Results 1 to 8 of 8

Thread: TM2P Tapping Problems

  1. #1
    Registered
    Join Date
    Oct 2006
    Location
    USA
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default TM2P Tapping Problems

    I've had some success with rigid tapping, mainly through the menu on the mill itself. I still have not been able to tap as reliably as I would like without breaking taps.

    So to start off I have some questions about what everyone is using.

    What type of taps. We order from Mcmaster so if you have a type they carry even better. Also what speeds and feeds are you running them. I know our machine is correctly setup for rigid tapping because I walked through it with the HAAS rep on the phone and then when another rep was here in person had him verify this.

    Also we use featureCAM as our cam software package and I wanted to know if there were any specific settings other than turning on rigid tapping that you used in this. There is a choice between auto feed/speed calculating and overiding to a certain speed.


    Anyways I'd love to get everyone's feedback. I'm always trying to increase my machining knowledge and nobody knows better than those with experience.

    In particular i'm tapping holes in the 2-56 to 8-32 range so nothing large. My best success has been with spiral taps and by squirting a little thread cutting oil into the holes prior to the actual tapping to provide some extra lubrication.

    Similar Threads:


  2. #2
    Registered Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1433
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by stevovee View Post
    I've had some success with rigid tapping, mainly through the menu on the mill itself. I still have not been able to tap as reliably as I would like without breaking taps.

    So to start off I have some questions about what everyone is using.

    What type of taps. We order from Mcmaster so if you have a type they carry even better. Also what speeds and feeds are you running them. I know our machine is correctly setup for rigid tapping because I walked through it with the HAAS rep on the phone and then when another rep was here in person had him verify this.

    Also we use featureCAM as our cam software package and I wanted to know if there were any specific settings other than turning on rigid tapping that you used in this. There is a choice between auto feed/speed calculating and overiding to a certain speed.


    Anyways I'd love to get everyone's feedback. I'm always trying to increase my machining knowledge and nobody knows better than those with experience.

    In particular i'm tapping holes in the 2-56 to 8-32 range so nothing large. My best success has been with spiral taps and by squirting a little thread cutting oil into the holes prior to the actual tapping to provide some extra lubrication.
    I am not familiar with FeatureCam, so someone else will have to assist you with that.

    To be honest, if I were to start over buying taps at this point, I would probably buy more form taps than cutting taps. They are so much stronger and work in almost all materials.

    For most holes in run of the mill work, not production, I usually run at 1000 rpm and that works well. Avoid going too slow, as this puts more stress on the tap.

    If you use a cutting tap, remember to drill deeper than you will tap, as you will need room for chips to build up. Taps that bring to chips up rather than down are good, but can be a weaker tap.

    Good taps last long than cheap taps!

    Mike

    Haas VF-2, HA5C, Hardinge CHNC 1, BobCAD V23


  3. #3
    Registered
    Join Date
    May 2004
    Location
    United States
    Posts
    4519
    Downloads
    0
    Uploads
    0

    Default

    Tapping is not a matter of just CNC programming. You have to get a lot of factors right to be consistently successful in tapping. The first is obtaining the correct hole size prior to tapping. This correct hole size will be different for different types of materials. You did not mention any material types. The next factor is what is the required final use/tolerance for the thread. Contrary to common knowledge, many times in general machining a 55% complete thread is acceptable. Most drill tap charts give drill sizes for 75% complete threads for cutting taps. Once you have determined you are achieving the needed pre-tap hole size, then you can dial in your RPM. (Feed rate for tapping is always based on RPM and thread pitch.) Machinery's Handbook and other sources can give a recommendation for a starting point for surface speed (RPM) for tapping. Remember, this is only a recommendation. The RPM you actually end up using will be based on what works best for your machine and part.



  4. #4
    Registered
    Join Date
    Oct 2006
    Location
    USA
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default material

    Pretty much entirely using 6061-T6 AL and I pretty much always use a 50% thread, most of our parts have very little force on them, just holding circuit boards etc



  5. #5
    Registered Machineit's Avatar
    Join Date
    Mar 2010
    Location
    USA
    Posts
    1433
    Downloads
    0
    Uploads
    0

    Default

    Txcncman made me think of one other thing that most don't know. He mentioned the 75% full thread that almost all drill and tap charts give you. But, what they don't tell you is that as the material thickens so does the size of the hole increase and still be a valid 75% threaded hole. Check your Machinery Handbook.

    For example, a 1/4-20 always calls for a .201 drill for the 75% thread. I don't have my charts here, but at 3 times the tap size (.75 thick for a 1/4-20) you can use about .207 drill for that same 75% thread. Believe you me,the change in size is everything to that tap. Much less breakage.

    The place I used to work was always breaking taps in the stainless they tapped. When I made up charts with the increased hole sizes, that pretty much eliminated the problem.

    Mike

    Haas VF-2, HA5C, Hardinge CHNC 1, BobCAD V23


  6. #6
    Registered
    Join Date
    Oct 2006
    Location
    USA
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default

    I almost always use the 50% column in this chart Tap Drill Chart



  7. #7
    Registered KenFoulks's Avatar
    Join Date
    Aug 2010
    Location
    USA
    Posts
    573
    Downloads
    0
    Uploads
    0

    Default Haas Factory Support

    1. Where is the tap breaking, going in or retract?
    2. What coolant/concentration are you using?
    3. How deep are the drill holes?
    4. How deep are you tapping?
    5. What RPM/Feed are you using?
    6. Which tap do you break more often?
    7. What is setting 130 set to? (Should be 1)
    8. How thick is your material?
    9. Before you tap, are there any chips in the holes?
    10. Have you checked the holes with a thread gage?

    As Machineit stated, form taps have been very successful, especially in taps this size.

    Your machines max spindle RPM is too low to achieve the optimum 635 SFM that is recommended for tapping aluminum, but here are some recommendations for 1xD tapped holes:

    Tap style: Spiral Fluted Tap with a 6-20 degree rake angle
    Coolant: High quality with a high concentration (high end of recommended concentration)
    2-56: Drill=.0737, 5992 RPM, 107 IPM
    8-32: Drill=.139, 5984 RPM, 187 IPM

    Thanks,
    Ken Foulks


  8. #8
    Registered
    Join Date
    Oct 2003
    Location
    USA
    Posts
    527
    Downloads
    0
    Uploads
    0

    Default

    I tap a lot of holes in 6061. If the hole is a through hole use a spiral point tap they push the chips in front of the tap. If your tapping blind holes use a spiral flute tap they bring the chips out of the hole, but they are weaker and chips build up in the flutes and sometimes the chips need to be removed by hand. For your thread sizes if they are blind holes a form tap would be best. Form taps will only work right with one size hole. Once you figure out the size that works stick with it. OSG form taps work great for us. For cut taps I have a chart from morse that lists 75, 70, and 60% IIRC. For thin materials I always use 75. For deeper holes or tougher material I'll use 70 or 60 percent. If I break a tap I usually look at the drill too. Sometimes it will be dull and not cutting the right size hole.

    Also look at the parameter for retract speed sometimes the machines can retract a tap faster than it went in. On smaller taps retracting at twice the tapping speed can break taps.

    Coolant plays a part in tap life too. I use a soluable oil coolant and run between 8-10% mix. If your running less than 8% or your using semi synthetic or full synthetic you might have problems.



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 from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed