Fadal 88hs making Z plunge as first move - Page 2
Close
Login to Your Account
Page 2 of 2 FirstFirst 12
Results 21 to 38 of 38
  1. #21
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    271
    Post Thanks / Like
    Likes (Given)
    230
    Likes (Received)
    122

    Default

    Quote Originally Posted by Cole2534 View Post
    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.
    Yes that is correct. My method, Perry's, kazlx's and the tool setting routine are all doing essentially the same thing in this regard, just using slightly different procedures.

  2. Likes Cole2534 liked this post
  3. #22
    Join Date
    Jul 2018
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    9
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1

    Default

    Some Fadal's (old Kitamura MyCenters as well) also need a G49 to go with the Z0 H0.

  4. #23
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    271
    Post Thanks / Like
    Likes (Given)
    230
    Likes (Received)
    122

    Default

    Quote Originally Posted by Darren Janecky View Post
    Some Fadal's (old Kitamura MyCenters as well) also need a G49 to go with the Z0 H0.
    H0 does the same thing as G49, tool offset cancel. This might be a format 2 quirk, never needed this on a format 1 machine.

  5. #24
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,163
    Post Thanks / Like
    Likes (Given)
    719
    Likes (Received)
    1758

    Default

    Still pulling my hair out here. If I set all tools with a 4" block I get various Z offsets, that makes sense. When I touch a tool to a fixture and apply that as the fixture offset it will return THAT tool to the correct Z, but when I switch to a diff length tool the Z is wrong.

    It's like the machine isn't summing the TCS with the WCS.

    It's fine to touch each tool for a run but it seems like there's def a better way.

  6. #25
    Join Date
    Apr 2016
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    271
    Post Thanks / Like
    Likes (Given)
    230
    Likes (Received)
    122

    Default

    Touch off tool on 4" block (or whatever your tool setting reference is). Take note of Z value, let's call this Z1.

    Touch off tool on desired Z0 for your fixture offset. Take note of this Z value also, call it Z2.

    Then:
    Z2 - Z1 = ZF

    ZF is the value to enter in the Z field of your fixture offset. So if you want your fixture offset Z0 to be your vise jaw top, and the vise jaw top is 0.75" higher in Z than the top of your tool setting 4" block, then ZF = 0.75" .

    I do it this way every day, only I use a dial indicator attached to the spindle with a mag base, cause I don't like using tools to touch off on hard surfaces like vise jaws. You definitely don't need to touch off each tool every time a fixture offset changes with this method.

  7. #26
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Quote Originally Posted by Cole2534 View Post
    Still pulling my hair out here. If I set all tools with a 4" block I get various Z offsets, that makes sense. When I touch a tool to a fixture and apply that as the fixture offset it will return THAT tool to the correct Z, but when I switch to a diff length tool the Z is wrong.

    It's like the machine isn't summing the TCS with the WCS.

    It's fine to touch each tool for a run but it seems like there's def a better way.
    you are calling up the right tool height for that different tool correct?

    all tools should match any fixture offset if you set the fixture offsets correctly and they are called out correctly in your program. providing all tools are set to one fixture

    your program sounds wrong. post a program with a few tool changes, something tells me your relying too much on your cam software .

  8. #27
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,163
    Post Thanks / Like
    Likes (Given)
    719
    Likes (Received)
    1758

    Default

    Carbonbl-

    Per your formula, the fixture Z offset value is the delta between the tool point reference plane and the fixture's plane. If the fixture is higher off the table, that value will be positive and if the fixture is lower than the tool ref plane that value will be negative, correct?


    Well when I do that it's like the fixture offset only carries to the tool I used to zero the fixture.

    Touch all tools onto vise solid jaw, results in various Z offsets. Set random point on vise soft jaw as E1, approx .5 taller than solid jaw. Z offset in DF table is 0.52".

    From Home-
    G90 G17 etc....

    G0 H1 E1 (tool goes to correct location)

    M6 T2 H2

    G0 Y1. Y1. Z1.

    G0 E1 (tool goes to correct XY, but head returns to same absolute position as it did for H1)

  9. #28
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,163
    Post Thanks / Like
    Likes (Given)
    719
    Likes (Received)
    1758

    Default

    Ran through all the procedures again, works just like it should.

    I think I'm losing it....

  10. #29
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Quote Originally Posted by Cole2534 View Post
    Ran through all the procedures again, works just like it should.

    I think I'm losing it....
    I think I know your problem.
    you need to get into the habit of spelling out the start code for every tool. you should have some consistency in your program.

