reaming holes on the cnc mill (can of worms open) - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 57
  1. #21
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    3,332
    Post Thanks / Like
    Likes (Given)
    1405
    Likes (Received)
    4350

    Default

    I can offer a few pointers.
    A lot is going to depend on what the hole is for, sowel pin, bearing, piston? Lets say we're doing a dowel pin hole where we want a tight diameter tolerance and tight positional tolerance. It's also going to depend a lot on the condition of your machine. IF it's relativly new and tight, you should be able to interpolate quite accurately. A little beat up and worn, you may ned to use uni-directional positioning.
    Also, you need to consider the condition of your reamer. Is it sharp? Did someone in the past attempt to hone it down and ruin it? You'll notice a 45 deg chamfer on the end of the reamer. This is probably the most important feature on the reamer. Make sue it's clean and unchipped.
    So, step one is to drill a pilot hole, in your case I would go about .232 dia. Spot drill it first and leabe about a .270 dia chamfer.
    Then, bore it .008/.010 undersize. If you have a grinder, you can spin down a 1/4 em, or you can buy what's called a pre-ream end mill.
    Last step is to ream it. Indicate the reamer in. It's got to run true. A lot of people run reamers way too fast on rpm and way too slow on feed. For a 1/4" in aluminum, I'd go 500 rpm and 5 ipm. As far as reamer size, go with the saize you want. Don't expect it to cut o/s. Coolant works just fine, but you will find cutting oil will make the hole a wee bit bigger. On a dowel pin hole, I would rapid out, however this can leave a mark on the finish. If it were a piston bore, I would feed out.
    Hope this helps. As with anything else, shortcuts are not your friend.

  2. Likes mhajicek, Kiwi2wheels liked this post
  3. #22
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    9,661
    Post Thanks / Like
    Likes (Given)
    16372
    Likes (Received)
    11768

    Default

    This may sound stupid, but here is one little trick I use when reaming.

    Ever notice that on occasion, the top of the hole ends up a little big
    for whatever reason. Floppy casting for example, where its not supported
    well at all...

    So if I have to face the material, I'll drill/ream first,
    then face, that way if the top of the hole is tick big, its getting turned
    to chips anyways.

  4. Likes Chris Attebery, mountie liked this post
  5. #23
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,411
    Post Thanks / Like
    Likes (Given)
    1391
    Likes (Received)
    1512

    Default

    Being cheap, for something like this I would get a .2500 HSS reamer and "adjust" it to size with a stone. Hold it in a collet, indicate it in for tir, and document all of the parameters used to get an on size hole in your test pieces. If you need to ream these holes again do not ever assume it will ream the size hole you expect, always confirm with sample holes in scrap before trying to make good parts. Learning how to "adjust" reamers with a stone is a good skill to have. It's not hard and you will grind on the reamer a lot more than expected to change its size.

  6. Likes Bobw liked this post
  7. #24
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,531
    Post Thanks / Like
    Likes (Given)
    1878
    Likes (Received)
    1566

    Default

    put some material in the vise, get some drill and reamers and experiment, that's what I do, it's not so hard.

    I would drill C or D drill dias first then ream and gage the size. I would use a ream cycle. I guess you could use a drill cycle but I've never tried that.

    One thing a friend of mine does is to ream .001-.002 undersize then ream to finish size, he says he gets more consistant hole sizes that way.

    I guess your next question is going to be "how do I measure the dia?" Deltronic pins

  8. Likes vegard liked this post
  9. #25
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,531
    Post Thanks / Like
    Likes (Given)
    1878
    Likes (Received)
    1566

    Default

    imho circular interpolating that hole your only going to get a round hole on a small percentage of machines, you might get a hole where a .2495 pin goes in, and a .2501 pin doesn't but is it round?

    My assumption is if a customer calls out a reamed hole he wants it nice and round. Using a reamer, not circular interpolated. On a very tight machine, the advantage with circular interpolation is the position is likely going to be more accurate than if you start with a drilled hole and then reamed.

