3dprintforums logo

CNCzone Network:  RFQwork :: 3Dprintforums :: Welderzone :: Google+ :: Our Facebook :: Twitter :: SiteMap



Page 5 of 6 FirstFirst ... 23456 LastLast
Results 49 to 60 of 67

Thread: I hate reamers!

  1. #49
    Quote Originally Posted by handlewanker View Post
    The amount of material left for reaming is the least the better, because the reamer has more flutes than a drill and cuts a small amount on the top corner of each one.
    This is from Kennametal, note the bit about material to leave:
    Often, we are asked for advice to recommend a drill size that will leave an appropriate amount of material for the reamer to efficiently size the finished hole. Those general guidelines are <1/4" = .010; " to " = .015 and " to 1-1/2" = .025
    Most leave too little, thinking it will be easier for the reamer to remove the material, but that does not give the reamer enough material to really cut and will rub or burnish and results in faster wear and poor finish.

    Speeds should be about 2/3 that of drilling SFM for similar material and feeds 2 to 3 times higher

    Qualified reamers:
    Perhaps the word "Qualified," in and of itself, truly reflects what we need to know about the tool.
    "Qualified for Rotation" means that the diameter of the shank and the O.D. of the reamer head run concentric to each other within .0002 (typically .0001) with less than .00005 taper. These characteristics lend themselves to the best angular and radial alignment of the reamer, no matter the application.

    We can use qualified reamers to great advantage in both rotating and stationary applications. Any time you are utilizing the shank diameter to align the tool in a high tolerance diameter or finish application, the tools should be qualified. If one does not request a qualified reamer, there is potential for angular as well as radial misalignment that you cannot correct at the spindle. This situation is most evident in lathe applications utilizing the "Barber Coleman" up-sharp" style reamer with the pin float hole in a conventional ER style collet chuck. These tools are designed to be run with a pin float holder, the tolerance is put into the cross hole with respect to angular alignment, not in the diameter of the shank. The shanks are ground for clearance in the float. It is important to note that a qualified tool runs equally as well in a pin float holder. An un-qualified tool may or may not run well in an ER collet style holder.

    When ordering, if you need "Qualified" tolerances, you will need to specify that in your request.
    Chucking Reamers typically hang out of hydraulic chucks, collet chucks, end mill holders, and even three jaw chucks in some cases. If you are using a hydraulic chuck, they require metric h6 shank tolerance.

    http://www.1dropdesign.com


  2. #50
    Gold Member dertsap's Avatar
    Join Date
    Oct 2005
    Location
    canada
    Posts
    3972
    Downloads
    0
    Uploads
    0
    Rep Power
    12
    reaming sounds far to complicated and technical , i think i'll stick to plunging endmills where applicable

    A poet knows no boundary yet he is bound to the boundaries of ones own mind !! ........
    http://microcarve.microcarve.biz/


  3. #51
    Registered handlewanker's Avatar
    Join Date
    Sep 2006
    Location
    Australia
    Posts
    3453
    Downloads
    0
    Uploads
    0
    Rep Power
    11
    Hi all, if you balk at reaming, try this dodge, take a slot drill and GRIND one of the flutes back a bit, that is the side and end of one flute so that only the other flute cuts.

    What you have is a very rigid hole boring tool that is a set diametre and depending on your holder will cut the same diametre every time.

    To sharpen you just regrind the end face only, not the side, unless you want to cut a special diam hole.

    It's not a patch on a proper reamer set-up, but you can rely on it whenever you want to put a hole in a certain position that is a required size, without having to set up a boring head etc, only limited by the length of the slot drill unless you go to a long series slot drill.

    So if you wanted a 1" hole dead to size you just centre drill and drill with the other drills to open the hole to 1/64" undersize and use the slot drill dodge to get the hole to size first time, saves a lot of time and measuring to get to size.

    I had a couple of them of different sizes, that I kept in my box, so that they were always available but more importantly sharp and ready for use.

    BTW, you can use this method to ensure that the hole is dead true to POSITION prior to reaming by using the prepared slot drill to cut a starting land at the top of the hole about 1/16" deep then the reamer will follow this true to position starting diam as it cuts the rest of the hole
    Ian.



  4. #52
    Gold Member dertsap's Avatar
    Join Date
    Oct 2005
    Location
    canada
    Posts
    3972
    Downloads
    0
    Uploads
    0
    Rep Power
    12
    with oddball diameters you can use the same idea and make an eccentric split sleave the cutter can fit into , works great for runs that you don t want to tie up a boringhead or take the time to search for a bastard sized reamer

    A poet knows no boundary yet he is bound to the boundaries of ones own mind !! ........
    http://microcarve.microcarve.biz/


  5. #53
    Banned
    Join Date
    Jan 2006
    Location
    Seattle
    Age
    54
    Posts
    883
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    Another way is to use Helical interpolation to bore a hole with an end mill.



