Problems with Solid/Rigid tapping
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 33
  1. #1
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default Problems with Solid/Rigid tapping

    Hello,

    I just joined PM and I was hoping to get a little help with Solid/Rigid tapping issue I'm having.
    The Machine I'm using is a Kitamura MyCenter3x with a yasnac I80M controller I'm still just using HSM Express that I downloaded for free and is baked into my Solidworks.

    My question is I have been trying to thread some aluminum parts using the solid tapping function and cannot get it to produce anything worthwhile. One weird thing is that HSM outputs a spindle speed at the beginning of the operation and then again in the G84 line of code. No matter what either one is set at before the tap goes into the part and while its initializing the spindle stops then begins to rotate very slowly while its descending into the part. I've deleted the Speed command in the G84 line and the same thing happens. I'm not quite sure what's going on or what if anything I'm doing wrong. Any help would be greatly appreciated. I'm attaching just a small example of the code I'm running for a tap cycle with a M10 x 1.5 hole. It looks like its working perfectly in the air but obviously something is off. I know that my spindle speed is too slow right now in the code below I'm just trying to keep it at something I can watch.
    Thanks!

    O00054 (M10 TAPPED HOLE)
    (T0014 D=0.3937 CR=0. - ZMIN=-0.625 - RIGHT HAND TAP)
    N10 G90 G94 G17
    N15 G20
    N20 G28 G91 Z0.
    N25 G90
    (DRILL3)
    N30 M09
    N35 T14
    N37 M06
    N40 S381 M03
    N45 M08
    N55 G00 G54 X1.875 Y-0.75
    N60 G43 Z0.6 H14
    N70 G00 Z0.2
    N75 M03
    N80 G93
    N85 G98 G84 X1.875 Y-0.75 Z-0.625 R0.1655 F0.0591 S381
    N90 G80
    N95 G94
    N100 Z0.6
    N110 M09
    N115 G28 G91 Z0.
    N120 G28 X0. Y0.
    N122 M05
    N123 T20
    N124 M06
    N125 M30

  2. #2
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,736
    Post Thanks / Like
    Likes (Given)
    1242
    Likes (Received)
    3555

    Default

    Don't know much about yaznak, but on a fanuc you need to start the spindle with an M29 S*** command. It's been a while, but I seem to recall the same results without it

  3. #3
    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 AMVERGINO View Post
    Hello,

    I just joined PM and I was hoping to get a little help with Solid/Rigid tapping issue I'm having.
    The Machine I'm using is a Kitamura MyCenter3x with a yasnac I80M controller I'm still just using HSM Express that I downloaded for free and is baked into my Solidworks.

    My question is I have been trying to thread some aluminum parts using the solid tapping function and cannot get it to produce anything worthwhile. One weird thing is that HSM outputs a spindle speed at the beginning of the operation and then again in the G84 line of code. No matter what either one is set at before the tap goes into the part and while its initializing the spindle stops then begins to rotate very slowly while its descending into the part. I've deleted the Speed command in the G84 line and the same thing happens. I'm not quite sure what's going on or what if anything I'm doing wrong. Any help would be greatly appreciated. I'm attaching just a small example of the code I'm running for a tap cycle with a M10 x 1.5 hole. It looks like its working perfectly in the air but obviously something is off. I know that my spindle speed is too slow right now in the code below I'm just trying to keep it at something I can watch.
    Thanks!

    O00054 (M10 TAPPED HOLE)
    (T0014 D=0.3937 CR=0. - ZMIN=-0.625 - RIGHT HAND TAP)
    N10 G90 G94 G17
    N15 G20
    N20 G28 G91 Z0.
    N25 G90
    (DRILL3)
    N30 M09
    N35 T14( M06 and T14 should be on same page)
    N37 M06
    N40 S381 M03 its not needed as you have it below in the g84 line
    N45 M08
    N55 G00 G54 X1.875 Y-0.75
    N60 G43 Z0.6 H14
    N70 G00 Z0.2
    N75 M03(you dont need this )
    N80 G93
    N85 G98 G84 X1.875 Y-0.75 Z-0.625 R0.1655 F0.0591 S381 your R should be .200 to match the "z" in line n70 (not required)
    N90 G80
    N95 G94
    N100 Z0.6
    N110 M09
    N115 G28 G91 Z0.
    N120 G28 X0. Y0.
    N122 M05
    N123 T20
    N124 M06
    N125 M30
    its going to go slow cause your only going 381 rpm

  4. #4
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Thanks for the reply, The Spindle is getting commanded in two places in the code on the yasnac its M03 S... and that's being commanded at the beginning. My problem is that it turns on at the speed commanded but once it enters the canned cycle it drops dramatically. Neither the speed at the beginning or the one in the G84 line make any difference. My guess is its around 100RPM maybe slower when its actually doing the tap cycle

  5. #5
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Thanks for the reply but its dropping to maybe 100 rpm the 381 is just a speed I put in so I can watch it. Like I explained above the spindle drops to a crawl as soon as it enters the G84 Canned cycle. I could have it set at 3000 rpm but as soon as it enters G84 it comes to a crawl

  6. #6
    Join Date
    Dec 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    29

    Default

    Quote Originally Posted by AMVERGINO View Post
    Thanks for the reply but its dropping to maybe 100 rpm the 381 is just a speed I put in so I can watch it. Like I explained above the spindle drops to a crawl as soon as it enters the G84 Canned cycle. I could have it set at 3000 rpm but as soon as it enters G84 it comes to a crawl
    This works on the one I ran.
    Same machine and control.

    N1 G0 G90 G40 G80 G17
    N2 G91 G28 Z0.
    N3 T32
    N4 M6(M11 X 1 TAP)
    N5 M3 S500
    N6 G90
    N7 G60
    N8 G0 G54 X-4.5638 Y-3.739
    N9 G43 Z0.375 H32 M8
    N10 G60
    N11 G0
    N12 G93
    S500
    N13 G98 G84 X-4.5638 Y-3.739 Z-1.3819 R0.125 S500 F.0394
    N14 G94
    N15 G80
    N16 Z0.375
    N17 G91 G28 Z0. M9
    N18 M05
    N19 M01
    N20 G91 G28 Z0.
    N21 G28 Y0. M5
    N22 G90
    N23 M30
    (ESTIMATED TIME CYCLE 0:00:37 HR/MIN/SEC)
    %

  7. #7
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Quote Originally Posted by JCarroll View Post
    This works on the one I ran.
    Same machine and control.

    N1 G0 G90 G40 G80 G17
    N2 G91 G28 Z0.
    N3 T32
    N4 M6(M11 X 1 TAP)
    N5 M3 S500
    N6 G90
    N7 G60
    N8 G0 G54 X-4.5638 Y-3.739
    N9 G43 Z0.375 H32 M8
    N10 G60
    N11 G0
    N12 G93
    S500
    N13 G98 G84 X-4.5638 Y-3.739 Z-1.3819 R0.125 S500 F.0394
    N14 G94
    N15 G80
    N16 Z0.375
    N17 G91 G28 Z0. M9
    N18 M05
    N19 M01
    N20 G91 G28 Z0.
    N21 G28 Y0. M5
    N22 G90
    N23 M30
    (ESTIMATED TIME CYCLE 0:00:37 HR/MIN/SEC)
    %
    Thanks for responding, so the main difference I see is your commanding a G60 on line N10 and on the G84 your S... is before the F...
    other than that I don't see any major differences. I've never used a G60 in the yasnac manual it is defined as a "unidirectional approach"
    Is this a necessity to run the tap cycle?
    Ill give it a try when I fire the machine back up

  8. #8
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,421
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1616

    Default

    IIRC You need an M29 Sxxx to start the spindle for tapping as Larry said. This was on a matsurra, Yasnac I80 control. Also I think you need a G95, not G93 for feed per rev OR you can try G94, but you need to adjust your feed move then...

    edit: I see it is G93. I don't recall that, but ?? I do remember I had to use M29 though, not sure if it applies to your machine...

  9. #9
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,569
    Post Thanks / Like
    Likes (Given)
    4170
    Likes (Received)
    2724

    Default

    change your G94 to a G95.
    You're feeding it at .0591 inches per minute and that's why it's so slow.
    You want inches per revolution which is G95.

    OR
    if you want to stay with Inches per minute then you need to figure out the correct feed for the pitch of the tap.
    And since you're going 381rpm, then you want F22.5171 as your G94 feedrate.

  10. #10
    Join Date
    Dec 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    29

    Default

    Quote Originally Posted by Mtndew View Post
    change your G94 to a G95.
    You're feeding it at .0591 inches per minute and that's why it's so slow.
    You want inches per revolution which is G95.

    OR
    if you want to stay with Inches per minute then you need to figure out the correct feed for the pitch of the tap.
    And since you're going 381rpm, then you want F22.5171 as your G94 feedrate.

    You are correct.
    I quickly posted code using an old IP post that was on my computer at home while I was getting it dialed in.
    IPR feed rates are the way to go on this control.

    I think I'll go back to lurking. The F360 thread was pretty good but I'm to old for this shit anymore.
    Sorry.

  11. Likes Mtndew liked this post
  12. #11
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,421
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1616

    Default

    Quote Originally Posted by JCarroll View Post
    You are correct.
    I quickly posted code using an old IP post that was on my computer at home while I was getting it dialed in.
    IPR feed rates are the way to go on this control.

    I think I'll go back to lurking. The F360 thread was pretty good but I'm to old for this shit anymore.
    Sorry.
    I think the yasnac I ran did want/default to IPR, just for threading though. IPM was fine for everything else...

  13. #12
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    549
    Post Thanks / Like
    Likes (Given)
    36
    Likes (Received)
    190

    Default

    I am guessing he doesnt know code very well.
    and he is relying on what the his software put out. in this case he could be using a fadal post/code generator. as fadal will use the thread lead 1.5mm = 0.0591 or 1/TPI x rpm = feed.
    or his post/code generator isnt set up for threading correctly.



    I didnt know Mitsubishi controls can use thread lead

  14. #13
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Quote Originally Posted by Delw View Post
    I am guessing he doesnt know code very well.
    and he is relying on what the his software put out. in this case he could be using a fadal post/code generator. as fadal will use the thread lead 1.5mm = 0.0591 or 1/TPI x rpm = feed.
    or his post/code generator isnt set up for threading correctly.



    I didnt know Mitsubishi controls can use thread lead
    You're Correct I do not know code all that well, I am still learning. That is why I am asking. My yasnac controller does not have a g95 option the F.. code is only for the pitch and .0591 is the pitch for a M10 x 1.5. Supposedly this pitch will be maintained no matter what speed I command the machine (within reason). I can only command solid tap on g93 and solid tap off g94. Then using g84 give all the parameters. Sorry I didn't respond earlier but I was out of town. I will try some of the above mentioned ideas but using g95 will not work.

  15. #14
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,421
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1616

    Default

    Quote Originally Posted by AMVERGINO View Post
    You're Correct I do not know code all that well, I am still learning. That is why I am asking. My yasnac controller does not have a g95 option the F.. code is only for the pitch and .0591 is the pitch for a M10 x 1.5. Supposedly this pitch will be maintained no matter what speed I command the machine (within reason). I can only command solid tap on g93 and solid tap off g94. Then using g84 give all the parameters. Sorry I didn't respond earlier but I was out of town. I will try some of the above mentioned ideas but using g95 will not work.
    So you are saying G95 is not an option on your machine? I am curious what your code looks like for something like face milling a part, or milling a contour. Is it outputting IPR instead of IPM there too?

  16. #15
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Quote Originally Posted by Mike1974 View Post
    So you are saying G95 is not an option on your machine? I am curious what your code looks like for something like face milling a part, or milling a contour. Is it outputting IPR instead of IPM there too?
    I used the incorrect term.. The yasnac controller has no g95 command. Also M29 has to do with magazine orientation and position and nothing to do with spindle speed. according to the yasnac manual with solid tapping F.. is only Z axis pitch per revolution mm/rev or in/rev. Also the range of the F has to be within .000001 to 7.874015 in. I have it correct in the code basically F.. on this machine is pitch only. I've tried the code that JCarroll posted above and it does the same thing comes down at speed and then slows to a crawl when its actually tapping. His code commanded speed 3x which I felt was redundant. For some reason our machine slows the g84 canned cycle as soon as its initializing before it enters the part and no matter what speed is commanded it slows to what I'm guessing is about 100rpm.

  17. #16
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,421
    Post Thanks / Like
    Likes (Given)
    1474
    Likes (Received)
    1616

    Default

    Quote Originally Posted by AMVERGINO View Post
    I used the incorrect term.. The yasnac controller has no g95 command. Also M29 has to do with magazine orientation and position and nothing to do with spindle speed. according to the yasnac manual with solid tapping F.. is only Z axis pitch per revolution mm/rev or in/rev. Also the range of the F has to be within .000001 to 7.874015 in. I have it correct in the code basically F.. on this machine is pitch only. I've tried the code that JCarroll posted above and it does the same thing comes down at speed and then slows to a crawl when its actually tapping. His code commanded speed 3x which I felt was redundant. For some reason our machine slows the g84 canned cycle as soon as its initializing before it enters the part and no matter what speed is commanded it slows to what I'm guessing is about 100rpm.
    That is weird. I *know* the Matsurra I ran with a Yasnac I80 used an M29 for rigid tapping. I wish I had a code to post but that was some years ago.

    Couple questions-

    Have you tried hand editing the code to input a G95, say one line before your tapping cycle? I was using a generic post at the time so I hand edited this every time.

    So you are saying "code basically F.. on this machine is pitch only" so everything is posted/uses IPR? Interesting for milling (it is a vmc yes?).... On Fanuc (lathe... only??) for threading you can use E instead of F to get to 5 decimal places...

    What is in your 'safety line' G20 or G21?

  18. #17
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Quote Originally Posted by Mike1974 View Post
    That is weird. I *know* the Matsurra I ran with a Yasnac I80 used an M29 for rigid tapping. I wish I had a code to post but that was some years ago.

    Couple questions-

    Have you tried hand editing the code to input a G95, say one line before your tapping cycle? I was using a generic post at the time so I hand edited this every time.

    So you are saying "code basically F.. on this machine is pitch only" so everything is posted/uses IPR? Interesting for milling (it is a vmc yes?).... On Fanuc (lathe... only??) for threading you can use E instead of F to get to 5 decimal places...

    What is in your 'safety line' G20 or G21?
    This is a Kitamura MyCenter3x Vertical Milling Machine. M29 is a chip conveyor command says so in my Kitamura manual sorry for the mixup. However, M54 is a rigid tapping M.. in the Kitamura manual but it doesn't explain anything past that. G95 is not on my machine and isn't recognized. The only 2 G codes for solid tapping are G93 solid tap on, and g94 solid tap off. IPM works in everything except solid tapping. In solid tapping I can only input IPR, it says so in my yasnac manual. G94 and G20 are among the default commands on the "safety line" of the machine.

  19. #18
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,569
    Post Thanks / Like
    Likes (Given)
    4170
    Likes (Received)
    2724

    Default

    I'm really confused here. Granted I haven't ran a Yasnac mill control ever, but have ran Yasnac lathe controls before so I'm sort of familiar with them. I know apples/oranges.

    You say that your machine only accepts IPR in tapping yet you're putting in a G94 which is IPM.
    G95 typically isn't an option and normally is standard on all controls.
    G93 is usually Inverse Time feed.
    M29 (for fanuc) is the code that "triggers" the rigid tapping motion.

    If your machine can't use the above 3 codes, then they must have alternate codes. For example IPR on your mill might be G295 or whatever.
    Do you have the manual that shows the format of your rigid tapping cycle?

    For my Fanuc mill this is how my tap cycle looks:

    N100T1M06( M10 X 1.5 RH TAP)
    /M08
    (MAX - Z2.)
    (MIN - Z-1.)
    G00G90G54X0.Y0.
    G43H1Z2.
    G95
    M29S485
    G98G84Z-1.R.5F.05906
    G80M09

    M05
    G91G28Z0.
    G91G28Y0.
    G00G90X-10.
    G90
    M30
    %

  20. #19
    Join Date
    Dec 2006
    Country
    UNITED STATES
    State/Province
    California
    Posts
    125
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    29

    Default

    Quote Originally Posted by AMVERGINO View Post
    This is a Kitamura MyCenter3x Vertical Milling Machine. M29 is a chip conveyor command says so in my Kitamura manual sorry for the mixup. However, M54 is a rigid tapping M.. in the Kitamura manual but it doesn't explain anything past that. G95 is not on my machine and isn't recognized. The only 2 G codes for solid tapping are G93 solid tap on, and g94 solid tap off. IPM works in everything except solid tapping. In solid tapping I can only input IPR, it says so in my yasnac manual. G94 and G20 are among the default commands on the "safety line" of the machine.

    You should call Gary Frost's people and get their help.
    Machinery Sales are/were the Kitamura reseller in California.

    1-626-581-9221

  21. #20
    Join Date
    Aug 2019
    Country
    UNITED STATES
    State/Province
    California
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    3

    Default

    Quote Originally Posted by Mtndew View Post
    I'm really confused here. Granted I haven't ran a Yasnac mill control ever, but have ran Yasnac lathe controls before so I'm sort of familiar with them. I know apples/oranges.

    You say that your machine only accepts IPR in tapping yet you're putting in a G94 which is IPM.
    G95 typically isn't an option and normally is standard on all controls.
    G93 is usually Inverse Time feed.
    M29 (for fanuc) is the code that "triggers" the rigid tapping motion.

    If your machine can't use the above 3 codes, then they must have alternate codes. For example IPR on your mill might be G295 or whatever.
    Do you have the manual that shows the format of your rigid tapping cycle?

    For my Fanuc mill this is how my tap cycle looks:

    N100T1M06( M10 X 1.5 RH TAP)
    /M08
    (MAX - Z2.)
    (MIN - Z-1.)
    G00G90G54X0.Y0.
    G43H1Z2.
    G95
    M29S485
    G98G84Z-1.R.5F.05906
    G80M09

    M05
    G91G28Z0.
    G91G28Y0.
    G00G90X-10.
    G90
    M30
    %
    So as I said above G94 turns off solid tap mode. The only two G codes related to solid tapping are G93/G94 I'm attaching below the explanation in the yasnac manual for my controller. IPR is used in solid tap you cannot use IPM.
    Attached Thumbnails Attached Thumbnails solid-tap-2.jpg   solid-tap-1.jpg  

  22. Likes 1cncmachinist 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
  •