G83Extended High Speed Asymmetrical Parametric File Converter

[dave benson]

A small Update.
I saw this Hass tip of the day a few weeks ago, https://www.youtube.com/watch?v=Euh_xrcJ5SI
and thought this was a good Idea.

So I’ve added the ability to the ‘chip breaking move with retract’ to
use a dwell to break the chip and or to leave an even planer finish on
the bottom of the hole.

There’s an extra check box for this and if checked with auto calculate
the required ms delay for the number of drill rotations you require, it was 1.5 turns
in the video. And you must have the actual spindle speed set in the mop.
I use Mach3 and so have set in the general config to ‘use milliseconds’.

I have tested this version with Mach3\UGS\GRBLgru.
I ran the CB file with normal retract and Dwell enabled chip breaking.
The Dwell mops ran a small margin faster and the machine ran smoother.
I tested with 30 mm MDF and will through the week test some steel.

Dave

[dave benson]

A tip for GRBL users:

Mach3 understands and can use some but not all canned cycles, GRBL has
no clue what they are (UGS pops up a nice little warning  in the sidebar) though
to tell you there’s a problem.

So for Mach3\4\Linux and the file above just re-enable the mop and your good to go.
For GRBL users you have to take a few extra steps.
First re-enable the mop.
Then enter a positive value in the Peck Distance (I use 3) it doesn’t matter.
This turns the spot drill mop from G81 to G83, now the plugin can see it and use it.
Then once in the plugin you can set it to make the mop into a G81 cycle again, and as
it’s the ‘long hand’ vanilla version of the canned cycle it’ll run on GRBL.
I’ve included the .nc file remember it’s Mach3 and metric so you can use it but remove
the G64, the pics show the plugin settings and results.

The procedure should go something like this, Prepare and
Generate your .nc file from within CB.
In the drilling mops that you want to adjust, set the Pecking Distance to a positive number.
Load the plugin.
Load the just generated .nc file.
Click the update mops button.
Select from the drop down list a mop to convert.
I live in metric land so if I click the calculate button the defaults and this CB file with -12mm holes and a
4 mm dia tool makes a G81 effectively it rapids to just above the hole then proceeds at the plunge feed rate
to the bottom of the hole.

So to make a G81 the I value should be set so that the depth of the
first peck is the depth of the hole.
The various variables (sorry) have a priority hierarchy and (I) has the
Highest  so if another setting conflicts with it, [It wins] and the other
operation will either be scheduled for later on or ignored completely.
Remember if you update your CB file and re-generate it then you need to
reload it into the plugin and press update mops list button.

Dave

[dave benson]

I got a lot of testing done yesterday, and made a few changes.
Fixed a bug where with some I,J,K settings caused an extra pause, was had to find.
I also put an extra Info warning for loading files.
Tip: If you are doing many files and get a warning when going to generate a new file
then you have forgotten to click the update mops button after loading the file.
Click the update mops button and enter the mops again. (or dismiss the plugin and restart it).
I tried to video the proceedings, but Kubric I’m not, couldn’t get the white balance correct.
I did some trials for countersunk screws with and without the 1.5 turns at the bottom.
The results were inconclusive, as they both looked pretty good ‘surface finish at the bottom of the hole wise’ and as
I didn’t have the correct angled tool for countersunk screws, I spun an angled plug up on the lathe. This didn’t help
much as even after bluing then up I couldn’t tell any difference.
The drills used were pretty small so, on the weekend I’ll try with larger tools where the errors will be more pronounced.

Dave

Edit to Add:
I fiddled around with the button style in the last up load and was rubbish
so I have fixed that, the buttons back colour indicates  that it needs pressing
and I couldn’t see that very clearly.
I’ll add the new one here and remove the old one.

Dave

[dave benson]

I did some more testing today as I wasn’t sure that the dwell was
of much benefit for the finishing of the bottom of the hole.
It turns out it is, I made a file with two holes and spot drilled
then pilot drilled and then counter sunk them shallow enough to
see the bottom of the hole.
In the pic Hole one on the left is a standard chip breaker with an extra chip break                       
which I used as a poor mans dwell really, and the other hole has Dwell.
There’s a clear difference between them  the Dwell being clearly better, I don’t
think it’s a panacea though as some plastics like a more violent chip break and
there’s no point wasting time fine finishing a hole where it’s not needed.
If you were cutting a ‘Seat’ or mating surface then it would be good for this.