  6. #54
    Registered handlewanker's Avatar
    Join Date
    Sep 2006
    Location
    Australia
    Posts
    3453
    Downloads
    0
    Uploads
    0
    Rep Power
    11
    Hell of an interpretation, LOL, yeah OK if you have CNC with totally zero back lash in the X & Y axis and the bore isn't too deep.

    I reckon the eccentric sleeve method would work OK if a boring head wasn't available, and once set it would bore the same size each time.

    I think to make it work well the sleeve would want to stick out of the collet a bit and have two flats on it to allow rotating while holding the cutter still.
    Just rotating the cutter only would throw the point geometry out.

    You could get quite a big bore size range variation if you used the biggest collet size, say an ER 40 type holder, or an Autolock chuck, 1" cutter size, and a 1/2" diam boring bar.
    Then the eccentric bush could have an offset of about 1/4" giving you a 1/2" bore size variation.

    As there are no graduations, it would be better to adjust it using a dial indicator to show the amount of offset as the sleeve is turned while holding the boring bar still.

    It's the boring head you have when you don't have a boring head.
    Ian.



  7. #55
    Registered
    Join Date
    Apr 2008
    Location
    USA
    Posts
    2
    Downloads
    0
    Uploads
    0
    Rep Power
    0

    Reaming is a snap

    Hold on with all these reaming problems, I just happen to be looking for some other info on this site and came across this thread.

    I donít want to step on anybodies ideas about reaming -v- boring, because there is more than one way to skin a cat and what will work for one guy may not work for the next.
    In fact you can set up two identical machines cutting the same materials with the same coolant, SFM and load and get different results. Reaming in most cases will out produce a single point boring tool, I donít care whose boring tool. I have a little experience in the arena of drilling and reaming holes, I will not mention the name of the company I work for but I have been doing nothing but helping people with drilling and reaming problems for the past 10 years and was a machinist for 11 years before doing what I am doing now.

    The material amount left will determine the outcome of your reamed and or bored hole.
    Not all reamers have Odd number of flutes, many have even numbers. What may be more important is the degree of the pitch or if the flutes are variable pitch, you usually only find this in higher end tools. What I mean is that if you have 6 flutes they will not all be 60 degrees apart. Most manufactures will make them even distance.
    Donít be afraid to push your reamers, HSS, brazed or solid carbide a reamer donít like to be babied, check with your manufacture for the correct SFM and advance per rev. because not all are the same. If you had a tooling salesman sell you the tool have them help you out, if they canít get in touch with the factory rep. Keep in mind the length of the tool will greatly effect the performance of the tool, the longer the slower SFM.
    In the event the reamer squeals slow the SFM down put keep pushing the tool at the same IPR, so to keep it relevant, donít just slow down the spindle and not change the ipm. Depending on your controller you may have to recalculate the IPM (rpm x ipr) (1000 x .010 = 10ipm)
    Your reamer will only locate as accurate as the hole it is going into so if you need to be tight, center drill, and drill then ream.
    TIR is important especially in higher end carbide, Cermet, PCD, or CBN reamers it is very possible to destroy your tool life or even the tool. Depending on the material I often can achieve 10,000 plus hits multiple inches deep. But the TIR must be less than .0005Ē thatís TOTAL indicator run out, (+.0002 on one flute -.0003 on another) thatís .0005.
    You always want to check this in the machining center not just a pre-setter.
    Coolant is another very important factor, full synthetics are tough, you can use them but they tend to offer more cooling properties than lubrication.
    Semis are pretty good but you will need to keep them at about 7-10 percent on the refractometer depending on the material, keep it high for Aluminum and Irons..
    I could go on but most of the time addressing the above will take care of most reaming problems. Good luck.






    Quote Originally Posted by handlewanker View Post
    OK, OK, hole size it is, the reamer WILL give you a hole to size every time, just where that hole is is another issue.

    The fact is to make a hole say for argument sake 1.000" diam you will need a reamer that is a certain amount UNDERSIZE, because if the reamer is exactly 1.000" diam it will cut OVERSIZE.

    You cannot get a 1.000" diam shaft into a 1.000" diam hole, unless you want a press fit, commonly known as "size for size".

    The amount of material left for reaming is the least the better, because the reamer has more flutes than a drill and cuts a small amount on the top corner of each one.

    One reason a reamer cuts round and true is because it has an UNEVEN number of flutes whereas the drill has two, and on it's downward passage the drill will hack into the wall of the hole as each cutting lip pushes against the opposite one.

    This is a broad reason why a single point tool well supported against deflection will cut a true circle about it's axis, and also the uneven number of flutes on the reamer cancel out any point activity that would otherwise deflect it.

