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


John Johnson
 

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 (TurboCNC (happy to see TCNC is still around!), Mach3, grbl, LinuxCNC, 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° 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




Art Eckstein
 

JJ,
You know I couldn't leave this one alone, so find my comments interspersed below.
Further, its great to see you posting on a regular basis again.
Now on with the thoughts of a weak mind.

On 8/10/2022 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?
Most definitely as this will allow a reduction in tool requirements. Again, we are talking PCBs and not general machining, so we probably have a small end mill or two already in our crib. Lots of times, we will have a one off hole size that doesn't justify the expense or time to get a specialized cutter or drill (which may not fit in the collet or chuck of our machine).
  • 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 (TurboCNC (happy to see TCNC is still around!), Mach3, grbl, LinuxCNC, etc.), so make it as generic as possible.
Yep, turbocnc is still the only cnc controller that I will run! Over the years, I have been able to customize it to do things that the box stock compile will not do. Its now been over twenty years that I settled on that program and still love it.
    • I'm thinking G03 (counter clockwise) for all holes.
For what we are doing, I am not sure it makes a difference, but there will be people who disagree with me on which direction of cut is best. So be it. Your choice.
    • From what I've read, using IJ is preferable over R, and I recall from my experience R arcs can get whacky.
Definitely use IJ instead of R and you will also be able to do full 360° moves. If you use R, and try major arcs, it doesn't know which direction to go as the results are infinite. 
    • I'm thinking 4x 90° arcs to make a circle. Again, to accommodate as many controllers as possible.
To the best of my knowledge, if your using IJ arcs, I know of no controller that will need a full circle to be broken up into segments. Again, somebody may prove me wrong. If so, I will learn something new.
  • 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.
On this one, because we are again talking PCBs and not thick metal and typically speaking relatively small holes (say typically <.375" (10mm) this will not be a problem and the "dot" will fly out of the way. On a larger scale, think about milling the outline of a pcb from parent stock. If its that big, hold it down with a pencil or something until its done. In our machines, we are not talking super fast cutting speeds any how! 
    • 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.
Yep, another way to handle it but at the expense of time. Been there done that with normal cnc milling metal projects.
  • 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.
At the risk of being to conservative, either add a new variable or just set it to something like 10% of cutter dia? Again thinking we are dealing with small cutters to begin with. I am basing this on my machine, where all my tools have 1/8" dia shank cutters and no choice for anything else.
    • 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.
See above.
  • 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.
From a cursory review, looks good to me.

Would appreciate your input and expertise!

Regards,

JJ

Country



Attachments:



joeaverage
 

Hi,

"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've been doing this for years. I use a 1.5mm diameter endmill to cut around the perimeter of the board. Any hole 1.5mm or more in diameter I use a circular

interpolation path, and that is provided by the arc feature of PCB-Gcode, and I have used it extensively for eight years.


Note that the circle feature does not work, but the arc feature does. Select the arc feature, select the 46 Milling layer, select the diameter of the tool, in my case 1.5mm

and draft an arc, usually one half a circle, then repeat the procedure for the remaining half of the circle.


I prefer to cut all the holes over 1.5mm diameter in this manner and ONLY THEN mill around the perimeter of the board. It means that while the holes are being milled

the PCB is still held perfectly stationary by the alignment pins.


This uses features that already exist and can be incorporated into your design now, nothing extra required. 


Craig



From: pcbgcode@groups.io <pcbgcode@groups.io> on behalf of Art Eckstein <art.eckstein@...>
Sent: Thursday, 11 August 2022 9:45 am
To: pcbgcode@groups.io <pcbgcode@groups.io>
Subject: Re: [pcbgcode] Helical milling drill holes with endmill #pcbgcode #drill #helical
 
JJ,
You know I couldn't leave this one alone, so find my comments interspersed below.
Further, its great to see you posting on a regular basis again.
Now on with the thoughts of a weak mind.

