Developments on my Home built 5C CNC Lathe - Polar interp. and Live tooling

NoJo,

No rush, appreciate your time.  Slowly digesting all the files & forum discussions.

Thx,
R

Attached is a zip of all the comps/remaps/ini/hal, etc
C axis mode is entered with G12.1 - this zeroes the C axis as well. L-CNC would tally all revolutions made by the spindle in turn mode, and then on entry to C mode, would unwind all those turns to zero the C axis - not desirable. So look in Caxis.comp and refer comments in gn_userkins.comp for how this is done on my machine.
G13.1 exits C mode back to TURN mode.
G12.1 selects C mode - POLAR mode - no cartesian , but C axis effectively becomes Y axis of a mill, etc.
The ATC is included in the attached files.

This Gcode is an example of that used to do the hex head on the end on the shaft, in two depths, each 2mm deep (final 4mm) 

In your config, is there a way to enter C-axis mode without polar interpolation?

I'm thinking of simple radial/axial drilling where it'd be simple to just use cartesian coordinates.

Not in the pure sense, no. However, when in C axis mode, the Gcode 'looks' cartesian - X = Xaxis, Y axis becomes C, and the cartesian to polar conversion is done in L_CNC - this gcode file is a simple square:

Tool offsets/cutter diameters, etc, you would have to take care of, as the above Gcode file puts the center of the tool on the X20/Y20 co-ord, ie, on the corner of the square, not offset by the cutter radius, if milling. A drill would have no diameter offset, but you may enter G43 Hxx for any length offsets, etc. if desired....
For axial drilling, perhaps simply move the drill to co-ord - G01 X20 C20 F(feedrate of the move- which will be a coordinated move, ie, Caxis and X axis), and at the end of the move, use Gcode to drill with the Z axis as normal.  I have not tried it, but you may be able to do a rapid (G00) to the X20C20 position, and then Zdrill, since you only want the drill at the X20C20 position and are not interested in how it gets there, ie, G01 coordinated move would 'mill' the contour ( a straight line) in the workpiece - this gets the tool to the end point, but wastes time.

My lathe has no radial drill/mill capability - the live tool axis is fixed in line with the lathe spindle axis, so have not even considered radial drilling/milling, but daresay it could be handled in the same way as proposed above - after G12.1, a G01 Cxx would move Caxis to that angle ( ie, no X axis move in the command is then only a Caxis rotation, no coordinated X/C move. That could line up the workpiece periphery at an angle that the radial drill will move along. If the radial drill is fitted to the X axis, then a G01 Xxx would move the drill into the workpiece - refinement needs more thought - radial peck drilling, etc - normally a Z axis motion - not sure of the drilling Godes works in X?

Been a while since I powered the little lathe on - 99% of my lathe work is on the manual lathes I have - The little CNC lathe was an exercise in design and build and turned out very nice indeed, but in my shop, it is a solution in search of a problem...

 

His work is very interesting, especially having been able to intelligently resolve everything related to the change of coordinates despite not yet being implemented in LCN, and his perseverance to carry out his project despite the costs. Could you share the 3D CAD file of the ATC designed by you, I think it's excellent how you described it, especially regarding everything related to the live tool, when using a BLDC RC motor, which, to me, would never have occurred to me even though I use them a lot in Drones and CABLECAM. Finally I have a question: Why do I implement its own ATC component, if the CAROUSEL component authored by ANDY PUGH already existed?

Your contributions to this thread are very interesting. You say you have paid for the design of a postprocessor for F360 to manage the C axis and you make it available to anyone who may be interested in using it, which seems very commendable to me. Could you then share it with me? Even if you had to contribute some money to obtain it.

WRT the ATC - If I recall, the basic carousel comp requires the ATC hardware to be able to rotate the carousel, past the tool locate point, a pawn then engages and the carousel is then rotated backwards to lock against the pawl ( EMCO style..)
If you study my ATC you will see it uses a hirth coupling and compressed air to disengage the coupler, a stepper to rotate to the next tool, with opto-sensing of tool position, and then air release to lock using compression spring discs. Also, the ATC has a live spindle as a tool select - none of this is available in the basic carousel comp - if you want fancy, you have to pay in pain..I paid a lot, nearly giving up many times...

I would not have succeeded if it were not for a LOT of help from Andy, Aciera and
DGarrett, and my good Wife, a really good software Guru.

Re the F360 processor - I think you have me confused with someone else - I never paid for F360 anything - I don't use F360, I dislike the marketing model and its Pro price, esp for hobby use...
I use Rhinocad-7 and Rhinocam - the latter cannot do Mill/turn, ie, no C axis capability in lathe CAM. For this lathe I use eCam - an Italian fellow's creation for Mill and Lathe, with a very usable C axis mode - it is very good, free on weekends, and two or three hundred Euro to buy.

I can share the 3D cad files for the lathe/ATC, etc, but it is all Rhinocad format (.3dm) - I can convert to other standards, but that always creates issues...

COFHAL wrote:

Your contributions to this thread are very interesting. You say you have paid for the design of a postprocessor for F360 to manage the C axis and you make it available to anyone who may be interested in using it, which seems very commendable to me. Could you then share it with me? Even if you had to contribute some money to obtain it
 

That was me.  I paid for a F360 PP for use with Emco's WinPC version of Fanuc 21TB.  It includes a bar-puller macro, as well as radial/axial live tool functions.  Milling/drilling is output using XZC moves and does not require G12.1 polar interpolation in the controller, although the Emco does, in fact, have G12.1 available.

The person who wrote the PP has gone missing.  Despite my best efforts, I've not been able to contact him since before covid and I fear the worst.

At this point I don't feel like there are any copyright or ethical issues and I'm the sole owner of the PP - and can share it with LCNC community.

My hope is that someone more skilled than me can modify the PP for use with LCNC.

Sorry re the confusion - As I had started this topic and COHAL's post did not address anyone specific ( that I can see) , I thought it was meant for me..

I wonder how that PP works in milling - it must do all the polar interp itself and output thousands of small moves to all the axis to follow a polar path in cartesian fashion. How is the PP written? Do you have source code?