Soft tapping and Fusion 360

Results 1 to 9 of 9

Thread: Soft tapping and Fusion 360

  1. #1
    Registered
    Join Date
    Dec 2017
    Location
    United States
    Posts
    45
    Downloads
    0
    Uploads
    0

    Default 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.

    Similar Threads:


  2. #2
    Registered
    Join Date
    Mar 2017
    Location
    United States
    Posts
    34
    Downloads
    0
    Uploads
    0

    Default Re: Soft tapping and Fusion 360

    Why not thread mill it?

    Sent from my SM-N960U using Tapatalk



  3. #3
    Registered
    Join Date
    Dec 2017
    Location
    United States
    Posts
    45
    Downloads
    0
    Uploads
    0

    Default 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
    Registered
    Join Date
    Mar 2017
    Location
    United States
    Posts
    34
    Downloads
    0
    Uploads
    0

    Default 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
    Registered
    Join Date
    Dec 2017
    Location
    United States
    Posts
    45
    Downloads
    0
    Uploads
    0

    Default 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
    Registered
    Join Date
    Mar 2017
    Location
    United States
    Posts
    34
    Downloads
    0
    Uploads
    0

    Default 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
    Registered
    Join Date
    Dec 2017
    Location
    United States
    Posts
    45
    Downloads
    0
    Uploads
    0

    Default Re: Soft tapping and Fusion 360

    Excellent, I will order a couple now.



  8. #8
    Registered
    Join Date
    Jun 2007
    Location
    USA
    Posts
    92
    Downloads
    0
    Uploads
    0

    Default 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
    Registered
    Join Date
    Jul 2010
    Location
    USA
    Posts
    467
    Downloads
    0
    Uploads
    0

    Default 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



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

Soft tapping and Fusion 360

Soft tapping and Fusion 360