On 8/10/2022 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?
Most definitely as this will allow a reduction in tool requirements. Again, we are talking PCBs and not general machining, so we probably have a small end mill or two already in our crib. Lots of times, we will have a one off hole size that doesn't justify the expense or time to get a specialized cutter or drill (which may not fit in the collet or chuck of our machine).
  • 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 (TurboCNC (happy to see TCNC is still around!), Mach3, grbl, LinuxCNC, etc.), so make it as generic as possible.
Yep, turbocnc is still the only cnc controller that I will run! Over the years, I have been able to customize it to do things that the box stock compile will not do. Its now been over twenty years that I settled on that program and still love it.
    • I'm thinking G03 (counter clockwise) for all holes.
For what we are doing, I am not sure it makes a difference, but there will be people who disagree with me on which direction of cut is best. So be it. Your choice.
    • From what I've read, using IJ is preferable over R, and I recall from my experience R arcs can get whacky.
Definitely use IJ instead of R and you will also be able to do full 360° moves. If you use R, and try major arcs, it doesn't know which direction to go as the results are infinite. 
    • I'm thinking 4x 90° arcs to make a circle. Again, to accommodate as many controllers as possible.
To the best of my knowledge, if your using IJ arcs, I know of no controller that will need a full circle to be broken up into segments. Again, somebody may prove me wrong. If so, I will learn something new.
  • 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.
On this one, because we are again talking PCBs and not thick metal and typically speaking relatively small holes (say typically <.375" (10mm) this will not be a problem and the "dot" will fly out of the way. On a larger scale, think about milling the outline of a pcb from parent stock. If its that big, hold it down with a pencil or something until its done. In our machines, we are not talking super fast cutting speeds any how! 
    • 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.
Yep, another way to handle it but at the expense of time. Been there done that with normal cnc milling metal projects.
  • 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.
At the risk of being to conservative, either add a new variable or just set it to something like 10% of cutter dia? Again thinking we are dealing with small cutters to begin with. I am basing this on my machine, where all my tools have 1/8" dia shank cutters and no choice for anything else.
    • 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.
See above.
  • 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.
From a cursory review, looks good to me.

Would appreciate your input and expertise!

Regards,

JJ

Country



Attachments:



Harald
 

Hi John,

as of my point of view, this feature would be highly appreciated.
In the past (and obviously still...) I drill holes on the CNC mill all with the 1 mm drill bit I use for through hole parts and lastly take the board to my drill press and drill the final diameter with a borer of fitting diameter.

I cannot follow Art Eckstein on leaving the dot in the middle of bigger holes alone.
Thinking of something bigger, let's say a 10 mm hole, using the mentioned 1,5 mm endmill, the remaining dot will probably interact in some way with the endmill.
So I would prefer digging into the board beginning in the middle and carving outwards (you proposed this as "sort-of center-out strategy").

There exists a german tool named Estlcam. This tool already has this feature implemented (for standard milling jobs) and it performs well in milling holes and planes. From there I know, that the the answer to your question:
What about increasing the diameter if concentric holes or multiple passes are used?
should be "not more than 45% to prevent remainders on some curvatures". Perhaps this is not true for circles only? Don't know.
--

Harald
_____________________


joeaverage
 

Hi, 
many of the holes I mill are 3.2mm diameter and bigger, ie they leave a little divot....so what, it still works.
I hold the PCB blank down with double sided tape and the little divot mostly stays in place, but even if it comes loose
it presents no problems. I did three 6mm diameter holes today without problem.

Craig

From: pcbgcode@groups.io <pcbgcode@groups.io> on behalf of Harald <harry0099@...>
Sent: Thursday, 11 August 2022 9:23 pm
To: pcbgcode@groups.io <pcbgcode@groups.io>
Subject: Re: [pcbgcode] Helical milling drill holes with endmill #pcbgcode #helical
 
Hi John,

as of my point of view, this feature would be highly appreciated.
In the past (and obviously still...) I drill holes on the CNC mill all with the 1 mm drill bit I use for through hole parts and lastly take the board to my drill press and drill the final diameter with a borer of fitting diameter.

I cannot follow Art Eckstein on leaving the dot in the middle of bigger holes alone.
Thinking of something bigger, let's say a 10 mm hole, using the mentioned 1,5 mm endmill, the remaining dot will probably interact in some way with the endmill.
So I would prefer digging into the board beginning in the middle and carving outwards (you proposed this as "sort-of center-out strategy").

