Hello Folks,
Here are some details about the logic of hole milling:
- If the hole size is smaller than the endmill, and between the
endmill's minimum and maximum as set in the rack file, the
endmill is used as a drill, and just drills the hole (no
pecking).
- If the hole size is larger than the endmill, the hole will be
milled as you have selected in pcb-gcode-setup:
- Concentric
- Begin in the center, plunge by FEED_ETCH_Z (Machine tab,
Feed Rates, Etch, Z)
- Feed +x to step_xy (as set in the rack file).
- Feed clockwise by FEED_RATE_ETCH_XY in an arc to the
left side of the hole
- Feed clockwise by FEED_RATE_ETCH_XY in an arc to the
right side of the hole
- Repeat until at hole diameter (- tool offset)
- Return to hole center
- Repeat until at hole depth (Machine tab, Z Axis, Drill
Depth)
- Helical
- Begin at right side of hole (- tool offset)
- Feed clockwise by FEED_RATE_ETCH_XY in an arc to the
left side of the hole, and in z-axis to step_z/2 (set it
rack file)
- Feed clockwise by FEED_RATE_ETCH_XY in an arc to the
right side of the hole, and in z-axis to step_z (set it
rack file)
- Repeat until at hole depth
- (clean up remainder at bottom from interpolation)
- Feed to hole depth
- Feed clockwise by FEED_RATE_ETCH_XY in an arc to the left
side of the hole
- Feed clockwise by FEED_RATE_ETCH_XY in an arc to the right
side of the hole
Here's a video of how helical hole milling is treated.
Art and Harald are alpha testing, let me know if you want in on
the fun!
Regards,
JJ
On 8/10/22 2:45 PM, John Johnson wrote:
toggle quoted message
Show quoted text
Hello Folks,
I've been thinking about and working on the long-requested (ca.
2018) feature that would let one mill holes of different
diameters using an endmill.
I would like your input.
- Is this useful?
- Do let me know if you have suggestions on gcode. My
knowledge on this is limited. I would like to support as many
controllers as possible ( (happy to see
TCNC is still around!), ,
, ,
etc.), so make it as generic as possible.
- I'm thinking G03 (counter clockwise) for all holes.
- From what I've read, using IJ is preferable over R, and I
recall from my experience R arcs can get whacky.
- I'm thinking 4x 90¡ã arcs to make a circle. Again, to
accommodate as many controllers as possible.
- I'm concerned about holes that are larger than 2x the tool
diameter.
- For example, in the image attached, the tool is
0.015"/0.381mm and the holes are 0.020"/0.508mm,
0.035"/0.889mm, and 0.050"/1.27mm. There is a 0.005"/0.127mm
post in the center hole, and 0.020"/0.508mm on the
right-hand hole.
- The debris left in the center (see attached pics), which
could potentially become ensnared by and break the tool.
- One way to eliminate this is as two (or more) holes, a
smaller one to full depth, then larger ones.
- This would probably need "pecking."
- I could also use a sort-of center-out strategy, where the
cutter starts in the center, then mills at increasingly
larger diameters until the desired size is reached. Rather
than the helical path shown, I would probably just plunge
some amount in the center, then start milling the concentric
circles at that depth out to the max diameter, plunge at the
center a bit deeper, rinse and repeat.
- How do we control chip load?
- Step down for Z axis as an absolute amount (e.g.
0.25mm/0.010") per pass?
- What about increasing the diameter if concentric holes or
multiple passes are used?
- Could be a fixed maximum, I suppose, or some percentage
of the tool diameter.
- Code that generated the images is attached.
- Let me know what you think about it too. I just generated
it in Excel for the time being.
Would appreciate your input and expertise!
Regards,
JJ
John Johnson