509,985 active members
3,821 visitors online
Register for free
Login
Page 3 of 3 123
Results 25 to 30 of 30
  1. #25
    Member
    Join Date
    Jun 2015
    Posts
    2874

    Re: Tips for straighter bores

    oau, i forgot this thread

    in production time is money and a reamer will save time every time
    all these are frequent aspects :
    ... tool costs, especially non-standard sizes
    ... tool delivery time
    ... setup time ( alignment, tir check, etc )
    ... adjusting cutting specs
    ... holes that are too big /too small, even if the reamer dimension is ok
    ... almost no chips at all, on a machine that is capable of delivering chips

    what about improving all these aspects ?

    That would be my first go to tool for a hole solution...…...alternatives go down the more time and less accuracy ladder.
    please, what alternatives exist, and why are those with less accuracy ?

    Reaming after drilling also is not an answer as the reamer will just follow the drilled hole and that can be out of position
    the reamer is not always following the hole; each setup is a balance between elastic & plastic deformation

    for a reamer to follow the hole, then the elastic component has to be dominant, alowing the tool to 'move' inside the hole, and shift back to it's original position, when it is out of the hole

    for a reamer to not follow the hole, the plastic component has to be dominant; this can be achieved, for example, with a rigid spindle + short overhang tool with long flutes

    each machine, in time, increases it's elastic behavior, thus is losing rigidity; for a process that delivers tight tolerances, then this effect has to be postponed as long as possible


    what can be done ? analyze the frequency of the holes, and dimensions
    ... get a set of after-drilling tools ( they look like a reamer, but with less flutes, and they are more rigid then a drill; the trick behind such tools is that they don't copy the hole, and can straigthen-up a tilted hole, delivered by a long drill )
    ... get an attachement ( eccentric boring or grinding attachment, honning attachements )
    ... put that attachement on a ' normal ' machine, and leave it there : voila, this is a low-cost specialized machine, that never runs roughing operations, spindle is not under frequent tool changes, etc; like this, the machine keeps it's accuracy for a looooong time
    ... get a specialized machine

    i don't say that a reamer is bad; i say that controlling costs and analyzing downtime requires patience and time, and seeing such alternatives in action may help / kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  2. #26
    Gold Member
    Join Date
    Sep 2006
    Posts
    6373

    Re: Tips for straighter bores

    If you aren't into reamers for hole sizing then you have missed the plot completely......even odd size holes will profit from a reground reamer if the volume is great enough.

    As I said, a reamer will ALWAYS follow a drilled hole without exception......because it has flexibility in it's length.

    If you apply the length to 4 times the diam rule you get a boring bar.

    Reamers also cut on their ends not on their sides.

    Reamers cannot make a hole true to a required position if the hole is off centre......then the reamer will be off centre too.

    There is an alternative way to make a hole to size and positioned accurately too but it is not profitable.....it's called EDM.

    When you approach the prospect of a design requirement then you must choose the best way to get an outcome.

    BTW....you "could" produce a hole to size and position with an end mill, but the flutes would need to be blunted to prevent them from enlarging the hole diam and in so doing making the endmill a short series reamer.

    You "can" make a drill cut to size by predrilling the hole with a drill 10% undersize and stoning a slight radius on the corner of the end flutes of the finish drill.
    Ian.

  3. #27
    Member
    Join Date
    Jun 2015
    Posts
    2874

    Re: Tips for straighter bores

    If you aren't into reamers for hole sizing then you have missed the plot completely
    hi, i discuss methods to deliver straighter bores; this also includes reamers

    a reamer will ALWAYS follow a drilled hole without exception
    with all respect, this is not true ...