There exists a german tool named Estlcam. This tool already has this feature implemented (for standard milling jobs) and it performs well in milling holes and planes. From there I know, that the the answer to your question:
What about increasing the diameter if concentric holes or multiple passes are used?
should be "not more than 45% to prevent remainders on some curvatures". Perhaps this is not true for circles only? Don't know.
--

Harald
_____________________


Harald
 
Edited

Hi Craig,

ok, so perhaps I’m too tentative?

I had such problems when milling the outer circumferences of my boards, but they where mostly rectangular. That may imply a difference.

 

Gruß

Harald

___________________

 


John Blanchard
 

All great ideas.

Now I drill all holes the same and use hand reamers to enlarge component holes and larger drills for mountiing hole.

My only suggestion is to ramp into the PCB rather than plunge. I use 0.8mm endmills and they break very easily.

The vernacular I'm familiar with refers to milling the perimeter of a hole as a profile and milling the hole from the inside out as a pocket. Pockets can also be milled using either conventional or trochoidal milling. The latter uses more of the side of the endmill while "conventional" milling uses more of the tip. I doubt the trochoidal approach would have any benefit for such small holes and would be more likely to break such tender endmills.

Thank you for your efforts.

John


John Johnson
 

On 8/11/22 9:03 AM, John Blanchard wrote:
I doubt the trochoidal approach would have any benefit for such small holes and would be more likely to break such tender endmills.
So clockwise (G02)?


John Blanchard
 

I may have introduced some confusion by referring to non trochoidal milling as "conventional". The normal definition of conventional milling is to move the tool opposite to the direction of the cutting edge while climb milling moves tool in the same direction as the cutting edge. Climb milling is likely to add additional side force to the tool and would not be the best choice for small delicate endmills. So assuming clockwise tool rotation I believe G03 would be less likely to break the tool but I have not tested the difference with small endmills..

I would also vote for a spiral profile tool trajectory. Something like this:

G3 F100.0 X0.10938 Y-0.02706 Z-0.01 I-0.03125 J0.0
G3 Y0.02706 Z-0.02 I0.01563 J0.02706
G3 X0.15625 Y0.0 Z-0.03 I0.01563 J-0.02706
G3 X0.10938 Y-0.02706 Z-0.04 I-0.03125 J0.0
G3 Y0.02706 Z-0.05 I0.01563 J0.02706
G3 X0.15625 Y0.0 Z-0.06 I0.01563 J-0.02706
G3 X0.10938 Y-0.02706 Z-0.07 I-0.03125 J0.0
G3 Y0.02706 Z-0.08 I0.01562 J0.02706
G3 X0.15625 Y0.0 Z-0.09 I0.01563 J-0.02706
G3 X0.10938 Y-0.02706 Z-0.1 I-0.03125 J0.0
G3 Y0.02706 Z-0.11 I0.01563 J0.02706

This is a segment of the code to drill a 0.25" hole with a 3/17" endmill. 


Jerry Lee Marcel
 

Le 11/08/2022 à 15:54, John Blanchard a écrit :
I may have introduced some confusion by referring to non trochoidal milling as "conventional". The normal definition of conventional milling is to move the tool opposite to the direction of the cutting edge while climb milling moves tool in the same direction as the cutting edge.
I believe it's the exact contrary. In conventional the cutter speed is in the same direction as the feed.

https://www.harveyperformance.com/in-the-loupe/conventional-vs-climb-milling/

Climb milling is likely to add additional side force to the tool and would not be the best choice for small delicate endmills.
Climb milling is traditionally used for finishing because it generates less forces.


Harvey White
 

Climb milling requires a more sturdy setup.  The tool tends to "climb" out of the cut, and force either the cutter or the work away from each other.  If the work holding is loose enough, then the cutter can move enough to get out of track (it wants to, anyway).

Conventional milling tends to force the cutter deeper into the work.

