How do I program a thread deburr pass

[MCImes]

I run a swiss lathe with a Fanuc 18i-TB control. I am making a part with an OD threaded end and a flat on the threads. I want to deburr the OD and threads in the machine.

Here's my process:
I turn the major,
-thread with a G76
-mill on the flat,
-repeat the path for the major to deburr the OD,
-deburr threads with 2-3 passes at minor dia with a G76 or G92. (heres my question)

I want to chase/deburr the threads with another G76 or G92 with 2 or 3 passes. My question is how do I program the G76 to only take 2 or 3 passes at the minor.

The G92 would obviously be easier since I define where to be in X but does the spindle always orient to the same position to begin the thread pass?
ie: can I thread with a G76 and deburr with a G92? like:

G0 x.(010 over stock)
G92 x.(minor dia) z.end F(m3x.5)
x.minor
x.minor
G0 x.over stock

if not, with the G76, where do I begin in X and how do I set it up to go to the minor dia right away and do 2 or 3 passes.

Thanks!

[ad64075]

You can set P equal to Q in your G76 line, which should net the specified number of finish passes only.

[MCImes]

Thanks! that makes sense. Just one question though. Do I input the first pass in radius or diameter?

So here what I come up with
First one:
G76 P101060 Q0010 R.001
G76 X.092 Z1.600 P0110 Q0050 F.01968 R-.002


Deburr pass:
G76 P301060 Q0010 R.001
G76 X.092 Z1.600 P0110 Q0110 F.01968 R-.002

does that look good?

[ad64075]

In your first G76 line, the first 2 digits of the P number designate the number of finish passes. It would appear that you are currently using 10 passes at finish depth? Perhaps with that small of a diameter it's necessary.

Anyhow, for your finish pass you can set your first depth of cut high, at or near the thread heigth.

Hope this helps you!

[fordav11]

it'd be easier using G76 and just set the depth of thread to the full depth minus a few thou and set parameter 5142 (G76 repetition count) to 2 or 3 or 4 or whatever number of spring passes you want assuming you are using one line (Fanuc 15 format).
If using 2 lines the Q on the 2nd line should be the full depth and the first 2 numbers of the P on the 1st line sets the number of finish spring passes. It looks like you don't know that because on your deburr pass you have that at 30?? 30 spring passes is a little extravagant isn't it? that's probably more cuts than cutting the whole thread from the start. Usually 2 or 3 spring passes is plenty.

as for using G76 and then G92 it should work but it depends on the specific machine/servos/encoders and how it sets the thread pick-up point. You can test it by running G76 then using a different offset (say T0101 for the G76 and T0111 for the G92, both geometry offsets for T01 and T11 must have the same tool geometry numbers). Put 0.500" on wear offset 11 and watch the tool when you call T0111. if it ends up in the middle of the thread at full depth then its OK to use G92 after G76. Otherwise you must use G76. I personally think G76 then G92 would work fine if you plunge with the G76 at 0 degrees. If you are plunging at 60 degrees the Z position at the minor diameter will be out of position by half of the thread width because G92 can only do plunging at 0 degrees. You could fix that by moving the G92 Z start point minus by that amount.
Just run it on the machine and watch the tool and make minor adjustments in Z if required. Or for simplicity just use G76

[MCImes]

i thought the G76 P301060 Q0010 R.001 finish passes were in .1 incraments. I only want a couple finish passes so should it be:

G76 P031060 Q0010 R.001
to get 3 finish passes?

[ad64075]

Actually, to get 3 finish passes, you would need to program 2. The machine will cut the programmed X value already, so when G76 is used as a finish pass, you will automatically get one pass more than you designate. Unless your machine is very different from any Fanuc I have been around, the P number breaks down as follows:

First two digits: Number of finish passes

Middle two digits: Thread lead-out allowance

Last two digits: Thread angle

[MCImes]

ah, good point. I think I got it now.
Thanks to all