[metal mania 01]

I have been around citizen and Tsugami machines for a little while now.I recently started a new job with a a company that has two star sr32's.they are older machines with a 16t controller.from what I see we are not utilizing features of the machines and nice things like a cutoff check current position macro and possibly better initialization of the start-up of the programs.currently we are putting the main z axis into position manually i realized there is a better way.also i noticed a page similiar to mc data on a citizen that carries info like stock dia,machining length,cutoff width,cutoff rpm.I am pretty certian that this page's variables could be used for cutoff check and also initialization of program.if anyone out there has info on this machine please help

[PixMan]

As always....RTFM. (Read The Fn Manual) first.

That required advice now fulfilled by me....

Great machines. Yes, there's a lot of those machines that they're not using but that makes them the same as many. I've worked at (too many) other shops that also don't use the features that save time and prevent crashes. One is the "Z axis stroke check" function for setting the initial headstock position.

What you're supposed to do is run through the main spindle program once with no stock in the "air cut" mode with the "Z stroke check" engaged. That sets the variable for the Z axis start position and assures no overtravel. In theory, this works perfect. In reality, no shop I've ever worked at uses it. Ever. I also notice few people use the data management page you mentioned to setup for the one-button cutoff. Use it, it can't hurt. Older machines may not even have that feature though. Any chance those are 16i-T controls?

You absolutely should be using the M code for broken cutoff tool detection. Unless you have a well-documented tool life management system for the cutoff tool and a very short cycle time that you're trying to reduce even further, that little mechanical arm is worth it's weight in gold for saving broken tools. I often see it in disrepair, frequently missing the arm completely.

That Fanuc 16 control is good, but Star is notorious for having minimal options lit up. If you have any documentation, see if there's a listing of what options the machines have. Some machines have C axis on both spindles, some have it on neither one. You are probably already missing my favorite Citizen feature: the tool set mode. You get accustomed to running the first part of a program (up to the M20) to do a cutoff.

I can probably help with developing a standard program format for you, but what's in the Star manuals is already good and proven.

[metal mania 01]

Yes, they are 16i-T controls.I really appreciate your feedback.I have only been involved with this machine for a week and have recently finished reading the manual and trying to memorize code so I understand what I am looking at.
The control seems like it has some issues with inserting a small buffer in the rear head program at the beginning . The machine has 1 deg indexing main and sub.

You mention running the first part program up to the M20 to do a cutoff.There is no cutoff set up in the top of these programs,therefore, no good yet. Do these 16i-T controls have current position variables?If so ,do you know what they are for the main X
axis.
I was thinking I need a safety cutoff check in the top of program.I would like to see what kind of format you have for initialization of program.Also I was thinking about a small macro for the morning to initialize X&Z and and sync spindles to ensure sync on on both heads.Go G28W0 on main Z axis.Then subtract machining length from available Z stroke of 12.2 inches and position Z to result of difference.Then G50Z0 to establish Z0.Also machine needs you to call T5 to reference machine in the morning.
I know it may seem like overkill but in a competitive world the faster I get the spindles making chips the better.
Also the little cutoff check arm is in operation on both machines.Seems like a very useful tool.
Thank You for your input.

[PixMan]

I've got a Fanuc handbook in my box at work and a PCMCIA card. I'll download the O9810 macro that is the cutoff program for you to see, though your machine should still have those O9000-series programs in protected memory.

If you do not see the 9000 programs, you can easily change that.

Go to MDI mode, then hit the offset page button twice (or once, and use the softkey for "settings".) Change the "PWE" (Parameter Write Enable) to "1". You'll get an alarm, but ignore it.

Now hit the "Systems" mode key to get the parameters. Search for Parameter No.3202, bit 4. It'll be labeled as "NE9". Change it to "1", then go back and change the PWE back to "0" and then the reset button. Now in edit mode BE VERY CAREFUL not to actually change anything in the 9000 programs. Yet. Search for program number 9810, that should be your cutoff/safety check program. If you have that, you're 90% there for safe operation.

