开云体育

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° 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

开云体育

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.

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 ( (happy to see TCNC is still around!), , , , 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:

• Screen Shot 2022-08-10 at 2.06.57 PM.png
• Screen Shot 2022-08-10 at 2.06.42 PM.png
• newfile.nc
• newfile.camotics

开云体育

---

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
_____________________

开云体育

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

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)?

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:

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.

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.

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

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?

开云体育

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

开云体育

开云体育

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

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

Harald
_____________________

开云体育

You nailed it!

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
_____________________

开云体育

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