¿ªÔÆÌåÓý

ctrl + shift + ? for shortcuts
© 2025 Groups.io
  1. Pcbgcode
  2. Topics

Helical milling drill holes with endmill #pcbgcode #drill #helical

 

¿ªÔÆÌåÓý

JJ,
Now if only real world tests go as smoothly as the simulation show!
Like the video and this will be a great addition to the software.

Also, please include me for alpha testing.

Thanks in advance.

Country


On 8/12/2022 5:10 PM, John Johnson wrote:

Here's a I ran on a test board.

The rack file looks like this. E means end mill, T is a standard drill.
step is the amount to step over in x,y, and step_z is the amount to step down in z.

This strategy mills from the center out at increasing depths.

Helical at the max diameter is a possibility too - for another day.

#tool??? drill_size??? minimum??? maximum??? length??? step??? step_z
T01??? 0.015in??? 0.001in??? 0.031in??? 1.5in
T02??? 0.032in??? 0.032in??? 0.035in??? 1.5in
E03??? 0.032in??? 0.035in??? 0.124in??? 1.5in??? 0.010in??? 0.015in
E04??? 0.125in??? 0.125in??? 0.375in??? 1.5in??? 0.030in??? 0.030in

If you're interested in alpha testing, let me know. Alpha software is not for circulation to others.

Let me know what you think of the video.

Regards,
JJ

On 8/10/22 2:45 PM, John Johnson wrote:

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?
      • Sounds reasonable.
    • 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



Attachments:
 

On Fri, Aug 12, 2022 at 11:11 PM, John Johnson wrote:
If you're interested in alpha testing, let me know. Alpha software is not for circulation to others.
Hi John,
please provide me with the Alpha version.
I will test it on my mill, but it may take me a few days to get to it.
?
--
Harald
_____________________
 

¿ªÔÆÌåÓý

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:

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?
      • Sounds reasonable.
    • 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

21 - 23 of 23