Offsets!! What is the secret?? NEED HELP - Page 2


Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 45

Thread: Offsets!! What is the secret?? NEED HELP

  1. #21
    Member
    Join Date
    Jul 2006
    Location
    United States
    Posts
    367
    Downloads
    1
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    I went through the same offset puzzle, with my 3016. Here is another youtube channel that helped me.



    pete


  2. #22

    Default Re: Offsets!! What is the secret?? NEED HELP

    Gade leave the Z in the fixture offset at ZERO. If you have set your tools using the UT and using your 2inch block the values in the Tool offsets will bring the tools to your part using the H-word. H1Z0, H2Z0, etc. etc.



  3. #23

    Default Re: Offsets!! What is the secret?? NEED HELP

    Or Gade post a video of what you are doing, or what its doing the control



  4. #24
    Member
    Join Date
    Jun 2012
    Location
    United States
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    this will make the 3rd time i uploaded this PDF to cnczone...

    maybe search for this stuff before making a new thread?

    if i were u i wouldn't mess around much with the DF menu especially for E1/G54. obviously you need to set the others.


    also, u should get some probes, would get rid of a lot of your issues

    Attached Thumbnails Attached Thumbnails Offsets!!  What is the secret??  NEED HELP-fadal-fixture-tool-home-setup-procedure-pdf  


  5. #25
    Registered
    Join Date
    Mar 2016
    Location
    Canada
    Posts
    10
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by mflux_gamblej View Post
    this will make the 3rd time i uploaded this PDF to cnczone...

    maybe search for this stuff before making a new thread?

    if i were u i wouldn't mess around much with the DF menu especially for E1/G54. obviously you need to set the others.


    also, u should get some probes, would get rid of a lot of your issues

    Yeah ok thx!! Maybe you should read what I wrote a cpl. Weeks ago. I've done plenty of searches already.. I've spent hrs. Searching/reading and comparing the issues that others have had.
    I've already downloaded your PDF about 5 times.. thx

    But, it's not helping!!!
    I will explain aigain.
    You say leave Z E1 at 0". Ok fine, spindle will stay up at CS position.
    Now, If I set tool lengths 1, 2, 3 etc off the top of my work piece which is now E2 ex of tool lengths: (T1 -20.00", T2 -19.00")
    Now if I use E2 for my work setup,, in order for tool 1 to come down to the top I must set E2 Z at -20.00".... if I send Tool 2 to the same place it will go 1" lower.
    I don't and shouldn't have to modify all my tool lengths.

    The only way I have found to be able to use (ex: 3 tools) in the same program,, is to use 3 different fixtures (same X, Y but just vary the Z depending which tool is being used)
    Yes it's still cheating,, but it works well with no risk of miscalculating a modified tool length.

    Rodney,,, I made a video, but I must setup a YouTube account.. in a cpl days.

    A big thanks to everyone who read/wrote in this post.
    I feel like I'm getting closer to a solution,, or maybe I'm just dreaming

    Note: on the DF screen menu there is an option (go to fixture) #8 I think..
    Is there any cons to useing this function to verify Z offsets?



  6. #26
    Member
    Join Date
    Jun 2012
    Location
    United States
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    lol, guess my pdf isnt all that its cracked up to be.

    on E2 you should set the Z difference between wherever E1 was and where E2 is. then you don't have to set any tools off your workpiece. I always used a depth setter like this cheapo from shars: Precision Magnetic Z Axis Zero Setter 2" Height x 0.001" you can use the blue setter to find the delta between E1 and E2. just put the blue piece on your work, then get a tool, program H1 (if using tool 1), then jog to the blue block, zero the dial, and read the zpos off the screen - that's the delta for E2. all the DT's stay the same. use an edge finder to pickup x and y for E2 relative to your home position. when your program H1 you may want to also program like H1 Z5. so that the tool doesn't move down to zero and crash into something. also set rapid to 25% and have hand on red button... and remember Z5 will go to 0.0005", Z5. will go to 5"

    I always set Z0 at the top of my vise - you could do it anywhere tho. all the tools are then set on that blue block which i put on my vise. I then use softjaws and also i draw my vise in my cam software - so then you machined xy 0, and z0 relative to your cam software. the best thing is probes, but i can understand if that's too much to chew right away. with probes the tools set themselves and u can find the workpiece automatically too.