Download the 9000-series programs and print them out for reference (though they should also be written into the manuals by Star), then be sure to change that 3202.4 parameter back to "0" so they're protected from accidental erasure or edits.

The front end of your programs for Head 1 should look something like this:

G99 G97 G80 G40
M62 (bar feeder on)
#529 = 3000 (cutoff cycle spindle speed in RPM)
#530 = .002 (feed rate for cutoff cycle in IPR)
#531 = 1.125 (stock diameter, no clearance need be added here)
#2601 = -10.125 (position of Z1 axis to start machining processes)
IF [#5041 LT 0] GOTO 1
M25 (coolant on)
M98 P9810
N1
M11 (collet open)
G4 U0.1
G0 Z.543 T0 (position Z for use with LH cutoff tool)
G4 U0.1
M10 (collet close)
M20
M200
G0 X2.5 Z-.05 T0
M27 (broken cutoff too detect)

....part program....

This sets the cutoff (machining) data variables, then looks at the position of X axis (system variable 5041). If the cutoff tool is in a safe position of having the X value lower than X0.0, the machine proceeds to line N1 and begins making a part. If the X axis is above zero, it executes the O9810 cutoff macro program.

Hope this helps.

Ken M.

[metal mania 01]

The information you gave me was exactly what I was looking for.I really appreciate it.#2601 exactly what I was looking for.It far simplifies what I was planning on doing.

I am somewhat familiar with the parameter write enable procedure but I am glad you refreshed me on this.I did not know about #3202/bit 4 .I will definately check this machine for the programs and do as you say about offloading the programs to hard copy.You have been a huge help!

Also I have some more questions about setting system variables for comp information ?On a Tsugami 18i-T Fanuc controller I would write tool comp information in the top of my programs to be loaded with the initialization of the program.These variables were used for assigning values to the offset page.For example:
#2900's = "r" radius value in offset page
#2800's = "z" value in offset page
#2300's ="t" number value (cutter comp)

There was also a seies for wear comp information to be set but cannot remember,maybe #2600's,or #2400's.

#2914=4 (You would assign a 4 to the tip column or "t" value for T14)
I would just like to know if you would know if this control was capable of setting this information in this same manner.If not 'then maybe a different series of numbers.I have tried setting these values in MDI and they are not affecting this page's values.

Or how about the current position variable for "z" and "y" axis for this controller.

Thank you.

[PixMan]

Those system variables should be the same for a 16i-T and an 18i-T control, and BTW the 16 is the better and more-expensive of the two. It can handle more axis and spindles. You should have rigid tapping on that machine, and may very well have G12.1/G112 interpolation, G7, and many more.

The variables you are looking for are one of those things that's in the handbook I have from Fanuc, but it's in my toolbox at work. In the past I also used them for setting T and R values, but even that is a waste of time if an operator puts a CCGT32.52 insert in where you specified a CCGT32.51 one.

Try again using a programmed command to set system variables which are the offsets, but use a regular program rather than an MDI command. There may be a paramter set which prevents them from being set via MDI for some reason. Honestly, I don't think I've ever seen two machines, even sequential serial numbers of like machines, have all the exact same parameter settings. With over 19,000 of them to set, it's little surprise.

[glenthemann]

can someone explain to me how exactly the #2601 works?

Coming from citizens im a bit lost about how it figures out its start position on its own. I understand the 2601 is the part length, plus a bit, minus the stroke of the machine which gives a negative number for 2601, but then I see its not used anywhere else?

After 2601 is set, G0 Z[cutoff tool width - .015] is called and then G120[cutoff tool width -.015] is called setting the Z zero point.

I just dont understand how 2601 sets the "start position"

I mean its obvously working for us, but we're just trying to understand exactly what is going on here. Ive tried looking for #2601 in the manuals but havnt had any luck yet.