The solution for this is to have a very secure setup and take very light cuts when climb milling.  If working on milling a pocket, the rough cuts are generally conventional milling, with the final cuts (finishing) being climb milling at a very shallow cut.

Harvey

On 8/11/2022 10:37 AM, Jerry Lee Marcel wrote:

Le 11/08/2022 à 15:54, John Blanchard a écrit :
I may have introduced some confusion by referring to non trochoidal milling as "conventional". The normal definition of conventional milling is to move the tool opposite to the direction of the cutting edge while climb milling moves tool in the same direction as the cutting edge.
I believe it's the exact contrary. In conventional the cutter speed is in the same direction as the feed.

https://www.harveyperformance.com/in-the-loupe/conventional-vs-climb-milling/

Climb milling is likely to add additional side force to the tool and would not be the best choice for small delicate endmills.
Climb milling is traditionally used for finishing because it generates less forces.





John Blanchard
 

I stand corrected. Thank you for the clarification. The picture makes it much more clear.

I got the direction wrong so I guess G02 is preferred?


Harvey White
 

I think that the direction depends on the stage of the operation.

The tolerances depend on the cutting tool, the rigidity of the setup (unimat NOT rigid, Seig X2 much better, Bridgeport no problem), and the material being cut (not only hardness but how smoothly it cuts).

Were this metal machining (and cutting a pocket in, say, aluminum, T6063), I would use conventional milling to within a certain distance, as a guess, I'd say about 25 thousandths.  I'd switch to climb milling and take off  no more than 5 thousandths each pass.

Now, PC boards?  Lots less experience.  Assuming a 1/16th board, and a 1/8 carbide roughing tool, you don't want to take off more than 1/4 of the width of the bit (IMHO), so about 32 thousandths per cut, then go down to the usual 5 thousandths or so (rather conservative perhaps) for the final passes.

The numbers are guesses, and I'd want to refine them under actual practice, but there they are.  Someone with more experience would be able to provide more accuracy.

Harvey


On 8/11/2022 2:24 PM, John Blanchard wrote:

I stand corrected. Thank you for the clarification. The picture makes it much more clear.

I got the direction wrong so I guess G02 is preferred?


mariob_1960@...
 
Edited

Hello people.
my opinion:
1- G2 and G3 can be used with R without problems (two 180° arcs) or I J mode (my Trochoidal 3d bCNC plugin uses R, without problem after years)
2- If the cut of the circle is to generate a cut of the material, I do not see it as essential to make a pocket
3-if pocketing, option a) by discrete jump to next circle (40% overlap?) or b) enlarge in spiral movement (it will always keep a lateral cut, in the other mode, each step to next circle is a slot ). I prefer spiral.
4- I think G3 generates a better finish (finish on the material on the left side of the cutter). Add option box CW - CCW?
5-Select descent step per lap (pitch). Flat final pass.
Perhaps this repeats other opinions: my English is terrible.
hugs, Mario


joeaverage
 

Hi,
as I have already posted any hole over 1.5mm diameter I use circular interpolation. Given that I use 1.5mm endmill for this purpose its fine to plunge and cut to full depth of the PCB at full speed (600mm/min) in one pass. That would fail with smaller diameter tools.

I do have, and use 0.8mm endmills, but have and use many 0.5mm endmills (Kyocera Tycom). I now seldom use them for PCB manufacture however I use them to bore holes in fractional sizes for which I do not have a drill. In particular drilling the hole to install a pointer on a meter shaft. If the shaft is 0.6mm in diameter (some Nissan tachometers for instance) then I need to bore
a hole 0.57mm to 0.58mm in order for the plastic of the pointer boss grip the shaft. For this purpose I would use 0.5mm endmill and a helical interpolated path.

