Need Help! Tool Decomp failsafe process


Results 1 to 5 of 5

Thread: Tool Decomp failsafe process

  1. #1
    Registered
    Join Date
    Mar 2012
    Location
    United States
    Posts
    16
    Downloads
    0
    Uploads
    0

    Default Tool Decomp failsafe process

    I have an operator on the shop floor that had a question. Is there a way to have the machine stop the program if the decomp value of a tool that is placed in the tool information has a radius to large to machine the part safely? An example of this would be if an operator changed out a tool and entered a tool radius of 1.325 and the safe decomp value would be under 1.3. Is there a way to have the machine recognize this and stall out the program and stop the machine to save a potential crash? Like a line that reads "If such and such isn't a certain value-Then either stop the program or let it continue to run". Thanks for any help.

    Similar Threads:


  2. #2
    Member christinandavid's Avatar
    Join Date
    Aug 2009
    Location
    New Zealand
    Posts
    684
    Downloads
    0
    Uploads
    0

    Default

    Using macro b and tool offset option c, you could put...

    IF[#[13000.+#4107]GE1.3]THEN#3000=1(incorrect compensation)

    This would stop pgm if last called D is bigger than 1.3 ( with message)

    I think..

    DP



  3. #3
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Never heard the term "decomp" used before. Thanks for a new term.

    You can also program using "Wear Compensation" where the center line of the tool is programmed and initial compensation is set for 0.0000.



  4. #4
    Member christinandavid's Avatar
    Join Date
    Aug 2009
    Location
    New Zealand
    Posts
    684
    Downloads
    0
    Uploads
    0

    Default

    The method txcncman proposes is probably least prone to catastrophic error if D is omitted or value omitted from tool table. Not my preferred method as I like to 'see' the size of the tools in the offset table as an extra assurance that I am altering the right tool - also, 'manual guide i' cycles will only work with a valid tool size (which is why I use them - automatic safety check ,). I would get operator opinion before changing methods.



    To involve your radius wear offset into safety check, you might put..

    IF[[#[13000.+#4107]+#[12000.+#4107]]GE1.3]THEN..etc

    Remember that your D must be invoked beforehand otherwise #4107 will not be updated. If your control has different tool compensation type, see the manual to determine where tool offset values are stored. You can obviously extend the formula/repeat this method to ensure that D lies within a valid range.

    DP



  5. #5
    Registered beege's Avatar
    Join Date
    Feb 2008
    Location
    USA
    Posts
    586
    Downloads
    0
    Uploads
    0

    Default

    In the absence of a macro option, you could write a non-cutting circle with comp on that would alarm out when the comp value got too large. (program a R1.300 circle so that a comp value of 1.301 would throw an alarm)



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

Tool Decomp failsafe process

Tool Decomp failsafe process