Cincom f16 problems

[mstorto]

I've been put in the great spot to getting an old machine running again and everyone who used to work on the machine have been let go. I have zero screw experience so we're going with the operators manuals to learn what is what. We got the tool setter fixed and have started to alter an existing program that used to work but, the guy who used to program fudged his programs without the tool setter and offsets so his programs are cr*p. Here is my problem...I have an machine over travel alarm and I can't figure out why. Maybe I'm just missing something but here is the program:
%
:3238
N10G69
N20G99M15
N30M07
N40G50X-0.12Z0.6M52
N50G0X3.Z0T1100 (face off tool)
N60M06
N70M16
N80M03S1000T1
N90G0X0.350
N100Z0.
N110G1X-0.05T2100F.002 (center drill)
N120G0Z-0.250
N130G0X3.0
N140G68
N150X3.
N160T2100
N170T2F0.001
N180Z-0.05
N190X0.
N191Z0
N200G01Z0.05
N210G00Z-0.25 (error happens here!!)
N220X3.
N230T2500
N240T4F0.001

it seems basic to me but I'm a vertical mill guy. Is it a problem because of the G50, and what is the G50 really telling it...part length?? Any help would be helpful with this machine. thanks guys.

[ProProcess]

G50 is the/a coordinate system set.
So the headstock starts at the start position.
In the program the G50Z.6 tells the work coordinate system that you are at Z.6, now all of your z coordinates are base on that.
I would say that your start position is too far back and that Z-.25 is unreachable.

[mstorto]

I made a mistake, the error is on the line before (N200). It will not go in z.05. It's final position at the error is z.648. I've tried changing the linear move to a g74 peck but that had the error as well. If I change the g50 to z.650 will that change the part length and is that associated to the part lenth? here is the rest of the program so you can see what else happens. So far the next tool does not error but I haven't corrected it's offset yet.

N240T4F0.001
N250G0X-0.880
N260G01Z0
N270Z0.600
N250G00Z-0.1
N260X3.0
N270G69
N280G0X3.
N290T1100
N300T1S1500F0.003
N310G00Z-0.01
N320X0.270
N321G1X-0.01
N322G1X0.280
N330G01Z0.0
N340Z0.005
N350G01Z0.560
N360G0X0.320
N380X3.
N390T1300
N400T6S1000F0.002
N410G0Z0.584
N420X0.320
N430G01X0.280F0.001
N440X0.270Z0.591
N450X-0.130
N460G0X0.320
N470X3.0
N480T1500
N490X-.120
N500Z0.6
N520M5
N530M2
%

[ProProcess]

I am not familiar with the F series.
Does it have an MC-Data page?
If so,what is the Machine Length set to?
If not, how do you set the heastock position at the start of the day?

[mstorto]

we don't have an MC page and the head stock doesn't move, the carriage is sent home. I'm assuming the machine length is set buy the g50 and how the program ends. Your asking the same questions I've been asking..my problem is the book doesn't show the answers. All of our errors are happening because we are setting each tools offests correctly and now the program wont work because of the corrections. The guy who used to run it just brought the tools down close with linear moves, then would add offsets to get the tool centered which worked but not correctly.

[ProProcess]

On the F machine, the heastock is fixed, and is all the way to your right, correct?
when you start the machine and send the carriage/guidbushing assembly to the Home position, where is that? i.e. is it all the way to the left or is it close to the headstock (to the right)?

[mstorto]

head stock is to the right and the carriage goes to the right at zero.

[ProProcess]

OK.
With the carriage all the way to the right, there is no more travel left to make your part.
The carriage need to be left with enough material to make your part and any other shifts that may be in place.

On newer Citizens, there is a Preperation Mode and in that mode you perform what is called a StartPosition where it moves Z as described above.
Does the F have a Preperation mode?

[mstorto]

no prep mode. we actually had a good day today. we changed the g50 to z.65, corrected all the offsets with the tool setter, changed all the linear drill paths to g74 pecks cycles and removed all the BS moves that don't belong there. That G50 was screwing me and the book really doesn't explain it well enough to wrap your head around it. We're going to write a thread program next so I'm sure i'll have problems with that.

