[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.

[Mitsui Seiki]

It's just an example to show how it works.

[VWSatOz]

I wasn't really being picky... but I though we better not lead the boy too far away!
I can hardly remember exactly how to correctly write the I & K values for G02 &G03 because it depends if you are in incremental or absolute mode.
Best to use a CAM system to get the PC to write it all with the post processor after verifying the path, too easy to make human errors the manual way on any complex sort of job.
All good fun...

[venomgrrrl]

LOL, well fiirst off, ima girl, but with all the help im getting you may call me boy!
and im having the same difficulty w remembering my I's and K's, but with what I have in this thread I am fairly confident I can make a hole (of some size, somewhere lol)
I have a mastercam guy coming to the shop today, so I hope that will aliviate some of my programing woes,
Ill keep you posted on what happens!
Thanx again, you guys rock!

[Mitsui Seiki]

I wasn't really being picky... but I though we better not lead the boy too far away!

I know,and you're absolutly right.

Good luck,venomg(i)rrrl.

[solid sender]

Hi Venomgrrl
D# retrieves the tool radius from tool offset # . You input your radius data on the same offset page as your tool length data.
ie Tool No 4 Length offset No 4 Radius offset No 24 or 34 or 44 whatever makes the most sense to you, as stated by VWsatOZ.
therefore the programme would be;

G43 Z1.0 H4
G1 G41 D24 F100

Personally, so long as you are not machining a toughened or wear resistent material, I would also climb mill a circular pocket bearing in mind you may have to run a spring cut to finish the diameter to size. I would also choose to cut up to the full diameter using a smaller radius to reduce the machining dwell marks that a G1 would give you, but that is up to you, some jobs don't require this kind of finishing.

[Mitsui Seiki]

This is another EXAMPLE of how to do a hole.

G0  G90 G17 G54 X0 Y0 S2000 M3 T1 
G43  H1 Z10 M8 
G1  Z-2 F50 
G41  X0 Y6 D1 F250 
G3  Y-6 I0 J-6 
Y10  I0 J8 
Y-14  I0 J-12 
Y18  I0 J16 
Y-22  I0 J-20 
Y26  I0 J24 
Y-30  I0 J-28 
Y34  I0 J32 
Y-38  I0 J-36 
Y38  I0 J38 
I0  J-38 
G0  Z10 
G40
X0  Y0 
G1  Z-4 F50 
G41  X0 Y6 D1 F250 
G3  Y-6 I0 J-6 
Y10  I0 J8 
Y-14  I0 J-12 
Y18  I0 J16 
Y-22  I0 J-20 
Y26  I0 J24 
Y-30  I0 J-28 
Y34  I0 J32 
Y-38  I0 J-36 
Y38  I0 J38 
I0  J-38 
G0  Z10 
G40 
X0  Y0
M5  M9 
M30

[solid sender]

Hi venomgrrrl
From what I can recall if you are in G17 plane (X,Y) the I & J are incremental from the current cutter position to the centre of the arc path to be cut, the X & Y are the absolute end position of the arc.

A simpler way to mill a circle with smaller interpolated arcs is the following;
N# T# M6
GO G21 G40 G80 G90
G56 X0 Y0 S5000 M13
G43 Z50 H#
G1 Z-10 F600
G1 G41 X14 Y41 D#
G3 X0 Y55 R14
G3 X0 Y55 I0 J-55
G3 X-14 Y41 R14
G40 X0 Y0
G0 Z100
G53 X# Y#
M30

if I have remembered correctly that should give you a 14mm radius arc into an 110mm diameter circle then leading off with a 14mm radius arc. Obviously you should have drilled out the centre first.

I would also add that if you follow the suggestion from thread #9, ie N# cursor down then you should also add in a safety line after every tool change otherwise you will have trouble with your modal G codes if you have not remembered to press data reset.
I would always programme this line just to be safe;

G0 G21(or 20) G40 G80 G90

[chuy]

U tryin to get the guy to crash!!! D is the call out for the cutter comp G41 D21 unless you want to cut through the entire part go ahead and use H