Fanuc Multiple Block Skips???


Results 1 to 3 of 3

Thread: Fanuc Multiple Block Skips???

  1. #1
    Member ADVCOLE's Avatar
    Join Date
    Dec 2019
    Posts
    1
    Downloads
    0
    Uploads
    0

    Default Fanuc Multiple Block Skips???

    I came from a shop with Makino Machines where each machine has, I believe, 9 different block skips. I am now in a shop with a variety of older Fanuc Controls, I know at least the lathes have multiple block skips as /2 is what the bar feeder toggles to kick the machine into the new load new bar program. My question is, will these machines have other block skips that I can be toggled from the machine? After poking around the control for some time, I can't seem to find a block skip screen to perform this function. For example, I want to alias M6 on the mills with a program like this:

    G00 G53 Z0.
    M9
    M5
    /2 G00 G53 X0.
    /2 G00 G53 Y0.
    M6
    M99

    Where when /2 is active, the machine performs a normal tool change, but turn /2 off and the machine moves to a safe tool change position. This is very simplified down, and I know there are other ways to do this. However, the program I plan on implementing will have much more code where the machine would check for a tool length offset when the tool is loaded into the machine then auto-set the tool if the offset is 0, among other functions that I want the operator to be able to toggle at the machine with block skips.
    Thank you!

    Similar Threads:


  2. #2
    Member
    Join Date
    May 2016
    Location
    United States
    Posts
    380
    Downloads
    0
    Uploads
    0

    Default Re: Fanuc Multiple Block Skips???

    Extra Block Skips on a Fanuc control are usually an option. I have two Fanuc Mills and one Fanuc lathe and none of them have multiple block skips.

    What model controls are you working with?

    As far as your auto tool measurement goes for not previously measured tools- one signal that the tool currently loaded has a zero offset set is when G43 is called the machine will over travel in Z+. That will sure tell an operator to measure the tool.

    Personally I find the idea of loading tools and not at the same time measuring or entering their offset a bit like asking for crash trouble. How perfect are the in house standard operating procedures to insure that old offsets are removed when tools are no longer needed or are removed? Meaning how certain can you be that if you load a new sayT22, that T22 offset is at 0? And if your SOP is to zero out the offset whenever loading a tool, I can't see how anything is saved by not then measuring the tool when the thought of the tool is at currently at hand. Still I"m sure you have your reasons.

    Regardless, your idea of having code set that auto measures any tool that has a zero offset in it's register when loaded, could be handled easy enough without using any block skips at all. Make checking for zero offset the norm after a tool change. Include it right before your safety line that follows a tool change. If it finds a non zero value it simply continues on as if nothing happened. If it finds a zero it measures the tool. There is no block skip needed in that scenario. To check on a tool offset register entry is Macro B programming anyway, so make the macro programming self answering without operator intervention. The only thing that might happen is the operator will be expecting the tool to go after the work piece but momentarily be surprised as it heads of for a tool measurement first. The program will progress normally as if nothing different is going on except for the couple microseconds it spends checking for a zero tool offset value after a tool change.

    Come to think of it. If your tool change macro is setup as a 8 or 9000 series sub/macro called by an M code, (M6 for instance) you could include your auto checking functionality right inside the tool change sub/macro.



  3. #3
    Member
    Join Date
    Apr 2011
    Location
    USA
    Posts
    738
    Downloads
    0
    Uploads
    0

    Default Re: Fanuc Multiple Block Skips???

    The ladder has to support this. Check and see if G045#0 to G045#7 are used. (Assuming 16/18/21 style controller) Also it's a paid option from Fanuc.



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

Fanuc Multiple Block Skips???

Fanuc Multiple Block Skips???

Fanuc Multiple Block Skips???