How do you counterbore?

[cyclestart]

Counterbores for smallish SHCS's, half inch SHCS and less.
Assumes a tool isn't available to simply plunge to correct size.

Pic of option #1. It's a canned cycle on most controls probably. The line represents center of tool path.

Edit/ Assume the bolt hole has been drilled before counterboring

[skullworks]

Yeah thats how I do it.

I use a G13 when available, (G3xx on Okuma, I forget the exact code)

From the look of your screen shot I should hurry up and port my G13 macro ( For FANUC's which DON"T support G13 ) to an EMC2 Osubcode.

[cyclestart]

Originally Posted by skullworks From the look of your screen shot I should hurry up and port my G13 macro ( For FANUC's which DON"T support G13 ) to an EMC2 Osubcode.

Caught me! Should have cropped that screenshot
It would be great if the emc interpretor had a canned cycle for this routine. If you have a macro, post it somewhere. Sharing is caring

There is an ulterior motive to this poll. I've been writing a few gcode generators for users of various experience levels. The c'bore module already does options 1 & 2. Been debating whether to include option #3. The fear is inexperienced users may get into a world of hurt with extreme ramp angles. Maybe #3 should be included with a warning attached.

For those who chose option #3; what ramp angles are you using? Assume the types of EM's generally used by hobbiests.

[skullworks]

Originally Posted by cyclestart Caught me! Should have cropped that screenshot Been debating whether to include option #3. The fear is inexperienced users may get into a world of hurt with extreme ramp angles. Maybe #3 should be included with a warning attached. For those who chose option #3; what ramp angles are you using? Assume the types of EM's generally used by hobbiests.

I was brought up in the trade with the understanding that the whole spiral ramp method was a psydo kludge, a way to skip drilling and get a non-centercutting insert type endmill to depth. It takes longer than a center plunge, loads all 3 axis, and doesen't cut as freely. Hitler lost the war fighting on 2 fronts, the same applies to endmilling on a less than rigid hobby type machine.

Also of note: "Economical" HSS 4 flute EM's, even when of the "center cutting" type don't have great chip ejection even with flood coolant and tend to load up.

As to ramp angle my rule of thumb has been to use 5% of the cutter radius as the max infeed per 360°. But again, spiral ramping is not one of my preferred methods.

Maybe let your macro tool calc the ramp & number of helical passes to get to the requested depth. Then if the user so decides they can edit the final code.

[cyclestart]

Originally Posted by skullworks Hitler lost the war fighting on 2 fronts, the same applies to endmilling on a less than rigid hobby type machine.

Yep, the flexi-flier factor can't be ignored. The software must work with desktop size machines.

Also of note: "Economical" HSS 4 flute EM's, even when of the "center cutting" type don't have great chip ejection even with flood coolant and tend to load up. As to ramp angle my rule of thumb has been to use 5% of the cutter radius as the max infeed per 360°.

My thoughts were to allow the user to enter a ramp angle. As the tool size approachs the target size, any other method could result in high ramp angles. Hmm, the clogging ... looks like some test runs will be needed.

But again, spiral ramping is not one of my preferred methods.

Back in the day I used option #1, sometimes option #2 on Milltronics. Judging by the poll this might be old school thinking. Then again I am old. Another birthday today as a reminder

[snowshovelbmx]

I helix almost all my holes that I can't just plunge to size almost all the time, with great results! as for ramp angle I like to use the ramp depth method instead and just pick the pitch the helix, I think that it is a lot easier to think of how much the cutter is actually cutting that way.