Any input is greatly appreciated

[PixMan]

According to the Fanuc manual I'm looking at right now, #2601 is the system variable for "G54 workpiece zero point offset value, 2nd axis". If you were to get into the 9000-series macro program that is run with the first macro in your program (I think it's 9810, not sure), you'd see that it uses that value which you'd input by virtue of the "#2601 = -xxxx" that you enter. The control likely takes that value, opens the collet, moves the Z axis to that position and executes a "G50 Zxxxx" to begin running the parts.

[glenthemann]

According to the Fanuc manual I'm looking at right now, #2601 is the system variable for "G54 workpiece zero point offset value, 2nd axis". If you were to get into the 9000-series macro program that is run with the first macro in your program (I think it's 9810, not sure), you'd see that it uses that value which you'd input by virtue of the "#2601 = -xxxx" that you enter. The control likely takes that value, opens the collet, moves the Z axis to that position and executes a "G50 Zxxxx" to begin running the parts.

aye indeed the program does run P9810 after its checked if x is below zero or not. However I coudlnt find anywhere in 9810 that it was used.

Before I got back on here I found in the fanuc book that 2601 is the z workpiece coordinate shift.

It works well and I should be happy with this fact, but I just like to know exactly how things are doing what theyre doing *shrug*

Also Ive been having issues threading, the machine seems to be having servo lag issues, and we cannot thread at 2800 RPM without the thread coming out tapered. We beat ourselves up trying to figure out why it was tapering until we tried a lower spindle speed and voila.. no problems. This is actually really irritating as this is a BRAND new machine and we can thread the same thread at 4000rpm on our 20 year old miyano.... Anyone have any ideas?

Thanks!

[chet470]

#2601 sets the machine coordinate system for Z0. It works as follows.....when the z axis is "zero returned" this is to be considered Z0. As you jog the headstock forward 1" that would be considered #2601=-1.000.
If your machine had a 8" stroke and you are producing a 4" part you would set your #2601 at about -3.5( .500 added to for tool geometry etc... This will always ensure that your headstock is working as close to the GB as possible. This is especially important when working with very small diameter matl's

[chet470]

A good way to see how this works is to first open headstock room door. Assuming its safe to do so, open main collet and zero return your headstock. Put control in Head 1, memory and one cycle. Run program to M20. You should see the headstock advance to the value that you have set in #2601. Now, reset your program. In Edit, change the #2601 value....add say negative 1" from what you previously had it set at (ie #2601=-2.500....change to #2601=-3.500). Now go back to memory and run to m20 again while watching the headstock and you will see it advance another inch. This is how you tell the machine where you want it to work from.
If you ever get a Z1 OT then you know your #2601 needs to be adjusted accordingly.
Hope this makes sense

o0001

[Finndus]

Does anybody have the O9810 macro?
I've started running a very old Star SR20 with 16tt controller and it seems that these easy safety features have never been used where i work.

Thanks,
Phil.

[DCogswell]

Does anybody have the O9810 macro?
I've started running a very old Star SR20 with 16tt controller and it seems that these easy safety features have never been used where i work.

Thanks,
Phil.

SR20 16T control (late 90's machine)

%
:9810
G99M25
G4U5.0
T200
T100
M10
M3S#529
IF[#4006EQ20]GOTO1
G0X[#531+1.0]
G1X-#528F0.02
GOTO2
N1G0X[#531+0.04]
G1X-#528F0.0008
N2M26
M5
M11
M99
%


In the main program, before the 9810, I have these variables:

#528=.080(CUTOFF DISTANCE PAST ZERO)
#529=2000(SPINDLE RPM AT CUTOFF)
#531=.4375(MATERIAL DIAMETER)

Hope this helps,

DC

[DCogswell]

Does anybody have the O9810 macro?
I've started running a very old Star SR20 with 16tt controller and it seems that these easy safety features have never been used where i work.

Thanks,
Phil.

Also, that 9810 program may be in there, if someone deleted it, then you'll need to upload it again.

If you can't get to the "9000" series programs then see the post by "pixman" on how to access the "9000" series programs.

[Finndus]

Thanks DC,

Thats exactly what I wanted and works perfectly!!!!