    M6 T20 (4.000 DIA. FACE MILL )
    G0 G90 E1 X-2.0 Y0.0 (try to get in the habit of putting this after every tool call out)
    M3 S6500
    G43 Z0.1 H20 M08
    G1 Z0.0 F50.0
    X24.0
    G0 Z0.1
    M09
    G91 G28 Z0.0 M05
    M01
    M6 T3 (0.500 DIA. END MILL )
    G0 G90 E1 X-0.5 Y-2.5
    M3 S10000
    G43 Z0.1 H3 M08
    G1 Z-1.0 F50.0
    Blah
    Blah Blah
    G0 Z0.1
    M09
    G91 G28 Z0.0 M05
    M01

    etc etc

  11. Likes Cole2534, Bobw liked this post
  12. #30
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Quote Originally Posted by Cole2534 View Post
    Carbonbl-

    Per your formula, the fixture Z offset value is the delta between the tool point reference plane and the fixture's plane. If the fixture is higher off the table, that value will be positive and if the fixture is lower than the tool ref plane that value will be negative, correct?


    Well when I do that it's like the fixture offset only carries to the tool I used to zero the fixture.

    Touch all tools onto vise solid jaw, results in various Z offsets. Set random point on vise soft jaw as E1, approx .5 taller than solid jaw. Z offset in DF table is 0.52".

    From Home-
    G90 G17 etc....

    G0 H1 E1 (tool goes to correct location) (Bad habit to get into)

    M6 T2 H2 ( very BAD HABIT and you forgot g43)

    G0 Y1. Y1. Z1.

    G0 E1 (tool goes to correct XY, but head returns to same absolute position as it did for H1) Extreamly bad habit as thats how crashes happen

    Highlighted in red

  13. Likes Cole2534 liked this post
  14. #31
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,163
    Post Thanks / Like
    Likes (Given)
    719
    Likes (Received)
    1758

    Default

    I looked through another program I'd run and it makes no mention of G43 anywhere in it.

    %
    O1001 (3/8" DRIVE)
    (T2 D=0.375 CR=0. TAPER=118DEG - ZMIN=-0.44 - DRILL)
    (T5 D=0.5 CR=0.015 - ZMIN=-0.44 - BULLNOSE END MILL)
    N10 G90 G94 G17 H0 E0
    N15 G20
    N20 G0 H0 Z0.

    (DRILL1)
    N25 M9
    N30 T2 M6
    N35 S900 M3
    N40 G4 P200
    N45 M8
    N50 G0 E4 X0. Y0.
    N55 H2 Z0.6
    N60 Z0.2
    N65 G98 G81 X0. Y0. Z-0.44 R0+0.16 F3.6
    N70 G80
    N75 Z0.6
    N80 M5
    N85 H0 Z0.
    Added a g43 and all is well. Now to get my CAM (Fusion 360) to recognize that need.

  15. #32
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Quote Originally Posted by Cole2534 View Post
    I looked through another program I'd run and it makes no mention of G43 anywhere in it.



    Added a g43 and all is well. Now to get my CAM (Fusion 360) to recognize that need.
    Cole
    you need to learn how to write g code and fast, that software code generator you have is 100% garbage. find the right code generator before you do anymore. your going to crash your machine.
    Theres a online manual out by haas I posted it before and others have as well, Get it read it and start modifying your programs before you hit any start button on any machine. If I find it I will post it again . hopefully someone else has the link for it. at the very least search for it on this website.

    dont take this wrong, if you cant read or understand code you have no business in front of a machine as its just going to cost you money in broken machines and tooling.
    I'm not talking about geometries I am talking about basic stuff

  16. #33
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,163
    Post Thanks / Like
    Likes (Given)
    719
    Likes (Received)
    1758

    Default

    No offense taken, but it's the Fusion 360 post that seems to work for everyone else.

    And I can write g-code, I used to hand cam my plasma table this is just more difficult.

    What's so junky about that snippet I posted? If i run that code and touch my tool to my parts it works like a top, making excellent parts.

  17. #34
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Quote Originally Posted by Cole2534 View Post
    No offense taken, but it's the Fusion 360 post that seems to work for everyone else.

    And I can write g-code, I used to hand cam my plasma table this is just more difficult.