    On the other hand none of my customers would know the difference between a reamed and interploated hole, as long as it's in the right place and size feels right their ok. None of them have the capability of measuring the hole size anyway.

  10. Likes Bobw liked this post
  11. #26
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    140
    Likes (Received)
    48

    Default

    After doing a lot of research, I found a lot of answers to my questions. I hope other people find this helpful. They are the following:

    1. Always indicate the reamer in. If the reamer is indicated in good enough to where it is concentric with the spindle, you probably don't need to use a floating holder in a mill. Sometimes a reamer will squeal a little bit at the top of a hole with a floating reamer holder because it is finding center. ALWAYS INDICATE IT IN. If your spindle runs out or you are reaming in a lathe and you cannot get the reamer indicated in, use a floating holder so the reamer can find center. If you are not using a floating holder, try to use a collet that runs true instead of a drill chuck. It depends on your tooling, but typically collets will run truer then your drill chuck.

    2. You can use coolant or oil or viscous tapping fluid. Opinions do vary on this matter and is a debated subject. Make sure your coolant is concentrated enough though and that you keep the part and reamer cool to get consistent hole sizes. Some reamers are made to accept thru coolant. Again, this is a debated issue between oil vs coolant vs viscous tapping fluid and which one produces finer holes when reaming. Try doing all three and see what works for you. Me, personally, I see better results using oil with other things (such as using a boring bar on a close ID). Again, try both oil and coolant to see which works best for you.

    3. On the mill, use a G86 drilling cycle (opinions vary), but the majority of people seem to have the best luck with a G86 cycle. This cycle feeds to the bottom of the hole, turns the spindle off, and rapids out. Other people like to use G81 (standard drilling cycle), G85 (feed into the hole and feed out of the hole at same speed, and G76 (feed to bottom of hole, oriented stop, and rapid out of hole) but it seems like G86 gives the best results for hole size and surface finish and is the most popular.

    4. The rule is to leave 2%-3% to be reamed. For example, if I want to ream a .500" hole, leave .010"-.015" for the reamer to remove. A .250 reamed hole would leave .005 - .0075". Don't leave too much material as this will overload the reamer and break it/cause premature wear. Also don't leave too little material as this will burnish and scar the hole somewhat. 2-3% material left is the rule according to the guide I attached and other sources.

    5. If you have a thru hole, a left spiral reamer will push the chips out of the hole and will leave the best finish out of all the machine/chucking reamers. For a blind hole, use a right spiral reamer and/or straight fluted reamer to pull the chips up out of the hole. DO NOT USE A LEFT SPIRAL REAMER FOR A BLIND HOLE. A straight fluted reamer is ideal for short chipping materials like brass, cast iron, etc. Flutes for reamers are similar to flutes of taps (i.e. spiral flute tap pulls chips out of hole, gun tap pushes chips through the hole, straight flutes taps is for short chipping material). You want to have the best chip evacuation possible so you do not oversize the hole, overload the reamer, and leave the best surface finish possible.
    Note: spiral reamers should also be used if the hole your cutting has some kind of interrupted cut (such as a keyway in the hole). DO NOT use a straight flute reamer for a hole that has an interrupted cut and/or keyway.

    6. To start the job, do what you always do when drilling: spot/center drill, & drill. If you want a reamer to run dead nut, run an endmill through the hole to straighten it out before running a reamer through the hole, since a reamer follows whatever hole is already there. A reamer will follow a straight hole and/or a crooked hole. Make sure the hole is straight before running the reamer through. If you don't want to run an endmill through before the reamer, try indicating your drill in so the drill creates a straight hole that the reamer can follow. Remember, a carbide drill/reamer will cut straighter and leave a more precise hole than a hss/cobalt drill/reamer so try using carbide before reaming (since carbide is so much stiffer since it has a much higher Young's modulus than HSS/cobalt).

    7. Always countersink your hole before reaming. This helps start the reamer and removes any burr at the top of the hole that may deflect the reamer and/or cause a bell mouthed hole and cause poor surface finish.

