Fadal Rigid Tapping problem. Feedrate synching on pull out.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 26
  1. #1
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default Fadal Rigid Tapping problem. Feedrate synching on pull out.

    Hello all. Ive been having some problems rigid tapping with the fadal EMC. Lots of broken taps. The first issue was the spindle speed designation of high or low gear. example is "S120.1" or "S120.2" or no setting at all. If the high/low gear waasnt set or ".1" was set, the spindle speed would be off relative to the feedrate. So now im setting the spindle speed with ".2" and the spindle speed when the tap is going in so that problem has been solved. The second problem im having is the feed rate changing when the tap is pulling out. Initially my program included a "P100" dwell time at the bottom of the tap, for some reason this was causing the feedrate to double on pull out and the spindle speed to become unsynchronized. After deleting the "p100" code the feed rate no longer doubled, but stayed the same but still slightly off. My feedrate is 3.75, but would pull out at 3.9. Spindle speed is 120 and thats constant now so no problem there. Attached is a video showing the spindle speed constant at 120, but the Feedrate changing to 3.9 on pulling out. If anybody can see whats wrong with my code or if theres a setting on the machine please let me know, thanks.

    Note: im using g84 instead of g84.1, its because the screen set with g84.1 becomes unreadable and the feedrate and spindle speed seems way off.

    %
    o6003
    N6 G40 G49 G80
    N9(Clockwise Tap)
    N12 T15 M6
    N15 G0 G90 E1 X12.007 Y4.668 S120.2 M5 F3.75
    N18 G43 Z0.201 H15
    N21 M8
    N24 G0 Z0.201
    N30 G98 G84 R+0.151 Z-0.549 F3.75 S120.2
    N33 G80 Z0.200 F3.75
    N36 G1 Z0.201 F3.75
    N39 M9
    N42 M5
    N45 G91 G28 Z0
    N48 M30
    %


  2. #2
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default

    i found a band aid solution. Because of the "PXXX" or dwell time, caused the pull out feed rate to change relative to the dwell time, i changed the dwell time to get as close to the desired feedrate as possible. When the dwell time of P100 was used, it would double the pull out feedrate from 3.75 to 7.5 (at the same time the rpm would almost double, but still not synch). So then i removed the dwell code all together, the feed rate then went from 3.75 to 3.9 on pull out. I then added the P Code back in with a "P-10" and it reduced the pull out feedrate to 3.4. So then i changed the dwell time to "-1.0" and now the feedrate is 3.7 which i think is close enough to tap a 3/8". Does anyone know why it does this? it seems like a machine setting. could the P code in Format 2 actually mean something else?

  3. #3
    Join Date
    May 2019
    Country
    GUADELOUPE
    Posts
    974
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    462

    Default

    I've never seen an S called in a G84 cycle, also never seen a + used either. Likely shouldn't be using second gear at 120 RPM either. I like to run G95 but a quick bit of reading and it looks like Fadals will accept a Q value kind of like a G95. Keep in mind I know nothing about Fadals and never ran one, your code just looks funny to me

    https://www.fadalcnc.com/media/pdf/F...ing_Cycles.pdf

  4. Likes InspireCNC liked this post
  5. #4
    Join Date
    Aug 2005
    Location
    Manchester, MD
    Posts
    267
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    37

    Default

    You aren’t using rigid tapping. Rigid tapping is G84.1. See the instructions in Hardplates link. G84 is standard tapping using a floating holder.

  6. Likes Bobw, InspireCNC liked this post
  7. #5
    Join Date
    Aug 2005
    Location
    Manchester, MD
    Posts
    267
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    37

    Default

    See page 96. https://www.fadalcnc.com/media/pdf/t...xed_Cycles.pdf

    G84 reverses from hole at 105% feedrate.

