Put both X and Z move in line N1000.
I am running a Citizen A20 with a Fanuc control and am trying to get a G71 stock removal cycle to work and am having trouble with it. The part has a radius on the end which transitions into a 8.5 degree taper and then into a .75 degree taper in a Z.528 long segment. I am not clear how to use the G71 but this is what I tried with the information I had.
(ROUGH FIRST SEGMENT)
G0 X.5 Z-.03
G71 U.04 R.02
G71 P1000 Q1010 U.003 W0 S1=#102 F#112 T02
N1000 G0 G41 X-.05
G2 X.0561 Z.0237 R.0278
G1 X.1226 Z.2463
N1010 G40 X.5
I am getting an alarm on the second G71 line that says, "PS0325 UNAVAILABLE COMMAND IS IN SHAPE PROGRAM " . I put a parenthesis around the G71 line to test the numbers and it ran just fine but I want the stock removal cycle so it doesnt take it all in one pass.
Does anyone have any suggestions for me or see something wrong with my code?
Put both X and Z move in line N1000.
I tried putting the Z in line N1000 and got the same results.
Try Taking the S1=#102 & T02 out of the G71 line, Select the offset and set the spindle speed before before going into the cycle. If that doesn't work, try turning on Rad comp, before going into the cycle as well, all though I wouldn't suspect that has anything to do with it.
Yes, spindle speed calls should be prior to the tool call if you ask me, to be sure the spindle is at speed before the index as it gets into position and starts cutting really quickly. Dont get me wrong, they jump to speed rather quickly, but its just a habit and a good one if you ask me. Also initialize your tool offset when you position the tool before your cut.
Lastly, I can't say ive used the cycle, but I'm willing to bet your part will have unwanted "bumps" where the tool meets its prior cut on the final passes, and that all the messing around youve done trying to get this to work you could have simply programmed a path yourself and been running. Since the part, at least this section is only just over a half inch long and about 1/8 diameter I have to wonder why you are even considering using this cycle unless your material is well over half inch. I hope your tooling is rather sharp because you're going to have deflection as well when its on its final pass and what your working on is no longer supported by the guide bushing.
My suggestion ... take the cutter comp out ... if you want to run cutter comp in the cycle, make the comp start up block before you call the G71 ... cancel the comp after the last line in the cycle.
The better way ... IMHO ... leave comp out ... run a final profile / finish cut with cutter comp on. The error caused by the TNR in roughing can be cleared up with a finish cut using comp ... and you'll have a lot less errors and problems in roughing.
Hope this works ... please let us know.
Real World Machine Shop Software at Kentech Inc. - Real World Machine Shop and CNC Software
I agree with bluechip -- the error is saying that there is a command that cant be used in the shape program. The only command other than G0/1/2 in the shape program is TNR comp. I would be willing to bet the Citizen prog manual says you can't call (or maybe even use?) TNR comp in G71.
Also agree with SirDennis -- I have been there and wasted time trying to get something that should be easy to work when I should have just done it long hand.
I have a part that I take in two passes (.625 down to .320), was getting a weird blend line on it resulting from unequal DOC as the tool made its final pass. Thought the rougher was going too far in Z and gouging the part. But it wasn't, just the DOC variation creating different pressures at the tool tip. Solution was to make the roughing pass an exact offset of the finish profile of the part.
Thanks for all the advice. I gave up on the G71. The reason I didn't wan't to long hand it was because I had several segments and thought the G71 would save some time. I ended up and roughed it out with a loop. I am cutting 42 Rc material and am getting very small steps at my blends. I roughed the bulk of material with T2 and then made a semi finishing pass to the exact geometry with a .006 positive "X" offset leaving only .003 per side for finishing. I changed to T3 and finished the segments to the geometry. I stayed .03 back to try to blend but am still getting steps. Is there a way to blend perfectly or will there inevitably be a step?
danrudolph- How did your blends end up coming out?
Blends are tough.
On the part I was talking about, it wasn't really an issue, I think i was turning about equal passes from .625 down to .320 and the length of the part is less than 1 inch. The part is basically a cone from .320 to .600 over 1 inch so my roughing pass was less than my GB land. Once I had the weird tool pressure issue figured out there was no blend on that part.
I have another part that I have to turn, use the live tools then pick up and turn again in the middle of a arc. I played with the tool approach when I come in to pick up the turn where I left off. Best thing I can recommend is trying to bring the tool in on a tangent arc to ease into the blend. Hard to describe, and there was still a slight blend line, but it was acceptable.
If you can maybe give a little more info about the shape of the part and where your blends are, maybe a sketch, we could probably give more pointed advice.
Essentially what Dan is saying is that the program numbers won't literally reflect the outcome numbers. I always try to make blend spots in grooves or other locations if possible or make it in one shot. I personally hate playing with blends and will avoid them as much as I can. No matter what a blend will never be perfect if you ask me.
The part I am trying to machine looks like a very simple Swiss part. The problem is the material is .500 diameter with a hardness of 42 Rc and gets machined down to a very small diameter. I had ok luck turning this the traditional Swiss way with a full depth cut. There is a tremendous amount of tool pressure and the sizes were unpredictable. This is why I thought I would rough small segments and try to blend them together.
Does anyone have any suggestions for tooling and speeds & feeds for this hard material with a large depth of cut?
I did come in on an arc to try to blend the segments staying back a little to blend in to the existing geometry. I am starting to also realize that just because the numbers are right in the code doesn't mean the outcome will be good. I think I should go back to one full depth cut but my speeds and feeds along with the right insert will need to be right on. Any suggestions?