554,259 active members*
3,877 visitors online*
Register for free
Login
Page 1 of 2 12
Results 1 to 20 of 22
  1. #1
    Registered
    Join Date
    Nov 2017
    Posts
    584

    taper reaming

    im working on a design that will need a very precise tapered hole in hardened steel, 58-60hrc. Doing it pre heat treat is definitely an option, but i would prefer to do it after if possible for best accuracy and finish. The hole is quite small, 1/4" at the top, 10:1 taper (2.86 deg per side or 5.72 included), and only 1/8" deep, through hole. The reaming operation will be removing very little material, about 6 thousandths off the wall at top edge. This will be done on cnc.

    So first question, can i do this in hardened steel with a carbide reamer? From what i understand about tapered reaming, it can be challenging because the whole length of every flute is cutting and it has to take a very small chip. I would imagine especially in hard steel, it will resist cutting and try to rub. should i even attempt this in 60hrc material?

    Next question, where do i get such a tool? Ive been searching around without much luck. Morse taper and taper pin reamers are very common, but im not finding other angles, especially not in carbide and not this small. This doesnt need to be exactly 10:1 taper, but something at least close to that for the geometry to work. I will be turning the tapered pin that drops into this hole so the exact angle is not important. I would say between 5 and 6.5 degree included angle should work. Ive searched ebay and found various used taper carbide reamers, but nothing that will work for me. Also i will need to be able to replace this tool when needed, so even if i happen to find the right one used on ebay, thats not gonna help me much. Am i looking in the wrong place, or Is this going to be a custom made tool?

    Im also open to other suggestions for making this hole. It needs to have a diameter tolerance of about 5 tenths, locational tolerance of about a thousandth and have a very good finish. I know that "very good finish" is vague, but i dont know well enough to give it an ra. I would say definitely better than what i would get by doing a helical bore with a ball endmill. The mating tapered pin will drop into this hole with about 20oz of pressure and it needs to easily release with absolutely no sticking. To me it seems reaming will be the easiest way to hit these requirements. If its not gonna work, i do have the option of turning this hole on the lathe, but it will be a big awkward fixture and an extra op requiring a lot of setup. I would very much prefer not to do it that way.

    Im also not stuck on the idea of doing it hard, theres a good chance it can be done pre heat treat and keep the necessary tolerance. I can measure the change in heat treat and adjust for that. It would just be better to do afterwards if possible.

  2. #2
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    This doesnt need to be exactly 10:1 taper, but something at least close to that ... I would say between 5 and 6.5
    hy turning ? a reamer is not critical, expensive, will require alignment, and may not cut into those 60hrc

    do have the option of turning this hole on the lathe, but it will be a big awkward fixture
    why is the fixture so tricky ?

    It needs to have a diameter tolerance of about 5 tenths
    relevant tolerance for conical surface is on z axis, in assamble; just saying

    theres a good chance it can be done pre heat treat and keep the necessary tolerance
    The mating tapered pin will drop into this hole with about 20oz of pressure and it needs to easily release with absolutely no sticking
    to release without sticking, means that the ring must be hard ( so to not deformate ), oiled ( for less friction ), and contact surface to be big ( so les pressure / area )

    consistency for those is better if machining after heat treat, but may work even if you make 10eq, heat treat, then chose 3 for example / kindly
    Attached Thumbnails Attached Thumbnails Untitled.png  
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  3. #3
    Registered
    Join Date
    Nov 2017
    Posts
    584

    Re: taper reaming

    I guess i shouldnt have said "turned". I meant the tapered hole could be bored on lathe if it absolutely had to be. Yes, the male taper part will be turned on lathe no matter what and i understand how to do that no problem. The hole is the part in question. It could be held in a fixture for boring on lathe, but trust me when i say it would be very inconvenient to fixture this otherwise mill part on the lathe for one operation. It would require constant changing back and forth of tooling on my lathe and unnecessary setup. its a possibility as a last resort, but i will try all other possibilities first including reaming pre heat treat. This is not a one off part, I am working on an efficient method for continued production.

    I guess i didnt specify this is a mill part. reaming would be done on mill, boring would require moving to another machine

  4. #4
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    okey so is not a revolution part; of course, a reamer now seems more likely

    another aproach, is to use a high rev air spindle ( cheap one ) and grind it; unfortunately, i don't know a stone that can cut consistent at such small diameters, because i don't grind much

    however, if you have in house a bunch of small stones, you can experiment; it may be possible to consume 2-3 of them per part, but may still be less expensive than whatever else tooling
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  5. #5
    Member
    Join Date
    Jan 2005
    Posts
    14302

    Re: taper reaming

    Quote Originally Posted by QuinnSjoblom View Post
    im working on a design that will need a very precise tapered hole in hardened steel, 58-60hrc. Doing it pre heat treat is definitely an option, but i would prefer to do it after if possible for best accuracy and finish. The hole is quite small, 1/4" at the top, 10:1 taper (2.86 deg per side or 5.72 included), and only 1/8" deep, through hole. The reaming operation will be removing very little material, about 6 thousandths off the wall at top edge. This will be done on cnc.

    So first question, can i do this in hardened steel with a carbide reamer? From what i understand about tapered reaming, it can be challenging because the whole length of every flute is cutting and it has to take a very small chip. I would imagine especially in hard steel, it will resist cutting and try to rub. should i even attempt this in 60hrc material?

    Next question, where do i get such a tool? Ive been searching around without much luck. Morse taper and taper pin reamers are very common, but im not finding other angles, especially not in carbide and not this small. This doesnt need to be exactly 10:1 taper, but something at least close to that for the geometry to work. I will be turning the tapered pin that drops into this hole so the exact angle is not important. I would say between 5 and 6.5 degree included angle should work. Ive searched ebay and found various used taper carbide reamers, but nothing that will work for me. Also i will need to be able to replace this tool when needed, so even if i happen to find the right one used on ebay, thats not gonna help me much. Am i looking in the wrong place, or Is this going to be a custom made tool?

    Im also open to other suggestions for making this hole. It needs to have a diameter tolerance of about 5 tenths, locational tolerance of about a thousandth and have a very good finish. I know that "very good finish" is vague, but i dont know well enough to give it an ra. I would say definitely better than what i would get by doing a helical bore with a ball endmill. The mating tapered pin will drop into this hole with about 20oz of pressure and it needs to easily release with absolutely no sticking. To me it seems reaming will be the easiest way to hit these requirements. If its not gonna work, i do have the option of turning this hole on the lathe, but it will be a big awkward fixture and an extra op requiring a lot of setup. I would very much prefer not to do it that way.

    Im also not stuck on the idea of doing it hard, theres a good chance it can be done pre heat treat and keep the necessary tolerance. I can measure the change in heat treat and adjust for that. It would just be better to do afterwards if possible.
    Is this for a Tapered Pin or a Sprue Bush, either you would cut the taper first before heat treating, and lap it with diamond paste to the finished size, sometimes you can find tapered Drills you can use to rough the taper and then use the hand tapered Reamer to finish close to size, heat treat and then lap

    Where to get these Reamers, any Mold making supplies will have what you need if it is a standard Taper, DME is a starting point even Ebay or MSC depending on what you need it for Pin Reamers or Sprue Reamers

    If the Pin gets stuck, you can add an internal thread, or an external thread if you have the room for it, then you can use a removal tool
    Mactec54

  6. #6
    Registered
    Join Date
    Nov 2017
    Posts
    584

    Re: taper reaming

    I didnt really consider lapping since its a taper, but maybe that would be a good option for machining pre heat treat. Keep in mind this is a relatively shallow taper at 10:1. Ive searched all over google including ebay and msc, not finding anything near the angle i need. Everything standard is much steeper. taper pins are about 50:1, i need 10:1.

