What's new
What's new

Attention Haas Rotary Users! G92?

munruh

Hot Rolled
Joined
Jan 3, 2011
Location
Kansas
Our Rotary Milling Post always posts a G92. Below is an example. This is on Haas VF3s and VF4s. In order to get our programs to work correctly we delete the G92 lines. I am going to modify our post to not put in G92s. Is there any reason I should not do this?

G54G90G0X5.3Y0.A-16.924S3056M3
G43Z10.H15
M97P102
G0X5.3A103.076
M97P102
G0X5.3A223.076
M97P102
M9
G91G28Z0.M19
G92A-136.924 (OFFENDING LINE)

THANKS
 
G92 as far as I know shifts the machine coordinate system so I don't see any reason for it in your post. What Cad/Cam software are you using? I've used both MasterCam and GibbsCam with 4th axis and have never seen a G92 in my program.
 
G92 as far as I know shifts the machine coordinate system so I don't see any reason for it in your post. What Cad/Cam software are you using? I've used both MasterCam and GibbsCam with 4th axis and have never seen a G92 in my program.

Using Gibbs post RM4614.20. I think I am going to have it changed.
 
Using Gibbs post RM4614.20. I think I am going to have it changed.

Yeah I'm using Gibbs right now and when we first purchased it they gave us about 4 different posts to try to see which one better suited our needs. I used it for a while then had them modify the post the way we wanted it. They give you posts that other people have used and modified for specific machines so sometimes you end up with garbage you don't need in the post. I'm suprised they gave you a post that outputted a G92 with an A value?
 
I guess I will send it to get changed. We don't do a lot of actual rotary milling, more positioning. On the actual rotary milling is where we are having trouble.
 
The only reason to have a G92 A at the end of the program is to cancel out the accumulated values of G92 A used during the program. If you never use any G92 A commands then you don't need one at the end to undo all the accumulated values.

If you use a bunch of G92 commands in your program, they will accumulate in the G92 offset register. Any residual amount left over at the end of the program run, should be inspected by looking in the offset register. Then put an equal but opposite value into that final G92 A command to neatly zero out the offset register for G92

However, if you use a Quick Rotary G28, at the end of a program where you've really 'wound up' the A axis, then you'll see the axis return to the nearest multiple of A0, however, it will likely still want to unwind to the real A0 when you rerun the program from the start. A G92 A0 command after the G28 A0 command can alleviate this problem.
 
That's a Blast from my Past, I had forgotten all about the Gibbs Library where they send you a handful of Posts and tell you to give them a whirl to see if they work properly for you.

Had a Lathe Post that sent tooling to X0 Z0 instead of a safe home position to index turret and before certain cycles

But in general it was fun to try and learn how to use a new CAM Program and then proof out its Generated Code so machine would not crash or make scrap. It's been 10 years and I still have to tweak my posts further. I just learned to do work arounds that take a few second...but not so much for the new hand that just stares at the machine scratching his head...Lathe Thread Cycle works great in long hand, but if one should hit the Canned Cycle the Post sends something funky to machine that makes something...just not a thread. Rigid Tap Canned works, long hand don't and a bunch of other Pain in the Butt things... I just hate tweaking posts because they fix one thing and then something always seems to PoP up down the road and the cycles continues...Still much better then Finger CAM
 








 
Back
Top