need code CHECKED PLEASE to mill a hole

[krfrea]

need code to mill a hole 1.22" in dia., in .750 Hot roll plate, located X6.375Y-3.5 using a .50 carbide end mill S2200F4.0. I will start by drilling a 1" hole.
Thank You in advance for any help

[timlkallam]

Here is a link to a free circle millimg program .
http://www.kentechinc.com/tip7.html

[APACHE]

G00 X6.375 Y-2.750
Z.1
G01Z-.76F25.
X6.735 F8.
G02X6.735Y-2.750 I-.360 J0.
G00Z1.M09

[APACHE]

G00 X6.375 Y-2.750
Z.1
G01Z-.765F25.
X6.735F8.
G02X6.735Y-2.750 I-.360 J0.
G00Z1.M09

[krfrea]

Thanks for your help. I have used the circle milling program mentioned above and wrote the following main and sub program. Any comments would be appreciated.

%
O0001

(1" INGERSOL DRILL)
M6T9
G00G20G40G49G80G90G98G54
G43X6.375Y-3.50Z0.2H9M3S1800
M8
G83Z-.90R.1Q.36F3.8
G00G91G28Z0.M19
G80M9
G00G91G28Z0.M19

(MILL 1.22" HOLE W/1/2" END MILL)
M6T5
G54
G90S2200M03
G00X6.375Y-3.50Z0.2H9M3S1800
M8
G01G90Z-.250F4.0
M98P0002
G01G90Z-.500F4.0
M98P0002
G01G90Z-.800F4.0M09
M98P0002
G00Z.2
G80M9
G00G94G28G53X-12.Y0.Z0.M5
M30
%

%
O0002(CUTTING PROGRAM 1.22 DIA)

G02G91G42X.36Y0R.18D15
G02I-.36
G02X-.36Y0R.18
G40M99
%

[Paul_S]

I'm not sure the reasons you have the code as you do. But it should work with some fixs.


This code reverts the RPM back to 1800 and calls the T9 length offset for T5.
G90S2200M03
G00X6.375Y-3.50Z0.2H9M3S1800

needs to be changed to:
G90S2200M03
G00X6.375Y-3.50Z0.2H5
(assuming the G43 was not canceled)

And I would also add to:

G01G90Z-.800F4.0M09
M98P0002

I would add a finish spring pass:
G01G90Z-.800F4.0M09
M98P0002
F19.
M98P0002

Also I would change the code from G42 G2 to G41 G3:

%
O0002(CUTTING PROGRAM 1.22 DIA)

G03G91G41X.36Y0R.18D15
G03I-.36
G03X-.36Y0R.18
G40M99
%

Since convental cutting tends to suck the tool into the work and cut bigger. (Now only if the material is harder on the outside than on the inside you would want your first cut G42 G2 and your last cut G42 G2 with the middle cut G41 G3 and the finish spring cut G41 G3. IMO)

Test your code out without any material in the machine and see if it looks and moves the way you expect. (Dry run.)

Also is there a reason that the SFPM for the drill is 471 and the mill is 287? Usually the drilling SFPM is less than the milling SFPM.

[cnc-king]

This would be my 2 cents

%
O0001
(1" INGERSOL DRILL)
G00G20G40G49G80G90G98G54
T5M6
G0G90G54X6.375Y-3.50M3S1800
G43Z.2H5M8
G83Z-.90R.1Q.36F3.8
G80
M9
G00G91G28Z0.M19
M1
(MILL 1.22" HOLE W/1/2" END MILL)
T9M6
G00G90G54X6.375Y-3.50M3S2200
G43Z.2H9M8
G0Z0
M98P0002L4
G0Z.2
M9
G00G94G28G53X-12.Y0.Z0.M5
M30

O0002(CUTTING PROGRAM 1.22 DIA)
G0G91Z-.2
G1G41X.18Y-.18F5.D15
G3X.18Y.18J.18
X-.72I-.36
X.72I.36
X-.72I-.36
X.72I.36
X-.18Y.18I-.18
G1G40X-.18Y-.18
G90
M99
%

[APACHE]

I DONT KNOW WHAT TYPE OF CONTROL THAT YOU ARE USING BUT ALL G CODE CONTROLS I HAVE G90 AND ALSO G91 ARE MODEL I HAVE AN OLD
FANUC 10M ON A MORI SEKI THAT I HAVE TO G91 G28Z0 BECAUSE IT DOES NOT HAVE ABSOULTE ENCODER SEEMS LIKE A LOT OF CODE TO MILL A CIRCLE.BUT IF IT WORKS FOR YOU THAT WAY GREAT!!! WE HAVE SEVEN MAZAKS SO I GUESS IAM SPOILED WITH THE SHORT CODE.GOOD LUCK

[krfrea]

Thank you guys for all your help. I managed to get the holes done and they came out perfect. When I get time I plan on using the changes and ideas from you and writing a program so when I need a hole all I have to do is enter the R etc.

thanks again, Ken