Problem with start and finish of G03 on FP2NC
Close
Login to Your Account
Results 1 to 19 of 19
  1. #1
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default Problem with start and finish of G03 on FP2NC

    My G03 circular cuts generally have problems at start and finish, that look like overruns. E.g. there is some extra metal removed on the inside and outside of the radius at the start and finish.

    Any ideas?

  2. #2
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    703
    Post Thanks / Like
    Likes (Given)
    914
    Likes (Received)
    139

    Default

    Could be a lot of things- ball screw backlash, servo tuning, feed rate, axis drift.
    Are you running tool compensation and using any additional G or M codes?
    Is the problem on inside or outside diameters and how big is the circle and cutter?
    Last edited by Colt45; 02-01-2020 at 09:55 AM.

  3. #3
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    390
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    138

    Default

    When Colt45 said it could be a lot of things he wasn't kidding. I'll add - how are you entering and leaving the cut? Are you rolling in and out of the cut as close to full radii as possible? What is the type, diameter and stick-out of the cutter and the bore size? Excessive feed rate? What happens when you let the cutter do two full revolutions instead of one? Better?

    The list goes on.

  4. Likes Colt45 liked this post
  5. #4
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    2,877
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1341

    Default

    Quote Originally Posted by rimcanyon View Post
    My G03 circular cuts generally have problems at start and finish, that look like overruns. E.g. there is some extra metal removed on the inside and outside of the radius at the start and finish.

    Any ideas?
    Yeah. Your programming is fubar.

  6. #5
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    Yeah. Your programming is fubar.
    OK, that is probably it Emanuel. Please add some value to the conversation. How do you avoid the problem, maybe an example of your code would prove the point.

  7. Likes Mud, ballen liked this post
  8. #6
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default

    Quote Originally Posted by Colt45 View Post
    Could be a lot of things- ball screw backlash, servo tuning, feed rate, axis drift.
    Are you running tool compensation and using any additional G or M codes?
    Is the problem on inside or outside diameters and how big is the circle and cutter?
    The problem shows up with a .25” plunge cut into aluminum with a ⅜” x 2 ½” cut two flute end mill designed for cutting aluminum, running at 2500 RPM, followed by a G03 with a 3 ⅜” inside diameter and a feed rate of 40mm/min (throttled to about 50%). The cut eventually will be 2” deep, done in .25” passes. No tool compensation.

  9. #7
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default

    Quote Originally Posted by 13engines View Post
    When Colt45 said it could be a lot of things he wasn't kidding. I'll add - how are you entering and leaving the cut? Are you rolling in and out of the cut as close to full radii as possible? What is the type, diameter and stick-out of the cutter and the bore size? Excessive feed rate? What happens when you let the cutter do two full revolutions instead of one? Better?

    The list goes on.
    I did some trial and error with different feeds and spindle speeds, but couldn’t completely get rid of the problem, even at what seemed to be very slow feed rates (20mm/min, 2500 RPM, ⅜” 2-flute cutter with 2 ½” of cut).

    The start of the cut was a direct plunge, also with a 20mm/min feed rate. No transition into the circular cut, since I did not approach from the side. Successively deeper cuts were done the same way.

    Dave

  10. #8
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    390
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    138

    Default

    Hello Dave,

    Everything you're doing I would do differently, but let's stick with what you got going on and not reinvent the wheel.

    How about doing everything your doing just the same, but do the whole thing 0.01" inside the finished diameter. Then once you're all the way through the part and the center slug falls out, do a final pass at full depth at the finished diameter. If you get too much chatter, try taking your finishing passes in 3 passes at 0.85" deep per pass.

    That mark or bump your getting is the tool deflecting as it's plunging. (Plunging is the worst possible way to enter the material.) It also has to do with the dwell of the tool in a static position as it's plunging and then transitioning to the arc move. So do all your plunging a short distance away from the finished profile and finish the profile after all the heavy, dirty work is finished like I said above.

    If your machine can do 3 axis simultaneously, instead of plunging, start your arc at Z0. depth and include a Z-0.25 at the end of every arc block. So you'll be doing a full helical ramping move all the way through the part. Then again finish like I said above. Programming something like this in incremental (G91) will make it copy and paste easy.

