Idea I got rid of canned cycles in my post for non peck drilling. Did I make a mistake?


Results 1 to 11 of 11

Thread: I got rid of canned cycles in my post for non peck drilling. Did I make a mistake?

  1. #1
    Member
    Join Date
    Aug 2008
    Location
    USA
    Posts
    93
    Downloads
    0
    Uploads
    0

    Default I got rid of canned cycles in my post for non peck drilling. Did I make a mistake?

    This is for a lathe, 2 axis
    Bob-Cad will only let you select canned cycle or separate lines once per drill operation. I did not like the spot drill to post a canned cycle. I edited my Siemens post to replace the canned cycle with just straight G-code. Seems to work fine. I cannot think of why I would not want to do this. If I'm not peck drilling it's most likely a shallow depth hole so it's just G1 Z-x.xxx Fx.xxx then next line is G0 Z0.1

    1124. Standard Drill Canned Cycle. Straight G-Code Version
    n,"X0.0 ", "F",program_block_20
    n,"Z",program_block_1
    n,"G1 Z",program_block_5
    n,"G0", "Z",program_block_1


    1125. Standard Drill Canned Cycle with Dwell. Straight G-Code Version
    n,"X0.0 ", "F",program_block_20
    n,"Z",program_block_1
    n,"G1 Z",program_block_5
    n,"G04 S",force_no_add_spaces,drill_dwell
    n,"G0", "Z",program_block_1

    The peck drill versions keep the canned cycles.

    I am not sure if this would apply to any posts other than a Siemens 840C

    Good idea or bad?

    Similar Threads:


  2. #2
    Member mactec54's Avatar
    Join Date
    Jan 2005
    Location
    USA
    Posts
    15362
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    Quote Originally Posted by BNR_RANDY View Post
    This is for a lathe, 2 axis
    Bob-Cad will only let you select canned cycle or separate lines once per drill operation. I did not like the spot drill to post a canned cycle. I edited my Siemens post to replace the canned cycle with just straight G-code. Seems to work fine. I cannot think of why I would not want to do this. If I'm not peck drilling it's most likely a shallow depth hole so it's just G1 Z-x.xxx Fx.xxx then next line is G0 Z0.1

    1124. Standard Drill Canned Cycle. Straight G-Code Version
    n,"X0.0 ", "F",program_block_20
    n,"Z",program_block_1
    n,"G1 Z",program_block_5
    n,"G0", "Z",program_block_1


    1125. Standard Drill Canned Cycle with Dwell. Straight G-Code Version
    n,"X0.0 ", "F",program_block_20
    n,"Z",program_block_1
    n,"G1 Z",program_block_5
    n,"G04 S",force_no_add_spaces,drill_dwell
    n,"G0", "Z",program_block_1

    The peck drill versions keep the canned cycles.

    I am not sure if this would apply to any posts other than a Siemens 840C

    Good idea or bad?
    A G81 can be used for spot drilling which is a feed in and rapid out, so much the same as what you have done, no not all post processors work with other controls

    A G81 most likely won't work with your control

    Mactec54


  3. #3
    Member
    Join Date
    Aug 2008
    Location
    USA
    Posts
    93
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    Quote Originally Posted by mactec54 View Post
    A G81 can be used for spot drilling which is a feed in and rapid out, so much the same as what you have done, no not all post processors work with other controls

    A G81 most likely won't work with your control
    Correct, almost none of the common G-code cycles work with my Siemens control. It's very different than my Fanuc.



  4. #4
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    If I'm not peck drilling it's most likely a shallow depth hole so it's just G1 Z-x.xxx Fx.xxx then next line is G0 Z0.1
    hy for most metal work, in order to protect the cutting edge, is good to dweel ( theoretically, for a drill, for half a revolution ) or feed back for 0.05 - 0.5mm ( less for small tools, more for bigger tools, thus this motion increases with initial feed ), and only after that move out of the hole

    idea behind is to avoid aggressive disengagement between tool and material / kindly

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  5. #5
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    The only canned cycles I use on my lathe is a rigid tapping cycle, G84, and the threading cycle, G32. I force the CAM software, Fusion 360 in my case, to generate G1, G2, and G3 moves for all other operations. This can sometimes create large files, but if your machine can digest that, you have much better control over what is happening, including easy editing of the G code if needed.

    Jim Dawson
    Sandy, Oregon, USA


  6. #6
    Member
    Join Date
    Aug 2008
    Location
    USA
    Posts
    93
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    Quote Originally Posted by Jim Dawson View Post
    The only canned cycles I use on my lathe is a rigid tapping cycle, G84, and the threading cycle, G32. I force the CAM software, Fusion 360 in my case, to generate G1, G2, and G3 moves for all other operations. This can sometimes create large files, but if your machine can digest that, you have much better control over what is happening, including easy editing of the G code if needed.
    I like to use canned cycles, right now all my turning code is separate lines. I do not have BobCad working with canned cycles yet, I will. I can edit a canned cycle right at the machine very easy. If I need to change DOC in a canned turning cycle it's only a one number edit, not dozens or hundreds of lines.

    In BobCad Ver 21 I have to draw in all my toolpath lines. Exactly where I want them, now that's total control of the toolpath, but it takes a long time to do. Ver 32 it does it all for me. (however it wants to, with a little input from me). Sometimes it puts in goofy moves which just bug the hell out me.

    For drilling a shallow hole, no pecking, it's only four lines of code.