    8. DO NOT PECK THE REAMER

    9. Always get speeds and feeds for your reamer from the manufacture's website. Speeds and feeds do depend on the material you are cutting, whether the reamer is made of carbide or HSS/cobalt, the number of flutes of the reamer, and the depth of the hole. Manufacturers do seem to overestimate their speeds and feeds, so always start at the low end of their recommendations. Having the incorrect speeds and feeds will leave poor surface finish and can oversize your hole.

    10. If you have a hole with a tolerance (such as .2496 -.0001 +.0004), buy the .2495 reamer so it gives as much room as possible in case the reamer cuts oversized.

    11. Try to pay close attention to the manufacture's reamer tolerance. Some manufacturers have a closer tolerance on reamers than others. Pay attention to this. Which one you buy depends on how close your hole has to be and your own budget.

    12. If your setup is good and your doing everything right and your hole is oversize, try stoning the cutting edges of your reamer. Sometimes the reamer is too sharp from the factory and there can be a little bit of "fuzz" on the reamer from the manufacturing process.

    13. Use the shortest reamer possible. Runout multiplies rapidly as the distance from the spindle increases.

    14. When buying a reamer, try to get the most flutes possible within your budget.

    This is the kind of info I was really looking for. If you have something I missed, please let me know.

    Thanks,

    Chris

  12. #27
    Join Date
    May 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    2,925
    Post Thanks / Like
    Likes (Given)
    289
    Likes (Received)
    1609

    Default

    Quote Originally Posted by cgrim3 View Post
    Greg White and plastikdreams....thank you for the rude responses. No need for that here. As you can see from my first opening post, I am trying to get the details, since the devil is in the details. Yes....I can take a reamer and just plow it through no problem. In fact, I did this very thing on 20 parts last week on the lathe and the holes turned out good. But if you read my opening post, I am trying to gage the processes of everybody here on PM since there is a ton of conflicting information on how to actually go about it. Yes I have successfully reamed quite a few holes. But I want to get to the bottom of the PROPER way to do it.

    Is this such a bad thing? Remember, you catch more flies with honey, not vinegar.
    I wasn't trying to be rude, just nudging you along.

  13. Likes Greg White liked this post
  14. #28
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    140
    Likes (Received)
    48

    Default

    You're all good man. To know what kind of detailed info I was really looking for, see my post above. After some reading of sources online, I wrote the post above to help out others who might be in the same boat as me. I hope you find it useful too.

    Chris

  15. #29
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    3,411
    Post Thanks / Like
    Likes (Given)
    1391
    Likes (Received)
    1512

    Default

    Your list is pretty good. The one thing I would stress is to spend several hours playing with it to learn for yourself what matters and by how much. Once you figure out what works, WRITE IT DOWN, don't leave it to memory. Every little detail matters. Don't underestimate sizing your reamer by stoning 45 degree bevels on the cutting edges, which is my MO, or running the reamer backwards rubbing a stone on it to size it, which I haven't tried yet. I don't think stub vs long reamer matters at all, as long as they are indicated in. ER collets work great for this since they are not as good as shallower single angle collets.

    There are many ways to size a reamed hole, but some are less consistent than others.
    1 - Feed rate, I like .001"-.002" chipload per tooth.
    2 - Spindle speed, I like 40-60% of drill.
    3 - How much material you leave for the reamer. I like .002"-.004" per side. I "think" this gives you more consistent size on the reamed hole. This I do like to circular interpolate. Harvey 5 flute mills for aluminum are the best for this that I know of, super stiff cores.
    4 - Feed in rapid out or feed in feed out depends on your machine, play with it. I like feed in feed out @ 200% feedrate.

    Like feed and speed recommendations from the tool manufacturer, these are only "starting" points, experiment to figure out what works and matters for your set up. Absolutely play with speeds, feeds, and trim stock, this is easy to do and will make small differences.

