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
toggle quoted message
Show quoted text
On 8/11/2022 10:37 AM, Jerry Lee Marcel wrote:
Le 11/08/2022 ¨¤ 15:54, John Blanchard a ¨¦crit?:
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.
|
Le 11/08/2022 ¨¤ 15:54, John Blanchard a ¨¦crit?: 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.
|
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.?
|
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)?
|
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
|
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.
?
Gru?
Harald
___________________
?
|
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
toggle quoted message
Show quoted text
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
_____________________
|
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 _____________________
|
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
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.
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¡ã 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¡ã 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?
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:
|
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.
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¡ã 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¡ã 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?
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:
|
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
|
This release implements Harald's code to always conventional mill, leaving better edges.
Thanks Harald!
Please test if you can.
Regards,
John
|
toggle quoted message
Show quoted text
On Aug 5, 2022, at 6:18 PM, John Johnson <john@...> wrote:
?
Hello Folks,
This addresses , where the spot drill depth was used for the
second and subsequent drill holes.
I've marked it as a prerelease, and would appreciate if some of
you could test it and let me know how it goes.
I ran a simulation using (pretty impressive!)
and it looks good. If you get the settings just right, you can see
the spot drills that just mark the board, then the thru-holes
after drilling. I also added the project files for the simulations
to this release.
Thanks,
JJ
 
|
Hello Folks,
This addresses , where the spot drill depth was used for the
second and subsequent drill holes.
I've marked it as a prerelease, and would appreciate if some of
you could test it and let me know how it goes.
I ran a simulation using (pretty impressive!)
and it looks good. If you get the settings just right, you can see
the spot drills that just mark the board, then the thru-holes
after drilling. I also added the project files for the simulations
to this release.
Thanks,
JJ
 
|
[pcbgcode:master] New Comment on Issue
By :
Sorry I couldn't get to this.
I'm assuming this has been resolved. Feel free to open a new issue if not.
[pcbgcode:master] Issue closed by .
|
[pcbgcode:master] New Issue Created by :
Eagle Ver 9.6
PCB_GCODE ver 3.6.3
Repeatable: Yes.
Requesting drill only:
First hole is OK, subsequent holes use the "Spot Drill" depth. This is a snippet from drill file.
Workaround: Make the "Spot Drill" depth the same as "Drill Depth". And don't forget to return to correct value for "Spotting" while requesting Outlines.
Regards, M.
[pcbgcode] New branch was created by JohnAtl.
1 New Commit:
[pcbgcode:master] By Johnson, John T <john.johnson@...>:
: Ignore the eagle bundle I might be working on.
Modified:
|
[pcbgcode:master] reported: When generating drill file, first drill OK. Remaing drills use "Spot Drill" depth?
#github
[pcbgcode:master] New Comment on Issue
By :
"... and we have to wait for Johns solution."
Good idea.
Regards, M.
|
[pcbgcode:master] reported: When generating drill file, first drill OK. Remaing drills use "Spot Drill" depth?
#github
[pcbgcode:master] New Comment on Issue
By :
Hi M.!
Your files seem been edited correctly to me.
As far as I remember, the problem addressed with Alexanders amendments, is, that if "spot drill" and "drill holes", respectively, are selected both, then the spot drills are executed with the depth defined for drilling the holes.
Whether these problems occur with two sided boards or only with one sided ones, I don't know. I didn't dig into it deeply.
I had those problems with one sided boards and the amendments of Alexander fixed the problem for me.
If your problem isn't solved with Alexanders amendments, then probably you found another problem in the code and we have to wait for Johns solution.
Harry
|
[pcbgcode:master] reported: When generating drill file, first drill OK. Remaing drills use "Spot Drill" depth?
#github
[pcbgcode:master] New Comment on Issue
By :
Hi Harry,
I'm not sure that the two problems are the same?
Using ver-3.6.3 (and previously ver-3.6.2.4) if I select "Generate bottom outlines" AND "Spot drill holes" I found no problem with the spotted points that were made. As far as I could tell the points were cut to the correct depth (0.2mm in my settings) by the V-Engraver after the track outlines were cut. i.e. both tasks were in the *.etch gcode file.
My problem, is different. If I select "Generate bottom (or top) drill" ONLY. The drill file will drill the first hole correctly but the rest will only be to the depth specified in the "Spot drill holes depth" field.
Lastly, just to be sure, I made the amendments described on your web page. As far as I could tell with the limited testing, I could detect no difference in the gcode output with or without these amendments! Now, it is highly likely that I have not done them correctly but I have attached them below in the hope that you could check them for me.
Regards, M.
|
[pcbgcode:master] New Comment on Issue
By :
Hi M.!
You might try the fix from Alexander Arkusha explained on my .
The fix is described as second topic on this page.
Please keep an eye on the line numbers, perhaps you and I refer to different vesions of pcb-gcode.
But given the context, you will find the correct lines, where to change the code.
Harry
[pcbgcode:master] New Comment on Issue
By :
Hi M.!
You might try the fix from Alexander Arkusha explained on my .
The fix is described as second topic on this page, starting with
"A further improvement over the original version was suggested by Alexander Arkusha in the end of 2017."
Please keep an eye on the line numbers, perhaps you and I refer to different vesions of pcb-gcode.
But given the context, you will find the correct lines, where to change the code.
Harry
|
John Johnson
