[SirDenisNayland]

Latest gen A20, we've had it since October so I like to think i know what I'm doing by now but this just has me dumbfounded.

The machine keeps overtravelling Z2 when making T31-T34 tool calls. It indexes to the first one fine, does its work, I retract, cancel offset as usual and call the next tool. The Z2 begins to move to return position as is normal, but then moves past zero into overtravel.

Now the kicker is, this only started happening once I touched off all the $2 tools. Prior to touching them off I set the values really far back (set the length to something like -2.0 so that there is just enough room for the tool retracts) and run head1 to get a part in the sub, and it runs fine, no overtravel. So I decided clear the touch off points back to what they initially were to get a part in the sub. Runs fine. Input tool setting values again and it begins to overtravel again...

I'm at a loss for words. The setting values are nothing out of the ordinary.. it just makes no sense at all. The only way I can get it to work is to input a W-.xxx value with the tool call, but that's a bandaid solution and doesn't let me know the problem at hand.

Also, did citizen California shut down or something? I'm on the east coast and I was staying late to get this job running and by timezone they're the only ones that were open.. yet the phone rang and rang and rang, no automated message or voicemail..

Bleh. Im starting to hate citizens more and more with all the god damn anomalies I've documented over the past years I've been doing this crap.

[danrudolph]

I think I gave this advice in another thread:

I've almost always used the Q3 argument in my T31-T34 calls. It forces a full retract of Z2 on the tool change. I've had the over travel problem as well and this is the solution, AFAIK.

I think if the tools are set right around 0.000 length in prep, you wouldn't need it, but when the length goes negative, I've needed the Q3.

How far is your part out of the sub? and is everything set correctly on MDATA?

[SirDenisNayland]

Thanks for the reply Dan. I'll give that a shot, bit like the W- argument I still see it as a bandaid solution.

Part is sticking out of the sub about an inch. I don't set part extension in mdata, I always leave it zero. I've run jobs with similar configs (part length sticking out of sub and same tool lengths) without issue.

All of my values are negative, as they usually are. The thing is, it only works when the values are an extreme negative, like -2"

Here is a picture of the back tools

Lengths are set to -.38, -.38, -1.9, and -.95 respectively. The drill works fine, and when I set all values back to -1.9 it works without issue, so I don't quite think that's the problem at hand, and as I said Ive run other jobs with similar sub/back tool configs..

Also, that damn part dump chute is retardedly placed, can't use t34 unless its sticking way out or the part is way out of the sub lol. As you can see I have to drill 8x deep as well as do turning and threading so I am required to have the part out of the sub as far as it is so I don't interfere with other tools. Fun fun.

Thanks again.

[danrudolph]

Are you calling T34 to spot, then T33 to drill?

If you think about it, when you have normal tools set within the -.5 to .5 length range, you see the sub do a sort of diagonal move to the next tool, advertised to save time.

I think the control has a problem when the tools are that long because the diagonal move can't be done without an OT or hitting the tool, just a guess.

I started using the Q3 to solve a similar problem. My tools were set, T31 -.5, T32 0, T33 -1.5 and T34 -1.5, with a "Back Work Ext" set to .75. The move from T31 or 32 to T33 would OT. Really similar to your setup. I had about .1 between the part and the long drills at full retract.



I'm not sure it's a control bug, well maybe, but the Q3 is there for this reason I always thought, after all the Citizen tech told me to use it...

[SirDenisNayland]

The sub always returns to zero when making tool calls, only time it makes a diagonal move that I know of is when using the Q1 argument which moves directly to the tool position point from the position its in. That or I'm guessing you make your tool calls with x and z arguments? I always just call T3x00; unless I'm trying to save some time because the main is waiting.

Yes I am spotting before drilling, but the same problem was exhibited moving from t31 to t32 which have their lengths set within .005 of each other

I guess ill just have to get used to using the arguments. It's just weird that in nearly a year and dozens and dozens of different jobs that I havnt encountered this problem. One reason I don't usually use arguments is that sometimes I have to use different tooling from the last time a job ran, and as such lengths/centers can vary and that would mean program editing, less plug and play.

May I ask what those white things are hanging off your drills?

Edit::

Now, this is going out on a limb but by any chance were you using sub programs? I'm using a sub program for a milling profile that's repeated on the main.. and its the first time I've actually run a sub program on this machine, and subsequently the first time I've run into this issue... Coincidence?

[danrudolph]

I'm not sure what it normally does anymore, I have Q3 on every T3X00 call now...

Not using subprograms at all on this program, not even macros or anything. I doubt that the two are related.

Sorry I can't be of much more help, but I'm sure someone at Citizen should be able to provide more insight, just a matter of finding the right person, probably in NJ.

As far as other quirks, don't bother trying to use C1-C2 superimposition... was trying to support a .055 dia part using the sub and the C1-C2 superimposition just doesn't work.

Those white things are nozzles I made to blow chips off the drills, worked well enough to run unattended machining delrin.

[SirDenisNayland]

Interesting, I thought that's what those may have been but had never heard of such a thing.

I've used the C1-C2 super imposition, but that was just for part support milling flats, nothing fancy. It worked flawlessly, but then again it was .271 solid 303 and Im guessing you had twisting issues haha.

I typically speak to John or Ron in NJ when all else fails, but sometimes the issues I have are so quirky and hard to explain, partially just me being anal, and I don't exactly like handing out my programs either (never know). I know if I called them they'll just say to put in the Q3 and don't worry about it. It works, but it just bothers me that its something that just started happening out of the blue using similar set up configs I've been using since day one lol.

I have problems running nonconform material and other glitchy random bugs on my K16 that I've given up trying to solve. Fanucs been in multiple times, CPU changed a few times, multitudes of diff coding etc. If the machine alarms it decides to turn the cutoff feedrate to 10x what's in mcdata for some reason and that's just the tip of the iceberg.

Ah well, I guess every machine has its quirks. Maybe we just weren't meant to get to know them so well :lol:

[cogsman1]

The macros that control tool indexing have defaults that make the index happen in the safest way for the machine. There are codes you can add when these are NOT what you like but you know it is safe. When the backwork tools index the machine is being told to put the END of the part 5mm from the TIP of the tool. IF the length of the tool, AND the protrusion of the part, "Back Spindle Length", together do not allow that 5mm distance then the machine will overtravel trying to get there. Reality is that very often your tools and part length create this problem so CITIZEN gave you that ability by simply adding a Q3 to make the spindle go to "Return" position or "position point". When this cannot be done you can use Q1 which will NOT PULL BACK AT ALL, just index sideways. This works fine but if YOU do not put the part in a safe position FIRST it can hit other tools on the way to the desired tool. You have full control in a Citizen at any time but there are default safetys to protect the machine from people that do not READ THE MANUAL and understand what they are telling it to do. "The BEST thing about a CNC machine is it will do EXACTLY what you tell it to do! The WORST thing about a CNC machine is it will do EXACTLY what you tell it to do!"