    As an aside, I'm not sure how you're dealing with the big slug that at break thru is going to be a problem. It wouldn't hurt to program within about 0.003-0.005" of full depth and pull out and stop the machine at that point. Then take a mallet and knock the slug out. Then re-start with your finish pass. This goes for all the ideas I've given. That big slug is a potential problem.

    If you can't do 3 axis, you might want to consider starting in the center of your part and ramping towards the start point of your arc. So on your fist move, put your cutter at Z0. in the center of the soon to be hole, and move to say the right while ramping down your 1/4" like you've been doing. Then when the arc finishes, without lifting the tool, G1 move back to the center where you started while including a Z-0.125 move and then back again to the arc start point with yet another Z-0.125 move. This will give you your 1/4" depth of cut, but the cutter will be doing a gradual ramp which it will like way better then plunging. So in short. A zig-zag ramping move to and from the arc center to the arc cutout radii. Again, programming the whole thing in incremental mode could make it easier. Once you have your zig-zag and arc move, you'll only need to copy and paste it over and over until you hit full depth.

    These are still not the ways I would do it, but it might be a better way for you as things are now using what you've been working with.

    Oh... your feed rate and rpm are both really slow. Though I have no idea what kind of machine you're on.

    EDIT: The above is mostly crap. See below.
    Last edited by 13engines; 02-02-2020 at 09:33 AM. Reason: Talking Crap

  11. #9
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,001
    Post Thanks / Like
    Likes (Given)
    186
    Likes (Received)
    923

    Default

    Sounds like cutter deflection is a lot of the issue. A 3/8" endmill with 2-1/2" flute length is going to be exceedingly flexible. I would expect you are getting a lot of squeal (chatter). Are you? I'd expect some challenge even with a 1/2" necked endmill. If it were up to me, I'd be using a 3/4" or even a 1" endmill. Does your machine not do cutter compensation (G41)? On my FP2NC, I'd use G41 and arc into the cut, which would take care of nearly all of the overcut, especially if I did a finish pass and, better still, repeated the finish pass. I'd still get slight bumps at the ±X and ±Y reversal positions due to backlash.

  12. #10
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    390
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    138

    Default

    This morning laying in bed, which is where I do all my best programming, I realize most of what I offered above is crap. Unless you're running a horizontal spindle machine with a couple of perfectly placed coolant nozzles blasting away, there is no way in hell you will get the chips out of the slot being created. The only way the techniques described might work is if you did two paths next to each other with the 2nd one being 70-80% of the first. This will give you more room for the chips. But really, the whole idea is wrong.

    Like rklopp said and others, (including me but I didn't want to go there) the length to diameter ratio of the cutter you're using is, well, unusable.

    You might start with the largest drill you have in the shop, then move to at least a 3/4 or 1" cutter with 3-4 flutes depending on strategy. I'll leave it at that. Arc lead-in lead-out moves. Cutter comp. Listen to your fellow fp2nc friends.

  13. #11
    Join Date
    Feb 2001
    Location
    Redwood City, CA USA
    Posts
    5,001
    Post Thanks / Like
    Likes (Given)
    186
    Likes (Received)
    923

    Default

    Oddly enough, the FP2NC has a horizontal spindle in addition to a vertical spindle, so the chip-clearing advantage of running horizontally is available. That won't fix what seems to amount to trying to mill with a fishing rod for a cutter (i.e., too flexible).

  14. #12
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    390
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    138

    Default

    Quote Originally Posted by rklopp View Post
    Oddly enough, the FP2NC has a horizontal spindle in addition to a vertical spindle, so the chip-clearing advantage of running horizontally is available. That won't fix what seems to amount to trying to mill with a fishing rod for a cutter (i.e., too flexible).

    Ha... "fishing rod." That's a good one.

