Acme threading, Mazak T32
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 37
  1. #1
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default Acme threading, Mazak T32

    Had a job walk in today that I need a little assistance with.

    It's a stepped shaft with opposing threads, much like you'd find in a self-centering vise. 1.75-4LH acme and 1.375-4RH acme, then some bother basic features. Material is 4140ph. I only have one to do, but I'm going to try to sell them two units because they have two identical machines and the other unit has worn the acme profile into a buttress thread.

    Question 1- what tools do you suggest? Tempted to use a ground HSS tool. My threading experience is limited to 16ir/er. How about a top notch style?

    Question 2a- how well does Mazatrol handle acme?

    Question 2b- any other tips?

    Or just do them on the Monarch manual? It'll be faster and easier, but I won't learn anything....

  2. #2
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default

    In my very limited experience I donít think you will have a problem justa program it correctly with the proper thread angle if you are doing it in mazatrol.

    Increase the number of passes also. If you are doing a coarse acme you may have issues

    I think you could get away with the hss but just run it like 60-80sfm so you donít burn the tool right up. Iím also pretty sure they make acme inserts for your lay down tools but I know they only go so large. I have no clue what size acme you need to cut and in my experience the larger the pitch the more difficult.

    Iíd be surprised if you could do it quicker on a manual.

  3. #3
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Kennametal has (somewhat) reasonably priced inserts and holders for the #3 Top Notch system, I think this is the way to go.

    Programmed via Mazatrol

  4. #4
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default

    Quote Originally Posted by Cole2534 View Post
    Kennametal has (somewhat) reasonably priced inserts and holders for the #3 Top Notch system, I think this is the way to go.

    Programmed via Mazatrol
    I was going to say top notch but didnít figure there was budget for new tools. I did start using the top notch stuff till recently and Iím finding that I like that style. Was soundly well for me with grooving

  5. #5
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Holder is about $120, inserts are about $20/ea, so I think can do this for $250.

    I'm kinda lost on the holder options though. Need 1in, right hand #3. Should be simple, but there are many many choices.

    As far as inserts, got a grade you like? Thinking KC5010 for this work.

  6. #6
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default

    Here is the tool holder code from Kenna and from toolflo

    Also I most recently in 4140 I was using a tool Flo insert and grade was ac3 which is equivalent to kc5010



  7. Likes Cole2534 liked this post
  8. #7
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Ordered up that same holder and a couple 4tpi inserts.

    I've never played with Top Notch stuff, it seems like a very versatile system.

    Programmed via Mazatrol

  9. #8
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    This is kicking my ass. The machine is being goofy, but that's likely an error in my program.

    What I don't understand is what's happening to my thread, it's like the tool is shifting in Z mid-way through.

    I cut a test thread, dialed in my pitch diameter then tried on the actual shaft. Same material, 4140ph, same insert, speed, etc. The threaded section is 7" long but length between chuck and center is 11".

    For thread angle Im using 29deg, height is .125" unknown pass count because the control won't display it.

    Ideas?

    Programmed via Mazatrol

  10. #9
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default Acme threading, Mazak T32

    Show me a picture of your program.

    Also Iíll try to see if I can program it for you but it will probably be a couple days as I wonít have any time till Thursday.

    Send me a picture of your tool holder and holder in the machine aswell etc

    Gotta also make sure your tailstock is not pushing the part on with the extra cutting force. Use a backstop or raise up that chucking pressure

  11. Likes Cole2534 liked this post
  12. #10
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Tool was minty at the beginning of the program.

    Programmed via Mazatrol

  13. #11
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default

    Can you take a picture of your tool data page for the threading tool?

    Just to make sure your tool is described properly


  14. #12
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Here ya go

    Programmed via Mazatrol

  15. #13
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default Acme threading, Mazak T32

    Well sorry canít remember too much on a Tplus didnít realize there was no angle setting in the tool data on those older machines. Everything there looks good.

    Did you check to see if the part is shifting?

    Also remember I mentioned chatter was going to be an issue.

    Try changing the threading cycle to the highlighted 0. And make a large amount of passes.

    Also hard to tell as the picture is blurry but that tool looks trashed.

    The 200 for sfm seems a bit high Iíd try slower to avoid chatter

  16. #14
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    The tool is definitely trashed, I think the chatter got it. I ran it at 200sfm and the same inputs for a test piece. After comping for PD the thread was excellent, it wired within a thou.

    But... I may have bit off more than I can chew on this job. It's the first time Ive- used the tail stock, used the 3j chuck, max'd the machine's length, and done acme thds. Bringing all that together has been a little bit challenging.

    Worst case scenario I'll cut the shafts on the ole Monarch.

    Programmed via Mazatrol

  17. #15
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default

    No reason you canít use a hss tool on the Mazak either.

    Try the highlighted 0 option with lots of passes and make sure the parts is not slipping and give it another shot.

    Personally Iíd slow the sfm down but the carbide may like the faster sfm. Is it 4140? Is the material hardened at all? I remember I was having some chatter issues with grooving and had to slow the sfm down a bit to get a good looking groove. That part had a pretty good surface finish requirement

  18. #16
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Ya, it's 4140ph. I'll drop the SFM and see what happens.

