CNC Drilling Question
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 23
  1. #1
    Join Date
    Sep 2019
    Country
    CANADA
    State/Province
    Ontario
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default CNC Drilling Question

    So im currently drilling alot of deep holes in our mould. Ive pre-drilled all the holes 3" deep with a shorter drill before going in with a longer drill to reach the required depth. My question is, is there a way to get it to start 2.9" down inside the holes, but come back up past the top of the piece for chip clearance. Right now we have it cutting 3" of air before it even starts to cut material. And add on top of that if the drill dulls having to sharpen it and start that hole all over again.

    Thanks.

  2. #2
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    2,462
    Post Thanks / Like
    Likes (Given)
    442
    Likes (Received)
    1748

    Default

    Yes, there is a way to do that.

  3. Likes mhajicek liked this post
  4. #3
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    3,124
    Post Thanks / Like
    Likes (Given)
    1722
    Likes (Received)
    2040

    Default

    are you using CAM ?
    With my CAM it is easy,when you change drill bit to longer size change top of job to the depth your shorter drill got to.Just be sure to add that amount to your rapid plane.Give us a little more to go on and someone can tell you for your specifics

  5. #4
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,180
    Post Thanks / Like
    Likes (Given)
    721
    Likes (Received)
    1761

    Default

    Quote Originally Posted by jrmach View Post
    are you using CAM ?
    With my CAM it is easy,when you change drill bit to longer size change top of job to the depth your shorter drill got to.Just be sure to add that amount to your rapid plane.Give us a little more to go on and someone can tell you for your specifics
    Emphasis on the part that will save you from a shiny new 2 piece drill.

    Sent from my SM-G973U using Tapatalk

  6. Likes jrmach liked this post
  7. #5
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    348
    Post Thanks / Like
    Likes (Given)
    68
    Likes (Received)
    103

    Default

    Quote Originally Posted by 2quix View Post
    So im currently drilling alot of deep holes in our mould. Ive pre-drilled all the holes 3" deep with a shorter drill before going in with a longer drill to reach the required depth. My question is, is there a way to get it to start 2.9" down inside the holes, but come back up past the top of the piece for chip clearance. Right now we have it cutting 3" of air before it even starts to cut material. And add on top of that if the drill dulls having to sharpen it and start that hole all over again.

    Thanks.
    In the time it took to drill that extra 3" of air on that first hole you could've hand coded the rest of the holes and had them ready to go by time that hole was done.

  8. Likes Bobw liked this post
  9. #6
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,433
    Post Thanks / Like
    Likes (Given)
    1480
    Likes (Received)
    1621

    Default

    Quote Originally Posted by dodgin View Post
    In the time it took to drill that extra 3" of air on that first hole you could've hand coded the rest of the holes and had them ready to go by time that hole was done.
    Or went back to the cam and programmed it correctly. What is your point?

    As others state, need a little more info. Yes there is a way to do that, but we need to know what cam, if any, you are using, or if you are fingercamming it or what. Plus machine and control would be helpful.

  10. #7
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2610

    Default

    Quote Originally Posted by 2quix View Post
    So im currently drilling alot of deep holes in our mould. Ive pre-drilled all the holes 3" deep with a shorter drill before going in with a longer drill to reach the required depth. My question is, is there a way to get it to start 2.9" down inside the holes, but come back up past the top of the piece for chip clearance. Right now we have it cutting 3" of air before it even starts to cut material. And add on top of that if the drill dulls having to sharpen it and start that hole all over again.

    Thanks.
    .
    i believe its usually use G98 or G99 to set initial Z
    G0 G98 Z2.0
    G83 X0. Y0. Z-6.0 R-2.9 Q0.5 F3.
    X2.0
    G80
    ....so initial Z set for Z2.0 it rapids to R-2.9 down into hole and peck drills to Z-6.0 when there it rapids to initial Z2.0 before going to next hole
    .
    with G99 it goes to R between holes so R must be above hole only when it sees G80 (end of drill cycle) does it go up to initial Z with G99
    .
    obviously you would have to test it on your cnc above or clear of part to confirm ok then put tool comp back to normal to run program

