New guy question

[Larry Myers]

Hi All,

I have a Sharp 2412 VMC with a Fanuc oi computer. I believe there are some canned cycles however the documentation is nasty at best. I am still very new to g-coding with about 6 months under my belt.

I want to mill a circle pocket (1.5” dia) and a rectangular pocket (2”x3”), both with the origin at 0,0, (two different parts) and using a 1/2” end mill. Both will be 0.025” in depth.

Can anyone advise me if there is a simple way to achieve this? Thanks very much in advance!
Larry

PS I also posted this in the G-Code section

[PBMW]

This is the 1.5 dia pocket
The origin is the center


%
O0000 (T)
(MASTERCAM - X)
(MCX FILE - T)
(POST - %MCAMDIR%MILL\POSTS\MPMASTER.PST)
(MATERIAL - ALUMINUM INCH - 2024)
(PROGRAM - T.NC)
(DATE - JAN-09-2008)
(TIME - 6:38 AM)
(POST DEV - IN-HOUSE SOLUTIONS)
(T1 - 1/2 FLAT ENDMILL - H1 - D1 - D0.5000")
G00 G17 G20 G40 G80 G90
T1 M06 ( 1/2 FLAT ENDMILL)
(MAX - Z.25)
(MIN - Z-.025)
G00 G90 G54 X-.2229 Y.1133 S10000 M03
G43 H1 Z.25
G8 P1
Z.1
G94 G01 Z.01 F25.
G02 X.25 Y0. Z-.025 I.2229 J-.1133 F50.
G01 X.0469
G03 X-.2344 I-.1406 J0.
X.4219 I.3281 J0.
X.0906 Y.4816 I-.5156 J0.
X-.0906 Y-.4816 I-.0906 J-.4816
X.49 Y0. I.0906 J.4816
X.0906 Y.4816 I-.49 J0.
G01 Z.075 F385.
G00 Z.25
X-.375 Y.1768
Z.1
G01 Z-.025 F25.
G41 D1 X-.4634 Y.0884 F50.
G03 X-.5 Y0. I.0884 J-.0884
X.5 I.5 J0.
X-.5 I-.5 J0.
X-.4996 Y-.02 I.5 J0.
X-.4595 Y-.1069 I.1249 J.005
G01 G40 X-.3676 Y-.1916
Z.075 F385.
G00 Z.25
G8 P0
M05
G91 G28 Z0.
G28 Y0.
G90
M30
%


And this is the rectangular pocket. 2.0 in X and 3.0 in Y
Origin at the top left

%
O0000 (T)
(MASTERCAM - X)
(MCX FILE - T)
(POST - %MCAMDIR%MILL\POSTS\MPMASTER.PST)
(MATERIAL - ALUMINUM INCH - 2024)
(PROGRAM - T.NC)
(DATE - JAN-09-2008)
(TIME - 6:42 AM)
(POST DEV - IN-HOUSE SOLUTIONS)
(T1 - 1/2 FLAT ENDMILL - H1 - D1 - D0.5000")
G00 G17 G20 G40 G80 G90
T1 M06 ( 1/2 FLAT ENDMILL)
(MAX - Z.25)
(MIN - Z-.025)
G00 G90 G54 X1.3971 Y-1.7222 S10000 M03
G43 H1 Z.25
g8 p1
Z.1
G94 G01 Z.01 F25.
G02 X.8514 Y-2.0149 Z-.025 I-.4584 J.1997 F50.
G01 X.8225 Y-2.1775
X1.1775
X1.2507 Y-2.2507
X1.1775 Y-2.1775
Y-.8225
X1.2507 Y-.7493
X1.1775 Y-.8225
X.8225
X.7493 Y-.7493
X.8225 Y-.8225
Y-2.1775
X.7493 Y-2.2507
X.635 Y-2.365
X1.365
X1.4382 Y-2.4382
X1.365 Y-2.365
Y-.635
X1.4382 Y-.5618
X1.365 Y-.635
X.635
X.5618 Y-.5618
X.635 Y-.635
Y-2.365
X.5618 Y-2.4382
X.26 Y-2.74
X1.74
Y-.26
X.26
Y-2.74
Z.075 F385.
G00 Z.25
X1.3536 Y-.5
Z.1
G01 Z-.025 F25.
G41 D1 X1.1768 Y-.3232 F50.
G03 X1. Y-.25 I-.1768 J-.1768
G01 X.25
Y-2.75
X1.75
Y-.25
X1.
X.98
G03 X.8032 Y-.3232 I0. J-.25
G01 G40 X.6264 Y-.5
Z.075 F385.
G00 Z.25
g8 p0
M05
G91 G28 Z0.
G28 Y0.
G90
M30
%

As you can see, I turn on HSM with G8's so if you don't have that option, delete them

[Larry Myers]

Hi PBMW,

Thanks so much. For the most part I follow however I am unfamiliar with the code G8 P1 and G8 P0. I looked up the G8 code in the manual and it says
"advanced preview control”. Can you shed some light on what this code does?

