584,850 active members*
4,428 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Milltronics > Soft tapping and Fusion 360
Page 1 of 2 12
Results 1 to 20 of 21
  1. #1
    Join Date
    Dec 2017
    Posts
    72

    Soft tapping and Fusion 360

    Anyone using the soft tap feature on a cent 5 (vm16) through fusion? I'm finding more and more need to drill/tap holes on mine.

    Do I just call for a tapped hole in the drill menu of fusion? Or is there a set of steps I must perform other than selecting a speed that the control and spindle agree is the same rpm.

    On a side note to this question, anyone ever soft tapped 1/2npt into 304 stainless? My current project calls for the end of a piece of 1.25" stainless to be drilled and tapped at one end with 1/2npt. It would be nice if I could let the cnc take care of the tapping as long as it's in there for other operations.

  2. #2
    Join Date
    Mar 2017
    Posts
    63

    Re: Soft tapping and Fusion 360

    Why not thread mill it?

    Sent from my SM-N960U using Tapatalk

  3. #3
    Join Date
    Dec 2017
    Posts
    72

    Re: Soft tapping and Fusion 360

    simply because I have a few of the taps on hand and am not sure about how to select the proper thread milling cutter. I like the idea of thread milling a lot, I just dont want to end up with an expensive cutter that I never use because its some weird version.

  4. #4
    Join Date
    Mar 2017
    Posts
    63

    Re: Soft tapping and Fusion 360

    single pitch thread mills can do all different thread pitches, this 1/2 inch thread mill can do 12-32 tpi. You can do 1/2-13, 1/2-20, 1/2-28, and 1/2 npt, with the same tool. 1/2" 12-32 TPI

  5. #5
    Join Date
    Dec 2017
    Posts
    72

    Re: Soft tapping and Fusion 360

    Hmmm, those are far more acceptable in price. Cheap enough to buy a second one for when I break the first due to a stupid mistake. Have you ever purchased from that supplier?

  6. #6
    Join Date
    Mar 2017
    Posts
    63

    Re: Soft tapping and Fusion 360

    All the time. I was eating 5/16 em in 304ss, and switche to one of their variable helix 5/16 with a corner rad, and finished the other half of the run with one end mill. I have used their 3/8 thread mill several times with great results. i will say that the code generated by bobcad for the thread mill is huge, and my cent 5 control couldnt process it very fast, but the code generated conversationally is only a few lines, and easier to edit at the machine. you might want to use a sub program to do your threads.

  7. #7
    Join Date
    Dec 2017
    Posts
    72

    Re: Soft tapping and Fusion 360

    Excellent, I will order a couple now.

  8. #8
    Join Date
    Jun 2007
    Posts
    98

    Re: Soft tapping and Fusion 360

    I tap with the soft tap feature built into the drill routine .
    We had to adjust the VFD values to get the RPM to match what the screen says , compared to a strobe light that is made to read actual RPM.
    Then we experimented by tapping soft plastic and observing what it does . You can also set up a piece of metal strapping that has one edge ground like a knife edge . clamp this down and engage the tap flute , and tap in air. then you can see if it is feeding , dwelling and feeding up , while observing what the metal strip is doing . You will never get it to synch perfect on soft tap . I bought an ER 25 tap collet from Technics .
    They have a spring loaded inner part that will pull out ( but will not compress in )
    So as long as the feed (lead ?)is a bit faster , the collet will compensate for a mis match in feed .
    I have tapped 1000's of 8-32 holes in alum with no problems . Just keep in mind that once you get an rpm /feed that works , don't go messing with a good thing by upping the rpm.

  9. #9
    Join Date
    Jul 2010
    Posts
    548

    Re: Soft tapping and Fusion 360

    Hi Tippman. the Milltronics uses G84 for soft tap. and G88 for ridged tap. Which is different then everybody else. (G84 is ridged tap for most) Why? because way back when, R Tap was VERY expensive $10K +. So, Milltronics cam up with an algorithm to make a "soft" tap cycle. but kept the same G code ( G84) The problem with "soft tap" is that it is based on 220VAC. if you run 208V it runs slow. if you run 230V it runs fast. The way around it is to adjust the spindle drive " MAX spindle frequency" parameter to read "right on" t the speed you want to tap at. IE: 100 RPM. that way it is correct speed for tapping, The down side is that you will be off at higher RPM's. so 6K might only "tach" out at 5950. ( be off 10RPM in a tap and you WILL be unhappy, be off 50RPM at 6K and you won't notice.

    Refer to G84 and G88 in the G code section of the manual. The "call outs" are different.

    Sportybob

  10. #10
    Join Date
    Aug 2013
    Posts
    35

    Re: Soft tapping and Fusion 360

    Yeah. G88 took me a while to figure out. Now if only I could modify the Fusion 360 post processor so I don't have to modify the G-code by hand to make it work. They have G84 for rigid tapping, and the Z feed rate is wrong.

    Rigid tapping is really, REALLY sweet though!

  11. #11
    Join Date
    Dec 2017
    Posts
    72

    Re: Soft tapping and Fusion 360

    So after ordering some threadmills to play with, I like that method. I have milled 1/2-13, 1/2-14NPT, then found an m3 version in a box at work that I tried successfully.

    I wont be trying soft tapping after Bob's information that voltage differences will throw it off. Tuning a matched speed is easy, but the house panel that supplies power to the garage also powers the 25kw resistive furnace. When that comes on I loose 10-20v.