  11. #8
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2610

    Default

    if using short peck G73 you can
    G0 G98 Z2.0
    G73 X0. Y0. Z-5. R-2.9 Q0.5 F3.
    G73 X0. Y0. Z-6. R-4.9 Q0.5 F3.
    G80
    .
    it rapids to R-2.9 into hole from Z2.0 short peck drills to Z-5.
    pulls out rapids to Z2.0 then rapids to R-4.9 to drill to Z-6.0
    .
    thus a short peck that pulls all the way out once then goes back in to resume drilling
    .
    obviously test it with adjusted tool comp well clear of part to confirm working as expected before putting tool comp back to normal and running program

  12. #9
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    1,064
    Post Thanks / Like
    Likes (Given)
    638
    Likes (Received)
    1026

    Default

    It's still only going to retract to the R plane between pecks. I think the OP wants to start in the hole and retract above the part for each peck.

    Haas does it but I don't know about any other controls.

  13. Likes Bobw, Nerdlinger liked this post
  14. #10
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    348
    Post Thanks / Like
    Likes (Given)
    68
    Likes (Received)
    103

    Default

    Quote Originally Posted by Mike1974 View Post
    Or went back to the cam and programmed it correctly. What is your point?

    As others state, need a little more info. Yes there is a way to do that, but we need to know what cam, if any, you are using, or if you are fingercamming it or what. Plus machine and control would be helpful.
    Point is I hate doing this kind of shit in cam. Obviously don't know the extent of what the OP is dealing with, but assuming deep hole drilling with spindle speed variations at certain depths going into and coming out of the hole, I'm hand coding this sans canned cycle, plugging it into a plotter and watching like a hawk before it goes into the machine.

  15. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,433
    Post Thanks / Like
    Likes (Given)
    1480
    Likes (Received)
    1621

    Default

    Quote Originally Posted by dodgin View Post
    Point is I hate doing this kind of shit in cam. Obviously don't know the extent of what the OP is dealing with, but assuming deep hole drilling with spindle speed variations at certain depths going into and coming out of the hole, I'm hand coding this sans canned cycle, plugging it into a plotter and watching like a hawk before it goes into the machine.
    <<shrug>> Different strokes and all. I am not sure what the OP has at his disposal, or control or whatever so I guess it is a moot point. We do 99% of any reworks to program in cam so it is saved for next time we run the parts. But if it is a one off I could certainly see making some hand edits at the control and just gitin' er done.

  16. #12
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    348
    Post Thanks / Like
    Likes (Given)
    68
    Likes (Received)
    103

    Default

    Quote Originally Posted by Mike1974 View Post
    <<shrug>> Different strokes and all. I am not sure what the OP has at his disposal, or control or whatever so I guess it is a moot point. We do 99% of any reworks to program in cam so it is saved for next time we run the parts. But if it is a one off I could certainly see making some hand edits at the control and just gitin' er done.
    I only do it that way because I haven't learned the custom drill cycles in Mastercam and I was ashamed to admit it.

    But yeah, the times I've done it have been for anywhere between 1 and 5 holes. Any more than that and I'd cam it.

  17. #13
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,749
    Post Thanks / Like
    Likes (Given)
    1246
    Likes (Received)
    3568

    Default

    Some controls will do it, but I think the easiest way is to just post It longhand. Done.
    If you've got a lot of holes, use a subroutine.

  18. Likes Nerdlinger liked this post
  19. #14
    Join Date
    Jun 2012
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    3,124
    Post Thanks / Like
    Likes (Given)
    1722
    Likes (Received)
    2040

    Default

    Quote Originally Posted by Cole2534 View Post
    Emphasis on the part that will save you from a shiny new 2 piece drill.

    Sent from my SM-G973U using Tapatalk
    Yeah,,to the OP,,,put emphasis on rapid plane

  20. #15
    Join Date
    May 2017
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    931
    Post Thanks / Like
    Likes (Given)
    1105
    Likes (Received)
    573

    Default

    The best way IMO is to add a custom deep-hole drilling cycle to your post processor. The tool mfg. often wants you to spin slowly while feeding in, then turn on thru-coolant and spin up, then feed in at a slow rate for a bit, then get to full speed, then at the bottom turn off coolant, spin slowly, and feed out. Once you set this up in your post processor it becomes as easy as programming any other hole.

  21. #16
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    I think something like this would work...the G99 in the G83 cycle would bring it up to Z.1 between pecks but the G01Z-2.9 line right before would move the drill down in the hole at a high feed rate before you start pecking. The P word in the M98 line calls the sub program that begins with the N number equal to the P number (100 in this case) and then zips back to the main program after the M99 line in the sub. So all you have to do is keep repositioning in X and Y and calling up the sub to do the drilling. Good luck!

