Interpolate all holes and thread mill all threads?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 22
  1. #1
    Join Date
    Mar 2009
    Location
    Valencia, CA, USA
    Posts
    391
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    59

    Default Interpolate all holes and thread mill all threads?

    Just got an email from Protolabs that led to this link:

    Design Tip: 6 ways to optimize part design for CNC machining

    I wonder what your opinion might be on the question of not drilling, but rather interpolating every single hole and avoiding taps in favor of thread milling.

    My first reaction was that cycle time and machine wear and tear would be increased. And then I realized this is Protolabs, a high volume operation. If this works for them, why wouldn't it work for everyone else?

    One of the other questions that popped into my head was: Do they also plunge entry into every hole they interpolate or do something else (spiral, etc.)?

    I can't see that thread milling for standard thread sizes can possibly compete with the cycle time of rigid tapping. Yes, you'd have to load the appropriate tool, etc. Maybe they've optimized their workflow so that a standard set of tools in the tool changer can handle 90% of what they get and they reserve, say, 5 tool positions for exceptions?

    We are not a production shop but it would sure be nice to simplify our prototype manufacturing to avoid having to setup a bunch of tools for every job. We have that to some extent but we still use drills and form taps. Our standard tool set looks something like this:

    VF2 with 20 position umbrella tool changer.

    01 2 in diameter carbide insert shell mill
    02 1/2 in 90 degree spot drill
    03 Drill chuck
    04 Drill chuck
    05 Tap
    06 Tap
    07 1/8 in carbide end mill
    08 3/8 in carbide end mill
    09 1/2 in carbide end mill
    10 3/4 in 4 inch long carbide end mill
    11 #3 82 degree center drill
    12 #6 82 degree center drill
    13 1/4 in carbide ball end mill
    14 3/8 in carbide ball end mill
    15 Engraver
    16 Open
    17 Open
    18 Open
    19 Open
    20 Renishaw Probe

    I tend to use the same tools (always the largest possible) for roughing and finishing. Again, not a production shop so dedicated roughers don't seem to make sense. I have a couple of 1/2 in roughers but never seem to use them. I'd be interested in opinion on whether or not this is a good approach.

    Finally, later in that article they say:

    "With parts larger than 10 in. by 7 in. (254mm by 178mm), only the top and bottom can be machined: no side setups!"

    I wonder why that is? Is it because of their process? What are they doing? Or is it the limitations of their machines (xyz envelope) or work-holding approach?

    Thanks.

  2. #2
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,437
    Post Thanks / Like
    Likes (Given)
    401
    Likes (Received)
    641

    Default

    Quote Originally Posted by martin_05 View Post
    I wonder what your opinion might be on the question of not drilling, but rather interpolating every single hole and avoiding taps in favor of thread milling.
    You asked for it, here it is.

    Interpolating is great if you're doing onesy/twosy stuff or making some truly massive holes, otherwise it's a big waste of time.

    Threadmilling is kinda the same way, but it does shine for doing pipe threads or weird sizes, etc.
    I always get a kick out of people that say rigid tapping is slow, hard on the machine, and inaccurate.
    At that point I know they've never watched a Brother Speedio tap holes.......

  3. Likes Mtndew, 2outof3 liked this post
  4. #3
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    3,017
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    1381

    Default

    Does a human even touch those parts? When I wear my designer hat, I detest interpolated holes. On precision parts they've given me nothing but trouble because they're never round. Just because you can, doesn't mean you should. Give me bored holes and form tapped threads whenever possible.

  5. #4
    Join Date
    Mar 2015
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    424
    Post Thanks / Like
    Likes (Given)
    95
    Likes (Received)
    146

    Default

    "The only downside is that holes much more than six diameters deep become a challenge due to an endmill’s limited length, and may require machining from both sides of the part."

    And, uhh, it's slower? With optimal conditions drilling will always be faster than helical/interpolating to clear out material. I understand the one tool do it all thing...if they're low volume and trying to minimize set up time.

    I almost think the threading portion is more design related than machine related - the article is about part design, after all. Try to design parts with like thread pitch in holes and if you can use one thread mill to get it all done, great. We're actually going to a lot of thread mills in our shop (prototype, job). I've never been one to back Carmex but they've got some great offerings for one shot thread milling. Top to bottom cutter path, single pass, and in various materials. Not necessarily faster than rigid tapping but totally infatuated with the idea that we won't break taps off in parts anymore, or have to hand tap the last .XXX" amount of hole after it's off the machine.

  6. #5
    Join Date
    Mar 2019
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    44
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    16

    Default

    Quote Originally Posted by martin_05 View Post
    I wonder what your opinion might be on the question of not drilling, but rather interpolating every single hole and avoiding taps in favor of thread milling.