  12. #12
    Join Date
    Jul 2006
    Posts
    130
    Quote Originally Posted by wfr8577 View Post
    Yeah. G88 took me a while to figure out. Now if only I could modify the Fusion 360 post processor so I don't have to modify the G-code by hand to make it work. They have G84 for rigid tapping, and the Z feed rate is wrong.

    Rigid tapping is really, REALLY sweet though!

    Can you show me the current output and the one you want?

    I'm going to play with rigid soon and can modify the post

  13. #13
    Join Date
    Aug 2013
    Posts
    35

    Re: Soft tapping and Fusion 360

    Hey! Thanks for your interest. Milltronics requires G88 instead of G84 for rigid tapping. I figured out where to change that.

    However, I can't get the feed rate right. G88 needs thread pitch as it's Z feed rate. So, for a 40 TPI tap it needs F=.025

    Currently, the post multiplies thread pitch * spindle speed. So it outputs Z feed at 12.5 instead of .025. I have changed the feed rate by hand and it worked great. I just can't get the post to do it for me.

    Also, I'd like to use G53 instead of G28 at the end of the post, ,but I think I can figure that out when I get some time.

    Here is a simple two hole tap post.

    O1015 (DRILL AND RIGID TAP TEST)
    (T21 D=0.115 CR=0 - ZMIN=-0.225 - RIGHT HAND TAP)
    N1 G90 G94 G17
    N2 G20
    N3 G32
    (RIGID TAP)
    N4 M9
    N5 T21 M6
    (4-40 TAP)
    N6 S500 M3
    N7 G56
    N8 M7
    N9 G0 X-0.25 Y0.3625
    N10 G43 Z0.6 H21
    N11 G0 Z0.2
    N12 M29 S500
    N13 G98 G84 X-0.25 Y0.3625 Z-0.225 R0.1 P0 F12.5 (This needs to be .025)
    N14 X-0.5
    N15 X-0.75
    N16 X-1
    N17 X-1.25
    N18 G80
    N19 Z0.6
    N20 M9
    N21 G32
    N22 G28 G91 X0 Y0
    N23 G90
    N24 M30

  14. #14
    Join Date
    Jul 2006
    Posts
    130

    Re: Soft tapping and Fusion 360

    Try this. It only works for explicit Right Tap and you have to have Use Rigid Tapping set to yes in the options when posting.

    If this works 100% I can fix Tapping and possibly left hand (what code is that?)

  15. #15
    Join Date
    Aug 2013
    Posts
    35

    Re: Soft tapping and Fusion 360

    Thank you so much!

    I just tried it. It gave a feed value of 0.3

    It rounded up?

  16. #16
    Join Date
    Jul 2006
    Posts
    130
    Quote Originally Posted by wfr8577 View Post
    Thank you so much!

    I just tried it. It gave a feed value of 0.3

    It rounded up?
    Oh I may have to make a new format for 3 decimals. Not hard it's just one line. my simple tests worked but I don't test the larger thread counts. (6mmx1 and 1/4-20)

  17. #17
    Join Date
    Jul 2006
    Posts
    130
    Quote Originally Posted by yugami View Post
    Oh I may have to make a new format for 3 decimals. Not hard it's just one line. my simple tests worked but I don't test the larger thread counts. (6mmx1 and 1/4-20)
    Change secFormat to xyzFormat. I'll update tomorrow

  18. #18
    Join Date
    Dec 2008
    Posts
    3110
    Quote Originally Posted by wfr8577 View Post

    Currently, the post multiplies thread pitch * spindle speed. So it outputs Z feed at 12.5 instead of .025. I have changed the feed rate by hand and it worked great. I just can't get the post to do it
    F12.5 is correct feedrate for 40TPI@S500
    but it needs to be set in feed per min(G99) instead of feed per rev(G98)..... might be easier to change in the post

    The only downside is if you edit RPM in the nc file.... you will need to re-calculate the feed rate.

  19. #19
    Join Date
    Aug 2013
    Posts
    35

    Re: Soft tapping and Fusion 360

    Milltronics uses G88 for rigid tapping. It kicks a fault with F = 12.5 saying something like "feed rate out of range". F = 12.5 would be correct for G84, which most mills use to rigid tap.

    F = .025 is correct for 40 TPI on my mill. I've tapped holes with it after hand editing the gcode.

  20. #20
    Join Date
    Aug 2013
    Posts
    35

    Re: Soft tapping and Fusion 360

    Bingo!!!

    N13 G98 G88 X-0.25 Y0.3625 Z-0.225 R0.1 P0 F0.025

    Thanks!

Page 1 of 2 12

Similar Threads

  1. Modifying the Post Processor for tapping - Fusion
    By RA-Bowtie in forum Tormach Personal CNC Mill
    Replies: 1
    Last Post: 03-01-2018, 02:06 AM
  2. Any interest in SL15 3 Jaw Chuck Soft Jaw Fusion 360 Model and CAM?
    By David Bord in forum Tormach Slant Lathe
    Replies: 4
    Last Post: 07-01-2016, 12:22 AM
  3. Free soft from CAD up to CAM soft
    By Laurent_parti in forum Uncategorised CAM Discussion
    Replies: 0
    Last Post: 05-15-2013, 04:19 PM
  4. tapping head vs hand/cordless tapping machine....
    By InspirationTool in forum Uncategorised MetalWorking Machines
    Replies: 6
    Last Post: 09-13-2005, 02:10 AM

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
  •