    Programmed via Mazatrol

  19. #17
    Join Date
    Jun 2018
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    214
    Post Thanks / Like
    Likes (Given)
    93
    Likes (Received)
    62

    Default

    So years ago we cut some much larger than these ACME threads on our Mazak. I can't remember exactly, but they we're at least 6" O.D. but shorter than your part. Used the same Kenna tooling you have but larger. Long story short chatter was an Issue because of the width of the tool. There was allot of tool engaged with the part and it didnt like that. What we ended up doing was taking a grooving/parting tool and running it down the center of the thread to the root dia. Then the threading bit just had to clean up the two sides. So if you have a grooving/parting tool just skinnier then the root width of your thread you might give that a try.

  20. Likes BT Fabrication liked this post
  21. #18
    Join Date
    Nov 2005
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    1,599
    Post Thanks / Like
    Likes (Given)
    19
    Likes (Received)
    204

    Default

    Quote Originally Posted by Cole2534 View Post
    Ya, it's 4140ph. I'll drop the SFM and see what happens.

    Programmed via Mazatrol
    I'd actually do the opposite...

    KC5010 is a hard subtrate PVD coated insert. It needs a bit of heat to perform and prevent chipping. For KC5010 in 4140 in the mid 30's RC I'd be running a minimum of 230 SFM, but should be able to do ok up to about 500. Heat will help the chip flow better. But no amount of feeds and speeds will solve a rigidity issue in the setup.

    Two things about the application you are doing.

    1) When you cut your test piece it worked out, correct? Likely you had a short part in the chuck, with no rigidity issues...

    2) You transferred over to the long part and now you have issues. This is because of tool pressure. No way around it with standard threading cycles so to speak. You have an .087 wide tool and as you get deeper the amount of tool engaged is .087" + the depth into the thread divided by the cosine of 14.5 degrees. So no less than a .087 depth of cut worth of tool pressure, but as you get to the depth of the thread, you are now talking almost a .quarter of an inch of tool engagement with the part assuming you are only cutting on the front edge of the insert, which if chattering is not the case....... That is a shit-ton of tool pressure.

    So anyway, you have learned your machine is rigid enough, but the part isn't right? How do we fix this you say?

    Two things:
    1) Switch to KCU25 or KC5025 grade. These are a bit softer and will handle the deflection and lack of rigidity better. You are still going to want to be running somewhere 230-350 SFM.

    2) You need to get creative on how you program this in order to minimize the amount of cutting edge engaging the part at a time. You can try a zig-zag/alternating flank cycle, not sure if you can do that on a Mazatrol, but my experience is it will still create too much tool pressure with an Acme due to the width of the land on the end of the insert. What you need to do is manually calculate out all of the thread starts and end points, for each diameter of depth of cut to go down the center, then front flank, then rear flank, repeat for each depth. You should be able to take about .010" to .015" per depth, but any more than that will likely get a bit greedy. As you calculate these, I would leave about .002-.003 on each flank for finishing, and before you get to the bottom you will want to flank the front and back at finish dimension, cheating off the bottom by about .005"-.010" this allows you to cut only with the flanks of the tool, with no end pressure, then take two final passes down the middle to final depth, leaving about .002" for the last pass, cheating the minor diameter a little if you can, but understand you will need to cut the flanks again to "dig out" the corners.

    If it still chatters while doing this:

    1) You can use a 5 pitch insert, but you may need to grind a little relief in it to get the depth. But it will have less tool pressure as the end is only .0689" wide or 20% or so less.
    2) You can use a narrow grooving tool and pick out the thread bit by bit, then surface the thread using the radiused corners of the inserts. Very time consuming, very tedious, but will get it done guaranteed. I have a friend who has done this before on a manual lathe..... When you look at the thread you would never know that's how he did it. I think that was a 4" - 2 pitch ACME thread for a mobile track pin press, might even have been a larger pitch than that.


    Best of luck. There is rarely an easy button when it comes to acme threading in the large pitch arena.

  22. Likes Cole2534 liked this post
  23. #19
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    5,877
    Post Thanks / Like
    Likes (Given)
    1184
    Likes (Received)
    2619

    Default

    Thank you for those tips, I'll try a few today.

    I do have 1 other option- switch material. They don't care what material I use, it just needs to be strong. As a matter of course, this means 4140ph to me. However, Fatigueproof may be the answer. I'll sacrifice some YTS, and some elongation, but its much easier to cut.

    The application is the leadscrew for a self centering vise. Customer is a rigging house, this vise grips the cables ends while the push on the ferrule prior to swaging. I'll see if I can snag a pic or 2.

    Programmed via Mazatrol

  24. #20
    Join Date
    Sep 2014
    Country
    UNITED STATES
    State/Province
    Georgia
    Posts
    1,163
    Post Thanks / Like
    Likes (Given)
    13
    Likes (Received)
    305

    Default Acme threading, Mazak T32

    Btw the poster above that mentioned the zig zag cycle thatís what the highlighted 0 is in mazatrol.

    Well the highlighted options are all different types of zig zag cycles

    Also in my part decreasing the sfm made the chatter go away but I think the other poster is correct about faster speeds being better for the carbide.


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
  •