[ProProcess]

The G50 should not be changed.
It is a calculation that you get based on your cut-off tool.

I would assume that you're using a Left Hand cut-off tool, is that correct?
If so, what the dimension on this crued sketch...

[Mountain_Hiker]

Yeah man, here I am, ha. I finally joined this forum after I have been observing it for some time. I figure it's time to put my part back in the industry, haha, and bestow some of my knowledge upon others, haha. Just kidding.

Sounds like we are in a similar circumstance. My shop has an older, probably mid 1980's or so, Citizen F20. Nobody seems to know much of anything about it, so I have had to start picking up bits and pieces. I don't think they care to use the machine much though, as I believe they told me they had it given to them, and I don't see many jobs for it, since all of them will leave the cut-off tang on the part since their is no pick-off on mine. There only appears to be a tail-stock support or something. Anyways, on to my other thoughts.

I can tell you a little about what I have picked up on, but by looking at your post, I was hoping the other individual could enlighten us on the matters of discussion.

I heard there was a tool pre-setter for this machine, which we don't have. I have been putting the tools in and shimming them until I don't get a nub when I turn a face. I can tell that G68 is utilized for my coordinates of the top turret, which would be my T21-T25, and then G69 is used for my lower turret, which would be my T11-T15. I'm supposing you would want your cut-off tool on the top turret generally since your parts catcher would hit the other turret tool if it were up, unless your just dropping your parts in the bottom of the machine.

My headstock is also on the right, and the "reference point return" selection on the control puts the support/guide bushing towards the right side of the machine, near the headstock/main spindle. Oh yes, one side note, is that my machine has a "over-run travel release" position on the control which allowed me to jog the machine when I over-travelled it. I didn't even know what some of all the buttons were on my machine. I have to kind of try them and see. There is one button that I don't even have a button cover on. All I know is that it is below "Cycle Start" and "Cycle Stop" buttons. It has two lights in there, if I push what's left of the button, the spindle will stop.

So what I have found to do is to use my cut-off, or start and stop tool, to tell the machine where it's at in the morning and when I mess the machine up. I call the tool up in MDI, making sure it's on the G68 system, then I jog and turn a diameter, measure it, and use the G50 to tell the machine what I just turned, so it knows it's "X" value. For the Z, I unclamp the chuck, which is very important to remember, haha, and I take it to the "reference point return" of "Z," I then tell the machine that is "Z0.0," with my G50 in MDI again, then I tell the machine to move out, maybe 3/4 of an inch past the length of my part. So, if it was a 5 inch part, I told it to move to 5.75 in MDI. I had to put in a "-5.75" because of the way my machine is or whatever. I also, by this point, have told my tool to come back down to my starting diameter value, kind of like a cut-off, cept I did it myself. I also used the MDI to do that with a "G01" and a slow feed-rate with the spindle on. I know what I have put in my program for a start point "X" value with G50 when the program starts, so that's the same diameter I take the tool down to in the beginning.

Now for some thoughts on my tooling, because we don't really have the right tooling necessarily. I used some .500 tools, but it looks like my holders actually use .750 tools or something. I had to put a lot of shims sometimes, haha. Basically, once I used G50 in MDI to tell my machine where that start tool was, then I call up the other tools in MDI, and tell them to go to their "X, whatever value," and "Z0.0" points. I don't do them both at the same time. I also have to MDI the machine into G69 if I'm about to set the lower turret. So then I turn a diameter, and a face pass, and see where my "X, whatever value" and "Z0.0" point is on those tools, and then I use the offset to put them where I want them to be. So far, after I have put in the offsets, then I have done it again, to make sure what I did was right, and make sure that my offset puts the tool where I want the "Z0.0" to be, and make sure it would be turning the right diameter also.

Hope these thoughts help, and I hope the other guy can tell us more about this stuff. My parts catcher isn't coming up and down like it should. I want it fixed, but I don't know how. The other morning I input a program to run continuously to move the thing up and down, but after I stopped it, then it quit working. It does this, one time it will work, and another time it won't. It won't come up at times, but the down has always worked. It's weird, I think it's some kind of "control" component based on what indications I'm seeing.

[MX1]

Guys it's your lucky day, I have been programing and setting up F machines for 16 years, we have 6 on line that we use everyday. By what i've read you guys are a bit lost, so I'll do what I can to get you back on track. These are very simple 2 axis machines that you can do a bunch of neat stuff with.

Lets start with the "zero return". This is at 3 oclock on your mode dial. Once set to "Zero" hold the joy stick down X+, some machines the cross slide will drop then go back up to home others you have to go to the X- position to get it to home. If you get an alarm, turn the control off and power up pressing the "p" and "can" keys, then try rezeroing again. A green light should come on the panel when it's zeroed. You can do the sme with the Z axis, home is all the way to the right, but you have to start near the middle or you'll get an alarm. On most of my machines the Z axis home dosen't work, just make sure the carriage is far enough to the left to make your part without overtraveling. If it does work then in MDI put in G0 W-(part length + cutoff width + .100). The carriage will move this amount to the left.

Now the toolsetter comes into play with the machine. When the X axis is Zero it is actually in the X-.120 position but your POS page may say something completely different. On the toolsetter you have a x scale and a z scale, set both on the red zero and find the closest 0 on the micrometer heads. Put a turning tool holder in and put your cutoff tool so the left side of the tool touches the right side of the center verticle line and the tip of the tool should be touching the center horizontal line. You may need to shim the side and bottom to get it centered. (f-12's & f-16's use .500 tools, f-20's .750). Your tool is now at "X0" and "Z0". When you mount it on the bottom turret it will be at X-.120 when zeroed. The right side of the tool will be Z0. I always use T1100 for my cutoff.

This is when G50 is used in the beginnig of the program. It should look like this:
O1234
G20 (ENGLISH)
G99 (FPR)
G69 (COMANDS TO FRONT TURRET)
G50 X-.120 Z0 (SET COORDINATES FOR X AND Z AXIS)
M6 (COLLET CLOSE)
M3 S2000 (SPINDLE START RIGHT HAND 2000 RPM)

At this point the collet is closed and the spindle is truning at 2000rpm and the machine is at X-.120 Z0. The axis positions should be the same as when you Zeroed them nothing should have moved.

Now I want to center drill and i'll use T2111 tool 2100 offset 11.
GOZ-.02 (CLEARS Z AWAY FROM THE CUTOFF)
T2111 (TURRET 2 WILL INDEX TO T2100 OFFSET 11 BECOMES ACTIVE)
N1(CENTER DRILL)
G68 (COMMANDS TO REAR TURRET)
G0X-1. (MOVES REAR TURRET DOWN INTO POSITON, DRILL HOLDERS ARE X-1. TO BE ON CENTER. TURNING TOOLS ARE X0)
G1 Z.1 F.001 T1311( FEEDS Z.100 AT .001 FPR INDEXES TURRET 1 TO T1300 OFFSET 11 STILL ACTIVE)
G0Z-.02(RAPID BACK TO Z-.02)
T0 (CLEARS OFFSET)
N2(DRILL .125 HOLE)
G69 (FRONT TURRET)
G0X-1.Z-.02T2313 (RAPIDS X-.1 DRILL HOLDER ON CENTER, REAR TURRET INDEXES TO T2300 OFFSETT 13 ACTIVE)
G1 Z.200 F.002(DRILLS AT .002 FPR)
G0 Z-.02
T0
N3 (FRONT TURN)
G68 (REAR TURRET)
G0X0Z-.02 T1113 (OFFSET 13, TURRET 1 INDEXES TO T1100)
G1Z0 F.001
X.150 C.005
Z.175
X.250 C.005
Z.25
G0X.5
T0
N4 (CUTOFF .060 WIDE)
G69
G0X.255 Z.260T01 (OFFSET 01)
G1X-.040 F.0005 (CUTS OFF .0005 FPR)
M7 (OPEN COLLET)
G0X-.120 Z0 (AXIS RETURN TO STARTING POSITIONS)
U0 W0 T0 (CLEARS ALL OFFSETS)
M2 (END OF PROGRAM)

This is for a machine with a gravity bar feeder, an automatic loader would start and end differently.
You don't need the N in front of everyline.
There is a lot of info here, if you have any questions just ask.
George