[Blosser5]

Can someone tell me how to program for Helical Boring, We currently drill then rough bore using either a Carbide ins. mill or carbide mill in steps. Say we have a two inch bore, we will rough it with the CIM stepping down .125 each pass(way slow in my book). I have watched a few HSM videos and see where we could be doing this by boring down in a helical patern without the step up each pass. We are using(severly outdated) solutionware Geopath software for our Fadal 4020s but believe that the programing would be very similar. I am fairly new to the programming, but have a pretty good grasp on it and am just tired of the old saying "Thats the way we have always done it". Time is money and if I can save 5 to 10 minutes per part it would really helpful. Thanks anybody and everybody!

[SORCHEROR]

with helical boring the program is usually quite large and not always faster then stepping
depends on your tooling and machine,most people use helical boring not for speed,but for better finish and less wear and tear on the tool,you say you drill it first,why not drop all the way down with the endmill and walk out wards .01-.02 a pass and than a few zero finish passes,i not sure what material your cutting or how deep,but this would be fastest way and simple to program

[Geof]

It does depend on your machine I think. I program on Haas and helical boring or interpolation is a single line command:

G91 G03 I0. J-.5 Z-.2 F10. L10

Does ten circles moving down .2" per circle for a total of 2.0". To do a 1" bore 2 inches deep using tool comp with the work zero at the center of the hole and the tool offset at the top of the part the complete set of commands is;

G41 D01 Y0.5 Z0.01 (this moves to the radius and just above the part)
G91 G03 I0. J-0.5 Z-02. F10. L10 (this does the ten circles down to 1.99" deep)
G90 G03 I0. J-0.5 Z-2.0 L2 (this moves down to the 2" depth and removes the bottom of the helical ramp and does a spring pass)
G40 G00 Y0. Z1. (this cancels tool comp and retract clear of the part)

[Blosser5]

Say we are doing the two inch bore using a 3 fluted carb. Ins. Mill. Material is CRS 1/2" thick. What are the ideal speeds and feeds for the stepping process? We run right around 3000 rpm and feed at 10 IPM 4 passes. When doing multiple parts this becomes a very tedious run, thus wanting to speed up the process by eliminating the center drill and drill. Rember this is a Fadal 4020, Leader of the slowest tool changes known to man.... I can change tools faster on a manual...ha, ha, ha. So on helical boring, do I want to use advanced ramp down, If so what do I put in for Zig? or is this just the wrong command when writing the cutting process?
All in all Just tired of crawling and wanting to run!

[ctate2000]

Forgot the material so fill in speed and feed as appropriate. Helical is the way to go. For a FADAL 1.0 dia tool. I would use a three flute carbide emill or indexable. Blast the hole with coolant to clear away chips.

Hole at X0 Y0

GOX0Y0E1
Z.1H1D1
G1Z.010F20.
G1G41X1.0Y0
G2X1.Y0I-1.Z-.125
G2X1.Y0I-1.Z-.250
G2X1.Y0I-1.Z-.375
G2X1.Y0I-1.Z-.500
G2X1.Y0I-1.Z-.562
G2X0Y0I-.5
G40
G0Z0H0M5M9