  15. #13
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,175
    Post Thanks / Like
    Likes (Given)
    1861
    Likes (Received)
    2507

    Default

    Dave:
    You are cutting a bore no island,yes?
    Does D2 not do G76?
    One line will do the whole job. Includes arc in and arc out on the finished profile...will cut to depth the lot....
    If you drill a big pilot hole G76 will account for that as well and only cut the remaining material....
    Does the cutter comp automatically.program to the size of the hole needed so no math required...just a "D" value in your case. Need larger tool (dia/length) However you will still get tool out cut marks
    no matter what size tool you run when doing straight depth moves at size.....All machines will....Gotta approach and depart from the finished surface with feed moving away from the surface....



    Cheers Ross

  16. #14
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default

    Quote Originally Posted by AlfaGTA View Post
    Dave:
    You are cutting a bore no island,yes?
    Does D2 not do G76?
    One line will do the whole job. Includes arc in and arc out on the finished profile...will cut to depth the lot....
    If you drill a big pilot hole G76 will account for that as well and only cut the remaining material....
    Does the cutter comp automatically.program to the size of the hole needed so no math required...just a "D" value in your case. Need larger tool (dia/length) However you will still get tool out cut marks
    no matter what size tool you run when doing straight depth moves at size.....All machines will....Gotta approach and depart from the finished surface with feed moving away from the surface....



    Cheers Ross
    Ross, actually, I’m making a big split collet: 3 ⅜” OD and 80mm ID, so I can fit a Bridgeport Quillmaster to the Deckel.

    Since you, Rich, 13engines, and colt45 all asked about use of cutter comp, I went back and reread the D2 Operator’s Manual about compensation on the contour. I could be using G41 to cut the outside of the bushing, and G42 to cut the inside. Or as you suggest, G76 (and G75), which have the advantage of doing the downfeed and the final cut.

    OK, got it. What was missing here for me is the need to consider cutter path entering and leaving a cut. i.e. I knew it was possible, saw the examples in the manual, but never understood the need for it. Using a long cutter really amplified the problem, so even the most dense of students might learn...

    Thanks for your help, even Emmanuel.

    I should mention a couple of things: cutter RPM is limited to 2500 RPM because at 3150 (fastest speed) the spindle howls like a banshee, while 2500 is nice and quiet.

    I had a couple of assumptions that some of you called into question: one, I thought a 2-flute end mill would be an excellent tool for a plunge cut, much better than a twist drill. It generated spiral chips like a drill and the plunge cut did not seem to be the cause of the overruns. Second, I thought that a slow feed rate would compensate for the long, fishing rod of a cutter. However, point taken, I will use a ⅝” cutter for the next iteration.

    -Dave

  17. Likes AlfaGTA liked this post
  18. #15
    Join Date
    Dec 2002
    Location
    Benicia California USA
    Posts
    8,175
    Post Thanks / Like
    Likes (Given)
    1861
    Likes (Received)
    2507

    Default

    Dave:
    If your looking for a true circle to get best fit and contact, i would finish the ID using a boring tool in a boring head.
    Profiling true circles requires lots of mechanical/electronic conditions to be optimal to get a good circle...better to use the truth of the spindle bearing for the circle over a profiled
    cut..... Really this sounds like a better lathe job than one run on the mill...
    Cheers Ross

  19. #16
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    390
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    138

    Default

    Hi Dave,

    Sounds great that you're figuring this out. Now I understand where your inside outside statement came from earlier, You're doing a split collar and not just a hole in a block of Aluminum. It never hurts to give the most information available right from the start. I think in general the more we know up front, the more relevant or pertinent the information offered will be.

    One note: As far as your cutter compensation goes. On a milling machine you will tend to use G41 cutter comp 99.9% of the time. That is if you're climb cutting, which in general is preferred. That's because on a bore you will cut in a counterclockwise direction, and on a boss or on the outside of a circle you will cut in a clockwise direction. In both case just mentioned, the offset of the tool will be to the left (G41) of the actual part feature. Don't forget you have to start and stop cutter comp with a linear (G1) move. It can be a tiny one right at the beginning of the lead in arc and at the end of the lead out arc. That's the rules on a Fanuc control. Your control maybe slightly different.

