Machsupport Forum
G-Code, CAD, and CAM => G-Code, CAD, and CAM discussions => Topic started by: alkassell on October 29, 2009, 12:26:56 PM
-
I'm wondering if there's a way to control the height at which the z transitions from rapid plunge to feed when using G83. It appears to be set at .010" now, but my machine's deceleration from rapid on the z takes more than .010", causing the quill to 'bounce' the bit into the part hard before it starts feeding (chipped a couple of bits trying to figure out what was going on). Thanks, Alex.
-
If you go into config ports and pins and them choose the mill options tab there is an option to change the G73/G83 peck distance.
-
Thanks Graham,
That's one of those settings that was buried away in Mach. Now I remember Brian commenting on it at the Cabin Fever Show when someone asked a similar question about peck drilling.
Not sure you will even find it in the manuals.
RICH
-
Thanks for the reply Graham, but I think that's the wrong variable for what I want. The problem I have is that the quill rapids back down to .010 above the last height it drilled to, and my machine rapids too fast to slow down to the feed speed in .010", resulting in the bit slamming down into the work at every peck. I think the variable under "ports and pins" controls the height that the bit retracts up to before rapiding down again. I've got Mach 3 , Ver. R3.042.029, which I think is current ( just making sure my " ports and pins" has the same options as yours). Thanks again, Alex
-
Hi Alex,
I suspected changing the value circled in the macro would adjust the clearance. I tried several times with different values and still it stays at .01 when running a file.
I may be barking up the wrong tree though. ::)
Just thought I'd give it a shot.
Anxious to see how it's done too.
Russ :)
-
Thanks Russ - I tried that too, with some trepidation ( I know almost nothing about programming ), and I also saw no change. I wondered if there was another macro I'm not looking at, or ? I spent some time on it, and decided to try and find someone smarter than me to figure it out ( that shouldn't be hard...). Alex
-
I think you will find that the macro M1083.m1s is for turn only. the mill ones are hard coded into mach from what I remember so your only option is to write your drill cycle as a sub program and call it as you need it.
Graham
-
The problem I have is that the quill rapids back down to .010 above the last height it drilled to, and my machine rapids too fast to slow down to the feed speed in .010", resulting in the bit slamming down into the work at every peck.
Are you sure it's slamming into the work? Just guessing here, but G83 puts Mach in exact stop mode. Is it possible the jerk from the stop makes it appear that it's hitting the work? Because If it's hitting the work, that would mean it's overtravelling and losing position, since your saying it's going at least .01 below where it's supposed to, right?
-
Thanks Graham, that's what I suspected but wasn't sure of how to say it.
Changing the macro does work in turn as you say though.
Alex, I'm with Gerry.
And......do you have any backlash in your Z ?
Is it a mill or router ?
Any flexing of the structure ?
Otherwise, how could the tool possibly hit the work ?
Russ
-
My machine is a Bridgeport cnc, upgraded in '08. It does take some time to decelerate from rapid - usually not an issue when I program with Mastercam, because by default it sets the feed plane to start .050 above the surface ( doesn't for G83, because it's a canned cycle control ed by Mach 3). The mill doesn't lose position on any axis, and the rapid takes more than .010" to decelerate in any plane. The quill will 'bounce' on a stop, and be at the correct height to start feeding at the end of the 'bounce', but unfortunately that 'bounce' brings the bit into contact with the work on a G83 ( yes I'm sure - chipped 2 bits on some 304 SS, the second because I thought it was an incorrectly set tool offset that chipped the first. Watched closely the second go round, and the bit bottomed on ever peck). I could slow down the rapid to below it's max, but that seems a waste for every other cycle. I know that many other machines, if not all, need some room for deceleration (not sure how you could go from rapid to zero without some 'bounce' - isn't that the reason for a slow zone with the soft limits, and not setting the feed plane to the exact height of the work surface?). I haven't checked carefully for backlash on the Z - my parts have been dimensionally correct, but since the Z really only cuts on one side of the work, this could still be accomplished with some backlash ( unlike X and Y, which cut with the ball screws loaded both ways). The frame is a dedicated cnc frame ( dovetailed J head, not fixed ) so it should be stiff enough.
It sounds like I'll have to learn to use a subprogram - if anyone can point me in the direction of good info on subprograms, I'd appreciate it ( new to me - until recently I had done all my programming line by line.... My first machine was originally run off punch tape). Thanks for all the input, Alex.
-
You are confusing me with the word 'Bounce' Mach decelerates before it gets to the stop position so there is no bouncing of anything. It in no way goes past the end point and then back. If it did then the axis would be out of position from then on.
The acceleration and deceleration are set within the motor tuning so you can make the axis slow down over a greater distance if needed. If the tool is hitting the work then you ether have a setting problem or major backlash issues and possibly tight axis gibbs causing drag and drop on the Z axis.
Graham
-
Thanks for the reply Graham - took 'till now for me to get the time to experiment. This is what I've observed: If I set the retract height to be high above the workpiece, then it seems I can escape the problem somewhat. The problem seems to be if the distance between the retract height and the last depth drilled is too short. If I leave roughly .8" between the work surface and the retract height, it works with essentially no 'bounce'. My theory is that it's still ramping up to rapid when it tries to ramp back down to feed if the retract / plunge height is too small (I was retracting to .1" originally). The result of increasing the R settings so far is that it pecks air for a few cycles while bouncing, then works properly when it gets to the top of the part: As the distance of the rapid increases, the 'bounce' at the end decreases until there is none. I've thought about playing with the motor tuning ( would faster acceleration help, so it gets to its rapid speed sooner, although it seems counterintuitive to go faster?), but since it's a little out of my comfort zone, I thought I'd consult first. If I were making a godzillion widgets, it would really matter, but for now I guess I can live with it as is, or long code around it ( small job shop - short runs usually). The spindle doesn't seem to lose position ( haven't yet tested it with an indicator, but it will drill multiple holes without a visible change - if I have time today I'll check it with an indicator at the start and finish of multiple cycles). I'm new to using Mach 3, and not the one who did the motor tuning - the people who did that are far more knowledgeable than me, so I'm reluctant to tinker with what they've done (it's a bridgeport upgrade, and I believe most of the values used are ones from bridgeport, but I could be wrong). So far this is the only cycle that's shown any issues - all parts have been within tolerance, although I've avoided G83 because of this issue.
