[Maddog Machine]

Not being much of a lathe guy I find myself suddenly in charge of programming multi-part runs on a TL-1. I've written a good program for a simple washer. Now I need to find out how to do a Z shift (canned cycle)of Z-.125 for each part to maintain proper dimension. To produce say 10 parts at time. Then reset program and bring down work stop to adjust the bar to begin the cycle allover. I know it's probably a setting in the setting page. Any help would be greatly appreciated.

[Geof]

Use G10 to move your Z work offset forward; we do this all the time.

Leave G54 at Z0.0, turn your program into nested subroutines and write a small program that calls the subroutine after changing the work offset something like this for a part that is 0.5" thick including a parting and facing allowance.

Some stuff is missing from this example I am just putting in the G10 stuff to move the offset and call the subroutine.

O00000
G10 L2 G90 P1 Z0.0 (Make sure G54 is at zero)
G10 L2 G90 P2 Z-0.5 (Set G55 forward one part thickness)
G10 L2 G90 P3 Z-1.0 (Set G56 forward two part thicknesses)
G10 L2 G90 P4 Z-1.5 (Set G57 forward three part thicknesses)
G10 L2 G90 P5 Z-2.0 (Set G58 forward four part thicknesses)

M97 P100 L20 (The L is how many times you can advance the bar)

M30

N100 G54
M97 P1000
G55
M97 P1000
G56
M97 P1000
G57
M97 P1000
G58
M97 P1000
G54
All the stuff for feeding the bar to a stop
M99

N1000 Your program


M99

You start with a new bar brought out to your stop.
Go to N100 and using G54 go to your part program at N1000
Return, set G55 then go to your part program.
etc.

Feed the bar to the stop, return and go through all the work offsets again.

Run it in Graphics it is perfectly clear.

G10 is the 'enter offsets command', L2 identifies work offsets P1 is G54, P2 G55, etc.

Dead simple, very powerful.

I hope I got everything correct I did this very fast; ask it it does not seem to make sense.

[Maddog Machine]

Thanks Geof...I'll give it a go. BTW I talk a designer out of using glass filled delrin for a project after reading a reply to a post you made in '06 concerning machining glass filled nylon. So thanks again.

[CNCRim]

Not being much of a lathe guy I find myself suddenly in charge of programming multi-part runs on a TL-1. I've written a good program for a simple washer. Now I need to find out how to do a Z shift (canned cycle)of Z-.125 for each part to maintain proper dimension. To produce say 10 parts at time. Then reset program and bring down work stop to adjust the bar to begin the cycle allover. I know it's probably a setting in the setting page. Any help would be greatly appreciated.

I think you can get a part puller and use program for single part........ ect

[Geof]

I think you can get a part puller and use program for single part........ ect

Yes you can but when the part is very thin like a washer but the material has a decent diameter so you can have a couple of inches or more sticking out of the chuck it is more efficient to part of half a dozen pieces for each time you pull the bar. This is where using the different work zeroes comes in; you step your way down the length of bar then pull out another length and step your way down again. Pulling, or feeding with a bar pusher, is a slow operation so you want to maximize the number of parts per pull.

[ChsBrown]

We use a simple looping program with incremental movements to accomplish this.


M97 P100 L5

G28 X0
G28

M99


M00


N100
W-0.206
G01 X0.2 F0.005
G00 W0.05
X0.7
W-0.05
M99


The biggest problem we have is the burr on the part off.

[SeymourDumore]

Since all of my previous attempts at asking folks have been utterly futile, I'll ask again.
What is the advantage of using G10 on a machinetool - ANY MACHINETOOL - that has multiple workoffset capability?
What does G10 accomplish that G54, 55, 56 etc does not????

Incremental programming... well I'm sorry but does not belong in cutting motions.

[Geof]

......What is the advantage of using G10 on a machinetool - ANY MACHINETOOL - that has multiple workoffset capability?
What does G10 accomplish that G54, 55, 56 etc does not????

Incremental programming... well I'm sorry but does not belong in cutting motions.

G10 can enter your G54, etc work offsets.

If you have dedicated setups with a base that remains in place and
fixtures that dowel into place which hold multiple parts you can have all the part locations as G10 commands that enter the work zero locations from the program. It just saves having to enter them all from a list of numbers; less error prone.

Of course then the question becomes 'why not use G52 commands within the program?' and the answer to this is; depending on your programming style the G52s may be spread throughout the program while the G10s are clustered near the top; easier for editing if/when needed such as if the base is removed and replaced in a slightly different position.

EDIT: Also remembered on a lathe doing bar work when it is feasible to part-off several parts per bar advance you can use G10 to shift the Z work zero forward to step along the bar.

Again this is possible with G52; I think I pointed out in another thread that G52 requires fewer keystrokes when writing the original program.



Regarding incremental how do I do helical interpolation using a single line command without using incremental?