    This is part of a locking assembly for a folding knife so there needs to be absolutely no sticking. The lock spring tension is about 20oz so theres not much force on it and it needs to release with no more than the 20oz pushing it in. The shallow angle is needed to avoid the sticking. Ive already done a few prototypes of my lock system and it works great. The current design uses flat tapered surfaces but its difficult to get the finish and tolerances needed consistently to avoid lock stick. switching to tapered cylindrical mating surfaces makes it much easier to consistently hit the tolerance and finish needed with minimal hand work, but i didnt foresee it being this difficult to find the tapered reamer needed.

    If i wanted to have a custom reamer made at the angle i need, who would i contact for that?

  7. #7
    Member
    Join Date
    Jan 2005
    Posts
    14302

    Re: taper reaming

    Quote Originally Posted by QuinnSjoblom View Post
    I didnt really consider lapping since its a taper, but maybe that would be a good option for machining pre heat treat. Keep in mind this is a relatively shallow taper at 10:1. Ive searched all over google including ebay and msc, not finding anything near the angle i need. Everything standard is much steeper. taper pins are about 50:1, i need 10:1.

    This is part of a locking assembly for a folding knife so there needs to be absolutely no sticking. The lock spring tension is about 20oz so theres not much force on it and it needs to release with no more than the 20oz pushing it in. The shallow angle is needed to avoid the sticking. Ive already done a few prototypes of my lock system and it works great. The current design uses flat tapered surfaces but its difficult to get the finish and tolerances needed consistently to avoid lock stick. switching to tapered cylindrical mating surfaces makes it much easier to consistently hit the tolerance and finish needed with minimal hand work, but i didnt foresee it being this difficult to find the tapered reamer needed.

    If i wanted to have a custom reamer made at the angle i need, who would i contact for that?
    You would make it yourself.

    If you want no sticking then that in itself will be a challenge, that is the idea of a tapered pin, is to lock parts into place, the less taper you have the harder it will be to remove the pin

    They are normally only made from HSS
    Mactec54

  8. #8
    Registered
    Join Date
    Nov 2017
    Posts
    584

    Re: taper reaming

    yes, an angle similar to a traditional tapered pin would be about impossible to not get stuck, but at 10:1 its about 5 times more taper than that. Again, it will also only be pushed in with hardly over a pound of pressure. I suppose it shouldnt be too hard to make one out of hss. Do you have any recommendations for best choice of tool steel, number of flutes, rake angle, and relief angle? I really have no idea what geometry the flutes should have. I do have a 4th axis setup so i suppose i should be able to do helical flutes if thats much advantage, obviously left hand down cutting flutes.

  9. #9
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    is hard to bit 60hrc with a hss reamer there will be no hrc difference, so may be better to ream before treat

    if you still think of reaming after heattreat, then also the reamer needs to be grinded after heattreat, so if you can make a reamer, then is possible to also skip the reamer and grind the part after heat treat ( you may grind them using a special fixture, or inside your mill with an air spindle ) .... is kind of a loop

    if you consider reaming before heat treat, then why bother to craft a reamer ? material is soft, simply interpolate a conical helix ... or there is no cnc ?

    i can design at least active length, for reference

    I really have no idea what geometry the flutes should have.
    the part is too short, thus L/D ratio is small, so you are more after a rigid taper endmill; such short 'reamers' have an advantage in chucking fixture, thus they rely less on the flutes to be guided inside the hole; once the tool gets longer and chucking gets less rigid, then the reamer needs the flutes to be guided, and in such a case, helix and more flutes will guide better than few straight flutes, but this does not mean that last variant won't work

    obviously left hand down cutting flutes
    why ? kindly
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  10. #10
    Registered
    Join Date
    Nov 2017
    Posts
    584
    Quote Originally Posted by deadlykitten View Post
    is hard to bit 60hrc with a hss reamer there will be no hrc difference, so may be better to ream before treat

    if you still think of reaming after heattreat, then also the reamer needs to be grinded after heattreat, so if you can make a reamer, then is possible to also skip the reamer and grind the part after heat treat ( you may grind them using a special fixture, or inside your mill with an air spindle ) .... is kind of a loop

    if you consider reaming before heat treat, then why bother to craft a reamer ? material is soft, simply interpolate a conical helix ... or there is no cnc ?

    i can design at least active length, for reference



    the part is too short, thus L/D ratio is small, so you are more after a rigid taper endmill; such short 'reamers' have an advantage in chucking fixture, thus they rely less on the flutes to be guided inside the hole; once the tool gets longer and chucking gets less rigid, then the reamer needs the flutes to be guided, and in such a case, helix and more flutes will guide better than few straight flutes, but this does not mean that last variant won't work



    why ? kindly
    yes, of course a hss reamer would not work in 60hrc material. i think you skipped over the post from mactec that i was responding to. hss reamer would be for pre heat treat, then lap afterwards.

    the whole purpose of reaming whether it be before or after heat treat is to get consistent tolerance and good surface finish. a conical helix tool path is obviously not going to give as consistent tolerance or as good of finish as a reamer.

    as for left handed down cutting flutes, because thats the direction they always go on tapered reamers if they arent straight flutes, do they not? if the flutes were right hand, it would grab and pull itself into the hole. same reason why i don't believe a tapered endmill would be good for this either. it will grab and wedge itself down into the hole.

    also i think you missed where i mentioned i am working on an efficient repeatable process for making many of these parts. this is not a one off, so of course spending the time to grind a reamer makes more sense than grinding the part. the reamer will be used many times

    also another thing i should mention, these parts are s45vn stainless that is vacuum heat treated. there is basically no scale and the surface finish is almost not affected. it will basically just go slightly matte and i believe a quick run with lap could clean it up nicely. dimensional change is something i will have to measure and account for. im willing to invest time in this process to make it reliable and repeatable in the long run for many parts

  11. #11
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    a conical helix tool path is obviously not going to give as consistent tolerance or as good of finish as a reame
    depends ... if you interpolare with an air spindle, then surface may be better than using a reamer, but it will take longer

    I do have a 4th axis setup
    this idea just hit me a few seconds ago : if you use the 4th axis tilted, then you may replace the conical helix with an up-down motion for the air spindle, and this will be way faster, and may be even more stable for quantity

    as for left handed down cutting flutes, because thats the direction they always go on tapered reamers if they arent straight flutes, do they not? if the flutes were right hand
    is good to diferentiate between right/left tool(reamer, etc) and s/z helix

    for example, a right hand reamer with z fllutes will bite at front, while with s flutes will 1st make contact at bigger diameter

    difference between s&z is when the cutting edge makes contact in respect to tool/feed position, on circumference; is a phase/360* thing

    tapered endmill
    may i clarify : is not reamer vs endmill, but tool rigidity : reamer are longer, prone to bend, so their active(flutes) lenght is longer, so to stablize during cuttting

    you can have a shorter reamer, but with same flutes lenght, but is poitnless, because, being shorter, it is more rigid, so it can have shorter or less flutes, and still be as stable as the long one

    how your part is short, thus that 1:10 taper is not long, you don't need a long reamer

    let me put it ohter way : if i parameterize the desing of a reamer, it may look as a tough short end-mill

    i think you skipped over the post from mactec that i was responding to
    sorry, i am a bit tired
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  12. #12
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    tilted 4th axis allows simpler toolpath + less complex tooling

    before heat treat, an endmill will blow any reamer in speed and consistency ( at least for some setups )
    after heat thread, you may replace lap with grinding, by using an air spindle + a small stone

    is easier to tilt a 4th axis, than crafting a reamer; also, if you heat treat after reaming, then it seems pointless .... so you need kind of a less precision reamer, so to say, thus a cheaper, less performant reamer

    is that 4th axis cnc ?

    if you wish, check attached / kindly
    Attached Thumbnails Attached Thumbnails Untitled.png  
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  13. #13
    Member
    Join Date
    Jan 2005
    Posts
    14302