  7. #27
    Member
    Join Date
    Jun 2012
    Location
    United States
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    Quote Originally Posted by Gade1000 View Post
    Yeah ok thx!! Maybe you should read what I wrote a cpl. Weeks ago. I've done plenty of searches already.. I've spent hrs. Searching/reading and comparing the issues that others have had.
    I've already downloaded your PDF about 5 times.. thx

    But, it's not helping!!!
    I will explain aigain.
    You say leave Z E1 at 0". Ok fine, spindle will stay up at CS position.
    Now, If I set tool lengths 1, 2, 3 etc off the top of my work piece which is now E2 ex of tool lengths: (T1 -20.00", T2 -19.00")
    Now if I use E2 for my work setup,, in order for tool 1 to come down to the top I must set E2 Z at -20.00".... if I send Tool 2 to the same place it will go 1" lower.
    I don't and shouldn't have to modify all my tool lengths.

    The only way I have found to be able to use (ex: 3 tools) in the same program,, is to use 3 different fixtures (same X, Y but just vary the Z depending which tool is being used)
    Yes it's still cheating,, but it works well with no risk of miscalculating a modified tool length.

    Rodney,,, I made a video, but I must setup a YouTube account.. in a cpl days.

    A big thanks to everyone who read/wrote in this post.
    I feel like I'm getting closer to a solution,, or maybe I'm just dreaming

    Note: on the DF screen menu there is an option (go to fixture) #8 I think..
    Is there any cons to useing this function to verify Z offsets?
    maybe this is the key piece of info:

    dont set your tools off of your workpiece, only set them from the same place all the time, like the top of your vise for example.

    then, set your fixture offset Z as the difference in Z from where you always set your tools to the top of your workpiece. (or if u use cam / softjaws you just need to draw the coord sys right).



  8. #28

    Default Re: Offsets!! What is the secret?? NEED HELP

    3 photos would work too Gade easier to post pic1 of the screen showing whats on the screen from the toolchange line down hopefully 10-15 lines. Pic 2 the DT page and pic 3 the DF page. And for doing what your doing you can allways forget the fixture offsets all together especially if your only working with 1 part and just pick-up your X and Y and do a SETX and SETY leave your Z at CS ... Set your tools and in your program NO fixture call NO E-word NO G54... and just use the H1 Z.100 for the tool to come down(will come down to .100 above part) as long as you have a G90G0 before calling the tool. and then when going to the next tool G90G0 and then the H2Z.1 for tool 2 to be .100 above the part etc. etc.



  9. #29
    Member
    Join Date
    Oct 2009
    Location
    New Zealand
    Posts
    51
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    Now you can probably see why I came up with "my" way of setting tools and fixtures when I first started out .... it was a logical way of doing it that I could get me head around and understand.
    I am not going to confuse the issue and throw anymore info into the mix .... there's plenty of there now ..... but I think the key to it all is for you to understand/work-out why its doing whats its doing.
    Once you work that out, everything else will make a whole lot more sense......



  10. #30
    Registered
    Join Date
    Mar 2016
    Location
    Canada
    Posts
    10
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    Hello again,,
    Sorry I can't show/post the pics that I took,, I'm using my phone,, I'll get it.
    So this is what I did,,,
    - I reset all my tool lengths,, with a 2" height/dial block on my work piece using the utility,,,, -19", -18.345", -21.324" etc etc
    - Now again using the utility,, I set fixture #1 X-13, Y 13, Z 0
    Then I set fixture #2 X-13, Y 13, Z +2"
    -in my program I set it to E2
    Note: CS is 0" and my work piece is at -19"+/- from CS.

    Then I pressed start!!
    Does anyone want to take a guess where the spindle went???

    Well the spindle DID NOT go down to my piece,, it went 2" up from CS.
    So I am sure that there is something that you're all not saying!!

    Any suggestions??



  11. #31
    Member
    Join Date
    Jun 2012
    Location
    United States
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    Quote Originally Posted by Gade1000 View Post
    Hello again,,
    Sorry I can't show/post the pics that I took,, I'm using my phone,, I'll get it.
    So this is what I did,,,
    - I reset all my tool lengths,, with a 2" height/dial block on my work piece using the utility,,,, -19", -18.345", -21.324" etc etc
    - Now again using the utility,, I set fixture #1 X-13, Y 13, Z 0
    Then I set fixture #2 X-13, Y 13, Z +2"
    -in my program I set it to E2
    Note: CS is 0" and my work piece is at -19"+/- from CS.

    Then I pressed start!!
    Does anyone want to take a guess where the spindle went???

    Well the spindle DID NOT go down to my piece,, it went 2" up from CS.
    So I am sure that there is something that you're all not saying!!

    Any suggestions??
    you called your TLO right?