    ;
    ;
    G0X0.Y0.;
    M98P100;
    X2.0;
    M98P100;
    X4.0;
    M98P100;
    ;
    ;
    ;
    N100;
    G01Z-2.9F100;
    G83Z-6.F16.Q.2R.1G99;
    G80;
    G0Z.1; (I think the G99 in the G83 line would put the tool here anyways?)
    M99;

  22. #17
    Join Date
    Jan 2019
    Country
    SWEDEN
    Posts
    154
    Post Thanks / Like
    Likes (Given)
    52
    Likes (Received)
    18

    Default

    "Custom drilling cycle"??? This is standard FANUC folks!!!

    G0 Z5
    G98 G81 R-2.5 Z-10

    Done!

  23. #18
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,033
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2610

    Default

    G98 and G99 and G83 and G73 can be used many ways. point is G98 at end on drilling EACH hole it goes back to initial Z and not to R like it does with G99
    .
    useful if you want R to be rapid down into the already drilled hole and drill to go to initial Z out of hole for moving to next hole location
    usually easier to write (short peck WITH a long peck)
    G17
    G0 G43 H1 Z4.0
    G98 Z2.0
    G73 X0. Y0. Z-5. R-4.0 Q0.5 F3.
    G73 X0. Y0. Z-6. R-4.9 Q0.5 F3.0
    G80
    the line with G98 sets initial Z and if on a line by itself its easier to read. since i have used it many hundreds (if not thousands) of times i prefer it written so easier to read. like i already said using a short peck with a long peck is useful too as when over 6" deep on horizontal holes external coolant does not normally reach drill tip and a pull out of hole to clear flutes of chips and wash it with coolant can help considerably. sometimes if rapid too fast the chips dont wash off flutes and fast rapid back into hole can compress chips still in hole and break a long drill bit
    ....and really long drill bits often you long peck but keep drill tip a inch or 2 in the hole as once out of hole the drill tip will whip around considerably. sometimes have to enter and leave hole at slower rpm and change to higher rpm when safely in the hole
    .
    obviously on a 5 axis machine you need to state G17 G18 G19 or the drilling plane or axis. not all machines only drill using Z some drill in X or Y too. same with tool comp G43 and G44, you can drill toward negative or toward positive direction. when complicated it helps to run cycle well clear of the hole drilling air to see if everything working as expected
    .
    remember you can program a hole at same XY location but with different Z and R. that obviously can be done in CAM too. same XY but program it like drilling 3 different holes
    .
    short peck is also useful if long drill if feed too fast the tip not drilling into as fast as tool holder is moving and long drill starts bending. the short pull back on short peck helps let the long drill straighten out. obviously if 2 holes at 90 degrees are suppose to meet 6" deep into part its not good if the holes are curved enough the holes do not connect. got to watch the feed rate with longer drills even if they do not break a curved hole can still be a big problem

  24. #19
    Join Date
    Aug 2013
    Location
    Chicago, IL
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    582
    Likes (Received)
    311

    Default

    Quote Originally Posted by Tichy View Post
    "Custom drilling cycle"??? This is standard FANUC folks!!!

    G0 Z5
    G98 G81 R-2.5 Z-10

    Done!
    Right, but I think OP wants to peck and retract above the part for chip clearance. Wait...does G98G83.... retract to initial Z point or R-plane while pecking for chip clearing???? I thought the individual pecks always back off to R plane and G98/99 only affect where it retracts to after reaching final z depth??

  25. Likes Booze Daily liked this post
  26. #20
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,749
    Post Thanks / Like
    Likes (Given)
    1246
    Likes (Received)
    3568

    Default

    Quote Originally Posted by Nerdlinger View Post
    Right, but I think OP wants to peck and retract above the part for chip clearance. Wait...does G98G83.... retract to initial Z point or R-plane while pecking for chip clearing???? I thought the individual pecks always back off to R plane and G98/99 only affect where it retracts to after reaching final z depth??
    it retracts to the R plane, R stands for Retract. When you post it longhand, you can make it do whatever you want, and it will run on any machine, any control.

  27. Likes Nerdlinger liked this post

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
  •