    What's so junky about that snippet I posted? If i run that code and touch my tool to my parts it works like a top, making excellent parts.
    it might work for everyone else because they have the correct code generator, theres no problem with the code its spits out gemometry wise its everything else. it not correct not even close thats why your having problems.

    look at your code compared to this. this profiles a 5x5 inch part and puts 4 holes in it. I didnt use any dia offsets,
    look at the green blocks thats how it should be done or close to.. notices where the E1 and tool offsets are(H numbers). if you want to use a g43 it goes here like this ***** N7 G43 Z0.2 H1 M8 ***** on fadals you dont have to use a g43 just an H number

    %
    N1 O1111 ( test.cod 07/27/19 )
    N2 M6 T1 (0.500 DIA. END MILL )
    N3 G0 G17 G40 G80 G90 E1
    N4 M3 S7500
    N5 X-1.0 Y0.25
    N6 G8
    N7 Z0.2 H1 M8

    N8 Z0.1
    N9 G1 Z-0.3 F50.0
    N10 X4.75
    N11 G2 X5.25 Y-0.25 J-0.5
    N12 G1 Y-4.75
    N13 G2 X4.75 Y-5.25 I-0.5
    N14 G1 X0.25
    N15 G2 X-0.25 Y-4.75 J0.5
    N16 G1 Y-0.25
    N17 G2 X0.2027 Y0.2478 I0.5
    N18 G1 X0.9209 Y0.4872
    N19 G0 Z0.2
    N20 G40 M5 M9
    N21 G9
    N22 G49 Z0.0
    N23 M01
    N24 M6 T2 ( 0.500 DIA. SPOT DRILL )
    N25 G0 G17 G40 G80 G90 E1
    N26 M3 M8 S2500
    N27 X1.0 Y-1.0
    N28 G8
    N29 Z0.2 H2

    N30 G98 G82 Z-0.175 R+0.2 F15.0 p200
    N31 X4.0
    N32 Y-4.0
    N33 X1.0
    N34 G80 G40 M5 M9
    N35 G9
    N36 G49 Z0.0
    N37 M01
    N38 M6 T3 ( 0.500 DIA. TWIST DRILL )Normal drilling
    N39 G0 G17 G40 G80 G90 E1
    N40 M3 M8 S1146
    N41 X1.0 Y-1.0
    N42 G8
    N43 Z0.2 H3

    N44 G98 G81 Z-0.65 R+0.1 F3.4
    N45 X4.0
    N46 G80 G40 M5 M9
    N47 G9
    N48 G49 Z0.0
    N49 M01
    N50 M6 T4 ( 0.500 DIA. TWIST DRILL ) peck drilling
    N51 G0 G17 G40 G80 G90 E1
    N52 M3 M8 S2674
    N53 X1.0 Y-4.0
    N54 G8
    N55 Z0.2 H4

    N56 G98 G83 Z-0.65 R+0.1 Q0.1 F10.7
    N57 X4.0
    N58 G9
    N59 M5 M9 G80
    N60 G0 G40
    N61 M30
    %

  18. #35
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,163
    Post Thanks / Like
    Likes (Given)
    719
    Likes (Received)
    1758

    Default

    Thank you for taking the time to help me. Let me digest what you've posted.

    Thanks!

  19. #36
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Play with your code generator to get what I have highlight in green, other wise replace it by writing it in manually and take the stuff out from fusion.

    doing it this way all tools will work 100% every time. even if you need to call up a tool in the middle of a program to rerun it.

  20. #37
    Join Date
    Sep 2008
    Country
    CANADA
    State/Province
    Nova Scotia
    Posts
    283
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    124

    Default

    Quote Originally Posted by Delw View Post
    Cole
    you need to learn how to write g code and fast, that software code generator you have is 100% garbage. find the right code generator before you do anymore. your going to crash your machine.
    Theres a online manual out by haas I posted it before and others have as well, Get it read it and start modifying your programs before you hit any start button on any machine. If I find it I will post it again . hopefully someone else has the link for it. at the very least search for it on this website.

    dont take this wrong, if you cant read or understand code you have no business in front of a machine as its just going to cost you money in broken machines and tooling.
    I'm not talking about geometries I am talking about basic stuff
    Calling a post a "code generator" doesn't lend credibility to your argument..

    OP, you don't need to hand code everything, just fix your post to work properly. The stock Fusion360 posts suck in a lot of ways but they're written in Javascript and so are pretty easy to modify. If I remember right the stock HSMWorks post had problems with rigid tapping and some small details like that, but a well-edited one is available in the support forums.

    I have a good one I run a CNC88HS with for HSMWorks which I'm pretty sure is the same as Fusion, I can send you that if you like.

  21. #38
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    Quote Originally Posted by isaac338 View Post
    Calling a post a "code generator" doesn't lend credibility to your argument..
    Isacc I am guessing your werent even a twitch in your Fathers pants when they were called code generators

  22. Likes Vancbiker 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
  •