    My first reaction was that cycle time and machine wear and tear would be increased. And then I realized this is Protolabs, a high volume operation. If this works for them, why wouldn't it work for everyone else?
    I doubt those yo yos are actually interpolating all holes, some enginerd must've wrote that artical. Who the hell would want to send an 1/8" EM down an inch just to get a 1/4-20?? Protolabs: "offers better surface finish than that obtainable with a drill" cough, cough *bullshit* cough, cough. (not at 6-8XD anyway)

  7. Likes Mike1974 liked this post
  8. #6
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,511
    Post Thanks / Like
    Likes (Given)
    1731
    Likes (Received)
    2163

    Default

    God only knows why someone would interpolate a clearance hole (with rare exception).

    Also, per thread milling, you can control size much better, say if you are trying to make 3b fits and stuff. Other than that, hard to beat a form tap with a modified bottoming chamfer, if material allows....

  9. Likes ChipSplitter liked this post
  10. #7
    Join Date
    May 2019
    Country
    UNITED STATES
    State/Province
    Michigan
    Posts
    1,437
    Post Thanks / Like
    Likes (Given)
    401
    Likes (Received)
    641

    Default

    Threadmilling works VERY well on pipe threads.
    A tap has a huge engagement because of the tapered thread.
    Oh, did I say threadmills are good for NPT?
    No more broken pipe taps
    Oh, and threadmills work great for pipe threads.......

  11. Likes Bobw liked this post
  12. #8
    Join Date
    Mar 2013
    Location
    Oslo, Norway
    Posts
    34
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    6

    Default

    If you run a 2xD full thread mill with a chamfer on the top, it doesn't take all that long to mill the threads vs tapping. Plus you don't have to sink out any broken taps.

  13. #9
    Join Date
    Aug 2009
    Location
    Oakland, CA
    Posts
    347
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    156

    Default

    It's 100% an artifact of their process. Everything is done with their automated CAM system standardized on common blank sizes and tooling. They only need one single point threadmill to cover a range of thread sizes/pitches. Same with interpolating all holes...they have stable machining parameters for the standard tooling in their Haas mills. They trade the speed of optimized tooling against their zero setup/programming time. In my experience as long as the parts aren't difficult 2.5D they always win on price and lead time.

    As soon as thing get interesting with undercuts, tight tolerances, 3D surfacing, or surface finish that doesn't look like poop the advantage is gone. That actually makes them a decent pre-machining service for high value parts. Why saw blanks or buy squared blocks from someone like TCI when you can get a qualified part within +/-0.005" on the cheap with all of the roughing and semi-finishing done.

  14. Likes mhajicek liked this post
  15. #10
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    3,017
    Post Thanks / Like
    Likes (Given)
    151
    Likes (Received)
    1381

    Default

    Also, when you use the same size screws the long suffering assembly person can assemble it with one wrench, hex key or whatever!

  16. #11
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,262
    Post Thanks / Like
    Likes (Given)
    14980
    Likes (Received)
    11106

    Default

    I know some folks believe a center drill is "code" for a spot drill. But
    why do you have 2 center drills and a spot drill in your standard mill tooling
    list? Do your parts regularly move from the mill to the lathe?

  17. #12
    Join Date
    Mar 2009
    Location
    Valencia, CA, USA
    Posts
    391
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    59

    Default

    Quote Originally Posted by Bobw View Post
    I know some folks believe a center drill is "code" for a spot drill. But
    why do you have 2 center drills and a spot drill in your standard mill tooling
    list? Do your parts regularly move from the mill to the lathe?
    Good question. I used to use center drills until I learned spot drills were the right tool and offered more flexibility, chamfering being an obvious application.

    This is the kind I have:

    https://www.mscdirect.com/product/details/06298681

    I also have a full set of 82 degree carbide center drills. If I need to countersink for 82 degree flathead screws I'll use a center drill. I found that having two sizes on the machine helps when having to deal with different screw sizes.

    I suppose I could buy some 82 degree spot drills and save the center drills for when I buy a lathe (which I intend to do as some point). Right now I am working with what I have. If this was a production shop I would probably stop using them and get more spot drills.

  18. Likes Bobw liked this post
  19. #13
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,184
    Post Thanks / Like
    Likes (Given)
    931
    Likes (Received)
    2813

    Default

    A lot of the parts I make are custom boat parts. One usually or two pieces once in a great while. I almost never set up a drill. I interpolate most holes. Below .16" or excessive depth then I'll drill. IME it is slower to get a drill set up and touched off and run than it is to use one of my "core" tools and just make the hole. Also when making a new part, I only slow down until the first tool checks out on the approach. After that as long as the program is using only "core" tools, I just let it run. If I'm using freshly set up tools then I slow the approach moves for them so I can verify I did not make any maistake in touching them off or entering offset values.

