1995 Fadal VMC rotary broach G-code
Close
Login to Your Account
Results 1 to 10 of 10
  1. #1
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    1

    Default 1995 Fadal VMC rotary broach G-code

    Hey folks, need a tech assist in getting some code set up for an indexed rotary broaching process on my VMC. I added a sample of a simple broaching cycle from a non-indexed broaching program I already use below. I have an inside spline broach that needs to index on features that have been machined in previous steps (roughed out). When I can afford it, it will be a two broach process with a rough and finish broach each making a run... for now doing the first cuts the hard way. The broach has a brake that holds the bit from turning in the broach holder until it starts to cut teeth. I need to move the broach from the umbrella tool holder where it is indexed at zero rotation. Once the part is positioned under the spindle, I need to move the spindle down to light contact with the part and only then start the spindle rotation. At end of broach run the spindle has to stop and re-orient to zero before withdrawing from the part. The next time the tool gets used it will be in the same clock rotation as last used. I think I can see where to move the spindle start command farther down in the code until the tool is in contact with the part. I think I can even stop the spindle before retracting. I am not so sure about how to cause the spindle to orient to the clock rotation for tool exchange before retracting...

    Does anyone have an indexed rotary broach program of this type working on this model machine? Would love to see some code samples to help me along. I have added comments as to purpose of each line below as I understand them... please let me know if I am off base. The first four lines appear to be getting the machine ready to work, but I don't truly get them. Any lines without a comment are mysteries!

    O0075 (TEST BROACH)
    (T14 D=0.375 CR=0. - ZMIN=0.1871 - FORM MILL)
    N10 G90 G94 G17
    N15 G20
    N20 G28 G91 Z0.
    N25 G90

    (DRILL2)
    N30 T14 M6 (change to tool 14)
    N35 S700 M3 (spindle on at 700 rpm)
    N40 G4 P257 (dwell for that time... why?)
    N45 M8 (coolant on)
    N50 G0 E1 X0.3101 Y-0.1218 (move table to bring part under spindle)
    N55 G43 Z1.2595 H14 (offset length of tool 14?)
    N60 Z0.8595 (z axis move to start location for feeding)
    N65 G1 Z0.1871 F0.7 (moving at feed rate of .007 per revolution to specified location?)
    N70 G4 P5000 (dwell for specified time -why?)
    N75 M5 (stop spindle)
    N80 G0 Z0.8595 (rapid home?)
    N85 M3 (spindle on again - why?)
    N90 Z1.2595

    N95 M9 (coolant off)
    N100 G28 G91 Z0. (does this index spindle to zero or is that next line?)
    N105 G90
    N110 G53 X0. Y0. (return table home)
    N115 M30 (end)

    As you can see I am far from a G-code genius. Using Solidworks 2017 with HSMworks2020 for CAM. Any help would be appreciated!
    Last edited by Tatertots; 05-11-2021 at 08:49 PM. Reason: clarity

  2. #2
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,313
    Post Thanks / Like
    Likes (Given)
    13568
    Likes (Received)
    5141

    Default

    Just to be specific... Which holder are you using, from which manufacturer, for an indexed rotary broach?

  3. #3
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,313
    Post Thanks / Like
    Likes (Given)
    13568
    Likes (Received)
    5141

    Default

    To be clear, I've never touched a Fadal, or even seen one in real life. But a lot of this is generic, so I'll answer what I can.

    Quote Originally Posted by Tatertots View Post

    O0075 (TEST BROACH)
    (T14 D=0.375 CR=0. - ZMIN=0.1871 - FORM MILL)
    N10 G90 G94 G17 ABSOLUTE POSITIONING, IPM FEED (SEE YOUR LINE N65... FEED IS .7IPM, NOT .007 PER REV), X/Y PLANE SELECTION
    N15 G20 CHECK FOR INCH PARAMETER SETTING...
    N20 G28 G91 Z0.ZERO RETURN, INCREMENTAL POSITIONING
    N25 G90 BACK TO ABSOLUTE POSITIONING

    (DRILL2)
    N30 T14 M6 (change to tool 14)
    N35 S700 M3 (spindle on at 700 rpm)THIS IS WHAT YOU MOVE TO TURN THE SPINDLE ON LATER, YES
    N40 G4 P257 (dwell for that time... why?)TO MAKE SURE THE SPINDLE REACHES THE COMMANDED SPEED, PROBABLY
    N45 M8 (coolant on)
    N50 G0 E1 X0.3101 Y-0.1218 (move table to bring part under spindle)
    N55 G43 Z1.2595 H14 (offset length of tool 14?)MOVE TO THE Z POSITION 1.2595 WHILE APPLYING TOOL HEIGH OFFSET 14
    N60 Z0.8595 (z axis move to start location for feeding)
    N65 G1 Z0.1871 F0.7 (moving at feed rate of .007 per revolution to specified location?)SEE ABOVE, THIS IS MOVING AT .7IPM NOT .007 PER REV
    N70 G4 P5000 (dwell for specified time -why?)WHY NOT?
    N75 M5 (stop spindle)
    N80 G0 Z0.8595 (rapid home?)RAPID BACK TO THE START OF THE HOLE, NOT HOME
    N85 M3 (spindle on again - why?)YOU'D HAVE TO TALK TO WHOEVER WROTE YOUR POST IS WHY
    N90 Z1.2595BACK TO THE CLEARANCE POSITION

    N95 M9 (coolant off)
    N100 G28 G91 Z0. (does this index spindle to zero or is that next line?)THERE IS NO SPINDLE INDEX TO ZERO ANYWHERE IN THIS CODE
    N105 G90
    N110 G53 X0. Y0. (return table home)
    N115 M30 (end)


    Did my best to answer above. But this comes down to my first question. What holder are you using to index?

    For most machines, and google says for a Fadal, too, M19 will orient the spindle, this is essentially your C0, it's what's used in a tool change. On some machines you can call M19 with a specified angle, and orient at 1° (or smaller) increments from the 0 position. But not all machines. And I'd bet not on a Fadal, as they're (apologies) budget machines. I could be wrong, they do have an encoder (at least, some of them do. Can your machine rigid tap?).

    If you're using something like this: Rotary Broaching Brake - Polygon Solutions

    You don't need to orient the spindle. It'll be oriented during the tool change, and the brake on the holder will ensure that the broach is oriented the same as it was after the last part, as long as you don't turn your spindle on until AFTER the broach engages the work piece.

    If you're not using something like that, then I need clarification on what type of holder you're using.

  4. #4
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,661
    Post Thanks / Like
    Likes (Given)
    16369
    Likes (Received)
    11766

    Default

    M19 is spindle orient. You can only orient in one spot, and that
    is the same one that is used for a tool change. Its a little roller
    on a spring that just goes into a detent, activated by an air cylinder.

  5. #5
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    1

    Default

    Thanks for the help. Yes this machine has an encoder and will rigid tap. It is exactly the polygon heavy duty broaching holder with their brake. I will have to run some tests, but it appears on stop command the spindle ramps down rpm and stops at a random location. When tool change is called it indexes to the C0 and changes tools. I should be able to find and confirm the M19 on one of my other multiple tool processes. It looks like I would have to stop spindle and return to C0 before exiting work piece to maintain indexing - which should hold through subsequent cycles as you indicated.

    I have been manual machining for decades, and this machine was given to me so I can't complain (much). The biggest problem I have with it thus far is CAM will occasionally come up with canned cycles it can't use. It has been a great teacher as I always learn more doing something the hard way. I always run a test cut at low feed and minimum rapid - if in doubt I use florist's foam blocks to simulate stock for the first full speed trial and have saved a bit or two with it.

  6. #6
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,486
    Post Thanks / Like
    Likes (Given)
    1059
    Likes (Received)
    2392

    Default

    Quote Originally Posted by Tatertots View Post
    Thanks for the help. Yes this machine has an encoder and will rigid tap. It is exactly the polygon heavy duty broaching holder with their brake. I will have to run some tests, but it appears on stop command the spindle ramps down rpm and stops at a random location. When tool change is called it indexes to the C0 and changes tools. I should be able to find and confirm the M19 on one of my other multiple tool processes. It looks like I would have to stop spindle and return to C0 before exiting work piece to maintain indexing - which should hold through subsequent cycles as you indicated.

    I have been manual machining for decades, and this machine was given to me so I can't complain (much). The biggest problem I have with it thus far is CAM will occasionally come up with canned cycles it can't use. It has been a great teacher as I always learn more doing something the hard way. I always run a test cut at low feed and minimum rapid - if in doubt I use florist's foam blocks to simulate stock for the first full speed trial and have saved a bit or two with it.
    Which CAM? And where did you get the post? Also, which Format are you in?

  7. #7
    Join Date
    Feb 2009
    Location
    Midwestern MN/Wi USA
    Posts
    1,414
    Post Thanks / Like
    Likes (Given)
    74
    Likes (Received)
    406

    Default

    I do not think you can accurately or even broach with a fadal. You may have a different experience with Dave jrs Nxgen control.

  8. #8
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,661
    Post Thanks / Like
    Likes (Given)
    16369
    Likes (Received)
    11766

    Default

    Quote Originally Posted by Speedie View Post
    I do not think you can accurately or even broach with a fadal. You may have a different experience with Dave jrs Nxgen control.
    Yeah you can... I did have to make a bracket to lock down the spindle, the spindle lock just
    wasn't quite enough. I was broaching sideways, and I don't even think it was technically
    broaching, it was more like shaping. 3D contour shaping to make an involute. The set up,
    and the finished product, 2 different splines, one on each end. That job sucked. It
    was one of those where I can say "Hey Look What I Did!!"... I can do that... Don't
    want to do it again.






  9. Likes Mud, mmurray70 liked this post
  10. #9
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    1

    Default

    I use Solidworks 2017 with HSMWorks 2020. I find some of the drill canned programs to be routinely ignored. For example a partial retract just bores right through without any pecking at all. I believe I am using the post for generic fadal that comes with the CAM, but to be honest my son helped me set this one up and it could have been sources elsewhere. Thanks!

  11. #10
    Join Date
    Feb 2018
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    25
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    1

    Default

    Thats a fine looking part... that I don't want to have to make )


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
  •