G91 G03 I J Z L

[SeymourDumore]

Geof

The point is, I like to restrict my part program to actually cut the part, while setup should include the setup of tools an fixtures.
If there is any discrepancy in the setup from one time to another, I do not want to edit the program itself.
G52 is useful, but I restrict it's use to within one fixture offset. Example, multiple identical pockets within one part. Each pocket is defined using a localized o coordinate, and G52 is used to shift the coordinate there.
The useage of G10 requires the editing of the part program in case of a location variation. I don't like it. The program should cut the part and not set it's location. The dedicated work coords are designed and well suited for that.
Of course, I'm not against a call-once-explicitly subprogram within the body of the part program that uses G10 to pick and set up the workoffsets. But that section need not be called any more than once during setup.

As far as incremental, I remain rigid about NEVER to use G91 for any reason.

[Geof]

Geof
.....Of course, I'm not against a call-once-explicitly subprogram within the body of the part program that uses G10 to pick and set up the workoffsets. But that section need not be called any more than once during setup.....

We do it more or less the reverse; our part programs are mostly subroutines and the G10 commands are at the head of the main program. Sometimes the G10 commands are in a separate program that is run just to enter the offsets.

We find this very convenient for changing from part to part because the operator does not need to worry about entering work offsets.

...As far as incremental, I remain rigid about NEVER to use G91 for any reason.

You didn't answer my question; how do I do a single line command for helical interpolation without using G91?

Do you mean you program an absolute Z position for each turn of the helix? In other words if you are thread milling 20 tpi one inch deep you have 20 lines of code to describe the move?

[SeymourDumore]

Duhhhh on the threadmilling part.
Not that it is the only way, but is certainly more convenient, in fact I use it too.
Sorry 'bout that.

As far as helical on a Haas, this will do a helical without G91

G00 X0 Y1. Z1.
G01 Z.01 F10.
G02 I0 J-.5 Z-.5
G02 I0 J-.5
G01 X0 Y0
G01 Z1. F200.
BLAHBLAHBLAH

[Geof]

Duhhhh on the threadmilling part.
Not that it is the only way, but is certainly more convenient, in fact I use it too.
Sorry 'bout that.

As far as helical on a Haas, this will do a helical without G91

G00 X0 Y1. Z1.
G01 Z.01 F10.
G02 I0 J-.5 Z-.5
G02 I0 J-.5
G01 X0 Y0
G01 Z1. F200.
BLAHBLAHBLAH

Yes if you are only going down to Z-.5 and can do that in a single circuit; ie big hole and big cutter so you have plenty of room for chips. Try going through 2" with a 7/8"hole in a single circuit; I know you can bang an insert drill through but then to open the hole up to 0.880" the easiest way is to interpolate and to get an acceptable finish it is necessary to limit the Z feed per circle and do several circles.

[SeymourDumore]

You may have a point about your own programming style, as long as you remain anal about making sure the G91 does not "stick".
I OTOH prefer writing that out longhand specifying each pass with it's own explicit Z-depth.
I did used to use G91 similar to you, but have all but abondaned it. I still have a semifunctional Kurt vise to explain the reason.
The endmill and the ER32 holder unfortunately did not survive the endeavor.:nono:

[Geof]

....I did used to use G91 similar to you, but have all but abondaned it. I still have a semifunctional Kurt vise to explain the reason.
The endmill and the ER32 holder unfortunately did not survive the endeavor.:nono:

Ah, I understand.

I often use this sequence or something like it:

G41 D01 G00 Y0.5, Z0.02
G91 G03 I0. J-.5 Z-.2 F100. L10
G90 G03 I0. J-.5 Z-2.0 F100. L2

Frequently I just copy the G91 line and change the G91 to a G90 with an absolute Z location; on occasion I have changed the Z but missed the G91 with the results you describe. Maybe not quite the results; so far I have only destroyed parts and severely maimed holders.

My luckiest one was years ago when I was doing a hole in a part clamped on top of a piece of 1" aluminum plate; I don't like putting things directly on the table. I went 0.95" into the plate and was very glad that I don't clamp directly onto the table.

But the usefullness of G91 is so good that I use it very often particularly with production programs that are thoroughly proved out before being put into regular use. My catastrophes have occurred on my prototype/tooling machines and most times I can hush them up.

[ChsBrown]

OK GUYS, Admittedly, I am only a newby at programming....why is my style ie. incremental programming wrong? It's fast, it's accurate, it's easy.
Am I missing something?

[Geof]

Absolutely nothing wrong with incremental but when you mix incremental and absolute in the same program you introduce a large potential error factor; you just have to try and remember your mental check list to make sure you are in the correct mode at the correct place.

[SeymourDumore]

As Geof said about the potential error.
IOW if you miss something, you'll know it.

Additionally, since every move depends on the previous, there is very little you can do about accuracy.
If you notice Geof's example, it is using G91 for a very specific circumstance for a very specific purpose. It spirals down to open a hole. I'm willing to bet that the very same hole is finished using absolute with real coordinates.
I have seen people making pockets and bosses using incremental, which makes my cringe and break out in sweats in the middle of the night.

[Geof]

.....Additionally, since every move depends on the previous, there is very little you can do about accuracy.
If you notice Geof's example, it is using G91 for a very specific circumstance for a very specific purpose. It spirals down to open a hole. I'm willing to bet that the very same hole is finished using absolute with real coordinates....

