Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: Merlin1965 on April 10, 2020, 07:45:21 AM
-
Hi Guys
I'm New to G Code ...but learning Fast
Have 3 Axis Cincinnati Mill i converterd to Stepper motors and Mach 3 ....Works like Charm
I have a M16 x 75 mm roughing end mill and need to create a 137 mm dia x 20 mm deep pocket in an ally block
My thoughts go like
Plunge cut to z 20mm the step out in radius to 137mm
Issue ...I need to oscillate the end mill down to 20 mm as the flutes do not go to the center of the tool
The Plunge hole could be 22mm ..no issue
Q What G code should i use to get the XY loop and Z plunge ??
John P
-
Not much help but that type of end mill was never intended for plunge cut and really does not make a very good job if forced to do it. Best option is to purchase the right tool, sometimes sold as slot drill, which has an end flute going to the centre. Just my 2 cents :)
Tweakie.
-
Hi,
Tweakie is right, get an end cutting endmill.
I use MillWizard ($75) from NFS. When it generates code to say create a pocket it ramps down to the depth
rather than just plunge. May I suggest download and experiment with it and you will see the code used to
enact the ramp down.
Note also that most if not all CAM programs offer different strategies to ram an endmill down to depth.
Craig
-
Assuming, the hole has no tolerance and the cutter runs true you could do something like this, centre of hole is 0/0 and top face is Z0
G00 G90 X60.5 Y0 Z25. S2000 M3
Z1.
G01 Z0 F100.
G03 I-60.5 Z-4.
I-60.5 Z-8.
I-60.5 Z-12.
I-60.5 Z-16.
G01 X55.
G03 I-55.
G01 X50.
G03 I-50.
G01 X45.
G03 I-45.
G01 X40.
G03 I-40.
G01 X35.
G03 I-35.
G01 X30.
G03 I-30.
G01 X25.
G03 I-25.
G01 X20.
G03 I-20.
G01 X15.
G03 I-15.
G01 X10.
G03 I-10.
G01 X7.
G03 I-7.
G01 X0
G00 Z25.
M30
-
Thanks for you response guys
I do have 3 flute end mills/ slot drills that will plunge and did use them to complete my task
But i have a couple of 16 mm roughing cutters ...just means i can run a higher cut/feed speed
Thanks the code Graham
my intention was to cut say a 20 to 22 mm hole with 16 mm roughing end mill with a fast oscillation and slower plunge
then expand the hole out
John P
-
Working from the large diameter and ramping in you can use none end cutting tool as the ramp angle is shallow that is why the gcode is written that way.