Fadal 88hs making Z plunge as first move
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 38
  1. #1
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default Fadal 88hs making Z plunge as first move

    I'm dead to rights new to 3d CNC, and this one issue is kicking my butt.

    I've reinitialized the machine, so there's no leftover offsets that I'm aware of, I've set the tools and fixture offsets appropriately (I think), but I can't stop the machine from homing to an obscure Z position before rapiding up to the R plane.

    I'm using Fusion 360 with a good post, provided by a reputable source.

    If I set the tool offset really high, as in above TC height, I can watch the motion without dinging the table or vise and it routinely does the same motion. Below is a snippet of the code, what am I missing?

    %
    O1001
    (T1 D=0.25 CR=0. - ZMIN=-0.25 - FLAT END MILL - 1/4" FLAT ENDMILL)
    N10G0G17G40G80G90
    N15G0H0Z0.
    (FACE2)
    N20G9
    N25M5M6T1(1/4" Flat Endmill)
    N30M3S3500
    N35E1
    N40X1.6625Y-0.9002
    N45H1Z0.6M7
    N50G4P2000
    N55Z0.2
    N60G1Z0.025F60.
    N65G18G3X1.6375Z0.I-0.025
    N70G1X1.5
    N75X-1.5F31.5
    N80G17G2Y-0.6778J0.1112
    N85G1X1.5
    N90G3Y-0.4555J0.1112
    N95G1X-1.5

  2. #2
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,048
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    656

    Default

    Look in your fixture offset page look at e1 see if there is a number in the z column it needs to be zero


    Sent from my iPhone using Tapatalk Pro

  3. Likes carbonbl, Cole2534 liked this post
  4. #3
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    2,280
    Post Thanks / Like
    Likes (Given)
    201
    Likes (Received)
    1249

    Default

    That g0 h0 z0 may be doing in for ya...not sure what h0 even is.

  5. Likes Ewindward liked this post
  6. #4
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    127

    Default

    How are you setting your tool and fixture offsets though?

  7. #5
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default

    Quote Originally Posted by carbonbl View Post
    How are you setting your tool and fixture offsets though?
    Using the tool setting routine and a 4" block on the surface of my material.

    Quote Originally Posted by plastikdreams View Post
    That g0 h0 z0 may be doing in for ya...not sure what h0 even is.
    That makes me think there's some crazy offset I'm unaware of, but it should have been cleared when I reinitialized, I think.

    Quote Originally Posted by D Nelson View Post
    Look in your fixture offset page look at e1 see if there is a number in the z column it needs to be zero


    Sent from my iPhone using Tapatalk Pro
    Z has a -11.xx" value in it for E1.


    BTW, I'm operating in Format 1.

  8. #6
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    127

    Default

    If you're setting your tools using a 4" block and using the tool setting routine, you should be entering a 4" Z fixture offset in the setting routine and the Z value for E1 should be zero. This is assuming you want the top of your material to be Z0. Basically any Z value in your E1/E2/Ewhatever fixture offsets is just the Z difference between the gauge point you use to measure tool lenghts and where Z0 for that fixture offset needs to be. The tool setting utility compensates for the 4" block (or whatever you enter when it asks for Z fixture offset) if you just have one Z height for your fixture offsets (hence it should be set to Z0), but if you have multiple fixture offsets you will need to measure the difference in Z between them and adjust the Z value accordingly.

    Clear as mud? I actually don't ever use the tool setting routine on my fadal and have a slightly different method. So I hope I don't have something confused. But the basic concept is that the Z in your E fixture offsets will always be the difference between where your fixture offset Z is and the gauge point where you measure the Z length of all your tools.

    BTW, H0/H1/Hwhatever is a Fadal format 1 way of calling tool offsets. I run format 1 in my fadal, looks normal to me.

  9. Likes Cole2534 liked this post
  10. #7
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default

    Quote Originally Posted by D Nelson View Post
    Look in your fixture offset page look at e1 see if there is a number in the z column it needs to be zero


    Sent from my iPhone using Tapatalk Pro
    You win 100 internet points and 10 thank yous.

