Plane or Coordinate Shift on Citizen A220 Backworking

[danrudolph]

I have a series of smaller and deeper concentric holes I need to peck drill in Ti with full retract out of the hole. I have G83 cycles written for each hole, but the G83 cycle start at Z0.0 no matter what I try. I'd like to start the second peck cycle at the bottom of the first hole, while still retracting completely to get oil on the drill.

I tried using a G50 to shift the coordinates and then R parameter on the G83 to get the drill completely out of the hole. Calling the G50 before moving to the tool causes the G50 to be canceled (per citizen manual) so I called the G50 after I was at the tool position. It works, but the G83 seems to cancel it out and starts pecking from Z0.0. These holes are all on the back spindle (tools T31-T34 and T52).

What else can I try...? Probably will end up writing the pecks long hand just to get it done, need to make the parts tomorrow... I am just curious to do this in the future.

[steve3three]

either write your own macro, or just issue a WHILE statement.

#123=0(current depth)
#124=.125(depth per pass)
WHILE[#123LE[.25]]DO1
GOZ[#123-.05]
G1Z#123F5.0
GOZ-.1
#123=[#123+#124]
END1

pretty simple. of course this wouldn't be exactly how it would look just an example but you should figure it out from there. having 1 or a few WHILE statements makes it easier to find an error or edit depths and feedrates compared to longhand writing the entire peck cycle. I do this with newer Stars using fanuc controls all the time, so tbh I'm not sure this will work for you but I'd imagine it will.

[danrudolph]

thanks steve.

I could write have written a macro, no big deal. However, I started using the program pre-analysis feature on the control which does not allow macros and saves significant cycle time.

Also, I was just curious if it was possible to do this with the G83 canned cycle which is allowed when using the pre-analysis.

Ran into another problem today -- making a double start 10-32 ID thread using a single point tool. What depth of cut would you try in titanium? I started with .005" but had issues. Hole diameter is .1695" and need to have the root of the thread at .1900" Bigger DOC will put more stress and deflection on the small tool while a smaller DOC will potentially work harden the Ti?

[steve3three]

Ti has been 90% of my work in the past 10 years, it does not work harden, at least I have never seen it happen. However it will melt your tool pretty quick if your going to fast. For a thread like that, small thread, ID thread, double lead, all those things means you need to baby it. It's almost impossible to even tap Ti, that secret I will keep to myself. I would suggest .0025 or even .002 DOC max. You could even take that down further if your still having troubles. Really what you can get away with depends on the tool your using, and the edge prep it has. Flat on the tip of tool.... your allowed a max of .0039 flat on the tip of your tool for a 10-32 thread. I would suggest shooting for that. you want light edge prep, but it needs some prep. to much prep results in tool deflection causing the thread to be tapered which you already know and explained, and can make the burrs worst.

Personally just take it easy, slower RPM's less DOC and should be in the clear.

Good luck.

oh and the pre-analysis feature... is that like the optimaztion I hear everyone talking about? I never ran a machine with that feature, I heard its awesome for speeding up cycles but becomes a nuisance with complex parts that you would typically have macros all over the place. I'm all for it tho, if you can get faster cycles even tho your program may be huge, in the long run it helps the company.

[danrudolph]

thanks again steve.

looking back on another job, cutting a 4-40 OD thread, i was using a .0025 DOC. should have looked at that job before starting this one.

the tip of the tool is a sharp point. i'll take it slow and make a bunch of passes, no big deal. just want to get these parts done.

the program pre-analysis saved us 2 seconds on a 22 second cycle on another job. we were blown away with a 10% improvement on such a sort cycle. i am curious to see what it would to on a longer cycle. it is very picky with respect to what you can and cannot do. no macros, specific bar change method, couple of canned cycles are banned as well. and you're right about it helping the company, especially when it's your own company!

[metal mania 01]

From what I have learned about tapping titanium,I have found it best to use a black-oxide(forming)roll tap. There was another coating that worked very well but it slips my mind right now,it was similiar to a TiaLN in appearance. It has been a while. I will try to figure out what it was called and post later. Also sharper the better with titanium. More force will be generated with larger radius. I used to hand sharpen under microscope to a pristine point and cut forever.