Standard endmills are typically three times longer than their diameter. In the case of my 0.5mm endmills the flute length is 1.5mm. Thus drilling a 1.5mm PCB is about as much as it could handle without the flare of the tool fouling the top of the hole. I use Fusion and/or MachMill to generate the tool path for the helical milling. This is a toolpath for a 0.75mm hole 2.5mm deep:

(posted for Brass )
(Strategy: Equal )
(Rapid height: 2.0000  Clearance height: 1.0000 )
G98 G80 G17 G90 G54 G64 G91.1

G21 G90
(***New Tool Selected***)
(ToolNum: 21  Diameter: 0.5000  )
(Feed: 240.0000  SFM: 168.0000  Plunge: 120.0000  ChipLoad: 0.0050  )
M06 T21 (0.5mm EndMill)
G43 H21
M03 S24000
(***Cut Circle***)
(Inside)
(Xorign: 0.0000  Yorign: 0.0000  Dia: 0.7500 Dir: 01  )
(Ztop: 0.0000  Zdepth: -2.5000  Zstep: 0.8333 )
(will make  3.0000  cuts of:  0.8333 )
G00 Z2.0000
X0.1250 Y0.0000
Z1.0000
G01 Z0.0000 F120.00
G00
G03 Z-1.0000 I-0.1250
Z-2.0000 I-0.1250
X-0.1250 Y0.0000 Z-2.5000 I-0.1250
X0.1250 Y-0.0000 I0.1250 J-0.0000 F240.00
X-0.1250 Y0.0000 I-0.1250 J0.0000
X-0.0625 Y-0.0625 I0.0625 J-0.0000
G00 Z2.0000
M09
M05
M30 (end of file)

It helically interpolates down in two 1mm deep steps, followed by one 0.5mm deep helical path at a cut speed of 240mm/min. In harder materials, this was meant for brass, a less aggressive cutting strategy is required. 

This path was generated by MachMill, nothing special. I can choose to mill a pocket or as in this case just on the inside of the circle. With a diameter of 0.75mm there would be no divot and therefore a pocket is not required. I have found no appreciable difference in climb or conventional milling, either being selectable. The good thing is that it takes two, maybe three minutes to generate this path at my machine and the job takes less than thirty seconds. It takes longer to set the part in the work holding and touch off than it does to generate the path and do the job.

I have used this and many similar toolpaths in plastic, brass and aluminium, and would suggest that anyone wishing to experiment with helically interpolated toolpaths use it as a starting point.

Craig


From: pcbgcode@groups.io <pcbgcode@groups.io> on behalf of mariob_1960 via groups.io <mariob_1960@...>
Sent: Friday, 12 August 2022 7:00 am
To: pcbgcode@groups.io <pcbgcode@groups.io>
Subject: Re: [pcbgcode] Helical milling drill holes with endmill #pcbgcode #helical
 

[Edited Message Follows]

Hello people.
my opinion:
1- G2 and G3 can be used with R without problems (two 180° arcs) or I J mode (my Trochoidal 3d bCNC plugin uses R, without problem after years)
2- If the cut of the circle is to generate a cut of the material, I do not see it as essential to make a pocket
3-if pocketing, option a) by discrete jump to next circle (40% overlap?) or b) enlarge in spiral movement (it will always keep a lateral cut, in the other mode, each step to next circle is a slot ). I prefer spiral.
4- I think G3 generates a better finish (finish on the material on the left side of the cutter). Add option box CW - CCW?
5-Select descent step per lap (pitch). Flat final pass.
Perhaps this repeats other opinions: my English is terrible.
hugs, Mario


John Johnson
 

I'd forgotten how tedious and terrible development is without a debugger and the ability to step through code and inspect variables 🙁

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 (TurboCNC (happy to see TCNC is still around!), Mach3, grbl, LinuxCNC, 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° 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




Harald
 

More or less like working with Arduino... Possible but without great fun 😉
--

Harald
_____________________


John Johnson
 

You nailed it!

On 8/12/22 8:23 AM, Harald wrote:

More or less like working with Arduino... Possible but without great fun 😉
--

Harald
_____________________


Harald
 

Ok, I cheated :-)
For Arduino I have Visual Micro on hands, so I can debug the code in some way. Not that I have much practice with it, but programming Arduino with all capabilities of the Visual Studio IDE is a fine thing, truely.
--
Harald
_____________________


John Johnson
 

Here's a video of a simulation 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 (TurboCNC (happy to see TCNC is still around!), Mach3, grbl, LinuxCNC, 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° 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