Again, my thanks!

Larry

[timlkallam]

Hello Larry after reading you post ,I went to the manual guide oi
in the sharp mini mill 2414 its remindes me of a conversational control it just asks alot of questions what tool number spindle speed coolant on or off ,tool ofset ect, then you can choose from a list of about 40 caned cycles to use .Drill cycles pocketing ect.
But after anserwing all the questions it spits out the program
. But the program is not in the corect order it will turn the spindle on then do a tool change.I can etit the program but then i get an alarm.This would be a very valuable and speed up programing
on some parts, But i just can't get it to work. Your not alone

[PBMW]

The G8's are controling the look ahead function of the control if you have that option. G8 P1 turns it on and G8 P0 turns it off. This option will control the feedrate so as to more closely follow the part geometry and to reduce the "Stuttering" that happens when you go too fast.
G5.1 also controls a slightly different form of contouring known as AI NANO
If you don't have that option...just delete them.

[Larry Myers]

Thanks guys!

This place is great.

Larry

[MASTERCAMMASTER]

A simple way to program a hole.

1.500 dia hole

.500 dia em

T1M6(1/2 EM)
G0G90G54X0Y0
M3S5000
G43Z1.H1
M8
G1Z.1F50.
G1Z-.025F10.
G91G01X-.5F8.
G03I.5
G1X.5F50.
G90
G0Z2.
M9
G0G91G28Z0Y0
M5
M30
%

When posting you can also use R's instead of I & J codes.
You should edit your post.
I worked at a place once where they actually had the address of the place in their programs.

[PBMW]

Of course I can program it by hand. What's the point?
Why should I edit my post?
Does it bother you that much?
I's and J's are in fact a little more accurate.
How come you got no comp in there to control the size?
Jeez....tough room.

[MASTERCAMMASTER]

Of course I AND J codes are better with cad cams, but R'S are easyer to program manually.
The guy is a novice why don't you give him something to use forever not a computer generated program.
P.S. You have 10 lines at the top of the program you can delete, lol
I BET YOU LEARNED CAD CAM THEN STARTED WORKING AT A MACHINE SHOP.

[holbieone]

Originally Posted by MASTERCAMMASTER Of course I AND J codes are better with cad cams, but R'S are easyer to program manually. The guy is a novice why don't you give him something to use forever not a computer generated program. P.S. You have 10 lines at the top of the program you can delete, lol I BET YOU LEARNED CAD CAM THEN STARTED WORKING AT A MACHINE SHOP.

use "I" and "J" when the end points are more important

use "R" or "P" when the radius is more important

the faster your feed rate the less accurate the machine will be so you need to tell it what's important

[PBMW]

Originally Posted by MASTERCAMMASTER Of course I AND J codes are better with cad cams, but R'S are easyer to program manually. The guy is a novice why don't you give him something to use forever not a computer generated program. P.S. You have 10 lines at the top of the program you can delete, lol I BET YOU LEARNED CAD CAM THEN STARTED WORKING AT A MACHINE SHOP.

Are you joking?
I've OWNED my shop since 1982
So what if there's 10 lines that can be deleted.
Know what, I catch someone programming a machine at the control instead of running it like I pay them to do they're out the door.
There's a much larger picture here...the machine has to run to make a dime. You don't use a hunnert grand CNC as a calculator if you have a lick of sense
You OBVIOUSLY don't own a machine do you.

[MASTERCAMMASTER]

Originally Posted by PBMW Are you joking? I've OWNED my shop since 1982 So what if there's 10 lines that can be deleted. Know what, I catch someone programming a machine at the control instead of running it like I pay them to do they're out the door. There's a much larger picture here...the machine has to run to make a dime. You don't use a hunnert grand CNC as a calculator if you have a lick of sense You OBVIOUSLY don't own a machine do you.

Today I made a program right on the machine 3 whole tools.
Spot
Drill
Ream

I happen to like perfect posts.

Quality is way more important than time, maybe thats because Lockheed Missle & Space, and Northrop Grumman both in Sunnyvale, Ca. pay so well I don't have to hurry.

Your computer must be closer to the machine than mine.

E-MAIL me at WHITE_MAN_BEST@yahoo.com and I can e-mail you a video of my shop. Here in silicon valley there is NEVER snow and you don't have to worry about freezing to death. Oh I forgot to say eh?
Land here is 1 million an acre how much is it where you live?