    One reason we resort to a reamer for final finishing is that it will give a smooth hole as the sides of the flutes burnish the hole after the top corners have cut it to size.

    Woe to anyone who reams with a blunt reamer because it gives a polished hole, the load on that poor tool is near breaking point.

    Unless you want a polished hole it is better, if you can measure it to just finish the hole with the boring head, given that you are able to get to within .002", and you won't have to move the table up and down on the knee to get the height.
    Ian.




  8. #56
    Registered
    Join Date
    Apr 2008
    Location
    USA
    Posts
    2
    Downloads
    0
    Uploads
    0
    Rep Power
    0
    Check TIR in the machine with a Tenths indicator, use a brass hammer, put your finger on the low side of the TIR and tap as close as you can to the collet on the shank of the reamer on the high side,
    don't hit it too hard because it will move, this is called tapping your tool in.
    Your collet nut could be bad also, try to use a new or newer one that has a true bearing on the surface that contacts the collet.
    Good luck. Reaming is not a difficult process. Leave enough material run about 2/3 the SFM of drill and don't be a chicken, push it.



  9. #57
    Gold Member dertsap's Avatar
    Join Date
    Oct 2005
    Location
    canada
    Posts
    3972
    Downloads
    0
    Uploads
    0
    Rep Power
    12
    as was meantioned ,there is more than one way to skin a cat ,

    i agree with Schvwartzeboy about using manufacturer specs
    reaming shouldnt be and isn t a difficult task ,if one doesn t work then turf it and buy a new one , its one of the simplest ways to accomplish an decently accurate sized hole with a mediocre finish , it is not the most efficient and has the potential for the odd disaster during production runs due to the odd chip being picked up , under production jobs the best suited types of tools would be tools that are comparable to kennametals tx drills or production tools of the sort ,which will drill and ream with an exceptional finish and dead nuts accuracy

    typically when deciding what tool to use and what tool to buy should be determined by how many holes and how many parts need to be done ,then the price of the tooling can be justified
    sometimes its just a matter of drilling a hole and chasing it with the proper sized drill , if it works and complies with drawing specs then its good enough

    Last edited by dertsap; 04-24-2008 at 03:31 PM.
    A poet knows no boundary yet he is bound to the boundaries of ones own mind !! ........
    http://microcarve.microcarve.biz/


  10. #58
    Registered
    Join Date
    Jun 2007
    Location
    USA
    Posts
    72
    Downloads
    0
    Uploads
    0
    Rep Power
    7
    I need a bit of help - Im getting a tapered hole while reaming, with the large side of the taper on the back end of the piece.

    The part: 303 stainless

    The sequence: c'drill, drill thru .250, chamfer, ream .2555" x 1.1" deep (thru).

    The tool: 4flute carbide tipped reamer, held about 4" out of the tool holder

    I have tried a variety of speeds/feeds, although suggestions here are welcome.

    I am going to continue to fiddle around, adjusting the length and checking whatever i can think of, but im hoping for some good suggestions here.

    What can cause a reamer to cut a tapered hole, to size on the entry side and oversize on the exit side?



  11. #59
    Registered
    Join Date
    Jan 2005
    Location
    SoCal
    Age
    73
    Posts
    224
    Downloads
    0
    Uploads
    0
    Rep Power
    10
    Smrtman5 - usually the reason the bottom is bigger dia
    is from chip buildup in the reamer flutes.
    Have you checked to see if all flutes are cutting equally?

    About 1/4-1/2 the drilling rpm is best for reaming.
    (& 2-4x the ipm).

    Trying to minimize the stringy type chip buildup from
    stainless is the main problem.

    Sometimes a chipbreaker (step/notch) in each tooth is necessary to minimize the stringy nature of machining stainless.

    Hth,
    Pres



  12. #60
    Registered
    Join Date
    Jun 2007
    Location
    USA
    Posts
    72
    Downloads
    0
    Uploads
    0
    Rep Power
    7
    Chip buildup was my suspicion.

    I put in a floating tool holder and started getting a taper on the front of the part instead of on the back.

    Maybe i should put the rigid holder back in and try again with that...idk.

    Got the reamer running at 300rpm / .011in/rev half way into the part then 600rpm / .011in/rev through the other half. This is eliminating the tapered mouth and gets me 12 seconds faster than the boring bar we were previously using.

    Still not entirely happy with the performance tho, any other ideas?



Page 5 of 6 FirstFirst ... 23456 LastLast

Posting Permissions



About CNCzone.com

    We are the largest and most active discussion forum from DIY CNC Machines to the Cad/Cam software to run them. The site is 100% free to join and use, so join today!

Follow us on

Facebook Dribbble RSS Feed