[Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread John Dammeyer 
I needed a small PC board.  I converted the short drill file .txt over to 
G-Code .nc or .tap.   Took a few tries to get it right for LinuxCNC which 
complained about a few things that MACH3 didn't.  Ended up using the CNC router 
with MACH3 because the router can do 20,000 RPM while my mill is limited to 
3000.  Better to turn the 0.035" drill bits at higher RPM I'm told.
 
Anyway.  Does anyone know of a Protel 99SE drill file conversion program to 
G-Code for CNC?  I've attached both.  Hopefully they will come through.  
 
https://youtu.be/5zh-28CHdj4   
 
Here's a short (very short) video of a few of the holes being drilled.  It's 
been so long since I did this that of course I first drilled from the copper 
side rather than the component side.  Came out mirrored of course.  Then 
flipped the piece of PCB around and did it correctly.  The parts just barely 
fit but that's fine.  It's just a prototype.
 
John
 
"ELS! Nothing else works as well for your Lathe"
Automation Artisans Inc.
www dot autoartisans dot com 
 


SSR_Buffer.nc
Description: Binary data
M72
M48
T1F00S00C0.035
T2F00S00C0.042
T3F00S00C0.100
%
T01
X00820Y00160
Y00260
Y00360
Y00460
Y00560
Y00660
Y00760
X00720Y00920
X00620
X00420Y00919
X00320
X00520Y00760
Y00660
Y00560
Y00460
Y00360
Y00260
Y00160
T02
X01100Y00260
Y00360
Y00460
Y00560
Y00660
Y00760
X01020Y01020
X00920
X00260Y00760
Y00660
Y00560
Y00460
Y00360
T03
X01280Y00100
Y01100
X00100
Y00100
M30
___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread andy pugh 
On Tue, 1 Nov 2022 at 21:23, John Dammeyer  wrote:

>
> Anyway.  Does anyone know of a Protel 99SE drill file conversion program
> to G-Code for CNC?


I found this: https://github.com/DJ027X/drl2ngc

But looking at the code I am not sure it copes with lines that have a Y
coordinate but no X coordinate.

-- 
atp
"A motorcycle is a bicycle with a pandemonium attachment and is designed
for the especial use of mechanical geniuses, daredevils and lunatics."
— George Fitch, Atlanta Constitution Newspaper, 1912

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread John Dammeyer 
Don't really need the hole carving feature either.   From what I can see it 
doesn't use the G81 either so results in a much bigger program.  

There are programs that use V bits and carve out around traces.   I have the 
bits but my CNC router is too shaky and not precise enough (yet) for that sort 
of work.  

Thanks for looking.
John

> -Original Message-
> From: andy pugh [mailto:bodge...@gmail.com]
> Sent: November-01-22 2:59 PM
> To: Enhanced Machine Controller (EMC)
> Subject: Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or 
> MACH3.
> 
> On Tue, 1 Nov 2022 at 21:23, John Dammeyer  wrote:
> 
> >
> > Anyway.  Does anyone know of a Protel 99SE drill file conversion program
> > to G-Code for CNC?
> 
> 
> I found this: https://github.com/DJ027X/drl2ngc
> 
> But looking at the code I am not sure it copes with lines that have a Y
> coordinate but no X coordinate.
> 
> --
> atp
> "A motorcycle is a bicycle with a pandemonium attachment and is designed
> for the especial use of mechanical geniuses, daredevils and lunatics."
> � George Fitch, Atlanta Constitution Newspaper, 1912
> 
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread Robin Szemeti via Emc-users 
Whenever I need to do this, I just export as DXF and use the standard
drilling tools in Cut2D .. works a treat, has automatic drill diameter
recognition etc.

Last board I drilled was 400 holes in some Rogers RO4003C  ... and then I
did DIY plated through holes :)

On Tue, 1 Nov 2022 at 21:20, John Dammeyer  wrote:

> I needed a small PC board.  I converted the short drill file .txt over to
> G-Code .nc or .tap.   Took a few tries to get it right for LinuxCNC which
> complained about a few things that MACH3 didn't.  Ended up using the CNC
> router with MACH3 because the router can do 20,000 RPM while my mill is
> limited to 3000.  Better to turn the 0.035" drill bits at higher RPM I'm
> told.
>
> Anyway.  Does anyone know of a Protel 99SE drill file conversion program
> to G-Code for CNC?  I've attached both.  Hopefully they will come through.
>
> https://youtu.be/5zh-28CHdj4  
>
> Here's a short (very short) video of a few of the holes being drilled.
> It's been so long since I did this that of course I first drilled from the
> copper side rather than the component side.  Came out mirrored of course.
> Then flipped the piece of PCB around and did it correctly.  The parts just
> barely fit but that's fine.  It's just a prototype.
>
> John
>
> "ELS! Nothing else works as well for your Lathe"
> Automation Artisans Inc.
> www dot autoartisans dot com
>
> ___
> Emc-users mailing list
> Emc-users@lists.sourceforge.net
> https://lists.sourceforge.net/lists/listinfo/emc-users
>

___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread gene heskett 

On 11/1/22 17:21, John Dammeyer wrote:

I needed a small PC board.  I converted the short drill file .txt over to G-Code .nc 
or .tap.   Took a few tries to get it right for LinuxCNC which complained about a 
few things that MACH3 didn't.  Ended up using the CNC router with MACH3 because the 
router can do 20,000 RPM while my mill is limited to 3000.  Better to turn the 
0.035" drill bits at higher RPM I'm told.
  
