In a moment of being overly generous a few years ago, someone asked if they could register the pcbgcode.com and I agreed. Seventeen minutes later, I regretted it. He was selling some modified version of pcb-gcode, which also didn't sit well. Since 2003, my goal has been for pcb-gcode to be a free tool available to everyone that wanted it.
?I checked this morning and the domain was available again, so I paid the ransom to Network Solutions and bought the domain.
It's still processing, and not active yet (it's only been 5 hours, and you know how slow computers are this century).
Anyway, should be live soon, and I'll probably just forward to the groups group, like pcbgcode.org does, but wanted to share what I think is good news.
ps. the beta of pcb-gcode with hole milling should be available soon. If you're interested in trying the alpha, send me an email. Thanks!
Regards,
JJ
|
Thanks Peter and Harald!
Actually, Textmate isn't that bad. I just added .ulp to the
extensions for C programming language, and it does pretty well.
When I tried it years back, things like:
?? ???? ??? // Process all the wires.
?? ???? ??? B.wires(W) W.pieces(P) {
Would throw all the indentation off if you ran Text | Indent
Selection.
Now the main thing that is kind of wonky are switch / case / break statements, so I
just won't try to format those.
I could probably change the indentation rules for the bundle, but
they are more complex than even pcb-gcode :-)
Thanks,
JJ
On 8/21/22 4:35 PM, peterg1000 via
groups.io wrote:
toggle quoted message
Show quoted text
Hi guys,
For what it's worth the FreeBasic ide? "FBide" will provide a
color highlighted presentation of a .ulp file. Available for
Windows, Mac and Linux so the blurb says.
Peter
|
Hi guys,
For what it's worth the FreeBasic ide? "FBide" will provide a color highlighted presentation of a .ulp file. Available for Windows, Mac and Linux so the blurb says.
Peter
|
Ok, thanks!
--
Harald
_____________________
|
Thanks Harald.
I don't use Windows, but posted a message on the thread. Someone
might have something.
On 8/21/22 11:05 AM, Harald wrote:
toggle quoted message
Show quoted text
Hi John,
just wanted to dig a bit through your code to get some
understanding on this "drill/spot drill" problem, still included
in your Alpha version.
I use Notepad++ for editing/viewing text files and so searched for
a means of syntax highlighting for NP++.
I succeeded here:
I don't know Textmate nor Emacs, but NP++ is worth a try...
HTH
--
Harald
_____________________
|
Hi John,
just wanted to dig a bit through your code to get some understanding on this "drill/spot drill" problem, still included in your Alpha version.
I use Notepad++ for editing/viewing text files and so searched for a means of syntax highlighting for NP++.
I succeeded here:
I don't know Textmate nor Emacs, but NP++ is worth a try...
HTH
--
Harald
_____________________
|
Corrected image. Nothing like hitting Send to bring these things
out.
On 8/20/22 2:05 PM, John Johnson wrote:
toggle quoted message
Show quoted text
Hello Folks,
The question recently came up about how pcb-gcode calculates
it's toolpath, and why pads aren't isolated when there seems to
be plenty of room between.
Hopefully, this will help show how this is done. I'll add this
to the manual at some point (or revise what's there).
Eagle has the ability to create "pours", which are usually used
for things like ground planes. It fills in around areas where
there aren't any tracks, and does this obeying a couple of
parameters that are relevant to this discussion, width, and
isolation.
Width is the size of the line used to draw the polygons that
make up the pour. For our purpose, this is the tool size. By
using tool size as the width, the outer edge of the polygon
becomes the tool path. This saves me from having to do tool
offset myself, which is a pain (especially in inner corners),
and the reason I abandoned a BASIC version I was working on in
another CAD program.
Isolation is a minimal amount that the pour (polygons) should
be from all tracks. This is the minimum isolation parameter in
pcb-gcode-setup.
So here's why the pads you think should be isolated aren't
isolated. As shown in the image below, the total width of
everything between the pads is isolation+width+width+isolation.
To give an example, say you have a 0.1mm tool, and have
minimum isolation set to 0.05mm. The total then is
0.05+0.1+0.1+0.05=0.3mm, which may be larger than the space
between the pads you want to isolate. Technically, yes,
everything might fit, but that would require my (or someone)
writing code to do tool offset, and that's not practical for
me at the moment.
How to work around this?
- Change minimum isolation to 0.0, if
your machine is rigid enough.
- Edit the parts in Eagle and make the
pads smaller (I think it's restring?).
- Use a smaller tool.
- Draw the pad outlines on the milling
layer. Set the line width to the width of your tool to see the
actual tool path.
- Fudge a little on the tool size,
realizing your tracks will be slightly smaller.
Maybe you folks have other workarounds?
Hope this helps!
Regards,
JJ
|
Hello Folks,
The question recently came up about how pcb-gcode calculates it's
toolpath, and why pads aren't isolated when there seems to be
plenty of room between.
Hopefully, this will help show how this is done. I'll add this to
the manual at some point (or revise what's there).
Eagle has the ability to create "pours", which are usually used
for things like ground planes. It fills in around areas where
there aren't any tracks, and does this obeying a couple of
parameters that are relevant to this discussion, width, and
isolation.
Width is the size of the line used to draw the polygons that make
up the pour. For our purpose, this is the tool size. By using tool
size as the width, the outer edge of the polygon becomes the tool
path. This saves me from having to do tool offset myself, which is
a pain (especially in inner corners), and the reason I abandoned a
BASIC version I was working on in another CAD program.
Isolation is a minimal amount that the pour (polygons) should be
from all tracks. This is the minimum isolation parameter in
pcb-gcode-setup.
So here's why the pads you think should be isolated aren't
isolated. As shown in the image below, the total width of
everything between the pads is isolation+width+width+isolation.
To give an example, say you have a 0.1mm tool, and have minimum
isolation set to 0.05mm. The total then is
0.05+0.1+0.1+0.05=0.3mm, which may be larger than the space
between the pads you want to isolate. Technically, yes,
everything might fit, but that would require my (or someone)
writing code to do tool offset, and that's not practical for me
at the moment.
How to work around this?
- Change minimum isolation to 0.0, if your
machine is rigid enough.
- Edit the parts in Eagle and make the
pads smaller (I think it's restring?).
- Use a smaller tool.
- Draw the pad outlines on the milling
layer. Set the line width to the width of your tool to see the
actual tool path.
- Fudge a little on the tool size,
realizing your tracks will be slightly smaller.
Maybe you folks have other workarounds?
Hope this helps!
Regards,
JJ
|
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° 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
|
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 _____________________
|
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:
toggle quoted message
Show quoted text
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° 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
Attachments:
|
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:
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° 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
|
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
_____________________
|
You nailed it!
On 8/12/22 8:23 AM, Harald wrote:
toggle quoted message
Show quoted text
More or less like working with Arduino... Possible but without
great fun ?
--
Harald
_____________________
|
More or less like working with Arduino... Possible but without great fun ?
--
Harald
_____________________
|
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:
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° 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
|
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
toggle quoted message
Show quoted text
[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
|
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
|
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:
toggle quoted message
Show quoted text
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?
|
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?
|
John Johnson