Blind hole technique


Page 1 of 2 12 LastLast
Results 1 to 12 of 13

Thread: Blind hole technique

  1. #1
    Registered
    Join Date
    Mar 2018
    Location
    United States
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Blind hole technique

    Please excuse the rookie questions;

    I want to mill a blind hole that is 2.9" deep (0.5 Dia). Can I just use 3/8 end mill that is extra long (4" or such) with flute LOC 2" and get it deeper to 2.9" or what is the proper technique for such a deep hole? I don't have a lathe.

    Should I get the speed lower to accommodate the extra long end mill? Would 2D Circular be the best approach for such a hole (on Fusion 360), maybe something to retract to get the chips out?!

    I've considered Drill/Ream, would this be better? Still will be good to learn the milling proper way.

    Thanks a lot, guys.

    Similar Threads:


  2. #2
    Registered RussMachine's Avatar
    Join Date
    Nov 2013
    Posts
    343
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    I would drill it to 2.9" deep, then just 'drill' it again with an extra long, 2-flute 1/2" end mill to get the flat bottom.



  3. #3
    Registered
    Join Date
    Aug 2014
    Posts
    138
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    What you would do depends on the hole requirements. As RussMachine points out the best way to remove material is by drilling first. This may meet your requirements unless you need a flat bottom. Then running a 1/2” EM down there will clean things up. Sometimes you need a better hole than this process can achieve such as size, straightness and surface finish and this is where boring and reaming come into play.

    Trying to use a 3/8” EM at that depth is probably the worst method to choose. Also, making round holes using interpolation introduces more errors than the other processes mentioned. But again, it comes down to hole requirements and what methods you have available. Machining a hole with a cutter LOC less than the hole depth is asking for trouble.

    In general, I always try to use a drill first then finish up as necessary. Drills are cheap and easy to sharpen and they save your cutters.



  4. #4
    Gold Member Steve Seebold's Avatar
    Join Date
    Mar 2009
    Location
    USA and proud of it
    Posts
    1774
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    Why not drill it 2.9 inches deep to the drill point then use a flat bottom drill to take out the point.

    Last edited by Steve Seebold; 04-15-2018 at 12:03 PM.


  5. #5
    Registered
    Join Date
    Jan 2016
    Posts
    39
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    How flat? End mills leave the center slightly high. End mill will give you a straighter hole,if you predrill undersize first.
    Boring is still the best choice for on location and straight but that is a long boring tool and there will be a lot of deflection.

    Dave



  6. #6
    Registered
    Join Date
    Mar 2018
    Location
    United States
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    Thanks guys.


    It needs to be as close to 0.5000 as it can with a very clean surface finish. Not a problem if not true flat; as there will be a spring at the bottom. This is going to be for a dynamic (moving) rod/piston with an o-ring for hydraulic seal.


    I figured with using Endmill, I can creep on the 0.5 with a final finish cut.


    Maybe drill undersized then ream? Been looking at those reamers @ MCMaster. Wow... the cost is really not for the hobbyist & personal projects. For the reamer, do I have to get one with flute length >= my blind hole? Or can I use a 1.5" Flute length reamer with a long shank that can reach down?



  7. #7
    Registered
    Join Date
    Nov 2005
    Location
    UK
    Posts
    134
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    A couple of points - if you're going to run a moving 'O' ring or other seal in there, then the finish you'll produce from a drill, end mill, or reamer, will not be nearly smooth enough to avoid any abrasion of the seal. For that you really need a lapped finish. A lap is easy enough to make, you can google for it.

    Secondly, a reamer cuts on the end and not along its length, so the flute length doesn't really matter, as long as it will reach down to the end of your hole.
    Thirdly, you can make a D-Bit, which is a home-made reamer that cuts very well indeed for the single hole or few holes you may need, and all you need is a bit of drill rod and a propane plumbers torch. Again, you can google for it.

    However, neither will give you the finish you need for a sliding 'O' ring.
    If I were making this, I'd make the entire thing with a though hole, drill a few thou' under. get it just-about-to-size with a D-Bit, then make a lap that I can pass through end to end to get the finish and final size, and then make a seperate end cap to close the blind end off.

    It sounds like you're fairly new to this, so this may be a fun learning curve for you, with new things to try.



  8. #8
    Gold Member Bob La Londe's Avatar
    Join Date
    Oct 2008
    Location
    USA
    Posts
    1807
    Downloads
    2
    Uploads
    0

    Default Re: Blind hole technique

    Quote Originally Posted by Peter Neill View Post
    A couple of points - if you're going to run a moving 'O' ring or other seal in there, then the finish you'll produce from a drill, end mill, or reamer, will not be nearly smooth enough to avoid any abrasion of the seal. For that you really need a lapped finish. A lap is easy enough to make, you can google for it.

    Secondly, a reamer cuts on the end and not along its length, so the flute length doesn't really matter, as long as it will reach down to the end of your hole.
    Thirdly, you can make a D-Bit, which is a home-made reamer that cuts very well indeed for the single hole or few holes you may need, and all you need is a bit of drill rod and a propane plumbers torch. Again, you can google for it.

