The Collected Wisdom
of the Haas Answer Man

Offsets

(Winter ’03
vol 7 # 24)

Dear Applications:

When I’m setting up a new job, is there a way to clear my offsets all at once? Right now I go through and zero each one separately, by pressing 0 and then F1 for each offset. I would like to be able to do them all at once.

     Walter Stevens

Dear Walter:

Yes, you can clear all of your offsets at once, with a single button and with verification. To do this, go to the offset display you wish to clear – tool offsets, work offsets or wear offsets – and press ORIGIN. The control will ask “ZERO ALL (Y/N)?” to verify the change. If you press Y, then all the offsets in that section will be zeroed. If you have the Haas macro option, this will also work for clearing macro variables. (Haas mill control software version 10.02 and above; Haas lathe control ver. 3.00 and above.)

     Sincerely,
     Haas Applications

(Spring ’03
vol 7 # 25)

Dear Applications:

When dealing with arc moves while cutting circles, is there a minimum straight line move required to have cutter compensation work?
     Dan Kafun

Dear Dan:

The short answer is “yes.” Cutter compensation can only be turned on and off in G00 (rapid) or G01 (linear) mode. After you’ve turned it on and before you start cutting, you must make a linear move that is the same or greater than the radial compensation value in your offset. If your radial cutter comp is set at 0.5”, for instance (for a 1” diameter tool), then you must make a linear cut of at least that length before you start cutting. Here’s how the program would look:

     Sincerely,
     Haas Applications

(Winter ’02)
vol 6 # 20)

Dear Applications:

I have a question about entering cutter compensation on the lathe offset page. On another CNC machine, I enter the tool radius and the tip direction on the wear page, and the tip measurement is automatically entered on the geometry page. On the Haas, the wear page only lists radius, and the geometry page lists both radius and tip. Do I have to enter the radius on both pages?

     Gene Calderone

Dear Gene:

No, the tool radius does not have to be entered on both pages. Both tool radius and tip direction are entered on the Tool Geometry page. Wear compensation is entered on the Tool Wear page only as the tool breaks down, and is returned to zero when the tool/insert is replaced.

     Sincerely,
     Haas Applications

(Spring ’99)
vol 3 # 9)

Dear Applications,

I own a small job shop with two Haas VF-1 machines. Since I mainly do short runs of any given part, I change setups and work offsets often. I recently nearly crashed my machine because I accidentally called up the wrong work offset. Since then, I always erase any work offsets I am not using to eliminate the chance of calling up the wrong offset and crashing the machine. The problem is that it takes some time to select and erase every individual offset. Is there an easy way to clear all work offsets?

     Sincerely,
     Brian Channing

Dear Brian,

You could write a simple program using G10 preparatory functions to automatically zero all of your work offsets. It may take a little time to write the program, but it certainly will save time in the future. G10 is usually used to alter offsets within a program, but it also can be used to set offsets to zero. See the programming example below:

Set G52-G59 work offsets to zero:

G10 L2 P0 G90 X0 Y0 Z0 A0    (repeat, changing the value of P, for P0 through P6)
G10 L2 P1 G90 X0 Y0 Z0 A0
 "   " "   "  "   "  "  "
G10 L2 P6 G90 X0 Y0 Z0 A0

Set G110-G129 work offsets to zero: 

G10 L20 P1 G90 X0 Y0 Z0 A0   (repeat, changing the value of P, for P1 through P20)
G10 L20 P2 G90 X0 Y0 Z0 A0
  "  "  "   "   "  "  "  "
G10 L20 P20 G90 X0 Y0 Z0 A0

This could be expanded to set tool offsets to zero by altering the L and P codes. L10-L13 references the geometry and wear columns of length and diameter offsets and P1-P100 reference the tool number offsets. 

     Sincerely,
     Haas Applications