Helical milling with HAAS

[dinger]

I'm editing my CAD postprocessor file for our HAAS machines. I need to know if the HAAS controller can read one or both of the following helical output types:

Option 1: This outputs a helix record for every 90 degrees of the helix.
X.28750 Y.00000 Z-.78000 F20.
G17 G03 X.28750 Y.00000 Z-.70860 R.28750
G17 X.25150 Y-.13940 Z-.64290 R.28750

Option 2: This outputs a helix record for every 360 degrees of the helix.
X.28750 Y.00000 Z-.78000 F20.
G17 G03 X.25150 Y-.13940 Z-.64290 R.28750

I have a third option, which is just XYZ linear moves. I'd rather use one of the first two, if possible.

I also need to know if the helix pitch type for HAAS should be "rise radian" or "rise revolution."

Thanks

[emckell]

Hello,

For the HAAS Controller, you must know how arcs work. On all our HAAS machines arcs can be created using G2/3 with an R or I/J/K. R can only be used for partial circles, not 360 degrees.

With that info, Option #1 works. You do not need to have G17 output on each line because G17 is a modal command and the Default mode at machine startup.

Your option #2 would require a change to use I/J/K values instead of the R value.

One additional note. Depending on the age of your HAAS, you may be limited on the Z travel during a helix. Our oldest mill (circa 1993) will only allow a Z movement that is less than or equal to the circumference distance on the arc in the helix move. On new controllers this has been changed.

I am not quite sure what you are asking in the last question "rise/radian" or rise/rev. I have never had to deal with that in any of the post processors I have used.

Hope this helps some.

[Tim Stevenson]

custom G code
full arc with I and J -- R is for 180° or less


G00 X0 Y1.685
Z1.
/ M08
G01 Z0.1 F50.
( 1/2-20 I/D THD )
(G200 COMMAND)
( C CUTTER DIA )
( D MAJOR DIA OF I/D THREAD )
( E THREADS PER INCH )
( W THREAD LENGTH )
( X CENTER OF HOLE )
( Y CENTER OF HOLE )
( Z FACE WERE HOLE IS )
G200 X0.0 Y1.685 Z0 W0.33 E20 D0.500 C0.35 F.5
G80
G00 Z1. M09
G65 P9100 ( HOME )
M01

!

%
O9010( THREAD MILL )
G00X#24Y[#25+0.02]
G01Z[#26+0.1]F50.
G41Y#25
Z[#26-#23]F10.
G03X[#24+[[#7-#3]/2]]I[[[#7-#3]/2]/2]J0F#9
X[#24+[[#7-#3]/2]]I-[[#7-#3]/2]J0Z[[#26-#23]+[1.0/#8]]
X#24I-[[[#7-#3]/2]/2]J0
G01Y[#25+0.001]
G40X#24Y#25F10.
Z[#26+0.1]F50.
M99

(G200COMMAND)
(#3= CUTTER DIA)
(#7= MAJOR DIA OF I/D THREAD )
(#8= E THREADS PER INCH)
(#9= F FEEDIPM)
(#19= S RPM )
(#23= W THREADLENGTH bottom of hole )
(#24= X CENTEROFHOLE )
(#25= Y CENTEROFHOLE )
(#26= Z FACE WERE HOLE IS )
%

[ObrienDave]

The Z Value would be equal to the rise per move.
The Z value in absolute mode, G90, would be where you want the tool to end at.
The Z value in incremental mode ,G91, it would be how far you want the tool to move.
Normally, you do not program "rise per radian", you program rise or fall per move.
Your "Option 2" would be equivalent to "rise per revolution".

P.S to emckell,
A radian is the angle at which the length of the arc equals the RADIUS of the arc.
1 radian = 180/pi = 57 deg 17' 44.806" = 57.29577951 degrees

[ndorin]

mr. stevenson:
u seem 2 b very knowledgable, what kind of cdes are those which u posted[ie:g200 command-G00x#24 etc..] ? r those macro calls?
just starting in this wide world of machining. & by the way i have been using MCam since v5.2. They sure have come a long way in 15 years.I have heard about the insanity of mastercam X, but dont have access to it.
thnx


Neil Dorin, "lilbastard"

[ndorin]

anyone;;
I finally got my post to output ij&k in g83, the only problem is , & its a pain in the as_, is that kis always "K0." if anyone knows what i have to modify in the post (for MC) so that the k will dump what its supposed to please try to inform me. Thank u very much. I have spent weeks , just to finally get for example/ G98G83Z-.3R.1 I.2 J.1 K0. F22.(KSHOULD BE K.1 )THERE MUST BE SOME TYPE OF FORMULA THAT HAS TO BE INPUT IN A SPECIFIC LINE OR LINES IN MY HAAS.PST & PROBABLY MY MILL9.SET FILE AS WELL??
I MAY BE VERY SLOW, BUT AT LEAST I'M STUPID.
NEIL,
SAN JOSE

[Paul_S]

If my memory serves me correctly an R for an arc less than 180 and an R- for greater than 180 but less than 360. A custom APT post processor I once used had a bug, where the helical output was R-. So instead of 4 quadrants of circle got 4 scallops. The arcs were not 90 but 270 degrees. I personally use I and J for arcs. (or K, I)(or J, k)

(I didn't know what the type of Vertical Mill it was nor its control, I was using a custom post for it. Anyway if I did know, I don't remember, except the CAD program was CAD KEY and with PC-APT)

[dinger]

We actually used to use I,J,K values. However, when we switched from MasterCAM to UG/NX three years ago, we began to have I,J,K out-of-tolerance errors at the machines. Since we switched to R values, things have run much smoother. Thank you all, for the input. I believe I can output a helix using the quadrant/rise per revolution method.

Chris Dingman
JSP Mold
Milledgeville, IL

[Malish]

Do you actually need to use the G17 or can you use the G2/G3 with the Z value included?

[Geof]

Originally Posted by Malish Do you actually need to use the G17 or can you use the G2/G3 with the Z value included?

It was mentioned in a post further up; G17 is the default mode to work in X Y plane. All you need is G02(3) I J Z which will do a single circle while moving the Z distance, with the center of the circle a distance I along the X axis and J along the Y axis from the start point. If you want to do more than one circle use G91 G02(3) I J Z L with the number of circles in the L.

[tobyaxis]

HAAS VF-3 can perform Helical Interpolation

tobyaxis