Homebrew PCBs

I just finished up my CNC quill drive conversion my Bridgeport and would
like to use it to drill boards.    I have not found a reference to what 
speeds and feeds to use for drilling.

I am looking for the  surface feet per minute and feed per turn numbers
for  small carbide drills in FR-4.    My 5400 RPM maximum  going to be
well below the 30,000 to 60,000 RPM used by a real PCB drilling spindle
but it should still work fine if  I use the correct feed rate.

Anyone got a reference for these parameters.



BP Quill Drive
<http://picasaweb.google.com/lh/photo/B-uAtxYUicys82cFdd5HYg?feat=direct\
link>





[Non-text portions of this message have been removed]

designer_craig wrote: 
> 
> I am looking for the surface feet per minute and feed per turn numbers
> for small carbide drills in FR-4. My 5400 RPM maximum going to be
> well below the 30,000 to 60,000 RPM used by a real PCB drilling
> spindle but it should still work fine if I use the correct feed rate.
> Anyone got a reference for these parameters.

I would point pages 24.16 and 25.8 from printed circuits handbook 6th
edition. But nothing real there, you need cutting speed (sfm) and chip
load values from your laminate datasheet, but i never found any of those
values for any laminate i have used. I use 'guessed' values after
stressing with this plenty of times too. But never got results as good
as i wish.
http://books.google.pt/books?id=g9Q8RekeKaAC&pg=PA5
http://books.google.pt/books?id=g9Q8RekeKaAC&pg=SA25-PA8
The same book also points 500 as sfm and 1mil for chip load as normal
values for fr4. I use this as example from one laminate:

Suggested Drilling Parameters For Isola DE104i
                SPINDLE   Surface Speed
DRILL SIZE      SPEED      per Minute    INFEED      CHIPLOAD
inch     mm       RPM     SFPM    SMPM    inch    meter mil    mm
                                          min.    min.  rev.   rev.
0.010  0.2540    89,763    235      71.63  65     1.651 0.70   0.018
0.015  0.3810    80,214    315      96.01  80     2.032 1.00   0.025
0.020  0.5080    60,161    315      96.01  90     2.286 1.50   0.038
0.025  0.6350    53,476    350     106.68  80     2.032 1.50   0.038
0.030  0.7620    47,747    375     114.30  85     2.159 1.80   0.046
0.035  0.8890    43,654    400     121.92  88     2.235 2.00   0.051
0.040  1.0160    42,972    450     137.16  107    2.718 2.50   0.064
0.050  1.2700    34,377    450     137.16  85     2.159 2.50   0.064
0.060  1.5240    28,648    450     137.16  72     1.829 2.50   0.064
0.080  2.0320    21,486    450     137.16  55     1.397 2.50   0.064

Similar to what i did for me i put this on a spreadsheet and trunk the
rpm to 5400 and reduced the feed rate proportionally to the rpm
reduction. But i give no warranties.

drill   speed   feed
inch rpm in/min
0.01 5400 3.9
0.015 5400 5.4
0.02 5400 8.1
0.025 5400 8.1
0.03 5400 9.6
0.035 5400 10.9
0.04 5400 13.4
0.05 5400 13.4
0.06 5400 13.6
0.08 5400 13.8

You put so many effort, dedication and cost on the bridgeport that you
may like to build a smaller, lighter and faster machine just for pcbs. 

Simao

Hi,

On my A360 (www.accuratecnc.com), I'm using feed rate 40 in/m at @60000. May be 
in your case (@5400) you have to reduce it up to 4 in/m ! 

Regards



________________________________

From: designer_craig <cs6061@...>
To: Homebrew_PCBs@yahoogroups.com
Sent: Wed, June 30, 2010 10:11:46 AM
Subject: [Homebrew_PCBs] PCB drilling speed and feed rates

  

I just finished up my CNC quill drive conversion my Bridgeport and would
like to use it to drill boards. I have not found a reference to what 
speeds and feeds to use for drilling.

I am looking for the surface feet per minute and feed per turn numbers
for small carbide drills in FR-4. My 5400 RPM maximum going to be
well below the 30,000 to 60,000 RPM used by a real PCB drilling spindle
but it should still work fine if I use the correct feed rate.

Anyone got a reference for these parameters.

BP Quill Drive
<http://picasaweb.google.com/lh/photo/B-uAtxYUicys82cFdd5HYg?feat=directlink>

[Non-text portions of this message have been removed]





      

[Non-text portions of this message have been removed]

Ivan Peterson wrote:

> May be in your case (@5400) you have to reduce it up to 4 in/m ! 

At 1mil per revolution would be 5.4in/minute. But it can be faster for
most diameters.

--- In Homebrew_PCBs@yahoogroups.com, "designer_craig" <cs6061@...> wrote:
>
> 
> I just finished up my CNC quill drive conversion my Bridgeport and would
> like to use it to drill boards.    I have not found a reference to what 
> speeds and feeds to use for drilling.
> 
> I am looking for the  surface feet per minute and feed per turn numbers
> for  small carbide drills in FR-4.    My 5400 RPM maximum  going to be
> well below the 30,000 to 60,000 RPM used by a real PCB drilling spindle
> but it should still work fine if  I use the correct feed rate.
> 
> Anyone got a reference for these parameters.
> 
> 
> 
> BP Quill Drive
> <http://picasaweb.google.com/lh/photo/B-uAtxYUicys82cFdd5HYg?feat=direct\
> link>
> 
> 
> 
> 
> 
> [Non-text portions of this message have been removed]
>

I uploaded two pdf files that have the information needed to calculate feeds and speeds. These files are scans of a slide rule drilling calculator that Excellon provided to their customers. Back in those days I was running three Excellon machines, two driller/routers and one drilling machine. Using those formulas, each machine was averaging a million holes per week with very few broken drills. The bits wore out before breaking so I would say those formulas worked pretty good! There is some good information on router feeds and speeds as well.

Thanks for the info.

I took a guess at a starting point and used 5400 RPM & 8.6 IPM on a .042" dia carbide bit. Seemed to work just fine, had some burs on the back side but they sanded off without much effort.  I was using some masonite as a backer but possibly I need something a little more dense to help reduce the burs.

Eventually I am going to build an accessory high speed spindle attachment to get the RPM up to 25K to 30K.

I also need to build some sort of holding fixture possibly a vacuum fixture to hold the blank boards.

Craig

--- In Homebrew_PCBs@yahoogroups.com, "designer_craig" <cs6061@...> wrote:

>
> 
> I just finished up my CNC quill drive conversion my Bridgeport and would
> like to use it to drill boards.    I have not found a reference to what 
> speeds and feeds to use for drilling.
> 
> I am looking for the  surface feet per minute and feed per turn numbers
> for  small carbide drills in FR-4.    My 5400 RPM maximum  going to be
> well below the 30,000 to 60,000 RPM used by a real PCB drilling spindle
> but it should still work fine if  I use the correct feed rate.
> 
> Anyone got a reference for these parameters.
> 
> 
> 
> BP Quill Drive
> <http://picasaweb.google.com/lh/photo/B-uAtxYUicys82cFdd5HYg?feat=direct\
> link>
> 
> 
> 
> 
> 
> [Non-text portions of this message have been removed]
>

A pressure foot on your drilling spindle will help with burrs or warped panels. It could be nothing more than a spring loaded ring or U shaped foot that compresses the stack of boards right before the drill bit enters. I always used .125" tempered masonite as the back up board. The entry material was .010" aluminum or phenolic sheet.

Most drilling machines use a pin and slot tooling plate. The stack of boards are pinned together with .125" dowel pins. We ran 12" x 18" and 18" x 24" panels that were pinned half way across the shorter dimension on each end. The dowel pin holes were drilled about .25" from the panel edge. One pin went into the bushing hole and the other end of the panel went into the .125" wide tooling slot. This pin and slot tooling allowed panels of any length to be pinned to the tooling plates. 

You could make a pin and slot tooling plate for your bridgeport that clamped to the t slots. MDF or aluminum would work good for this. Just clamp the plate to the table and write a program that drills a tooling hole and cuts a long slot. 

I've never seen a circuit board drilling process that left no burrs. That's why every plant has a conveyorized deburring scrubbler. For small jobs you can wet sand the panels with 220 grit sandpaper. That works fine for deburring. 


--- In Homebrew_PCBs@yahoogroups.com, "designer_craig" <cs6061@...> wrote:

>
> Thanks for the info.
> 
> I took a guess at a starting point and used 5400 RPM & 8.6 IPM on a .042" dia carbide bit. Seemed to work just fine, had some burs on the back side but they sanded off without much effort.  I was using some masonite as a backer but possibly I need something a little more dense to help reduce the burs.
> 
> Eventually I am going to build an accessory high speed spindle attachment to get the RPM up to 25K to 30K.
> 
> I also need to build some sort of holding fixture possibly a vacuum fixture to hold the blank boards.
> 
> Craig
> 
> --- In Homebrew_PCBs@yahoogroups.com, "designer_craig" <cs6061@> wrote:
> >
> > 
> > I just finished up my CNC quill drive conversion my Bridgeport and would
> > like to use it to drill boards.    I have not found a reference to what 
> > speeds and feeds to use for drilling.
> > 
> > I am looking for the  surface feet per minute and feed per turn numbers
> > for  small carbide drills in FR-4.    My 5400 RPM maximum  going to be
> > well below the 30,000 to 60,000 RPM used by a real PCB drilling spindle
> > but it should still work fine if  I use the correct feed rate.
> > 
> > Anyone got a reference for these parameters.
> > 
> > 
> > 
> > BP Quill Drive
> > <http://picasaweb.google.com/lh/photo/B-uAtxYUicys82cFdd5HYg?feat=direct\
> > link>
> > 
> > 
> > 
> > 
> > 
> > [Non-text portions of this message have been removed]
> >
>