Edit to add: this photo that’s been put through a filter.
It’s a standard G81 and you can see the position that the drill
began to leave to work the smearing the a bit of material on the
work surface. I choose that drill because it was not a regrind and
looked pretty sharp however you can see on comparing the  left and right
side of the pic that one edge was cutting cleaner.

The point of doing the pic was, I wanted to know at what ‘spindle speed’ in
RPM  could my machine safely execute the minimum dwell in milliseconds that I
would require for my spindle speed range or maximum chip breaking retract distance
in mm. (the B value)

It worked out for my machines Z axis settings and the spindle speed range (max 3600)
that the Z axis could perform a chip breaking (retract and back to work piece) a move
16 mm in length so I’m never going to have worry about it as this value is usually
sub millimeter.
For users with a standard type router config then 12000 RPM to 15000 RPM would
be ok,  but for 20000 RPM and up both your Z axis velocity and acceleration must
be very high, so to be prudent I would do the dwell mops with a max spindle speed of
12000 RPM.

Dave

[dave benson]

I continued experimenting today with spot drilling, spot facing
and countersinking and found that for some shallow holes where
the depth of hole is small compared to the drill diameter, that I
needed to turn off pecking altogether so I’ve added a new check
box to turn off pecking.
This essentially gives a G81 with integrated spot facing.

Dave

[dave benson]

I continued on with the last series of tests, just spot facing.
I made a simple spreadsheet that showed me what resolution in deg that I could control
the cutting edges of the tool with different spindle speeds and Z Axis Acceleration and
more importantly at what point will the axis be unable to respond to commands.

My Z Axis is heavy and I had set a conservative acceleration for the original motor
an old SloSyn motor which I believed was 570 0z/in and on searching to replace it
found out it was 380 oz/in, which is kinda small for a Nema 34, anyway I replaced
it with one I had on hand an 960 oz/in motor, but didn’t adjust the Accel\Velocity settings.

I made a CB file with four mops for spot facing. Each with a different hole finish applied to it.

First      mop            drill to full depth ---> rapid out of hole.
Second mop             peck to depth -------> rapid out of hole.
Third    mop            peck to depth (using pauses) -------> Pause 1.5 turns then rapid out of hole.
Fourth  mop            dill to full  depth -------->  Pause 1.5 turns then rapid out of hole.
All the test were done with a 14 mm centre cutting end mill which from new tended to chatter
because it was ground slightly concave and off centre.
Because the tests were about timing, I warmed up the spindle and set it at various
speeds and checked it with a Tycho. And used these values in the mops.
It is a V belt driven spindle and so will vary with belt slip\creep.
For example the 400 rpm setting yielded 396  +-  4 at 1780 it was +- 2.
I have a cheap non contact tycho and they are not accurate at low speeds (400 pulses is low).
So I don’t know if the 396 is accurate.

I had organised the mops so that one would be executed then a tool change move out of the
way so that I could see the surface of the hole clearly and take a picture of it.

[dave benson]

I stepped through the mops and noted the surface and took a picture.
The first two mops (for that end mill and that material)  looked ok no chatter pretty smooth.
The second two Dwell mops were no good at all and the marks indicated that the Z Axis was to
slow and this is when I checked the acceleration I found that it had been set 56 and not 156
so I must have fat fingered the keyboard and not noticed and for the kind of work I usually do, it didn’t
matter and raised no red flags.
This is why I was nonplussed  with the drilling tests of the smaller holes (where the rpm is high )   
as they were not being performed.

I re-calibrated the axis in progressive steps until the axis failed and set it back 20% this turned out to be 800 mm/sec/sec.
The picture is of the same hole with only difference being Z Axis acceleration was set from 56
to 300. (on the way to 800) It looks ok to me and I now know that my machine has at 400 rpm a
theoretical resolution of 3 deg plus or minus spindle speed variation.
On a side note, I realise now that with a specially ground tool and a servo spindle, that you could mill
(for the want of a better term) very simple geometric features on the bottom face of the hole
for example you might be able to make a keying feature to keep two parts aligned whilst being fastened.
I checked  the spindle speeds up to 1780 and the machine is performing well and has a resolution of 13.35 deg
plus or minus spindle speed variation.
For a high speed spindle of 24000 rpm the resolution would be 180 deg so no adjustments in quarters or thirds
just halves. (with 800 mm/s/s)
If your machine is capable of it and you set the accel to 5400 then you’ll get the same resolution
I get at 1780 rpm. For nearly all practical purposes 90 deg would be plenty

Dave

[dh42]

Hello Dave

I do not use this plugin, but a guy on a french forum always get an error ; I tried too and get the same error, any advice to solve this ?