    Re: taper reaming

    Quote Originally Posted by QuinnSjoblom View Post
    yes, an angle similar to a traditional tapered pin would be about impossible to not get stuck, but at 10:1 its about 5 times more taper than that. Again, it will also only be pushed in with hardly over a pound of pressure. I suppose it shouldnt be too hard to make one out of hss. Do you have any recommendations for best choice of tool steel, number of flutes, rake angle, and relief angle? I really have no idea what geometry the flutes should have. I do have a 4th axis setup so i suppose i should be able to do helical flutes if thats much advantage, obviously left hand down cutting flutes.
    If the taper needed is short you could, Grind a D-Bit out of carbide to cut the Taper you need
    Mactec54

  14. #14
    Registered
    Join Date
    Nov 2017
    Posts
    584

    Re: taper reaming

    kitten, yes, grinding with air spindle after heat treat would give the ultimate finish and accuracy. Couple issues with that in my case. My 4th will not tilt, i have a custom built mill/turn setup. Its a servo driven horizontal lathe spindle and also vertical bt30 milling spindle. The 2 spindles are always 90 degrees to each other. I could mount air spindle on milling head at the angle needed and feed in and out of taper as a z/x move, but this type of operation just doesnt fit in well with the rest of my production. I am trying to keep this as lean and automated as possible. The assemblies consist of 8 mill parts (7 titanium parts and 1 steel part with the taper in it) and 7 lathe parts (titanium screws). The titanium screws run fully automated out of 1/4" ti bar with bar puller. A 2ft bar makes 80 screws, about a 2hr cycle. probably spend one day per month doing screws, 4 cycles. The mill parts will be loaded on pallets, every part of assembly at once, 4 full assemblies per pallet, 2 assemblies on op 1, 2 assemblies on op 2. About 5 hours per pallet (titanium runs very slow). Every press of cycle start gives 2 completed assemblies of mill parts. There are a couple exceptions to this lean process where i have to do batch work. The screws are one of them. Heat treating of the 1 steel part needs to be done in multiples so i have to stop and heat treat now and then when i build up a pile of parts. One thing that remains true for this whole process is that there is never any setup change. Always the same set of milling tools in tool changer, always same turning tools on gang tool head. All i have to do is load bars, swap pallets, replace worn tools.

    so long story short, i am trying to avoid any specialized type of setups or anything that i have to monitor none stop and load one part at a time. The 5 hour cycle times allow me to concentrate on other tasks like bead blasting, ti anodizing, heat treat, assembly, etc. If i can throw a reamer into my tool changer to become part of the lean automated process, it fits in much better than a specialized process like setting up an air spindle and running one part at a time, then removing it to go back to running pallets. I want to avoid any bottleneck in the process that causes me to have many assemblies that are 99% ready to go and held up by one special process. There have to be exceptions to this, but kept to a minimum. If i have to lap the tapered hole after reaming and heat treat, that would be something i have to be present for and run one part at a time, but it can be a permanent setup on a drill press and very quick to run through a batch of parts after heat treat.

  15. #15
    Registered
    Join Date
    Nov 2017
    Posts
    584

    Re: taper reaming

    mactec, You're probably right. Yes its extremely short, 0.130" deep, 0.25" diameter at top. It would be a very short rigid tool so i probably dont need multi flute stabilization that a reamer would give. It would only need to stick out from holder about 3/8" to clear fixture. I think ill try the D bit.

    deadlykitten, i understand what you mean now by a short rigid "endmill like" tool instead of flexible reamer. I think a carbide D bit as mactec mentions could fit the bill here. Easy to grind, and opens up possibility to do this post heat treat.

