Need Help! Drilling problem - machine crash


Page 1 of 3 123 LastLast
Results 1 to 20 of 60

Thread: Drilling problem - machine crash

  1. #1
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    36
    Downloads
    0
    Uploads
    0

    Default Drilling problem - machine crash

    Hi Guys

    I'd appreciate if someone with experience of tormach / g-code could cast their eye over this.

    I have done drilling operations before with no issues but this has me stumped.

    Scenario - step 4 of a program (I'm having to run them individually as the ATC is offline).

    1 to 3 work fine, All tools are correctly measured and offset.

    Then this simple drilling operation is run. In this case the drill is driven deep beside the work for no reason I can see. Then dragged into the side of the work (snap) and across to the start point of the hole. The chuck then raises and the program works as I would expect it to. Then it slams back down far too deep into the work.

    The code was created in Fusion 360 and the simulation runs fine. The post processsor has not changed. The machine has been updated to 2.7.3 but I rolled it back to 2.7.2 and it still does the same thing.

    I"d appreciate any insights !

    Similar Threads:
    Attached Files Attached Files


  2. #2
    Member
    Join Date
    May 2013
    Location
    United Kingdom
    Posts
    35
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    According to this article
    The G98 and G99 G Codes
    The G98 and G99 G Codes
    Here is this program explained line by line

    Z15.0 M08;

    First, we bring the drill down to 15mm above the surface of the material and turn on the coolant with M08

    G82 G99 Z-4.0 R1.0 P500 F50.0;

    This line sets our counterbore canned cycle by using G82 and sets the movement to our hole with G99, this tells the machine that once the first hole is drilled to retract to the R1.0 value and not the Z15.0 set by the line above.
    The Z-4.0 is the depth of the counterbore
    The P500 value is the dwell time that is set to 500 milliseconds that will take place once the drill has reached the bottom of the hole.
    F is our feed rate in mm/min.

    X20.0;

    This is the distance from the first hole to the second along the X axis, it is taken as an incremental move and can include a Y movement and an optional Z depth if the depth of the hole differs from the first. The G99 code is still active from the line above so the drill will retract to 1.0mm above the surface as defined by the R value.

    G98 X40.0;

    This line drills our third hole 40mm in the plus direction along the X axis. It retracts to Z15.0 above the surface of the part after drilling the previous hole. The G98 code tells the control that we wish to ignore the retract value of 1mm that we defined by R in our canned cycle line and to return to the Z15.0 distance. Safely above our clamp.

    G99 X20.0;

    The final hole is drilled 20mm in X from the last hole, the G99 code tells the machine to retract back to the R position and not the Z position.

    G80;

    The G80 command is the G Code we use to tell the control that the canned cycle has ended.

    It is common to make the mistake of putting the G98/G99 on the wrong line. An easy way to remember it is that we add it to the hole position after the obstacle and not on the hole position before.




  3. #3

    Default Re: Drilling problem - machine crash

    Nothing is jumping out at me. Are you sure your tool length is properly set? Are you using the right work offset? Can you share the entire program instead of just the drill op?



  4. #4
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    12258
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by oldlock View Post
    Hi Guys

    I'd appreciate if someone with experience of tormach / g-code could cast their eye over this.

    I have done drilling operations before with no issues but this has me stumped.

    Scenario - step 4 of a program (I'm having to run them individually as the ATC is offline).

    1 to 3 work fine, All tools are correctly measured and offset.

    Then this simple drilling operation is run. In this case the drill is driven deep beside the work for no reason I can see. Then dragged into the side of the work (snap) and across to the start point of the hole. The chuck then raises and the program works as I would expect it to. Then it slams back down far too deep into the work.

    The code was created in Fusion 360 and the simulation runs fine. The post processsor has not changed. The machine has been updated to 2.7.3 but I rolled it back to 2.7.2 and it still does the same thing.

    I"d appreciate any insights !
    What's the G30 for is this your control requirement???

    Header has code that can cancel your tool offsets

    G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49

    This is all you need in the header

    G90 G17G40G80

    G90 is only needed in the header if you don't have it in your program
    G49 can cancel your tool offset in some controls

    Your post processor is of poor design

    Really need to see the whole program to see where the real problem is

    Mactec54


  5. #5
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by mactec54 View Post
    What's the G30 for is this your control requirement???

    Header has code that can cancel your tool offsets

    G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49

    This is all you need in the header

    G90 G17G40G80

    G90 is only needed in the header if you don't have it in your program
    G49 can cancel your tool offset in some controls

    Your post processor is of poor design

    Really need to see the whole program to see where the real problem is
    the processor is a turd . g30 is return home which is handy when hand bombing tools . A G64P#### is also important to have in the header but not necessary in this case



  6. #6
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    12258
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by metalmayhem View Post
    the processor is a turd . g30 is return home which is handy when hand bombing tools . A G64P#### is also important to have in the header but not necessary in this case
    Yes that is obvious, what is the G64P#### used for that you would want it in the header

    G30 why would you want your machine to return to home at the start of a program is this what they have you do with PP control or just a goofy Post processor

    Mactec54


  7. #7
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    you can go with a g53 or just return home g30 , nothing goofy about it if a tool change may be needed . it doesn't necessarily have to been in the header but it doesn't hurt anything either
    G64 is toolpath control the p value is a tolerance , I punch g64p.001 into all my headers . I've had pathpilot do some funky stuff without the tolerance added



  8. #8
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    something I missed with that code was g30 is alone which is goofy
    I automatically think g30z0



