G83Extended High Speed Asymmetrical Parametric File Converter

[dave benson]

The planetary gearbox turned up a couple of days ago, On Inspection It looks very well made and for
a smallish unit (to suit a Nema 23 motor) it's quite heavy.
While I was waiting for the gearbox to show up, I made a servo to gearbox adapter plate  and machined
the spider coupling to suit, on one end the output of the gearbox and on the other end to suit  the
top of the Spindle, and made an motor\gearbox sliding mount so that I can quickly disengage it
when not wanting to  use it.

I ran the electronic abacus over the numbers for the motor and gearbox to get some understanding as
what to expect from the unit. If I include the seal friction of the double lip seals of the spindle, and a gearbox
efficiency of 90 %, then I should be getting 5.2 NM delivered to the Tap, from 5.6 NM gross.
With the worm drive gearbox the gross output with a 5\1 ratio was 1.75 N/M.
With the worm drive gearbox I could tap up to M4 well,but M5 stalled the spindle, and what I really wanted
was, to be able to Machine tap, using Hand and Spiral Point\Flute Taps from M3X0.5 to M8X1.25.

I made up a test file with:

M10 X 1.5 mm  blind and through holes.(Hand Tap)
M6  X 1     mm   blind and through holes.(Spiral Point Tap)
M3 X 0.5  mm   blind and through holes.(Hand Tap)

I couldn't use the M8 Tap as when I picked it up and had a good look at it, It looked dull and I remembered that
a few weeks earlier I had done 32 M8 X 15 mm threads in some mild steel plate and some of the plates had
hard spots, which I think added to the taps early demise.

The M3's  went by un-remarkably , and as I want to do 500 of these this was encouraging.
The M6's with the Spiral Point tap went well and at higher feedrates than the Hand Taps.
The M10's went well too, the first time I used a slightly larger Tapping Drill  as I feared that the spindle might stall.
So I then re-did the threads using the correct Tapping Size and that went well too, the whole time while doing this
I had my hand over the stop button and watching the tap, on the last hole I glanced up to see that the rubber spider
in the SKF Spider coupling  was,  "on the cutting  rotation of the Tap"  had been compressed to maybe halve its
width, and that coupling is spec'ed at 3 N/M, the spiders come in different stiffness and that one is the hardest so
I'm afraid that to do anything larger that M10 I'll have to replace the coupling.

I made a lot of changes to the plugin, and tomorrow I'll post the .dll along with a tut file with a series of threads from
M3 to M10 both blind and through holes and an example of an imperial thread in a metric file 1/4 20.
One of the changes I made was to remove the trajectory code as it's been rendered obsolete by the planetary
gearbox (18 Arcmin backlash) is minuscule.

[dave benson]

The .dll and CB tut files are in the zip folder.
Extract to your CNC folder, open up the CB file and save it, this will set the directory.
Generate the Gcode, There should now be a CB file and a  .nc file in the folder.
There are Four Parts each with one Drilling MOP.

The Spot drilling MOP will not be touched as it's a G81 (the pecking distance is zero).
It's just there to demonstrate how to exclude mops from showing up in the the plugin's
list of mops to process, as this helps when you have lots of drilling mops but only want to
adjust a few of them.

The second MOP has it's peck distance set to 1 any number will do other than zero.
This means it can be modified by the plugin.
It's a through hole so the target depth is set to -15 with 12 mm stock.
It's also being tapped with a Spiral Point Tap, so Spiral Point tapping Gcode will be output.

The third MOP is a copy of the second MOP with the target depth set to 10 mm, so not right through
the stock. "A blind Hole".

The fourth MOP is a 1/4 inch 20 TPI, a common camera mount size even if the rest of the camera is metric.
It will be tapped using a mode suitable for use with a hand tap in a CNC machine.

At this point you have your CB and Gcode .nc file, now it's time to make either a Drilling only or
Drilling and Tapping file.
The generated Gcode from the plugin is compatible for most controllers including GRBL and
is viewable in Camotics although you cannot see the rotary axis degrees value.

cont

[dave benson]

OK, it's time to open up the plugin and Drill and Tap the three holes.

Load up the nc file you've just made with CB and press the Update Mops List button.
looking in the Dropdown List shows the mops in the file, including the Spot Drill MOP
we won't need to modify this mop so in the CB file tree disable the mop and press the
Update MOPs list button again and it will have been removed from the drop down list.

Now select the first mop in the list and press the Calc button.
A Error will pop up in the “I” value textbox and an Error message will tell you what's wrong with it.
in this case for a hole of this depth “I”  too large.

I've set the I,J,and K values to suit the hole and checked the "Use slow feedrate at end of hole"
checkbox. What this does is slow the Z Axis feedrate down as the cutting edges pass through
the bottom of the hole to stop the drill's cutting edges from being damaged.
At this point once you are happy with the settings, you can press the "include this mop in
 output file button" and your done with this mop. the button will turn green.

At this point you could generate a file with your changes to this Drill MOP and drill this hole
with those settings, however we will do the others as they will have different settings.
for demonstration purposes.

Select MOP Two and press Calc and then press press the "include this mop in
 output file button" and your done with this mop. the button will turn green.
cont

[dave benson]

Select MOP Three and press Calc and then press press the "include this mop in
 output file button" and your done with this mop. the button will turn green.

If you only want to drill these holes and not tap them then press the convert button
and a Gcode file will be generated identical to the original .nc file with the drilling
mops modified.

Now as we want to thread the holes, the first thing to do is select the first mop
a M6 X 1 through hole for spiral point tapping.

Check the tap this hole checkbox and press enter.

The thread depth textbox has changed colour indicating that a possible tap breakage is
imminent a warning will pop up explaining that if you have a blind hole, it is not deep
enough to accommodate a thread that depth, If on the other hand if you have a through hole then
its fine to tap it.

