work, and sometimes in 4-axis work as well. It’s a way of translating the linear (inches/min) feedrate assigned to the program – F30, say – into a value that takes rotary motion into account. When G93 is activated, the F value will tell you how many times per minute the stroke (tool move) can be repeated, based on the linear F value.

 

Haas has been able to accommodate full 5-axis machining for many years; however, this feature, in conjunction with aftermarket CAM systems and their post-processors, offers even more flexibility and versatility.

---

HAAS Automation

[John13]

My chart on my mini mill says G93 Inverse Time Feed Mode On

[Toolfab]

So is there a code that Haas will read that would act the way that I am thinking? Say i want to move a contour pass .005 in Y. In the Maho I would use G93 Y.005 and it would shift the Y value .005. Kinda like a cutter comp (G41) but it only effects one axis rather than 2 on a G41 because of the radius call.

 

Am I pissin in the wind or is there some trick or code that I am missing.

[Guest]

AFAIK, your pissin' in the wind on this one.

 

sorry

[Toolfab]

so the only way is to edit the geo and repost? that sux, thanks John. I appreciate the help.

 

[htm01]

i think you might want to look at G92(shift WCS)

[Storkman]

On a Fanuc it is G52.

 

Just put in G52 X.004 to shift the entire program 4 thou. use G52 X0 at the end to shift it back.

[Lucky]

G52 may be what you are looking for. Be careful because it will remain in affect and apply to all programs until it is zeroed out again! It may be possible to use G10 to load a value into the G52 register then use G10 again at the end of the program to "zero" it back out. More involved editing but safer. I've been bit using G52 shifts before.......

[Guest]

To use a G10 line you could do it like so

 

G10 L2 P0 G90 X.004 Y0 Z0 A0

 

shift your X.004

 

at the end of the program

 

G10 L2 P0 G90 X0 Y0 Z0 A0

 

and shift it back

 

You guys were right I haven't used it in quite awhile and forgot all about it.

[Toolfab]

You guys rock! The G52 is what I needed. THANK YOU ALL!

 

Pauly teh print this out and give to operator

[Chris Rizzo]

g92 will also work for a global offset. it is zeroed anytime an axis zero is hit, or power up, or reset.

 

It also relates to what setting 33 on the machine is set at: Fanuc , Yasnac or Haas.

 

In haas format anything entered into g52 is a global offset to all g54-g129. A g92 will cancel it.