LinkBack URL
About LinkBacks
Probably. But this will be specific to your machine and does not relate directly to being Fanuc control. You will need to consult your manuals or MTB to see if you even have this function and how to implement it.
change insert part way through cut? We have a Samsung turning center, SL-35MC, with live tooling.
I cant figure out how to stop the program & the spindle, pull the tool away from the part to change the insert, and then get back in where
I left off. Is there a way to do this? (Fanuc controls)
Probably. But this will be specific to your machine and does not relate directly to being Fanuc control. You will need to consult your manuals or MTB to see if you even have this function and how to implement it.
http://www.kirkcon.com/
Closest I get to this on my VMC OiMD is by stoping the machining and doing a restart, starting from the last tool change.Originally Posted by ksmith0110
1) Press feed hold (stop)
2) Press reset
3) Jog the machine into a postion for tip / tool maintenance.
4) Switch to edit, scroll down to the last tool change line (say N1234)
5) Switch to auto and press restart hard key
6) enter 1234
7 select Q type restart using soft keys (press the < > arrow keys to see this on the screen)
8) turn off restart hard key
9) press start button.
The machine will make some preparation moves - normally to the previous location so can move in an unexpected direction !!!
Then it will start running the program again.
I always do a restart with rapids at 0 and % feed set low ;-)
Havent tried this on a lathe though.
ATB
I think the biggest problem I'm having is that I'm using G71 and I'm part way through. Im not sure if the Q Type thing will work. I only have 2 line numbers. N100 & N200. (The start and Finish of my profile)
Well, before continuing this discussion, I would like to know why you are blowing out inserts before finishing a part. What material? What speed? What feed? What depth of cut? What other cutting conditions?
http://www.kirkcon.com/
I'm starting with 304 SS 8.2" in diameter and cutting it down to 6" dia. with a taper to 8" roughly 13" long. The oal is 33". I have quite a bit of stock to come off. I'm going a little less than the handbook calls for, 275 fpm/ .025/rev and cut depth .100" on a side.
on Fanuc you can stop the machine in the middle of a cycle. here's how.....
press feed hold
record X and/or Z position in memory (the memory in your head)
switch to manual mode/handle
do NOT press reset
move the tool away (usually move one axis is enough)
usually spindle will stop when in manual mode but if not, stop spindle with panel button
turn coolant off using panel button
change insert
start spindle
move tool to pre-recorded X and/or Z position (tool will be cutting/rubbing at final position)
turn coolant on
change mode to memory (spindle will probably stop but don't worry)
press start (spindle will start if not already spinning)
press start (program/cycle will continue)
something similar will work if RESTART is available but it is an option not usually common to find enabled.
but yeah, your inserts should last the whole part. try reducing speed/feed or depth of cut or all.
Last edited by fordav11; 01-27-2012 at 02:39 AM. Reason: updated 'stop while in auto mode' procedure
Thanks. My first guess is you have the wrong grade insert and wrong coating too. What is your insert size? Are you trying to rough and finish with the same tool?
275 actually seems a little fast to me for your cutting speed. 200 sounds better to me. 0.025 feed is also a little high. I would start about 0.014. And on depth of cut, I would try to find that happy place that will break chips at whatever feed rate I end up with.
A work around, if you can't get the the right insert and speed/feed/depth combination to run the entire part on one insert, is to break your program up with appropriate M01 option stops where the tool backs off to a neutral position each time to be checked and changed as needed. If you write your program correctly with spindle start and tool offset commands, you will be able to restart at any position prior to the insert failure.
Yes, either of these options slows the entire machining process down. But think how much time you are already losing by changing inserts and restarting by cutting air. Not to mention the cost of inserts. There are some laws of physics that you cannot overcome with gorilla machining tactics. Sometimes you gotta use some fineness and make sacrifices to the machining gods.
Last edited by txcncman; 01-27-2012 at 12:50 AM.
http://www.kirkcon.com/
or apply your Texas methodology and shoot the operator and maybe the next one will do it better
I have found the guide books are usually too fast. after all they want you to buy their inserts so sometimes the feeds and speeds are a bit over the top.
0.025" feed is WAY too much for stainless. 0.012" - 0.015" is more like it and a surface speed of 150-200.
0.100" depth of cut is ok. you could get better grade inserts suited to stainless but general grade is usually ok if you use realistic speeds and feeds.
Restarting half-executed G71 is not possible. It has to be repeated all over again, involving air-cutting for several roughing passes.
If you want to skip previously executed roughing passes (referring to type 1 cycle), use smaller start-X; it would not do roughing above this X. This, however, is a little dangerous method because, after the step-removal pass, the tool would come to the new start-X showing dog-leg effet. This may hit the job.
restarting a G71 IS possible as long as you don't press reset. If you simply break an insert use the restart method I provided at post#7
otherwise to restart from the beginning is the only way sure, but air cuts are not a problem if you use dry run it will take only a few seconds to get back to where you left off.
After pressing the manual button, I can't get the spindle to start again.
Posting Permissions
| | |