    because it has flexibility in it's length
    when the reamer follows the hole, it is because of a few factors; this includes the length/dia ratio of the tool, but is not the only one; another aspect is the console&chucking flexibility

    for example :
    ... classical lathe : you expand the tailstock, or even push the entire tailstock by hand
    ... classical mill : you lower the head
    * in above situations, the console is flexibile

    on a cnc, consoles are much more rigid, so:
    ... if you wish to to achieve flexibility inside the chucking, you may use floating-chucks, or long-collet-chucks, etc
    ... if you don't wish for flexibility inside the chucking, then a rigid chuck with short tool overhang is required, preferably with tir adjustemnt ( for mills ), or radial & tilting adjustment ( for lathes )

    depending on all these factors, a reamer, during cutting, is somewhere between "reaming" and "boring"

    If you apply the length to 4 times the diam rule you get a boring bar
    3d : normal quality steel, no internal coolant
    5d : higher quality, internal coolant
    7d : carbide, internal coolant
    deeper : vibration-dampening

    and there are special ones, with section<>circle

    Reamers also cut on their ends not on their sides
    by design, a reamer for cilindrical holes has to cut, preponderantly, on front end; if it would cut on both ends, it will recut the hole when it is retracted; or, even worse, it may get stuck inside the hole

    a reamer for cilindrical holes should not have cilindrical od, but conical; depending on applications, the conicity of such a reamer can be with bigger diameter towards the front, or with bigger diameter towards the tail ( greater life-spam, etc )

    Reamers cannot make a hole true to a required position if the hole is off centre......then the reamer will be off centre too
    use a rigid console, rigid chucking, and low overhang rigid tool, so to corect the hole position before finishing, with a normal/rigid reamer, or a grinding attachement, etc

    There is an alternative way to make a hole to size and positioned accurately too but it is not profitable.....it's called EDM
    edm can deliver such things, but it was not designed for such tasks

    when it comes to accuracy tolerated holes ( dimension, position, etc ), one may use a coordinate grinding machine:
    ... the classical hauser
    ... classical mill with eccentric attachemnt
    ... interpolating on cnc, with a simple air driven attachement, etc

    When you approach the prospect of a design requirement then you must choose the best way to get an outcome
    just saying : a while ago, it was needed to deliver many parts with non-standard holes; i crafted the reamers, i crafted the plungers before the reamers, intenal coolant, tilted flutes, 2 diameters / same tool, etc; all you need is an y-lathe and a grinding machine

    many believe that a reamer crafted in H7 will deliver a H7 hole, and in reality a lot depends on real scenario, material hardness, fixture tension, etc : all these will affect the life spam and the consistency of the output dimensions; i talk about long setups

    BTW....you "could" produce a hole to size and position with an end mill, but the flutes would need to be blunted to prevent them from enlarging the hole diam and in so doing making the endmill a short series reamer
    instead of blunting the flutes, you may grind the od a bit conical; it's faster kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  4. #28
    Registered
    Join Date
    Aug 2004
    Posts
    710

    Re: Tips for straighter bores

    Lots of excellent posts and comments on hole size, reamers, production, straightness, cylindricity.

    Basically only holes bored on lathes or bored via boring heads or boring tools on mills are "straight" and "true".

    The size of the hole via modern boring head on a lathe or mill, today, is approx 1 micron incremental size.
    So holes with 1 micron incremental sizes are easily made in steels if modern boring heads can be used.

    Likewise, if the hole has a "good" near-net bore, any reamer will finish it to size, usually with great surface finish.

    If better hole sizing is required, after reaming a "good" bore, roller burnishing or ball sizing can make better finishes and smaller incremental sizes.
    It is perfectly possible to make ball-burnishing tools.
    Sub-micron incremental sizes are reportedly easy to do.

    In auto production, VMC cnc mills rough bore the piston holes.
    The hole is finished with a single rigid hone coated by diamond abrasives.
    Take about 20 secs or less.
    The hone lasts 300.000 parts, full year.
    Accuracy is better than 0.01 mm in size and tir.

  5. #29
    Gold Member
    Join Date
    Sep 2006
    Posts
    6373

    Re: Tips for straighter bores

    As the actress said to the Bishop, there are many ways to do it.....reaming with a rigid tool is just one way, and the required quality of the end product dictates how you get there.....also, and more pertinent, the volume of the order is the most deciding factor for hole production, and the tolerance just decides the cost.
    Ian.

