OSP 300 Hi Cut can't turn it off
Close
Login to Your Account
Results 1 to 9 of 9
  1. #1
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    947

    Default OSP 300 Hi Cut can't turn it off

    We don't work with close tolerances very often so we generally only use High Cut when engraving part numbers and use G130 to cancel the cycle. Recently, for some unknown reason and I don't think anyone has messed with the parameters, Hi Cut is coming on with HSM roughing and severely slowing the feed rate. Have tried adding G130 at the beginning of the program and also before a HSM op and it still flashes and cuts the feed rate in some cases in half.

    Anybody else have had this experience and if so how did you solve it?

  2. #2
    Join Date
    Mar 2011
    Location
    NY USA
    Posts
    826
    Post Thanks / Like
    Likes (Given)
    171
    Likes (Received)
    545

    Default

    I leave hi-cut on all the time because most of what I'm doing requires decent tolerances. That being said I've only ever turned hi-cut on and off via the hi-cut parameters page. I was never able to get the g-code to function the way I thought it would so I just turned it on and left it.

    I opened up the tolerances on the hi-cut parameters page and I haven't noticed any severe changes in commanded feed rate during HSM. Maybe I'm not pushing things like you are, I'm usually in carbon or stainless so my feeds might not be that high.

    I've done some very nice surfacing in 6061 at 400 IPM and not seen a problem once I played with the hi-cut parameters.

  3. #3
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    947

    Default

    Any chance you could take a pic of your High Cut parameters?

  4. #4
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    71
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    25

    Default

    Quote Originally Posted by Captdave View Post
    Any chance you could take a pic of your High Cut parameters?


    In your parameters you can turn it on to stay on all the time regardless of the Gcode. 100% its turned on in the system parameters. Check there first.

  5. #5
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    947

    Default

    Quote Originally Posted by TangentCNC View Post
    In your parameters you can turn it on to stay on all the time regardless of the Gcode. 100% its turned on in the system parameters. Check there first.

    I don't mind if its on all the time but I don't want it slowing down like it is now. Never adjusted it so I really not sure where to set it. If someone has a good setting then no reason to reinvent the wheel and I'll leave it on all the time.

  6. #6
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    947

    Default

    Took a quick peek and found 2 pages, high cut control and guide. Neither have edit fields so must not have found the correct page.

  7. #7
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,461
    Post Thanks / Like
    Likes (Given)
    4051
    Likes (Received)
    2636

    Default

    It's called Hi Cut Pro Control parameter.
    It's right around page 33 or 35 on the parameters page depending on how many you have set to be visible.
    I keep ours set to "Standard" and about a .002/.003 tolerance.
    If you have it set too tight, it will bog down the feeds in corners for sure.

    After you change the settings make sure you hit the "Para update" softkey.
    If you change it while running a program it will change when it hits a G00, or after the read-ahead completes its buffer.

  8. Likes Captdave liked this post
  9. #8
    Join Date
    Mar 2011
    Location
    NY USA
    Posts
    826
    Post Thanks / Like
    Likes (Given)
    171
    Likes (Received)
    545

    Default

    Para menu 36 (on mine)

    Hi-cut Pro parameters

    on in control
    upper limit 500 ipm
    tolerance .003
    mode: High Speed

    I used that for making a really nice surface in 6061 at 11k and 400ipm with a 5/8 ball. It was an automotive part and the total profile accuracy wasn't that critical. It fit air...lots and lots of air. Not overloading the tool was critical for finish reasons and those settings worked nicely. It slowed down only in the tighter radius where the machine was switching direction. The rest of the cut was right at 400ipm commanded.

  10. Likes Captdave liked this post
  11. #9
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    947

    Default

    Ok found the right page and made the adjustments.

    Thanks for the tip on the obscure "save" button, I'm sure I would have over looked that one.

  12. Likes Mtndew, XD341 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
  •