  8. Likes InspireCNC liked this post
  9. #6
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    994
    Post Thanks / Like
    Likes (Given)
    89
    Likes (Received)
    360

    Default

    You must use a g84.1 or g84.2 other wise you will be breaking taps .
    no ifs and or butts about it.
    Also your code will change dependign on what format your doing. hardplates posts a good link and code

  10. Likes InspireCNC liked this post
  11. #7
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default

    Quote Originally Posted by Hardplates View Post
    I've never seen an S called in a G84 cycle, also never seen a + used either. Likely shouldn't be using second gear at 120 RPM either. I like to run G95 but a quick bit of reading and it looks like Fadals will accept a Q value kind of like a G95. Keep in mind I know nothing about Fadals and never ran one, your code just looks funny to me

    https://www.fadalcnc.com/media/pdf/F...ing_Cycles.pdf
    Quote Originally Posted by RH68 View Post
    See page 96. https://www.fadalcnc.com/media/pdf/t...xed_Cycles.pdf

    G84 reverses from hole at 105% feedrate.
    Quote Originally Posted by Delw View Post
    You must use a g84.1 or g84.2 other wise you will be breaking taps .
    no ifs and or butts about it.
    Also your code will change dependign on what format your doing. hardplates posts a good link and code
    Thank you. Ill go ahead and read the manual. I was using the 84.1 code but the rpms were way off. perhaps it was the wrong code per format, however i was posting the program with a specific fadal format 2 post processor.

  12. #8
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    994
    Post Thanks / Like
    Likes (Given)
    89
    Likes (Received)
    360

    Default

    Quote Originally Posted by InspireCNC View Post
    Thank you. Ill go ahead and read the manual. I was using the 84.1 code but the rpms were way off. perhaps it was the wrong code per format, however i was posting the program with a specific fadal format 2 post processor.
    I had figured you uses cam to due it as the program looks like bad post.

    g84.1 cycles are easy print that PDF file out and magnet it to your machine. I did that 20 years ago and I still have them there because of running different controls in the shop.
    I did the same thing about 8weeks ago. but hand coded it I forgot the .1 a few parts came out perfect how I have no clue gage went fine no go didnt go at all. about 1/4 way into the day my thread gages started to feel funny. ( I was using the knobs to fine tune the endmills) and well it was reading the overrides. took me about 3 hours to figure out what was wrong. wanted to kick myself in the ass when I saw the typo

  13. Likes InspireCNC liked this post
  14. #9
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,283
    Post Thanks / Like
    Likes (Given)
    15060
    Likes (Received)
    11133

    Default

    Quote Originally Posted by RH68 View Post
    See page 96. https://www.fadalcnc.com/media/pdf/t...xed_Cycles.pdf

    G84 reverses from hole at 105% feedrate.
    And that is what the P word controls. P1 is 1% feedrate over ride,
    and P100 is 100% override which perfectly coincides with doubling of
    the feed. And oddly at least on my older machines P0 should be
    0%, and it should feed in and out at the same speed, but it reverts
    back to the 105%.

  15. Likes InspireCNC liked this post
  16. #10
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default

    Quote Originally Posted by Delw View Post
    I had figured you uses cam to due it as the program looks like bad post.

    g84.1 cycles are easy print that PDF file out and magnet it to your machine. I did that 20 years ago and I still have them there because of running different controls in the shop.
    I did the same thing about 8weeks ago. but hand coded it I forgot the .1 a few parts came out perfect how I have no clue gage went fine no go didnt go at all. about 1/4 way into the day my thread gages started to feel funny. ( I was using the knobs to fine tune the endmills) and well it was reading the overrides. took me about 3 hours to figure out what was wrong. wanted to kick myself in the ass when I saw the typo
    Im working on getting the right code for 84.1 now. Ive tried programing with 84.1 but I was still breaking taps.

    Quote Originally Posted by Bobw View Post
    And that is what the P word controls. P1 is 1% feedrate over ride,
    and P100 is 100% override which perfectly coincides with doubling of
    the feed. And oddly at least on my older machines P0 should be
    0%, and it should feed in and out at the same speed, but it reverts
    back to the 105%.
    after reading the manual it makes sense. thanks.

  17. Likes Bobw liked this post
  18. #11
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default

    Heres my code for rigid tapping (84.1) in format 2. Does anyone know what the number at the top right represents that use to be RPMs (attached video, warning some noise from the way covers that will make you cringe)? It cant be RPMs since the spindle is actually running around 120rpm from my own measurement. I want to make sure things are synchronized before i start breaking taps again. Thanks again for any help, its much appreciated.