++
David

[dh42]

I also get another strange thing as on this picture



Why it said that the value of Depth of first peck is 15 ? it is set to 3 in the "I" box
(and in the previous picture, it said it is = 0, but in the "I" box it is set to 1)

++
David

[dave benson]

HI David

That error is caused because, the hole depth from the mop = 10 mm and the
(I) variable = <3>   equates to 3 x 5 (the drill diameter) = 15 mm which is greater than
the hole depth he is trying to drill which is equal to 10 mm.

The variables in the plugin start out as default values, and must be changed
to suit the mop values.

In this case the OP would set the <I> value to (1)  (the depth of first peck) = 1 x 5 = 5.
or any value that equates to less than 10 (the actual depth of the hole from the mop).

And in this case the <k> and <J> values must be less than the <I> value.
So, they might be set at one or less than one.

If the OP or you can post the file, I’ll go through it step by step with a picture of the errors
that pop up as you adjust the variables to suit the hole parameters.
The I, J and K values have an order of preference, set the I value first then the J and K values.
Unlike normal canned cycles these will work with Camotics, so if you set the plunge feed rate to
something like 5 (edit it in Camotics) then you can see the hole being drilled in slow motion enabling you to
see what the “programmed operations” in the hole are actually doing as it’s being drilled which is very handy.

The Mantra goes like this:
If at all possible, use a G81, for example if the hole is a shallow 6 mm hole in MDF or particle
board.

If the hole has some more challenging requirements like the hole is deep (necessitating chip clearance move), then use a G83.

If you have a hole that is very challenging, and which cannot be done with a G81 or 83
and there are many occasions where this is the case, for example the hole may be very deep or the material
is rubber or plastic or gummy like aluminum, or the hole ‘finish’ has to meet certain criteria or if you have a
counter bore a ‘seat’ that needs to be flat, or perhaps you need to drill and tap the hole then use the plugin.
The .nc file has a simple hole 10 mm deep with a 5 mm drill it has a chip breaking move at 5mm
all the I J and k values are set to one.

If the OP’s stock is a softwood just use a G81 if it’s hardwood or metal and a through hole, then add a slow feed
rate operation to the end of the hole which stops the drill from excess heating or chipping.
This works very well and prolongs the life of the drill.
Edit: spelling
Dave

[dh42]

Hello Dave

Thanks for the reply, I'll transmit to the user

++
David

[dave benson]

Here is an update fixed spelling and some logic.
Dave

[dave benson]

Update and bug fix.

I was using the plugin today, to drill some holes in the Top Hat for a digitizing probe
and discovered that I've moved a label last edit and forgot to place it back where it
was supposed to be.

On a side note, I ran a test on the probe, once constructed by probing an 10mmx15mm section of our 20 cent piece.
It worked out that the point cloud consisted of 15200 ish points and took over 3 and a half maybe 4 hours to complete, so I won't
be doing that again in a hurry, this is where one of those cheap and cheerful small format cnc's would be a better option, if you had a lot of probing to do.

The plugin was designed to work with Stock heights of zero or less meaning that you could have
various stock heights in the one file as long as they were at zero or anything less than that.
I recall bubba saying that he uses a router and likes to set the stock height to a positive number
so have added this logic and have included a the plain cb file, the plain .nc output and the plugin
output showing the drilling and tapping file.

Dave

[dave benson]

more files
Dave

[pixelmaker]

There is something wrong with the version numbers.
I have V 1.0.1.4 in the download - date: 11.02.2025
and now an update V 0.0.8.9 - date: 10 March 2025

The version numbers should be written directly into the file. I am very happy that Dave is still working on his plugin and sharing it with us. But I am not able to find the last version anymore. Does the version number or the date count?
In the source code of the plugin itself I see 0.0.8.9

I also see these version jumps in the download. Probably the result of a night of programming.