    I guess my fixture and tool offsets were compounding.

  11. #8
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default

    Quote Originally Posted by carbonbl View Post
    If you're setting your tools using a 4" block and using the tool setting routine, you should be entering a 4" Z fixture offset in the setting routine and the Z value for E1 should be zero. This is assuming you want the top of your material to be Z0. Basically any Z value in your E1/E2/Ewhatever fixture offsets is just the Z difference between the gauge point you use to measure tool lenghts and where Z0 for that fixture offset needs to be. The tool setting utility compensates for the 4" block (or whatever you enter when it asks for Z fixture offset) if you just have one Z height for your fixture offsets (hence it should be set to Z0), but if you have multiple fixture offsets you will need to measure the difference in Z between them and adjust the Z value accordingly.

    Clear as mud? I actually don't ever use the tool setting routine on my fadal and have a slightly different method. So I hope I don't have something confused. But the basic concept is that the Z in your E fixture offsets will always be the difference between where your fixture offset Z is and the gauge point where you measure the Z length of all your tools.

    BTW, H0/H1/Hwhatever is a Fadal format 1 way of calling tool offsets. I run format 1 in my fadal, looks normal to me.
    Thank you very much for the detailed explanation. I redid the E offset with a Z0 and it ran like a top.

  12. #9
    Join Date
    Nov 2010
    Location
    Tustin, CA
    Posts
    386
    Post Thanks / Like
    Likes (Given)
    228
    Likes (Received)
    115

    Default

    These guys have it right. I was thinking it was your post. I didn't think to ask if you had any additional Z offsets entered. I usually set all my tools to the top of my fixed jaw (which on the Oranges, is one and the same as the bottom of the part). Then any other offsets that differ from that are +/- from there. So maybe you have soft jaws on E2 that are a 1/4" higher in a second setup, E2 would just be 0.25".

    If you use the tool setting menu and tell it you are using the 4" block, it will automatically compensate and add to the offset when it stores the value. The H values are a height comp like D for diameter comp.

  13. Likes Cole2534 liked this post
  14. #10
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    44
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    28

    Default

    Also clear your machine offsets.

    Send machine "home for power off" Then go to axis offsets or home positions. "H" for store all.

  15. #11
    Join Date
    Jun 2016
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    237
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    105

    Default

    "Post from a reputable source"...unless that source is someone running 10 fadals on this website, I wouldn't trust a fusion360 post without looking through it myself. Just saying. Looks like you got squared away though.

  16. Likes litlerob1 liked this post
  17. #12
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default

    Quote Originally Posted by EndlessWaltz View Post
    "Post from a reputable source"...unless that source is someone running 10 fadals on this website,
    Actually, it is. After I cleared the redundant offsets the program ran like expected it to do.

    But now my spindle drive is showing various fault codes, so back to the troubleshooting mode.

    Sent from my SM-G973U using Tapatalk

  18. #13
    Join Date
    Oct 2006
    Location
    Klamath Falls, Oregon
    Posts
    3,639
    Post Thanks / Like
    Likes (Given)
    418
    Likes (Received)
    1008

    Default

    The Fadal post provided with Fusion 360 works fine for me.

    I don't set offsets off the part, I don't want to touch off tools for every part.

    I use a 3" gage block and touch off each tool to the table with the block.

    You can then touch off tool 1 on the part with paper, then transfer the raw Z value to the fixture Z offset.

    The 3" cancels out, if you use a gage block on the part, you need to subtract 3" (-3 + -8 = -11) from the raw Z value to get your fixture Z offset.

    I learned to start touching off on a 3" gage block back when I got a Brother with a 7.87" min Z distance, been doing it since.

  19. #14
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default

    Quote Originally Posted by carbonbl View Post

    Clear as mud? I actually don't ever use the tool setting routine on my fadal and have a slightly different method. .
    Would you mind elaborating on your method? Im open to learning new ways.