    M6T1
    G0 G90 E2 X1Y1
    G43 H1 Z0

    should take you to 2" above E1 with whatever tool 1 is.



  12. #32
    Member
    Join Date
    Jun 2012
    Location
    United States
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    here's a setup of mine:

    Offsets!!  What is the secret??  NEED HELP-chamfer-png

    it uses E2, for which Z is zero in my case, because I have tool setter. it's DF is 1.11" or so for Z, its located at E24. so, in reality my tool setter's trigger point in z is 1.11" above the top of my vise (not vise jaw - see the coord sys in my picture).

    here's the G-code for that tool path. its a chamfer on the upper edge of the part.
    N1 G90 G17 G80 G00 G40

    N141 T1 M06 *90 Deg 1/4" Chamfer - 4FL - MariTool 3500-.250-90DEG*
    N142 *F-contour2*
    N143 G00 E2 G90 X2.4417 Y-1.995 A0. S6500 M03
    N144 G43 H1 Z1.25 M07
    N145 G04 P100
    N146 X2.4417 Y-1.995
    N147 Z1.25
    N148 Z0.8635
    N149 G01 G40 Z0.7085 F26.
    N150 G03 X2.2917 Y-1.845 I-0.15 J0.
    N151 G01 X0.9583 F26.
    N152 G02 X0.8083 Y-1.695 I0. J0.15
    N153 G01 Y-0.895 F26.
    N154 G02 X0.9583 Y-0.745 I0.15 J0.
    N155 G01 X2.2917 F26.
    N156 G02 X2.4417 Y-0.895 I0. J-0.15
    N157 G01 Y-1.695 F26.
    N158 G02 X2.2917 Y-1.845 I-0.15 J0.
    N159 G01 X2.0917 F26.
    N160 G03 X1.9417 Y-1.995 I0. J-0.15
    N161 G00 Z1.25
    N162 M09
    N163 M05
    N164 G00 G90
    N165 G53 Z0
    N166 M6 T1
    N167 E0 X0 Y0 A0
    N168 S.1
    N169 M30
    %



  13. #33

    Default Re: Offsets!! What is the secret?? NEED HELP

    E2 in your program yes will go up in the Z axis 2 inches, so after your E2 the next line when you type G90G0H1Z.100 your tool #1 (if its in the spindle will come down to .100 position)



  14. #34
    Registered
    Join Date
    Mar 2016
    Location
    Canada
    Posts
    10
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    Here are a few pics,,
    1. is where I set my tools from today
    2. my tool length menu screen
    3. my fixture menu screen
    4. the code that my post processor gives me,,, the only things that I change everytime before I send it to the machine, is
    Line 45 (I inert the right fixture #)
    Line 52 ( add z +,,,)
    Once in the machine I delete the last 3 lines and add the machines End of Program (A bit of laziness on my behalf) ask and i'll explain!!

    Offsets!!  What is the secret??  NEED HELP-1-jpg

    Offsets!!  What is the secret??  NEED HELP-2-jpg

    Offsets!!  What is the secret??  NEED HELP-3-jpg



    %
    O0039 (G2 17.5)
    (T11 D=0.25 CR=0.125 - ZMIN=-0.6624 - BULLNOSE END MILL)
    N10 G90 G94 G17 H0 E0
    N15 G20
    N20 G0 H0 Z0.

    (2D CONTOUR2)
    N25 M9
    N30 T11 M6
    N35 S8000 M3
    N40 G4 P23
    N45 E2
    N50 M8
    N52 z 0.02
    N60 G0 X-0.025 Y-1.0125
    N65 H0 Z0.04
    N70 Z0.0394
    N75 G1 Z-0.3174 F60.
    N80 G19 G2 Y-1.0375 Z-0.3424 J-0.025
    N85 G1 Y-1.0625 F60.
    N90 G17 G3 X0. Y-1.0875 I0.025
    N95 G1 X1. F60.
    N100 G3 X1.2411 Y-0.9448 J0.275



  15. #35
    Member
    Join Date
    Jun 2012
    Location
    United States
    Posts
    516
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    H0 - bad.

    u need H11.

    looks like u have some work to go here. read the fadal manuals especially all the g-code ones.



  16. #36
    Registered
    Join Date
    Mar 2016
    Location
    Canada
    Posts
    10
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    well like i've already mentioned,, I know Jack-Sh,t about writing code.
    But still,,, even thought the beginning of that code my not be good... my jobs are getting done.
    The machine takes it, and doesn't say a word or error so maybe one cold/rainy day I will sit and read.
    I'm using what I have,, Fadal generic post processor in Inventor Hsm works
    The issue that i'm having is still there,, code or no code.