    Those boat parts rarely have tapped holes so kind of a non-issue for my work. The boat guys usually like through holes and screws and bolts with Nyloc nuts to hold things together.

  20. #14
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,200
    Post Thanks / Like
    Likes (Given)
    270
    Likes (Received)
    1067

    Default

    To a certain extent the cost for tooling and or time far outweigh the cost and time of interpolating/thread milling.

    Of course it greatly depends on your work.

    Last shop I worked at built production machinery. The engitard that designed the machines spec'd everything as diverse and stupid as humanly possible. A few were past what would be considered humanly possible. Somewhere I have a picture of a part that has inch thread, metric thread, helicoil insert threads, NPT threads, inch dowel, metric dowel, press fit, slip fit, clearance holes, along with inch and metric bolt holes. I actually got up and was walking across the shop to slap him in the face when I was intercepted by the owner who was three steps ahead of me.

    The owner complained at one point why I kept asking for more tool holders.

    I had about 20 setup with metric tap drills and taps.
    I had about 20 setup with inch tap drills and taps.
    I had 6-8 setup with helicoil.
    I had 6 or so setup with NPT
    then in addition I had a set of maybe 20 or 30 setup with "standard" drills for clearance, dowel, stupid, and more. I combined tap drills wherever possible.

    I argued that having a dozen holders setup with thread mills would carry all the inch, metric, npt and helicoil threads, but it was too expensive.

  21. Likes dodgin liked this post
  22. #15
    Join Date
    Mar 2009
    Location
    Valencia, CA, USA
    Posts
    391
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    59

    Default

    Quote Originally Posted by Fal Grunt View Post
    To a certain extent the cost for tooling and or time far outweigh the cost and time of interpolating/thread milling.
    That's an interesting perspective. Even though I don't do production it is still a huge pain to have to load drills and taps in a design where you have no choice but to have a mixed set of holes you have to fabricate.

    I am doing a part right now that will have a mixture of metric and imperial components mounted to it. I have no choice but to have several sizes of clearance holes and threaded holes. With a 20 tool carousel and a limited number of drill chucks (I have two) and tap holders (don't know how many I have, not many) it can be truly painful to do these kinds of parts.

    One of the things that comes to mind is the probability for error. I've done this many times, where I forget to touch off the tool or assume I have a 0.266 drill in the chuck when I actually have a 0.201 from a prior part. It's a testament to the strength of the Balax form taps I use when a 1/4-20 tap taps 10 holes drilled with a 0.201 bit and doesn't break (1/8 in aluminum, so it wasn't that bad...but).

    Then there's the issue of having to divide the process into multiple programs because you just don't have enough drill and tap holders and have to reload and touch off a new set of drills and taps to complete the part. Just the other day I had to make 24 pieces where this happened. I had to run program #1 on all parts, install new tools, touch them off and re-clamp and run all the parts one-by-one using program #2.

    So, yeah, I can see that switching to interpolating holes and machining threads could be more efficient or, at the very least, reduce the pain in the behind factor significantly. In my case cycle time isn't critical at all. I literally don't care if a part takes twice as long to make. So, taking a little bit of a hit by interpolating and thread milling (if there is a hit) isn't a big deal for me.

    Just trying to learn.

  23. #16
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,200
    Post Thanks / Like
    Likes (Given)
    270
    Likes (Received)
    1067

    Default

    If it is a standard tool/standard element it takes what, 5 minutes to grab the tool, find a collet, build the tool, load the tool, touch off the tool?

    But the problem is always I have a ER20 collet, and a ER25 holder....

    Can't find the #18 drill...

    What can I take out of the magazine and tear down...

    Can't use tool 15, I know I'll need that on the next part...

    So instead you wind up spending 15 minutes trying to find some combination that will work. I spent the last 2 days working on a 10pc order.

    Monday



    I tried to do a job for a friend of mine earlier this year. I was going to run it in the Brother, but I didn't have ANY of the tooling I needed. 5/8" bolt hole 6" deep, 1/2" dowel pin hole clearance 6" deep, press fit bottom 2" of the 8" thick part. Stuff like that. I wound up setting it up and making it on my Moore, took me damn near 5 hours. S7 tool steel by the way... $600 chunk of it. When I dropped it off my friend teased me about how long it took me. Usually takes him an hour. He showed me the rack of tool holders, setup, with all the drills, core drills, counter bores, to do the job.