Thanks again for the help, Alex
-
My theory is that it's still ramping up to rapid when it tries to ramp back down to feed if the retract / plunge height is too small (I was retracting to .1" originally).
Impossible without losing position.
-
I still suspect backlash as being the problem.
Assuming you have a ballscrew on the quill, the counter balance spring will hold the quill up against the drive at all times. (or near neutral weight)
The momentum of a rapid Z down could overcome the spring and coast through the backlash.
If you have the rack and pinion drive method, it could be much worse as far as backlash goes.
I'd check the backlash closely.....then go from there.
Russ
-
I am not sure of which drives you are running but it sounds like the PID tuning is out of whack. When setting up mine it was possible for the position to oscillate if the tuning was off.
-
Hey alkassell
Any updates on what the problem was?
Mike
-
Thanks for the interest Mike - I haven't had a whole lot of time to spend on it - have to make those widgets, and I have a workaround. Here's what I have done:
I ran a program peck drilling 80 holes, with 10 pecks per hole, and touched off on an indicator before and after to see if it's losing position, and it was roughly .0006" off (from memory) - considering my quick set up, that the tool's not flat and the machine was made 20 years ago, I consider that to be no error. A friend of mine who is a lot more knowledgeable than me ( that's most people ) said "We should probably stop calling our term "bounce" and call it servo following error on rapid moves...as I understand it all machines have this, and that is why a programmer never rapids right to the start of cutting, or even .010" close!". He also told me on the phone that Mach 3 has a closed loop feedback with the galil motion control card I have so it knows in real time what the encoder shows, so indeed, it can overrun its mark, and then correct without losing position, unlike most other systems ( hope I got that right ).
Anyway, I think that motor tuning can cure it, but since it doesn't lose position it would mean that my rapid would be slower for everything else, and I don't do that much peck drilling, so I've been reluctant to slow it down. I probably shouldn't worry about speed - I do short runs, so the difference would be negligible, and if it keeps me from chipping a tool down the road, it would time ( and $$) saved.
Alex
-
FWIW,
A little off thread.
Haven't done much peck drilling, but have tried out the macros that Melee posted. The latest updates include macros for the mill. See link below. The ones on the lathe worked here and need to check the mill ones out.
I will say that if you are going to peck drill the axis doing the pecking needs to be solid ( that's why i don't do much
peck drilling on my Atlas mill ( quill just has too much backlash ). I did experiment with the lathe ones and will tell you they worked great. Peck drill little .020" holes and rapid peck drilling where the return to start the drilling is within .001" and if bad ....broken drill.
My only point is that if your axis is not accurate, has backlash, or just dosen't work very well ( for whatever reason), peck drilling may not be a something to do.
http://www.machsupport.com/forum/index.php/topic,13400.msg87932.html#msg87932
Like i said FWIW,
RICH
-
Thanks Rich, any input is welcome. If the macro allows me to change the height at which it changes from rapid to feed, it should cure all my ills ( at least for pecking ). Whatever the reason, .010 isn't enough room for my quill to decelerate to the feed speed. My workaround has been to drill a few cycles of air above the surface first, making it start feeding higher up - obviously a waste of time if it can be cured. I'll check out the macro when I get some time - I've got a few glitches to work on anyway ( VFD speeds with cone pulleys, soft limits, etc. ), so I'll have to make some time.
Thanks, Alex
-
Thanks for posting back Alex...I was very curious as well.
He also told me on the phone that Mach 3 has a closed loop feedback with the galil motion control card I have so it knows in real time what the encoder shows, so indeed, it can overrun its mark, and then correct without losing position, unlike most other systems ( hope I got that right ).
This is great info that I/we were not aware of......it explains a bunch.
Thanks again,
Russ
-
Hi Guys.
The DSPMC that I use does the same thing with the encoders. It closes the loop and then feeds the actual position back into Mach3. As I said prior and you friend has just said, it is the PID tuning of the servo drive.
If you slow down the rapids you can run a tighter following error. If you retune the PID loop the problem may go away without losing rapid speed. On the DSPMC there is a nice tuning "wizard which graphs the commanded versus actual position so you can see where and how much you are out of position. I believe that Galil has something similar.
On slow moves I bet it tracks within tenths or better. On rapid moves and if the tuning is not correct, you can be off significantly and in your case the servo will overshoot and if the tuning is far enough out you can actually see it move back and forth until it settles in. Using too much "I" term in the PID will cause it to take time to settle in.
Hope this helps.
Merry Christmas.
Mike.
P.S. The reason I asked, other than I am a nice guy, is that a lot of times people forget to give the final solution to a problem and although only a few people have participated in the thread there are sometimes hundreds of people waitng for the answer.
-
Thanks Mike, I'll check into this some more - seems like very good info ( I'll see if I can get my friend to help - I've run cnc's for a while, but new to figuring out what makes them go - onsite, real time help will be a huge plus, and might save me from catastrophic mistakes). I always intended to post more, but since I didn't have any real resolution, or even progress, I thought I'd wait. I guess I should've been more impatient - I'm getting some good info. Thanks again, Alex