G73-g83?

[Nanker]

We have a Miyano BNC-34C lathe with a Fanuc OT control.
It's a new animal to us as our other lathes are Okumas.
We want to peck drill a 1.75" deep hole, .250" pecks, but we want the drill to retract out of the part, not just break the chip. G83 is not listed in the manual. The manual is very confusing.
Can anyone give me an example of what the code should look like? Are there any parameters to set?

[WOLOG]

It should look like this:

G83 Z-1.75 Q.25 R.1 F.003;

Q= .250 peck depth
R= rapid to .1 in front of part

This is for a Haas control, but it runs in fanuc mode. The G83 will peck and retract like you want it to.

Good luck
James

[Nanker]

Thanks for the reply James. But we still have problems.
Here's a bit more of an explaination of what we have tried.
The face of the chuck is part .000. Stock is sticking out 1.750.
Drilling 1.335 deep.
We have tried the following:

G83 Z.415 Q.250 R1.8 F.003
G74 Z.415 Q.250 R1.8 F.003
G74 Z.415 Q.250 R.1 F.003

We get the same error "007" for all of them:
Decimal point "." input error (A decimal point was input after an address with which it cannot be used. Or two decimal points were input.)

The manual does not show a G83 so I'm not sure if it is valid. The best we can find in the manual is G74, which their only example appears to be for breaking a chip for OD turning (G74 X__ Z__ P__ Q__ R__ F__). It also says that "if X and P are not specified, only one operation is made in the Z direction, This motion can be used for deep hole drilling."

Any help will be greatly appreciated.

[HuFlungDung]

I don't know if that is unorthodox programming, but I would redefine the face of the part as Z0 and rewrite the command line to suit. There might be some constraints in the logic of the macro that forbid working in positive Z. Just a guess.

[Nanker]

We thought of that, but the manual shows examples of using both the chuck and face of part as Z .000. The rest of the program is written that way and we only have a problem with this one line. All of our Okuma's are programmed that way. That's what they taught a Okuma school. Might give it a try though.
Thanks.

[wms]

Some controls will not accept a decimal point in the "Q" value.

You may want to remove that decimal and use a "Q250" or a "Q2500".

[Nanker]

That seemed to help.....kind of.
We didn't get an alarm and it ran, but after drilling to the final depth, it went to
X3.6 (there goes the drill) then Z1.850 then X.000 before going to line N0203

Here is a section of the code in the machine:
N0200G97S525M08
N0201G00X0Z1.85T0202
N0202G74Z0.415Q2500R1.8F.003
N0203G00X0Z5.25T0200

I don't know where it is picking up the X3.6 move as there isn't a X3.6 anywhere in the program. We're really confused now.

[wms]

If this a Fanuc OT control Model C you would need two lines for the G74 command.

Like this :

N200 G74 R.010 (R is the retract amount for the peck)
N210 G74 Z (final depth) Q(peck amount without decimal) F (feed)

Bear in mind that the builder of the machine can set things up differently as they see fit. Have you contacted them or the dealer? It could be the case that the builder has "special setting".


That said First I would remove the R1.8 from your line N202. and the X0 from line N203 and try it.

[WOLOG]

This is another one of those times that I can not understand why G-code from one manufacturer is different from another. Decide on one format and stick to it!!!!!

To lighten things up a bit...

[wms]

Nanker,

There really is no way to get it to retract back to Z1.800 and then rapid back to just above the last peck. Not with a Fanuc OT (C or b).

You can get it to retract out of the hole all the way like you want but it will then feed back to above the last peck. Not ideal but maybe it will work for you. It will be slow at the .003 feed you are using.

I would suggest you hand code the cycle and be done with it.

But if you want to try it here is the code:

G97 S525 M8
GOO X0.0 Z1.800
G74 R1.800
G74 Z.415 Q2500 F.003
GOO Z5.25

If you put the Q value on the same line as the second G74 with the Z it will as you found out move Radially In X at the end of the hole. Hence the 1.800 x 2 = X3.600 as you saw. Not good for hole drilling to say the least. How did you put it "there goes the drill".

If you try a G83 you will find that it too only retracts to break the chip and not all the way out of the hole. And that is if it is even available on your control as some OT's don't offer it. It had to be ordered and turned on by the builder.

Maybe someone else or the builder know of a parameter that would change the way it retracts.

[tex]

Here's what I've got while running 1.75" deep hole drilling throught FANUC0 posptprocessor...I don't get it, but it looks like it is a 3-axis milling posprocessor...I doubt that this would be of any help, but here it is:

N5 X0 Y0 S1200 M3
N6 G43 Z.1394 H1
N7 Z.0494
N8 G95 G83 X0 Y0 Z-1.8549 R.0494 Q.25 F.002
N9 G80
N10 G0 Z.1394

[Nanker]

First off, thanks for all the replies.
WMS, you're dead right on everything. Using two lines of G74 and removing the "R" from the second line did it. It retracts the first line "R" valve but doesn't rapid back to where it last drilled. Starts at the front and goes into feed rate. Totally unacceptable, too much time. This machine also doesn't read a G83. It appears that the only way to do it is as you said, "write it by hand and be done with it."
I'm sure I'll be back in the near future for more help from everyone as we try to figure this machine out. Great forum! Thanks to all.