  6. #30
    Member
    Join Date
    Jun 2015
    Posts
    2874

    Re: Tips for straighter bores

    Basically only holes bored on lathes or bored via boring heads or boring tools on mills are "straight" and "true".
    hi hanermo, yup, and also those delivered by coordinate grinding machines, especially because they grind, thus cutting force is low, and remanent tension, inside the part, is really low : this helps to deliver consistent dimensions in soft materials, that, otherwise, because of heavy cutting, may deform in time, at least at micron level; there are cases when parts are ok right after machining, but after a few days, if they are checked again, they are out of tolerances

    there are cases when the client is not accepting a process that is finishing a part with high cutting forces; so far, this had no been discused in this thread, but, whatever

    about this "straight & true", i needed to deliver some parts with non-standard tolerated holes, with length between 6-9D, that were checked with a go-gauge as long as the hole; it was a bit tricky, because :
    ... at that length, all drills would bend, so, after drilling, the hole was not cilindrical, and this was breaking the reamers like crazy; i managed it but using plungers ( some custom tools that would improve cilindricity after driling ), and reamers inside floating chucks; also, i had shorten the active length of the reamer ( thus shorter flutes, but overall tool length remained the same ), to make it a bit more flexible
    ... also, each part had at least 2 such holes, with tolerated reciprocal positioning : imagine a few H7 holes, that are not paralel, required to be at H7 coordinates, something like a " tolerated swiss cheese "; it was a bit hard, because, if the hole diameter was near the minimal value, then there was a chance to miss the reciprocal positioning; to manage this, i had delivered all the holes near the maximal diameter, i had crafted my own go-gauges ( with bigger diameter then the original ), and i was working in a tolerance that was much smaller then the original tolerance of the technical drawing; in the end, it worked, but it took me a while to figure it out

    It is perfectly possible to make ball-burnishing tools.
    Sub-micron incremental sizes are reportedly easy to do
    i don't have experience with such tools; i know that they can deliver smooth surface and increase the cilindricity specs, but i don't know what tolerances they can deliver, and, for the adjustable ones, i don't know what is the finess/accuracy of the adjusting system

    i believe that they should somehow have a radial play, so to be able to copy the hole ...

    i have seen that there are some burnishing tools that may turn, and other types doing some things; i shared the videos at the end of this post

    The hole is finished with a single rigid hone coated by diamond abrasives.
    Take about 20 secs or less.
    in automotive, it won't be long until they will finish all the engine with a single tool, just like a snake, going from one hole to the other

    i have seen a documentary about engines, and it said that, if you wish to increase the power, you have to craft the engine with less play between the pistons and the holes, so to lose less power during combustion; when tolerances are tight, it is recomended to heat-up the engine before starting it, because, otherwise, if it would start cold, the pistons may damage the engine; motorsport / kindly


    https://www.youtube.com/watch?v=eAwqtMtzNYs

    https://cogsdill.com/videos/burnishing-tools/

    https://www.youtube.com/watch?v=B6YxFxMCKkQ
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

Page 3 of 3 123

Similar Threads

  1. 2 flute Counter Bores
    By Michael58 in forum Machinist Hangout
    Replies: 0
    Last Post: 02-19-2017, 03:26 PM
  2. Manufacturing of ejector bores
    By jens67 in forum DRILLING
    Replies: 1
    Last Post: 10-07-2009, 05:02 PM
  3. Sloping bores
    By ideefix in forum HEIDENHAIN -> GENERIC
    Replies: 2
    Last Post: 03-24-2009, 07:11 PM
  4. Replies: 0
    Last Post: 09-29-2006, 07:17 PM
  5. bearing bores
    By eschless in forum Uncategorised MetalWorking Machines
    Replies: 20
    Last Post: 10-20-2004, 12:03 AM

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
  •