Yes it is; the final G90 G03 does an absolute Z position and as I explain this is where an error potential arises. If I forget the G90 it tries to increment down 2 inches on the final circuit. Sometimes it will give a Z overtravel alarm other times it generates any of, or all; Spindle Following Error, Spindle Overload, Z Axis Following Error, Z Axis Overload.

Incidentally my example runs on a Haas and I believe not all machines will allow the addition of a Z incremental move in G03 or G02. Then you have to crunch out each circuit or get technical and write a macro.

[g-codeguy]

Since all of my previous attempts at asking folks have been utterly futile, I'll ask again.
What is the advantage of using G10 on a machinetool - ANY MACHINETOOL - that has multiple workoffset capability?
What does G10 accomplish that G54, 55, 56 etc does not????

Incremental programming... well I'm sorry but does not belong in cutting motions.

Can't speak for anything but a lathe, but I guess "Nothing" would have to be my answer, yet I still prefer to use G10.

We also make a lot of washers. This is more a 'How to" example for Maddog.


:5982 (EWA-10490-REV.NONE MAIN)

#143=0 (3=CARBIDE 4=HSS DRILL)

N100G10P0Z-7.53 (BARSTOP)
G65P9018X.86F.01S900M4000T202
M1

N900M91 (DRILL)
IF[#143EQ3]GOTO23
IF[#143EQ4]GOTO24
#3000=2 (SET #143)
N23T0909S2350M63 (CARBIDE DRILL)
X0Z.5
Z.05
G1Z-.765F.005
GOTO29
N24T0909S517M63 (HSS DRILL)
X0Z.5
Z.05
G1Z-.5F.005
G0Z.5
G4U.5
Z-.48
G1Z-.775
N29M92
M1

N200M91 (ROUGH TURN)
T0202S3951M63
X.87Z.005
G50S4500
G96S900
G1X.33F.01
X.28F.015
G0X.698Z.02
G4U.02
G1U#510Z-.69F.012
U.03
M92
M1

N1M98P2844 (RUN 1ST PART)
G10P0W.135
M54 (PART COUNTER)
M1

N2M98P2844 (RUN 2ND PART)
G10P0W.135
M54 (PART COUNTER)
M1

N3M98P2844 (RUN 3RD PART)
G10P0W.135
M54 (PART COUNTER)
M1

N4M98P2844 (RUN 4TH PART)
G10P0W.135
M54 (PART COUNTER)
M1

N5M98P2844 (RUN 5TH PART)
/M54 (PART COUNTER)
/M99
M30

:2844 (EWA-10490 SUBPROGRAM)

N300M91 (FINISH TURN)
T0303S4500M63
X.73Z0
G1X.36W#500F.0035
Z.01F.015
X.6386
Z0F.002
G3U.0268Z-.0056R.019
G1U.0114W-.0057
G3U.0112W-.0134R.019 (X.6878)
G1Z-.0458F.003
G3U-.0112W-.0134R.019F.002
G1U-.02W-.01
G97X.72F.008
M92
M1

N400M91 (BORE)
T0404S3000M63
X.4538Z.5
Z.02
G1X.415Z-.0333F.001
Z.05F.02
X.5Z.03
X.4681Z.01
Z0F.002
G2X.4436Z-.0086R.013
G1X.4236Z-.0361
G2X.4225Z-.0392R.009
G1Z-.1F.0032
X.41F.015
M92
M1

N600M91 (BACK CHAMFER I.D.)
T0606S2000M63
X.38Z.5
Z.02
G1X.4Z-.0742F.015
X.4225F.003
G2U.003W-.0035R.005F.001
G1U.011W-.0055
X.38F.015
M92
M1

N1200 (CUT-OFF)
G65P9019X.75Z-.13F.002A.406B.428E#501S300M3500T1212
M99
%


Seymour, as you can see I not only control the increment between parts, but also the workshift. Of course it can be run with G54-G59 offsets, but I don't know how to set the G54-G59. I've tried the G10L2P_ shown in Peter Smid's book on Fanuc custom macros, but it doesn't work on our lathes. Parameter change? It appears to take a G10P0Z_ command (MDI), but nothing changes in the workshift.

I specify the shifts in the header, but that requires faith in the set-up person. Well placed most times, but....

Nice thing about lathes is I don't need to use G90/G91 on most of them. So no worry.

EDIT: Normally the bore is also programmed with incremental moves on the chamfer. Bore size gets changed, change one word. Done. Chamfer sizes are the same size on a lot of parts. Making a new program, cut & paste, change one word. Modify Z depth if necessary. Done. Pretty sure I can manually program many of our parts faster than the other programmer does using Mastercam. And he is good with it.

[Geof]

....Nice thing about lathes is I don't need to use G90/G91 on most of them. So no worry.

When I read this I realised I am guilty of swiching tracks midstream. This thread started on lathes but answering Seymour I segued over to mills.

Sorry about that.

Incremental on a lathe? I think you have to be out of your mind.