    I have learned that I can't do everything, and I don't care to do everything. For me, I don't drill and tap a lot of holes, so I thread mill and interpolate. I recently did a job with some 4-40 and 6-40 holes. To do them, I would need 2 tap drills and 2 taps. I only had 1 spot left in my magazine. So I used a thread mill, drilled undersize with a drill from another detail, opened the hole up with a 2mm endmill from another detail, and thread milled.

    Plus, I think I have PTSD from the Doosan I ran at that place mentioned above. We broke taps all the time. ALL the time. I broke a 1/2-13 tap, it DETONATED. Everything in the shop stopped. We ultimately found out that machine had been built incorrectly, something in the PLC, I forget, but it took 4 Korean guys several hours to fix and it hasn't (to my knowledge) broken a tap since.

    Threadmills are STUPID quick if you run them ragged. Especially on small holes.

  24. #17
    Join Date
    Nov 2004
    Location
    WI
    Posts
    4,749
    Post Thanks / Like
    Likes (Given)
    518
    Likes (Received)
    1105

    Default

    Sometimes.... Sometimes.. It is Way faster to interpolate than to drill.
    I had a job for 40,000 pieces 12" X 13" 1/4" aluminum plate.

    About 30 holes to drill, bunch of sizes, some totally non standard sizes, and about .0005" tolerance.
    Tool change to an 1/8" endmill and blast them all with one tool. FASTER than you could tool change all the drills.
    Helical plunge to the bottom, and interpolate.
    Changed the tool comp value for the various sized holes.

    This was the job that bought the first Robodrill for me.

  25. #18
    Join Date
    Aug 2007
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    1,506
    Post Thanks / Like
    Likes (Given)
    213
    Likes (Received)
    482

    Default

    I have had a few jobs over the years that any idiot that could use a go / no go pin on one hole could run and we have done it that way, one tool finishes all features and checking one hole checks the whole part.

  26. #19
    Join Date
    Mar 2009
    Location
    Valencia, CA, USA
    Posts
    391
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    59

    Default

    Quote Originally Posted by 3t3d View Post
    I had a job for 40,000 pieces 12" X 13" 1/4" aluminum plate.
    Nice one! That's when you really have to think about optimization.


    about .0005" tolerance
    Is that center-to-center, diameter, concentricity, all-of-the-above-and-then-some?


    1/8" endmill ... Helical plunge to the bottom, and interpolate.
    Where these through holes? Did you use a stubby end mill or just plung down as far as you could to limit flex and interpolate the full 0.250 depth of cut (that's my assumption from your comment).

    I'm still not comfortable pushing small enc mills like that hard and doing full face cuts in general.


    Changed the tool comp value for the various sized holes.
    That's an interesting one for me. Wouldn't the different size holes and interpolating them be a part of the CAM process while you comp value on the machine stays at zero?

    I've used comp value changes to adjust dimensions by a few thou (< 5) post machining but never thought of it as a way to make holes of different sizes with the same program. Maybe I misunderstood.

  27. #20
    Join Date
    Nov 2004
    Location
    WI
    Posts
    4,749
    Post Thanks / Like
    Likes (Given)
    518
    Likes (Received)
    1105

    Default

    Quote Originally Posted by martin_05 View Post
    Nice one! That's when you really have to think about optimization.




    Is that center-to-center, diameter, concentricity, all-of-the-above-and-then-some?

    Diameter


    Where these through holes? Did you use a stubby end mill or just plung down as far as you could to limit flex and interpolate the full 0.250 depth of cut (that's my assumption from your comment).

    I'm still not comfortable pushing small enc mills like that hard and doing full face cuts in general.

    all through holes, stubby end mill, 5/16" LOC Helical plunge to near net size, interpolate to finish size.


    That's an interesting one for me. Wouldn't the different size holes and interpolating them be a part of the CAM process while you comp value on the machine stays at zero?

    No, they were all various sized holes and all interpolated to correct size....
    The reason for individual comp values was that I was pushing the feed rates so hard.
    First if i didn't get a (Very) small amount of taper, I assumed I wasn't pushing the feed rate hard enough.
    Second, small holes would need slightly different comp values than larger holes.
    If I slowed the feed rate to sane levels, only one comp value would have been needed.

    I've used comp value changes to adjust dimensions by a few thou (< 5) post machining but never thought of it as a way to make holes of different sizes with the same program. Maybe I misunderstood.
    See above..
    All these parts were run on a vacuum plate. Full machined around the perimeter, 1/4" end mill at 24000 RPM and 250 IPM And various features milled and countersinks.
    Total of 2.5 minutes run time.


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
  •