IF you are Happy with the settings then press the "include this mop in
 output file button" and move on to the next mop.

The next mop is a blind hole  so you will have to change the Thread depth, if you are not
sure about the maximum thread depth then type a big number into the thread depth
textbox and the warning to pop up and at the bottom of it will be a suggested maximum
threading depth, this is the absolute maximum depth and practically you would leave
a bit of headroom. in this case the suggested value is  8.35 mm so I will enter 8.0 in the
textbox. When happy with these settings press the "include this mop in
 output file button"

The last mop is  a 1/4 inch 20 TPI blind hole in a metric file.
Just enter the values from the settings pic press Calc and then press convert
and a file named :
"Rigid Tapping spiral point and Hand Taps through and blind test run M6 and 1-4 X20 TPI G83Extended Tapping Included"
will be produced, this is the file you run on the mill as it has all of the original .nc file mops
plus the drilling mops you have processed into expanded canned cycles.

I have squared and sized some stock with the intention of finding out how fast I can push those M6 spiral point taps.
I will do a grid pattern of holes and tap each hole successively increasing the feedrate until the tap breaks or the spindle
stalls or maybe with a bit of luck get through the job, the M10s were done at 40000 Deg/min and Mach3 max for that
feedrate number is 16 bit so if I get to 60000 Deg/min I'll be happy. that'll be 8.6 seconds per hole  at 12 mm depth of thread  hell I'd be happy with 15 seconds a hole  as long as I don't have to tap them by hand.

I couldn't post yesterday and in the meantime I've made another file and drilled and tapped it.
It's  18  M6 X 1 through hole s and two M3 Blind Holes 8 mm deep 7 mm thread in 12 mm
stock.40000 Deg/min.
If you have many through holes to do then the Spiral Point tap works well, just navigate to
the hole and dive in to the bottom (at full speed) and exit at rapids rinse and repeat.
Dave

[dave benson]

pics

[dave benson]

pics

[dave benson]

pics

[dave benson]

pics

[dave benson]

pics

[dave benson]

pics + dll
Dave

[Bubba]

Nice job Dave, Personally I don't have the machine to use this plugin but I'm sure there are many who run those. I appreciate the time and the effort. Nice write up, BTW.

[EddyCurrent]

Dave,

It's one hell of a plugin but the process seems complicated and I can't determine if I need to use it, I just spiral drill in wood and that works great for me.  In a nutshell, under what circumstances should I be using the plugin ?

[dave benson]

Thanks Bubba, if you ever have the need to tap a few holes on your router then you could, with this gearbox
and a 425 0z/in motor tap up to 1/2 inch 13 all day long, After Tapping those 18 M6 holes in a row I
felt the gearbox and servomotor and they were cold. I originally was going to attach the tapping unit to
the side of my spindle, But after temporarily lashing it to the spindle and checking how much working area
I would lose I decided to put it directly over the top of the spindle and directly couple it, and I put the
spindle mount on slots so that it can be disengaged easily which works well.

Eddy for your purposes drilling holes or pockets in wood then the general purpose Drilling cycles would
be good G81 or G83, or spiral milling like you do,which saves toolchanges, I do this sometimes in steel and Aluminium
when the tolerance allows, if however you need a very accurately positioned deep hole that is actually round and does not
deviate from perpendicular,then you need to drill and ream the hole with a canned cycle like the ones shown
in the Hass video "what the aim of the game" is  to evacuate the chips out of the hole, because if you don't
then they contribute to the hole being maybe oversize, out of round, and or deviate from a straight path
somewhat like a directional boring rig, the deeper the hole the more trouble will you have.

There are a couple of pics of the Hybrid Tufting machine I made, to show you what I'm going to do with the plugin.

The first pic is some of the components of the machine, the transparent part shows to holes that intersect at an
acute angle, one hole holds a hook the other is for a grub screw to secure the hook.
Those holes 46 of them must be straight and evenly spaced, for example in the old money a 1 thou cumulative error
on the holes means the last hole would be 45 thou out of place, and you've just made a doorstop.

The holes in the blocks are both ten times the diameter of the drill deep.
with a hole this deep and a 2.5 mm drill bit, your feeds and speeds must be
adhered to very closely  just slightly to much feed and the drill will bend a little
and hole position will deviate and of course you must get the chips out of the hole.
Another thing about this job is that you have to tap the hole, and a broken Tap is almost a sure thing if the
intersection where the two holes meet is off a little, I broke a few this way until I wised up, and now I inspect
hole intersection with a bright light.

I use the plugin to make a drilling cycle that rapids to the stock surface and evacuates the chips  consistently
and at the intersection where the two holes meet I slow the plunge feedrate down to half speed to stop
the cutting edges on the drill bit from destroying themselves, if you don't do this they don't last long. Maybe 10 or 15 holes and they only good for general purpose work whereas with the
custom canned cycle they last two blocks 92 holes even with all these precautions they are not perfect though, but in the practical world good enough to work
The other thing on this particular job it saves 4 hours machining time as compared to
the regular G81/83's
I've always hand tapped the grub screw holes so being able to do it in the mill is
a godsend.

Dave

[Bubba]

Dave, the cnc machine I have now is flimsy router for routing wood, some plastics, that's all. Any time I need something repaired or made out of steel I do have Bridgeport, metal lathe with couple attachments and ton of cutting tools. And, I enjoy run those manual machines.. So taping couple holes nonissue for me.

[EddyCurrent]

Dave, thank you for the insight.

Some of the plugins I made were to help myself first and foremost, so that fact you will personally benefit from this plugin is great and that alone makes all your work worthwhile.