  9. #9
    Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    12258
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by metalmayhem View Post
    you can go with a g53 or just return home g30 , nothing goofy about it if a tool change may be needed . it doesn't necessarily have to been in the header but it doesn't hurt anything either
    G64 is toolpath control the p value is a tolerance , I punch g64p.001 into all my headers . I've had pathpilot do some funky stuff without the tolerance added
    Neither a G53 or a G30 is required at the start of any program

    You don't need a G30 because you are going to do a Tool Change, as soon as a Tool is called T26 in his case the Z axis will move to the tool change position

    Mactec54


  10. #10
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by mactec54 View Post
    as soon as a Tool is called T26 in his case the Z axis will move to the tool change position
    with atc yes , without atc no



  11. #11
    Member
    Join Date
    Nov 2012
    Location
    United States
    Posts
    572
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    with atc yes , without atc no
    In PathPilot, any M06 (too change) macro will move the spindle to the G30 height, even if you don't have the ATC.



  12. #12
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    935
    Downloads
    3
    Uploads
    1

    Default Re: Drilling problem - machine crash

    ...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool. Very sloppy programming looks like to me.

    %
    (1005)
    (Machine)
    ( vendor Autodesk)
    ( description Generic 3-axis)
    (T26 D=5. CR=0. TAPER=118deg - ZMIN=-15.5 - drill)
    G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
    G21 (Metric)
    G30

    N10(Drill5 3)
    T26 G43 H26 M6
    S5000 M3 M8
    G54
    G0 X17.214 Y27.
    G0 Z15.
    G0 Z5.
    G98 G81 X17.214 Y27. Z-15.5 R2.5 F1000.
    X-17.1
    G80
    G0 Z15.
    M5 M9

    G30
    M30
    %



  13. #13
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by jwatte View Post
    In PathPilot, any M06 (too change) macro will move the spindle to the G30 height, even if you don't have the ATC.
    I haven't done anything to the macro and none of mine move to g30 on an m06 call , which is why I have my cam post a g30



  14. #14
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by machinehop5 View Post
    ...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool. Very sloppy programming looks like to me.

    %
    (1005)
    (Machine)
    ( vendor Autodesk)
    ( description Generic 3-axis)
    (T26 D=5. CR=0. TAPER=118deg - ZMIN=-15.5 - drill)
    G90 G54 G64 G50 G17 G40 G80 G94 G91.1 G49
    G21 (Metric)
    G30

    N10(Drill5 3)
    T26 G43 H26 M6
    S5000 M3 M8
    G54
    G0 X17.214 Y27.
    G0 Z15.
    G0 Z5.
    G98 G81 X17.214 Y27. Z-15.5 R2.5 F1000.
    X-17.1
    G80
    G0 Z15.
    M5 M9

    G30
    M30
    %
    it's a pretty bad format , plus it's poor to have 2 m codes on the same line



  15. #15
    Member kstrauss's Avatar
    Join Date
    Apr 2013
    Location
    Canada
    Posts
    1768
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Quote Originally Posted by machinehop5 View Post
    ...is it just me or is this normal format of a program that F360 produces? Why would they put the G43 H26 on the same Line as the TC and before calling the Workoffsets? Also, should have G49 H0D0 at the end of each Tool.
    I'm certainly not a gcode expert but I don't understand your criticisms. The H26 is redundant but what is the problem with putting the G43 on the same line as the tool change? Keeping them together is, in my opinion, just good programming style. Why is it required (or even desirable for that matter) to include a G49? Won't the G43 on the next tool change change the offset?



  16. #16
    Member
    Join Date
    Jun 2018
    Location
    on my feet
    Posts
    483
    Downloads
    1
    Uploads
    0

    Default Re: Drilling problem - machine crash

    the g49 isn't absolutely necessary but there's nothing wrong with safety code . I think machinehop is trained to think the same way as most guys in the trade . While everyone may have a different approach to the rest of the coding the below is the most common start code from tool change on . I think it's neater myself and it just becomes automatic in ones mind over time

    T4M6
    G0G90G54X8.5Y0S6000M3
    G43H4Z1.M8
    Z.1



  17. #17
    Member number40Fan's Avatar
    Join Date
    Nov 2019
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    Are you drilling with a feed of 1000?



  18. #18
    Member
    Join Date
    Dec 2015
    Posts
    36
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    I tend to agree with kstrauss and like to keep the G43 Hxx on the same line,probably because I hand write all my code and it is easy to check the H number corresponds to the tool number
    I also have no ATC and have never had a G30 added to a tool change.Nor would I want it to as I give sufficient clearance to change the tool but without the excessive travel a G30 brings.



  19. #19
    Member
    Join Date
    Jun 2010
    Location
    Australia
    Posts
    36
    Downloads
    0
    Uploads
    0

    Default Re: Drilling problem - machine crash

    It was the G30. Never having done a manual tool change on the machine until the ATC died I had no awareness of it !

    Thanks everyone.



  20. #20
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    935
    Downloads
    3
    Uploads
    1

    Default Re: Drilling problem - machine crash

    [QUOTE=kstrauss;2449352]
    The H26 is redundant but what is the problem with putting the G43 on the same line as the tool change?
    no problem if, the machine can handle the Code on the same Line.
    Why is it required (or even desirable for that matter) to include a G49?
    good practice safe block G49H0D0.
    Won't the G43 on the next tool change change the offset?
    yes, but what happens if the Operator does something in between Tool changes in MDI and does not realize a Tool Comp is active still.

    Murphy's Law



Page 1 of 3 123 LastLast

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Drilling problem - machine crash

Drilling problem - machine crash

Drilling problem - machine crash