    %
    o6003
    N6 G40 G49 G80
    N9(Clockwise Tap)
    N12 T15 M6
    N15 G0 G90 E1 X12.007 Y4.668 S120.1 M5 F3.75
    N18 G43 Z0.201 H15
    N19 G8
    N20 G84.2
    N24 G0 Z0.201
    N30 G98 G84.1 R+0.125 Z-0.549 F3.75 S120.1
    N33 G80 Z0.200
    N36 G1 Z0.201 F3.75
    N39 M9
    N42 M5
    N45 G91 G28 Z0
    N48 M30
    %


  19. #12
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    150
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    31

    Default

    You have no Q which is the thread pitch.
    Attached Files Attached Files

  20. Likes InspireCNC liked this post
  21. #13
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    758
    Post Thanks / Like
    Likes (Given)
    249
    Likes (Received)
    336

    Default

    The C value?
    Yeah, thats how many rotational degrees on the spindle

  22. Likes InspireCNC liked this post
  23. #14
    Join Date
    May 2019
    Country
    GUADELOUPE
    Posts
    974
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    462

    Default

    Quote Originally Posted by InspireCNC View Post
    Heres my code for rigid tapping (84.1) in format 2. Does anyone know what the number at the top right represents that use to be RPMs (attached video, warning some noise from the way covers that will make you cringe)? It cant be RPMs since the spindle is actually running around 120rpm from my own measurement. I want to make sure things are synchronized before i start breaking taps again. Thanks again for any help, its much appreciated.

    %
    o6003
    N6 G40 G49 G80
    N9(Clockwise Tap)
    N12 T15 M6
    N15 G0 G90 E1 X12.007 Y4.668 S120.1 M5 F3.75
    N18 G43 Z0.201 H15
    N19 G8
    N20 G84.2
    N24 G0 Z0.201
    N30 G98 G84.1 R+0.125 Z-0.549 F3.75 S120.1
    N33 G80 Z0.200
    N36 G1 Z0.201 F3.75
    N39 M9
    N42 M5
    N45 G91 G28 Z0
    N48 M30
    %

    If you don't want to risk taps you can grab a lathe threading bar in the spindle and just dust the side of a piece of material thats been blued up. Should leave some tattle tail marks if things are in sync

  24. Likes InspireCNC liked this post
  25. #15
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default

    Quote Originally Posted by VTM View Post
    You have no Q which is the thread pitch.
    Thank you. From my understanding the Q value is only for format 1, is this true? Im in format 2 but im considering switching to format 1 so that i can actually try a program with a q value.

  26. #16
    Join Date
    Apr 2020
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    27
    Post Thanks / Like
    Likes (Given)
    9
    Likes (Received)
    1

    Default

    I tried to tap with my new code. the first hole didnt break, it broke on the second hole. I recall this happening once on another program ive tried.

  27. #17
    Join Date
    Jul 2008
    Location
    Milverton, Ontario, Canada
    Posts
    758
    Post Thanks / Like
    Likes (Given)
    249
    Likes (Received)
    336

    Default

    grab a bolt of known pitch in the spindle, set indicator on thread flank, start rigid tap program with indicator engaged.
    This will show your roughly where the problem is.

    A buddy is rigid tapping m6 holes at 2000 rpm in his old DC Fadal.... fwiw

  28. #18
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    150
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    31

    Default

    Yes, Your right the Q is not necessary for format2. I use format 1 so I'm not positive if there is anything else different.

  29. #19
    Join Date
    Mar 2006
    Country
    PHILIPPINES
    Posts
    2,726
    Post Thanks / Like
    Likes (Given)
    742
    Likes (Received)
    1075

    Default

    Am I the only one who cringes because the G90 is not called until the first positioning move? I detest a G91 G28 move rather than a G53 but since Fadal cant take G53 I see getting stuck with G28. It's that reason right there why my modal calls are on line 1 of the program and always a with a G90.

  30. #20
    Join Date
    May 2019
    Country
    GUADELOUPE
    Posts
    974
    Post Thanks / Like
    Likes (Given)
    342
    Likes (Received)
    462

    Default

    Quote Originally Posted by g-coder05 View Post
    Am I the only one who cringes because the G90 is not called until the first positioning move? I detest a G91 G28 move rather than a G53 but since Fadal cant take G53 I see getting stuck with G28. It's that reason right there why my modal calls are on line 1 of the program and always a with a G90.
    G90 is always the first call in my programs just incase. I use G28 G91 but always call a G90 on the next line.

    Can you call a S code inside a G84 cycle? I've never tried it.


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
  •