    Seeing as it sounds like you're only making one, if you had on offset or adjustable boring head, you could start with the biggest drill possible and bore the rest. A bored hole will always be rounder and straighter then one machined with an end mill. Even if you milled out the bulk of it, ending with a boring tool will clean and straighten everything up. Plus an 80mm hole is big enough that you can use a pretty stout boring tool.

    Good luck,

    Dave

  20. #17
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default

    Quote Originally Posted by AlfaGTA View Post
    Dave:
    If your looking for a true circle to get best fit and contact, i would finish the ID using a boring tool in a boring head.
    Profiling true circles requires lots of mechanical/electronic conditions to be optimal to get a good circle...better to use the truth of the spindle bearing for the circle over a profiled
    cut..... Really this sounds like a better lathe job than one run on the mill...
    Cheers Ross
    That thought had occurred to me, before I even started this on the mill. Right now the lathe is down, it is undergoing an 80th birthday overhaul, and I needed the quillmaster to help with that work. I like the suggestion to use the boring head, but I am not sure I have the tooling to do the 3 3/8” external surface, I will have to think about that and see what I can come up with.

    Dave

  21. #18
    Join Date
    Nov 2004
    Location
    SLC, UT
    Posts
    703
    Post Thanks / Like
    Likes (Given)
    914
    Likes (Received)
    139

    Default

    Quote Originally Posted by 13engines View Post

    Don't forget you have to start and stop cutter comp with a linear (G1) move.
    This is not the case with the Dialog control- when you program G41/G42, there are 3 different approaches available and they are prompted by the control dialogue. Likewise, when G40 ( tool compensation "off") is programmed, the same 3 moves are prompted by the control, but as departures.

    FWIW- I thought your (13engines') above replies were excellent and you were a bit hard on yourself.

    RimcanyonDave- Ross is correct about G76, I use it almost every day. It's very easy to program and if your machine is in good condition/tune, will make excellent circles- but typically not as good a circle as one generated by a boring head in a decent condition FP spindle. Hard to make good suggestions when you don't give very much info in your first post/question.

  22. #19
    Join Date
    Sep 2002
    Location
    Salinas, CA USA
    Posts
    3,937
    Post Thanks / Like
    Likes (Given)
    216
    Likes (Received)
    183

    Default

    Quote Originally Posted by 13engines View Post
    Hi Dave,

    Sounds great that you're figuring this out. Now I understand where your inside outside statement came from earlier, You're doing a split collar and not just a hole in a block of Aluminum. It never hurts to give the most information available right from the start. I think in general the more we know up front, the more relevant or pertinent the information offered will be.
    Dave, thanks, point taken. Actually, the inside/outside applied to the single cut. The cut looked like I had used a 7/16 drill at the start point, but the G03 was done with a ⅜ cutter. The overrun went in both directions, inside and outside the circular path. Maybe the start of the cut pushed the cutter to the inside and the finish to the outside? I don’t understand how the forces work at the cutter tip.

    Quote Originally Posted by 13engines View Post
    One note: As far as your cutter compensation goes. On a milling machine you will tend to use G41 cutter comp 99.9% of the time. That is if you're climb cutting, which in general is preferred. That's because on a bore you will cut in a counterclockwise direction, and on a boss or on the outside of a circle you will cut in a clockwise direction. In both case just mentioned, the offset of the tool will be to the left (G41) of the actual part feature. Don't forget you have to start and stop cutter comp with a linear (G1) move. It can be a tiny one right at the beginning of the lead in arc and at the end of the lead out arc. That's the rules on a Fanuc control. Your control maybe slightly different.

    Seeing as it sounds like you're only making one, if you had on offset or adjustable boring head, you could start with the biggest drill possible and bore the rest. A bored hole will always be rounder and straighter then one machined with an end mill. Even if you milled out the bulk of it, ending with a boring tool will clean and straighten everything up. Plus an 80mm hole is big enough that you can use a pretty stout boring tool.

    Good luck,

    Dave
    Good suggestion, will take that approach. Thanks for the reminder to use G41 for both inside and outside.


Tags for this Thread

Bookmarks

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •