Lathe OD Turning

Hey John,

For someone with a slow connection you are keeping busy.
Looks like this one now combines the rough and slow passes.

Rick G

Yes, but I'm not 100% sure it works all the time...

John

It looks like if the depth of cut and the final diameter come out even it may skip the finish cut?
Perhaps a field with the finish cut depth and add that to the final diameter before running?
Then run the finish cut.

Never mind it looks like it's already there. Maybe it's the new glasses.

Rick G

I did a complete re-write of the OD sub this morning as there were several mistakes in my logic...

This sub will allow you to specify roughing and finishing tools, depth of cut, feed as well as the normal things needed like OD, final diameter, start Z, end Z. If the finish cut is equal to or deeper than the difference between start diameter and final diameter / 2 then the roughing cuts are simply skipped. The roughing cuts are as close as possible to the specified roughing depth and not deeper but evenly divided up so each cut is the same. The finish cut follows the complete profile left to give a wiping cut on the Z shoulder.

And here it is completely re-written and much better behaved...



Enjoy
John

Cool, I will have to try it when I get back out to the shop.


Rick G

Just loaded. When I use this with my .axisrc setup for backtool I receive an error from ngc when I post. Also how woud you add cw ccw selection to each tool.


Jim

While Im addmitting late to this thread,Ive thought about this one my self.I used to own an Ikeagai lathe that didnt have the full g70/g71 ruffing cylces,it had a G94 cycle like your sub above.

For what it is worth,you can use drilling cycles G81 and G83(real handy when you cant get the chips to break,especially when you are boring small holes)as one pass ruffing cyles like so

G0 X.45Z.03
G81R.03F.015Z-1.
G80

This will turn a .45 dia back 1 inch,you substitute G83 and break the chip the value of Q.

Adding to this you can make an incremental sub.

O100 sub
G81R.03F.015Z-1.
G91
G0X-.1
G90G80
endsub (or M99 or however Emc ends a subroutine)



Then call like so
G0 X1.01Z.1
o100 call repeat [5]

This will create a .1 step ruffing cycle that cuts the dia to .51 in .100 steps.

It also looks like this would work

G0 X.1.Z.03
G81R.03F.015Z-1.
G91X-.1L5
G90G80

These are for simple step turning,For what it is worth.....

jbunch wrote:

Just loaded. When I use this with my .axisrc setup for backtool I receive an error from ngc when I post. Also how woud you add cw ccw selection to each tool.
Jim

Use an if statement to select between M3 and M4. You can only pass numbers so use if variable EQ 0 then M3 else M4.

John

When I use this with my .axisrc setup for backtool I receive an error from ngc when I post

What is in your .axisrc ?

Rick G

I did a copy and paste from the WIKI on changing axis display for use with backtool. I also have two lines that invert the up arrow and down arrow for the X axis.

Jim