    The next time you are in front of your machine,, try this.

    On the DF menu,,
    option 1,, choose a fixture,, any one you want. from 2 to 10
    now on the same screen choose option 8 (I think,,) go to fixture.
    It should go to the fixture of your choice,, right?

    Last edited by Gade1000; 07-06-2017 at 06:18 PM. Reason: grammar


  17. #37
    Member
    Join Date
    Jun 2013
    Location
    USA
    Posts
    1041
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    It's doesn't seem right to touch off 2 inches above your part and then add a positive number to your z fixture offset. Your already 2 inches above the part where you set your tool. It would make more sense to put negative 2 in the z fixture offset instead of positive 2 if you really want to make it to the part. Also if the h number in your code doesn't match your t number then how is the machine supposed to know where to look to find the offset for that tool.

    Ben

    Sent from my HTC6525LVW using Tapatalk



  18. #38

    Default Re: Offsets!! What is the secret?? NEED HELP

    Gade you definately need to edit your post (your getting alot of junk code) . Running fadal format 1 your first bit of code (safe line should be something like this what i always use) G90G0G17G80 then your rpm M3 then position XandY then H(whatever tool number) with a Z.100 (stays .100 above the part) If you want Gade private message me your number and i can walk you through it (and help you understand better the control). Format 1 is very safe Format 2 (Fanucish) is a little tougher because it retains Modal code unlike Format 1 (it always resets to your SETP everytime you exit a program.



  19. #39

    Default Re: Offsets!! What is the secret?? NEED HELP

    Another thing Gade when ever you upload a program into the fadal always renumber with the NU command.

    this is what your program should look like (If your going to be using 1 fixture then your only going to use E1 or G54) G94 not used you dont need the G20 the G4P23 is a dwell of 23 milliseconds which is basically nothing remove that. And get rid of H0's

    I HIGHLY recommend finding another post processor

    O0039 (G2 17.5)
    (T11 D=0.25 CR=0.125 - ZMIN=-0.6624 - BULLNOSE END MILL)
    N10 G90 G0 G17 G80



    (2D CONTOUR2)

    N30 T11 M6
    N35 S8000 M3


    N50 M8

    N60 G0 X-0.025 Y-1.0125E1
    N65 H11 Z0.04
    N70 Z0.0394
    N75 G1 Z-0.3174 F60.
    N80 G19 G2 Y-1.0375 Z-0.3424 J-0.025
    N85 G1 Y-1.0625 F60.
    N90 G17 G3 X0. Y-1.0875 I0.025
    N95 G1 X1. F60.
    N100 G3 X1.2411 Y-0.9448 J0.275


    Remember to renumber the program after you upload using the NU command or the quick key



  20. #40
    Registered
    Join Date
    Nov 2016
    Location
    United States
    Posts
    4
    Downloads
    0
    Uploads
    0

    Default Re: Offsets!! What is the secret?? NEED HELP

    Quote Originally Posted by Gade1000 View Post
    well like i've already mentioned,, I know Jack-Sh,t about writing code.
    But still,,, even thought the beginning of that code my not be good... my jobs are getting done.
    The machine takes it, and doesn't say a word or error so maybe one cold/rainy day I will sit and read.
    I'm using what I have,, Fadal generic post processor in Inventor Hsm works
    The issue that i'm having is still there,, code or no code.

    The next time you are in front of your machine,, try this.

    On the DF menu,,
    option 1,, choose a fixture,, any one you want. from 2 to 10
    now on the same screen choose option 8 (I think,,) go to fixture.
    It should go to the fixture of your choice,, right?
    How are your jobs getting done if you can't get the machine to put tools to them? And why are you using six different fixture offsets when it sounds like one is challenge enough for you?

    Set X/Y coordinates in the DF page as #1(clear the rest) and leave Z at zero - period. Use E1 in your program and nothing else for now(no E0's or E2's etc...).
    Set your tools using the UT/Tool Setting function(watch the video on it that someone already posted in this thread).

    Not trying to be a dick but your code is definitely NOT OK(even though you assured everybody the code wasn't the problem). As already mentioned, you need to use an H# that corresponds to the tool your using. That calls up the correct tool length offset from the DT table.

    Slow down, take a deep breath, forget everything you've taught yourself and START OVER



Page 2 of 3 FirstFirst 123 LastLast

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

Offsets!!  What is the secret??  NEED HELP

Offsets!!  What is the secret??  NEED HELP