0-M programing help please

[venomgrrrl]

Hi I am a new member and I could use some programming advise. I have a new cnc milling center, (Shizouka Millmaster B-3V) and i am a little unframiliar with the currrent programing, so i am trying to modify what is currently in the machine from the previous owner. (I am most accustum to programming Haas, and Maho)

The commands I am not framiliar with is the H1 and the M3 ( i am shure the H's are for tool length comp? I will be manually imputing my tool lengths into the nc.)

Here is a program that was already in the cnc (sorry about the lack of spaces)

\H1&HE:% (IS THIS "\H1&HE" NESSASARY, I KNOW THE % IS)
:1011
(LUG BODY)
(DRILLING)

G28 G91 X0 Y0 Z0
M0

(CNTR DRILL) (THE N1, N2, N3, FOR MULTI. CYCLES??)
N1 G90 G80 G49 G40
G92 X4.319 Y9.674 Z0
G0 X0 Y0
G0 X1.508 Y3.64
G43 Z1.5 H1 M3 S1000 (ITS THIS LINE THAT I DO NOT UNDRSTAND)
G98 G82 Z-0.3 R0.1 F3.5 M8
X-1.508 Y3.64
X-3.64 Y-1.508
X-1.508 Y-3.64
X1.508 Y-3.64
X3.64 Y-1.508
X3.64 Y1.508
G80 M9
G28 G49 Z0 M5
G0 X-6.0 Y9.5
M1

(21/32 DRILL)
N2M6T18
G0X1.508Y3.64
G43Z1.5H2M3S450
G98G73Z-1.35R0.2Q0.1F2.3M8
X-1.508Y3.64
X-3.64Y1.508
X-3.64Y-1.508
X-1.508Y-3.64
X1.508Y-3.64
X3.64Y-1.508
X3.64Y1.508
G80M9
G28G49Z0M5
G0X-6.0Y9.5
M1

(COUNTER-SINK)
N3M6T17
G0X1.508Y3.64
G43Z1.5H3M3S250
G98G82Z-0.425R-0.2F2.4M8
X-1.508Y3.64
X-3.64Y1.508
X-3.64Y-1.508
X-1.508Y-3.64
X1.508Y-3.64
X3.64Y-1.508
X3.64Y1.508
G80M9
G28G49Z0M5
G0X-6.0Y9.5
M6T7
M0

(3/4-10UNC TAP)
N4
G0X1.508Y3.64
G43Z1.5H4
M29S100
G98G84Z-1.13R0.5F10.0
X-1.508Y3.64
X-3.64Y1.508
X-3.64Y-1.508
X-1.508Y-3.64
X1.508Y-3.64
X3.64Y-1.508
X3.64Y1.508
G80G28G49Z0M5
G0X-6.0Y9.5
M6T1
G91G28X0Y0Z0
M0
M99P1
%

ThanxsFor looking this over...been out of programing lil while, am a bit rusty!

[Mitsui Seiki]

G43 Z1.5 H1 M3 S1000 (ITS THIS LINE THAT I DO NOT UNDRSTAND)

G43=Tool length compensation positive
Z1.5= Stops 1.5 over the work piece
H1= Retrieving the tool length from tool offset # 1
M3=Spindle rotation CW
S1000=Spindle speed 1000 RPM

[dcoupar]

\H1&HE: aren't necessary. I believe they're control codes that didn't get stripped out when the program was sent. You need the % signs, though.

[cutsall]

H offsets are also used for applying offset value for radius of tool when applying cutter compensation.


N1 (3/4 END MILL)
G90 G80 G49 G40
T1 M6
G92 X4.319 Y9.674 Z0
G0 X0 Y0
G0 X1.500 Y3.750
G43 Z1.5 H1 M3 S1000
G0 Z-0.250
G01 G41 H21 X1.000 Y3.25 F15.0 (H21 Value Is Radius Of Tool)
Y-3.25
G40 X1.5 Y-3.75
G0 Z1.5
G28G49Z0M5
G0X-6.0Y9.5
M1

[venomgrrrl]

Thanx that pretty much anwsers all my quetions, M3...M03 *smacks forhead* DOH! That one i naly set my tooling
do knonw! Now i can finally set my tooling

[solid sender]

Hi venomgrrrl
I have experience of Fanuc OMD for VMCs. I have never used H# in conjunction with G41, I have always used D# for cutter radius compensation. You can also use M13 for spindle CW coolant on instead of M3 and then M8. Unlike Maho, which uses G98 & G99 for the graphics display, G98 and G99 are used to call up the 'initial plane' and 'rapid plane' on your drilling cycle. Hope this helps.

[solid sender]

Personally I would also put any repetative hole positions (as in your lug body) in a sub routine so that any alterations need only be made once thus reducing the posibilty of mistakes.

[VWSatOz]

I use H1 from the offset list for the tool length of T1, H2 for T2 etc... this avoids any confusion

[Ozemale6t9]

The N1, N2, N3 are simply line numbers so you can easily restart the program from somewhere other than the beginning (eg. after a tool breakage). Eg, with the program reset, type N2 and press the down cursor key, and the program will go to N2. Only problem is, the N4 really needs to have the M6T7 after it, or you have to change to that tool before you start from N4.

[venomgrrrl]

I have not seen any D's (dia) in any of the m/c's previous programming and have no idea how to use it.

I can sucessfuly drill holes, but now I am trying to mill a 2" hole (w. 3/4" mill) and have no idea how to pull it off.

Being quite paranoid about the G92 after every block of programming (N1, N2, ect) i am bringing the m/c home, then to safe point.

Any examples on how to do a G02 line of programming would be gratefully appricated, as I mentioned, I do not know how to proporly use the "D" command,

[Mitsui Seiki]

G40 G80 G49 G17
T6 M6
G0 G90 G54 X0 Y0 S1000 M3
G43 Z1.0 H6
G1 G41 D6 F100
X0 Y10.0
Z-0.1
G2 X0 Y10.0 I0 J-10.0
G0 G40 Z10
X0Y0

This makes a 20mm circle
G41 is radius compensation left. Tool motion is on the left side of the part.
D is the tool radius. Tool dia is 6mm. 6mm/2=3. D is 3mm.
When you use a D value you can easily compensate for tool wear.

[VWSatOz]

wont this prog with G41 cut over size? as it is GO2 for clockwise when milling around the OUTside of a circle? Should be G42?
I would use G03 to climb mill a hole so it cant come out oversize from cutter deflection.
& won't you be left with a little high spot near the end if you start with the straight move? Some programs use a 45 deg G1 move from centre to a smaller radius, which then enters into the full circular path, but this is a bit more complex for manual programming.