  7. #7
    Member
    Join Date
    Aug 2008
    Location
    USA
    Posts
    93
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    Quote Originally Posted by deadlykitten View Post
    hy for most metal work, in order to protect the cutting edge, is good to dweel ( theoretically, for a drill, for half a revolution ) or feed back for 0.05 - 0.5mm ( less for small tools, more for bigger tools, thus this motion increases with initial feed ), and only after that move out of the hole

    idea behind is to avoid aggressive disengagement between tool and material / kindly
    True for blind holes, when drilling thru it does not matter. My post modifications still allow for dwell. The Siemens drilling canned cycle allows for a dwell at the bottom of the hole and at the retract point on every peck. BobCad only has the dwell at the bottom.



  8. #8
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    Quote Originally Posted by BNR_RANDY View Post
    I like to use canned cycles, right now all my turning code is separate lines. I do not have BobCad working with canned cycles yet, I will. I can edit a canned cycle right at the machine very easy. If I need to change DOC in a canned turning cycle it's only a one number edit, not dozens or hundreds of lines. .......
    I have Fusion 360 on both my lathe and mill computers, as well as my desktop and laptop. Allows me to make changes right at the machine and re-post the G code to the working folder. Then just open the new file in my CNC software.

    Jim Dawson
    Sandy, Oregon, USA


  9. #9
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    True for blind holes, when drilling thru it does not matter.
    hy that was a mere sugestion, not a must-do thing, thus only be aware, and chose whatever you wish as for through holes, recomandation is to reduce feed when tool gets out on the oposite side, because heat disipation no longer occurs as normal, because material section is no longer constant, but variable

    again, only recomandations

    I have Fusion 360 on both my lathe and mill computers, as well as my desktop and laptop. Allows me to make changes right at the machine and re-post the G code to the working folder. Then just open the new file in my CNC software.
    this method of doing things should change, even if it is there for decades

    whatever is there to fix, should be done before posting, minimizing the need for near machine editing, unless for cuting specs parameteres but even that can be aproached somehow

    of course is ok to have fusion on pc laptop, etc, but what about a unique center, posting for everything else ? thus a single install, that spits code for whatever machine, yet being able to be accesed by 2 3 or more seats ? this is what i am after

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  10. #10
    Community Moderator Jim Dawson's Avatar
    Join Date
    Dec 2013
    Posts
    5717
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    Quote Originally Posted by deadlykitten View Post
    hy

    I have Fusion 360 on both my lathe and mill computers, as well as my desktop and laptop. Allows me to make changes right at the machine and re-post the G code to the working folder. Then just open the new file in my CNC software.
    this method of doing things should change, even if it is there for decades

    whatever is there to fix, should be done before posting, minimizing the need for near machine editing, unless for cuting specs parameteres but even that can be aproached somehow

    of course is ok to have fusion on pc laptop, etc, but what about a unique center, posting for everything else ? thus a single install, that spits code for whatever machine, yet being able to be accesed by 2 3 or more seats ? this is what i am after
    I think you are confused We have 3 seats of Fusion 360, and each seat can be accessed from any of several computers in our facility, or any computer with internet access. The Fusion 360 license goes with the user and is not computer specific. We can design parts and post G code to any machine, from any machine, desktop, or laptop.

    Also, we own the parts and the designs, we don't do job shop work. The parts may have design changes done at the machine during first run setup, but normally are not changed after that. However I did make a change in a part yesterday, mid run. I changed the order of operation and added an operation to get better tool life, and saved 45 seconds/part on a mill/turn part in the process, all done at the machine. Saved me walking 150 feet to my office computer

    Jim Dawson
    Sandy, Oregon, USA


  11. #11
    Member deadlykitten's Avatar
    Join Date
    Jun 2015
    Location
    Antarctica
    Posts
    4131
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    hy jim actually i deleted my long reply, and only write that short messy thing, i am sorry ... your initial reply in this tread got me re-thinking about the actual stage of things, how they are, and really, seing someone still balancing between canned and g-code, etc

    i didn't continue writing about it, because i should 1st get things done, then speak; what you saw was a rushed thing, sorry

    i totaly agree with you, i understand the importance of saving 150feet, the difference between 1/2 keystrokes, acces on account or whatever needed to make an application initialize more than once ?! i was not reffering to an install to a pc, that's why i called it center, that you acces from different locations, or send/edit programs from home, but whatever, in the end it has to work

    i wish to make things as simple as possible .. and yes, i am confused, what i have thougth a few months ago, now is recycled, and latest idea poped up a few weeks ago it changes as i go with it

    we are merely at the start of " Internet of Things / Industrial Revolution 4.0 " era : a mix of AI, plastics, human estrangement, powerful non-state actors ...


  12. #12
    Member
    Join Date
    Aug 2008
    Location
    USA
    Posts
    93
    Downloads
    0
    Uploads
    0

    Default Re: I got rid of canned cycles in my post for non peck drilling. Did I make a mistak

    I am still working on getting more of Bobcad to work with canned cycles. I find them very easy to modify, If I want to change depth of cut I need to edit one single number field, not hundreds of lines of code, or go back to my computer and edit then repost it. I can edit a canned cycle right at the machine super quick. I do have older machines with limited memory for large files.



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

I got rid of canned cycles in my post for non peck drilling.  Did I make a mistake?

I got rid of canned cycles in my post for non peck drilling.  Did I make a mistake?