Anyway.  Does anyone know of a Protel 99SE drill file conversion program to G-Code for CNC?  I've attached both.  Hopefully they will come through.
  
https://youtu.be/5zh-28CHdj4  
  
Here's a short (very short) video of a few of the holes being drilled.  It's been so long since I did this that of course I first drilled from the copper side rather than the component side.  Came out mirrored of course.  Then flipped the piece of PCB around and did it correctly.  The parts just barely fit but that's fine.  It's just a prototype.
  
John

Eeek!

I don't see but one speed command in that whole file, john, and its only 
for table transport.
No spindle speeds at all. In metric, that F5 would similar to a glacier 
for speed, or watching oil paint dry.


Take care and stay well
  
"ELS! Nothing else works as well for your Lathe"

Automation Artisans Inc.
www dot autoartisans dot com
  



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users



Cheers, Gene Heskett.
--
"There are four boxes to be used in defense of liberty:
 soap, ballot, jury, and ammo. Please use in that order."
-Ed Howdershelt (Author, 1940)
If we desire respect for the law, we must first make the law respectable.
 - Louis D. Brandeis
Genes Web page 



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread John Dammeyer 
> From: gene heskett [mailto:ghesk...@shentel.net]
> On 11/1/22 17:21, John Dammeyer wrote:
> > I needed a small PC board.  I converted the short drill file .txt over to 
> > G-Code .nc or .tap.   Took a few tries to
> get it right for LinuxCNC which complained about a few things that MACH3 
> didn't.  Ended up using the CNC
> router with MACH3 because the router can do 20,000 RPM while my mill is 
> limited to 3000.  Better to turn
> the 0.035" drill bits at higher RPM I'm told.
> >
> Eeek!
> 
> I don't see but one speed command in that whole file, john, and its only
> for table transport.
> No spindle speeds at all. In metric, that F5 would similar to a glacier
> for speed, or watching oil paint dry.
> 
> Take care and stay well

T01
S20 M3

The router is a Bosch Colt and doesn't have speed control other than the dial 
on the side.  So the S20 is just so LinuxCNC wouldn't bitch with the M3.  And 
for testing the code on the Mill I didn't really need the spindle going faster 
than 20RPM.  It will do 1RPM if I want.  But on MACH3 it just switches on power 
to the Bosch Colt.

This was inches so F5 is 5 IPM.  It was about the same speed I'd do with a 
0.035" diameter bit using the DREMEL drill press.

Speeds up to the original Z in the G81 are fast as are down to the Z.  Then G81 
switches over to F5 because the original G81 has a G01 in front of it.  The 36 
holes were drilled in about 1:15.  At least according to the original video 
drilling from the wrong side.

It's a pretty kludgy CNC router but it does work.

John




___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-01 Thread Jon Elson 

On 11/1/22 16:58, andy pugh wrote:

On Tue, 1 Nov 2022 at 21:23, John Dammeyer  wrote:


Anyway.  Does anyone know of a Protel 99SE drill file conversion program
to G-Code for CNC?


I found this: https://github.com/DJ027X/drl2ngc

But looking at the code I am not sure it copes with lines that have a Y
coordinate but no X coordinate.

Since drill files were often sent to the CNC drill on paper 
tape, terse coding was pretty important.  So, any axis that 
didn't change from one hole to the next was omitted, the 
decimal point was omitted, and trailing zeroes were 
suppressed.  This was the standard "Excellon drill format", 
which actually was a dialect of RS-274D.   I have sent John 
D. my Pascal program that does the conversion.  It also 
compensates for the extra depth that needs to be drilled for 
the flank of the drill to make it through the bottom of the 
board, based on drill diameter.  And, it also calculates the 
best feedrate depending on drill diameter.


Jon



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users

Re: [Emc-users] Protel99 SE Drill file to G-CODE for LinuxCNC or MACH3.

2022-11-03 Thread Peter Homann 

Hi John,

If you have Sheetcam, I'm fairly sure that it can take in drill files 
and produce G code for Mach3 or LinuxCNC.


Cheers,

Peter


On 2/11/2022 8:19 am, John Dammeyer wrote:

I needed a small PC board.  I converted the short drill file .txt over to G-Code .nc 
or .tap.   Took a few tries to get it right for LinuxCNC which complained about a 
few things that MACH3 didn't.  Ended up using the CNC router with MACH3 because the 
router can do 20,000 RPM while my mill is limited to 3000.  Better to turn the 
0.035" drill bits at higher RPM I'm told.
  
Anyway.  Does anyone know of a Protel 99SE drill file conversion program to G-Code for CNC?  I've attached both.  Hopefully they will come through.
  
https://youtu.be/5zh-28CHdj4  
  
Here's a short (very short) video of a few of the holes being drilled.  It's been so long since I did this that of course I first drilled from the copper side rather than the component side.  Came out mirrored of course.  Then flipped the piece of PCB around and did it correctly.  The parts just barely fit but that's fine.  It's just a prototype.
  
John
  
"ELS! Nothing else works as well for your Lathe"

Automation Artisans Inc.
www dot autoartisans dot com
  



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users


--
-
Web : http://www.homanndesigns.com
email : gro...@homanndesigns.com
Phone : +61 421 601 665



___
Emc-users mailing list
Emc-users@lists.sourceforge.net
https://lists.sourceforge.net/lists/listinfo/emc-users