    Sent from my SM-G973U using Tapatalk

  20. #15
    Join Date
    Mar 2004
    Location
    Waukesha, WI
    Posts
    7,365
    Post Thanks / Like
    Likes (Given)
    711
    Likes (Received)
    1824

    Default

    I don't understand how it even is working now. Line 15 he has G0 Z0 H0. That still tells the machine to rapid to Z0 with no offset called up. How is that working?

  21. #16
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    127

    Default

    Quote Originally Posted by Dave K View Post
    I don't understand how it even is working now. Line 15 he has G0 Z0 H0. That still tells the machine to rapid to Z0 with no offset called up. How is that working?
    Fadal Z0 with no offset active is the toolchange position. Well above where anything bad could happen.

  22. #17
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    1,048
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    656

    Default

    Quote Originally Posted by plastikdreams View Post
    That g0 h0 z0 may be doing in for ya...not sure what h0 even is.
    The H0 is to go to the home position after the program runs to bring table to the front of machine to load vises. That needs to be at the end of his program


    Sent from my iPhone using Tapatalk Pro

  23. #18
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    127

    Default

    Quote Originally Posted by Cole2534 View Post
    Would you mind elaborating on your method? Im open to learning new ways.

    Sent from my SM-G973U using Tapatalk
    It's pretty simple and mostly done out of force of habit since when I learned how to run my Fadal when it had early version control boards with no toolsetter utility.
    • Load tools into carousel and place Edge Technologies touch off gauge on machine table
    • Load tool to be measured into spindle
    • Jog tool down to touch off gauge until gauge reads 0
    • Go back to command entry screen, type SL, [number of current tool]
    • Load next tool and repeat
    • If setting a new fixture offset, measure the distance in Z from the gauge height of the touch off gauge to the Z height of your fixture offset. I usually do this with an indicator attached to the spindle with a mag base. This difference is the Z value on the fixture offset. In other words, if your desired Z for E1 is 0.5" above your touch off gauge height, enter 0.5 in the Z field for E1.

  24. Likes Cole2534 liked this post
  25. #19
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    285
    Post Thanks / Like
    Likes (Given)
    242
    Likes (Received)
    127

    Default

    Quote Originally Posted by D Nelson View Post
    The H0 is to go to the home position after the program runs to bring table to the front of machine to load vises. That needs to be at the end of his program


    Sent from my iPhone using Tapatalk Pro
    It's fine unless for some reason you have changed the default home position on your Fadal to some weird spot. I know some people do this but why I will never understand, the default home position on fadals are at the right spot to "home" axes on startup and Z0 is at the toolchange position, it just works well.

    Every Fadal program I have from the HSMworks or Fusion360 post has this and they all run great. I don't have to hand edit any programs from the F360 post unless I'm preparing a program for DNC or trying to do something special.

  26. #20
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,459
    Post Thanks / Like
    Likes (Given)
    769
    Likes (Received)
    1845

    Default

    Quote Originally Posted by carbonbl View Post
    It's pretty simple and mostly done out of force of habit since when I learned how to run my Fadal when it had early version control boards with no toolsetter utility.
    • Load tools into carousel and place Edge Technologies touch off gauge on machine table
    • Load tool to be measured into spindle
    • Jog tool down to touch off gauge until gauge reads 0
    • Go back to command entry screen, type SL, [number of current tool]
    • Load next tool and repeat
    • If setting a new fixture offset, measure the distance in Z from the gauge height of the touch off gauge to the Z height of your fixture offset. I usually do this with an indicator attached to the spindle with a mag base. This difference is the Z value on the fixture offset. In other words, if your desired Z for E1 is 0.5" above your touch off gauge height, enter 0.5 in the Z field for E1.
    So this logic works like this-
    All tool points are brought to the same Z position, determining what is in essence a reference. The fixture offset then determines the fixture's desired point in reference to that plane.

    If that's true, I feel like this is the best way to achieve my means.


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
  •