    However, neither will give you the finish you need for a sliding 'O' ring.
    If I were making this, I'd make the entire thing with a though hole, drill a few thou' under. get it just-about-to-size with a D-Bit, then make a lap that I can pass through end to end to get the finish and final size, and then make a seperate end cap to close the blind end off.
    To the OP. The advise to drill is spot on. Your biggest problem with a hole that deep is getting the chips out of the hole. A twist drill is going to do that better than any other tool. When you go back to ream or bottom mill or bore or however you bring it to near final size you still have the same problem. Getting the chips out of the hole. You won't have the bulk of chips you had to start with but packing up all the chips from reaming at the bottom of the hole can cause you to leave a ridge at the bottom. This does leave a conundrum. I hate to run a ream thru a hole twice. Atleast with the cheap chucking reamers I have the run out tends to slightly over size the hole from the reamer size.

    Lapping and polishing is a good advise, but you have to take some care not to pear shape the cylinder, or bell mouth the hole. Maybe you can account for that to some degree by how long the piston is beyond the o-ring, and how much you engage the o-ring. Since this is a moving application and not just a static seal you have to consider how much engagement you need to contain the pressure you will be working with and still move as easily a you need it to. Remember that a piston ring is a wear part. Whether its a chromoly ring in a gas engine or a rubber ring in a "home built" device.

    All is not lost though. An o-ring can make up for a lot. I sometimes make hand injectors for soft low (290-350F) temperature plastisol injection. (for my own use) My pressure is low and unless there are visible imperfections inside the tube I just use the raw extrusion's mill finish. I don't size. I don't polish. I just machine a piston (on the lathe I admit) to a rough dimension that easily drops into the tube. Then I measure the ID of the tube and cut a ring groove in the piston so that the o-ring has too much engagement. Then I slowly deepen the groove until I get engagement that "feels" good with the tube or cylinder of the injector. This is what I call "machine to fit" as oppose to "machine to spec." Its not suited to mass producing injectors, and depending on the source of the tube the parts may not interchangeable, but they all work.

    I'm definitely not saying you should take either a sloppy or a machine to fit approach. Just that you should consider what you actually need to be able to do to accomplish your end goal. Is a precision exactly perfectly 0.5000 hole necessary. Is the cycle rate of your piston fast or slow. Will a slight variance in diameter of the hole matter. Will your piston bump on the cylinder walls or will the o-ring(s) be such as to prevent that. How much pressure are you dealing with. Is it necessary for the hole to be blind or does it just need a ridge to stop the spring. If the hole has to be blind how will you deal with back pressure or vacuum behind the piston. I agree the hole needs to be polished smooth, but how smooth. If it only sees a few cycles an hour or possibly in its lifetime that may not be as important to be perfect as if it see a rapid high number of cycles in an hour... or a minute. Is it more important that it seal perfectly or move easily.

    They hardest thing I have had to learn in machining is that chasing perfection can sometimes cause more problems than it solves. The hardest thing I've found to design is acceptable tolerances. Sometimes I have to step back from a projecting and think , "How crappy can it be before it fails? How good can I possibly make it? What is something in between that will work and can be achieved with a reasonable amount of effort relative to the value of the project?"

    Bob La Londe
    http://www.YumaBassMan.com


  9. #9
    Registered
    Join Date
    Mar 2018
    Location
    United States
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    These are all excellent tips.


    Yes. New at this. Just started. I figured the best way to learn is just go at the project I want to do and learn as I am building the components.


    Here are photos of the valve body I milled last week (Beta 0.0.1), this is 5" so I did do it from both sides, figured I may be close enough, well, I was not far off getting the holes to match from both sides but boy, did I learn a lot from that approach!! (no end mill or machine were harmed during the making )


    Ok, so to go through from one side, I will order 118° extra-long drill and give that a shot. Will look at D-Bit and Lapping


    Indeed, brain/eye-opening information here; the o-ring will only move the first 0.7" of the bore. So I guess I can bore that to spec and leave the rest of the hole to envy the top.





    Attached Thumbnails Attached Thumbnails Blind hole technique-1-jpg   Blind hole technique-2-jpg   Blind hole technique-3-jpg  


  10. #10
    Registered
    Join Date
    Mar 2018
    Location
    United States
    Posts
    11
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    So this one? https://www.mcmaster.com/#4380A32

    Just use a lapping paste and get it in? (no pun intended )

    Any suggestion on feed/speed? (PCNC 440)

    How about the extra long drill? Speed? low?





  11. #11
    Registered
    Join Date
    Nov 2012
    Location
    United States
    Posts
    147
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    How crappy can it be before it fails?
    In all honesty, this is the essence of engineering!



  12. #12
    Registered
    Join Date
    Apr 2016
    Posts
    81
    Downloads
    0
    Uploads
    0

    Default Re: Blind hole technique

    If you need a CHEAP reamer to get it in close before lapping I have half a dozen reamers from these guys that I've purchased for non-uber critical applications. Sometimes I need a smooth precise slip fit for a pin size nothing else on earth uses, and I only need it once or twice.

    https://www.ebay.com/itm/1-2-X-2-MT1...item43c7a1744a

    Also look over some of the other tools and end mills that seller has. A few are good deals and they combine shipping. It's a good place to get an order of a few cheap tools that might actually make parts, but you can afford to break constantly as you learn. I broke half a dozen 1/8" 4 flute stubby end mills and a couple of 1/4 HSS and carbides from them while I learned the ropes. So cheap it didn't matter.

    I don't buy much from them currently, except for the reamers. They have every diameter of cheap reamer imaginable. If the shank is too long on the smaller ones, you can always cut them off. (sacrilege I know, but you don't have to feel bad about murdering a $2 reamer to finish one job.)

    What they don't carry that makes me sad are end mills with odd flute numbers (3 or 5) or with high or variable helix. But hey, you can't have everything super cheap.



Page 1 of 2 12 LastLast

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

Blind hole technique

Blind hole technique