[VSO]

Hi all, we bought a 2001 Star SR32 machine last week, we put it in the shop but did not get it to run, yet. I was looking in the manuals and program samples and i found that this machine does not support the G300 code like in 18i-tbs. Then, what i am curious is how do we set up the difference between guide bush and main spindle right after main collet opens? As far as i could understand, when cut off is done, the machine opens the main collet and pouppe goes back to reference position G0G28.. :S + i did not see the G150 code,too. G150 is very useful for me as i allways use a LH tool for cut off process. I thought i could just give negative geometry offset (cut off tool width minus cut off bite width ) to the other tools except T1 to work it out? Also, i noticed there is not an automatic cut-off M code like M7 or M91 codes? I found a macro program named something like 09801 - looks like auto cut off but do not know how to change the variables? What is the M code to call it? It is my first Star experience and i feel a little bit nervous..

[miki2432]

HI
look this
http://www.cnczone.com/forums/cnc-sw...c-control.html

[MCImes]

A few things:
That’s weird that a 18i-TB does not support G300 or G150. Every 18i machine ive run has had those codes. That’s fine though. There’s other ways to program:
As a workaround for the G300, Look at the Machine Position data. When the main is all the way up to the Guide bushing, look at your machine position data. It should either be near Zero or Maximum Z+ depending on where the axis zero is. Based off that number, you could begin each program with a G53 machine coordinates position like this:
<Open collet>
G0 G53 Z70. (Z number was made up, you’ll have to figure out what number works)
<close collet>

As for G150, G50 works in its place. If you’re using a left hand cutoff, instead of G150 Z13.8 you’d use G50 Z13.8 at the top of your program (assuming a 16mm tool, 2mm insert and .2 facing stock =16-2-.2). G50 and 150 are the same code more or less.
Also, its ‘bad form’ to give every tool a negative geometry offset. Instead, its best to give a G50 W-2. To your cutoff tool. Conversely, you could just give your cutoff tool a 16mm Z+ geometry offset, but most people waould say G50 W- is “more correct” programming

As for the auto cutoff program, every one is different and machine specific. The variables depend on who wrote it. You will have to look at the program and see what variables are used. If you post it, I can help you decipher it.

Edit: looking at the other program, it looks like star uses G120/G200 for the start position. Goofy

[VSO]

guys is not SR32-Junior, it is only SR32, 6 axis machine with 16-TB...

[DCogswell]

Go into the Workshift for Z axis. Then set a negative number. OAL+ Max tool geometry + safety. And put that value in the z axis workshift as a negative number. Then your Z0 will be positioned with enough travel.

I don't remember all the key strokes to get there...is this one of the "Yellow" machines?

[VSO]

And i need to know how to get there..
Thanks anyway, it is not one of those yellow machines, i now sr16s and 20s are yellow. but this one is simply white.. )
Just like below

http://www.cercotorniousato.it/media...e-assi-cnc.jpg

[DCogswell]

It may be in the offset page.

Hard key: offset
Soft key: right
Soft key: WK. SHFT

I think that's where its at but, it's been a couple years since I've been in front of one of those.

[Benpen]

Yikes. I'm gonna make this a lot easier for you. Firstly what control is it? It should support G120/G121 This make it easy. At setup you set your part length and then give the machine a G120. This will store this Z in memory and it can be recalled any time using G121. Even after a power cycle. So Your Header in your program should looks something like this.

:0001(Part name here/SR1-F)
(1." matl)
(5-28-14)

(T1- ISCAR P/O)
(T3- .008R TURN)
(T4- .078W FLAT KYOCERA P/O)

(T11- #3 CENTER DRILL)

G99G40G80
G97M5
M11
G121
G0Z-.002T0
M25
M200
M20
M10
M25

If you want to compensate for your cutoff tool, Do it in the tool. Then you get to program with real numbers that match your print. Lot's easier this way. Just use G50. So here's basic End of program.

T100 (parting tool)
G50W-.088 (parting tool width)
G0X[#531+.05]Z6.078T1
M1
M899
S1000M3
M900
G99G1X.8F.01
M901
M82
M40
G99G1X-.05F.0008
M41
M83
M902
G50W.088 (set zero back where it belongs)
M903
M5
M80
/G4P1000
/M98P7000
M81
M99
%

This way you don't have to worry that the monkey setting it up forgot to put in an offset or tool geometry. Also it keeps the machine from moving when you don't want it to. When you use a geometry offset it is called automatically when you call the tool. So if you use a Z number you could end up hanging material out that you didn't want to because of the way it calls it. This way the machine is moving exactly the way I want it to.

If you don't have G120/G121 (you should) You can always just use G50Z0 to set Z when you boot the machine. Then as long as you don't have a G28W0 anywhere it will stay there until power off.

You could also just use a system variable too. Let me know if g120 works or not first.

[DCogswell]

Yikes. I'm gonna make this a lot easier for you. Firstly what control is it? It should support G120/G121 This make it easy. At setup you set your part length and then give the machine a G120. This will store this Z in memory and it can be recalled any time using G121. Even after a power cycle. So Your Header in your program should looks something like this.

:0001(Part name here/SR1-F)
(1." matl)
(5-28-14)

(T1- ISCAR P/O)
(T3- .008R TURN)
(T4- .078W FLAT KYOCERA P/O)

(T11- #3 CENTER DRILL)

G99G40G80
G97M5
M11
G121
G0Z-.002T0
M25
M200
M20
M10
M25

If you want to compensate for your cutoff tool, Do it in the tool. Then you get to program with real numbers that match your print. Lot's easier this way. Just use G50. So here's basic End of program.

T100 (parting tool)
G50W-.088 (parting tool width)
G0X[#531+.05]Z6.078T1
M1
M899
S1000M3
M900
G99G1X.8F.01
M901
M82
M40
G99G1X-.05F.0008
M41
M83
M902
G50W.088 (set zero back where it belongs)
M903
M5
M80
/G4P1000
/M98P7000
M81
M99
%

This way you don't have to worry that the monkey setting it up forgot to put in an offset or tool geometry. Also it keeps the machine from moving when you don't want it to. When you use a geometry offset it is called automatically when you call the tool. So if you use a Z number you could end up hanging material out that you didn't want to because of the way it calls it. This way the machine is moving exactly the way I want it to.

If you don't have G120/G121 (you should) You can always just use G50Z0 to set Z when you boot the machine. Then as long as you don't have a G28W0 anywhere it will stay there until power off.

You could also just use a system variable too. Let me know if g120 works or not first.

+1

[VSO]

I did it with #2601 in the begining of the program. Machine does not support G120 code. #2601 (z axis stroke minus part length) works well, I tried using G50 instead of G150. It worked well, too. Thanks everybody.

[ill]

I program and run a Star 32 J. Often times I will run the programs that were originally from our Star 32 and have to convert them. The gentlemen in this post were correct when they told you to use the g50. You can edit the cutoff macro by just pressing edit->type in o9801 then press down arrow. Use this on drills as well. Each drill, mill, and sometimes bore I give a g50 z clearance move.