  16. #16
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    i onestly, don't know what a D bit is ... please, do you have some infos ? googleing a bit, seems to be a carbide shank, that you grind the way you like ? if so, then simply get a broken 6mm carbide endmill; this D bit tool, you wish to plunge, thus not to interpolate?

    some time ago, i had to deliver atipitcal dimensions, so no standard reamer could fit, so that's when i started crafting reamers; in case you wonder, it was a 6 flutes reamer, cutting 2 diameters at once (6 and 14), so to ensure some concentricity requirement

    but offcourse, your part is too short for a normal reamer
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  17. #17
    Registered
    Join Date
    Nov 2017
    Posts
    584

    Re: taper reaming

    Yep, its ground from a carbide shank, broken endmill works fine. The term D-bit comes from the cross section of how its ground. if looking at the end of the tool, it looks like a "D". The shank is first ground to the taper needed, it is then ground down from the side to the half way point leaving a D shape of material left. Relief can then be ground behind the cutting edge. This makes a single flute tool. Pretty much the same as how you would make a reamer, but more simple because its only one cutting edge and the flute can be ground all the way through the shank. And yes, it would plunge straight in. If the taper was deep, thi would not work well because of tool deflection, but since its 6mm diameter and only a few mm deep, there will be no deflection so single flute should be ok.

    heres what my D-bit tool would be, but no relief ground into it yet. Notice how the end looks like a "D"

  18. #18
    Member
    Join Date
    Jun 2015
    Posts
    3714

    Re: taper reaming

    Pretty much the same as how you would make a reamer, but more simple because its only one cutting edge
    also a reamer can cut only with one flute, or more to one side, especially when chucking is too rigid and prevents the reamer from folowing the hole, or the previous drilled hole is a bit out of cilindricity spec

    The term D-bit comes from the cross section of how its ground.
    k, good luck with your taper; mactec's hint, on those D bits, definitely worth trying
    Ladyhawke - My Delirium, https://www.youtube.com/watch?v=X_bFO1SNRZg

  19. #19
    Member
    Join Date
    Jan 2005
    Posts
    14302

    Re: taper reaming

    Quote Originally Posted by deadlykitten View Post
    i onestly, don't know what a D bit is ... please, do you have some infos ? googleing a bit, seems to be a carbide shank, that you grind the way you like ? if so, then simply get a broken 6mm carbide endmill; this D bit tool, you wish to plunge, thus not to interpolate?

    some time ago, i had to deliver atipitcal dimensions, so no standard reamer could fit, so that's when i started crafting reamers; in case you wonder, it was a 6 flutes reamer, cutting 2 diameters at once (6 and 14), so to ensure some concentricity requirement

    but offcourse, your part is too short for a normal reamer
    A D-Bit is what can take any form you can think up, originally it was the only way to Grind cutters for Engraving
    Mactec54

  20. #20
    Member
    Join Date
    Jan 2005
    Posts
    14302

    Re: taper reaming

    Quote Originally Posted by QuinnSjoblom View Post
    Yep, its ground from a carbide shank, broken endmill works fine. The term D-bit comes from the cross section of how its ground. if looking at the end of the tool, it looks like a "D". The shank is first ground to the taper needed, it is then ground down from the side to the half way point leaving a D shape of material left. Relief can then be ground behind the cutting edge. This makes a single flute tool. Pretty much the same as how you would make a reamer, but more simple because its only one cutting edge and the flute can be ground all the way through the shank. And yes, it would plunge straight in. If the taper was deep, thi would not work well because of tool deflection, but since its 6mm diameter and only a few mm deep, there will be no deflection so single flute should be ok.

    heres what my D-bit tool would be, but no relief ground into it yet. Notice how the end looks like a "D"
    It will depend how much back relief as to how stable it will be when cutting you may have to experiment with the back relief to get it perfect
    Mactec54

Page 1 of 2 12

Similar Threads

  1. Replies: 25
    Last Post: 04-28-2014, 10:19 PM
  2. manual tnc taper radius taper
    By bookwurm99 in forum G-Code Programing
    Replies: 3
    Last Post: 04-25-2014, 07:57 AM
  3. Difference in Female Taper angle using Taper Cutter
    By Buntron in forum General Material Machining Solutions
    Replies: 5
    Last Post: 06-07-2011, 06:53 AM
  4. Reaming Ti ?
    By Sprew in forum General MetalWork Discussion
    Replies: 5
    Last Post: 06-29-2007, 08:41 PM

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
  •