  16. Likes cgrim3 liked this post
  17. #30
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,531
    Post Thanks / Like
    Likes (Given)
    1878
    Likes (Received)
    1566

    Default

    Once in a while you find the perfect reamer, cooks, cleans, takes out the trash etc. Reamers can be like wives, takes a few to find the right one.

    I have a few reamers I use for tight slip fit holes for fixturing, they've been in the toolholders for a few years, they work so well I don't want to take them out. I can't remember what nominal size they are, but whatever it is, their perfect. I also use the same size drill and speeds/feeds, so as best I can I replicate an op that works well.

  18. #31
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    530

    Default

    going to take a wild guess this is a press fit for a 1/4 dowel pin.

    Spot drill the hole first, then use a .238 or .242 drill, then ream the hole. Pretty simple.

  19. Likes Greg White liked this post
  20. #32
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,677
    Post Thanks / Like
    Likes (Given)
    280
    Likes (Received)
    1895

    Default

    Oh, I remember another thing. Reamers tend to be supplied very long. If you only have 1" or so in the collet, it'll sing like a tuning fork and is much more likely to chatter and cut wonky. Choke up on it, then indicate it carefully.

    Regards.

    Mike

  21. #33
    Join Date
    Oct 2014
    Country
    CANADA
    State/Province
    Ontario
    Posts
    175
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    95

    Default

    So much hypothesizing for a relatively simple hole .

    Drill with a 6mm or 15/64" stub carbide drill, chamfer, followed by a stub .2496/.2497 carbide reamer. Since you're cutting aluminum, I'd start around 1000rpm/10ipm and play around from there depending how fast you want to get the job done.

  22. Likes Greg White, toolsteel liked this post
  23. #34
    Join Date
    Jan 2007
    Location
    Pinckney Mi.
    Posts
    3,066
    Post Thanks / Like
    Likes (Given)
    7835
    Likes (Received)
    908

    Default

    I have NEVER indicated a flipping reamer.
    I use the the full lenght of the shank as a flex o meter ,it will follow the bored/stabbed hole if one pushs it hard enough,reamers are for making size,NOT location.
    The write up above sounds like a tenth grade report.
    And again,dead spindle retract,so as ya aint spinnin chips on your nice finished hole, or maybe I should turn in my Tool&Diemakers card,and recall the 100,000 reamed holes I shipped?
    Or maybe they just dont make reamers like they did 50 years ago??? or people who use em.
    Sir, with all due respect,you come on here with a question,then the end all answer?
    Hey ,call me digger Doug,but I dont get it.
    Peace
    Gw
    P.S,
    mite be the ft of snow I ama lookin at here,
    I checked my Wheatys,nothun in em.

  24. Likes Shawnrs liked this post
  25. #35
    Join Date
    Dec 2020
    Country
    UNITED STATES
    State/Province
    Maryland
    Posts
    241
    Post Thanks / Like
    Likes (Given)
    140
    Likes (Received)
    48

    Default

    Greg White, in case you actually read my posts, after doing a lot of searching and reading online on the proper way to do it, I posted the answers so in case anybody had the same questions as me, they could refer to it. I came here for help and almost nobody was willing to help me at first, and a lot of people just acted cocky. Is that really the right thing to do? Wasn't this forum designed to be a resource people can come to for help? So enlighten me, what I exactly am I doing wrong here?

    More skilled people really don't want to help the younger people (I am in my early 20s) who are newer to the trade? How is this a good thing? The post I made above has a lot of very good information. I just graduated college and am looking for as much information as possible so I can learn. Is that such a bad thing? People like you ruin for me and everybody else. You are nothing more than a troll on this forum.

    Thank you for the cockiness and arrogance you provided Practical Machinist. If you are going to act like a school child, then there is no place for here on this forum. In fact, they teach you NOT to act that way in Kindergarten. Please leave this thread and do not come back.

  26. Likes Greg White liked this post
  27. #36
    Join Date
    Jun 2006
    Location
    Near Seattle
    Posts
    5,261
    Post Thanks / Like
    Likes (Given)
    3864
    Likes (Received)
    1596

    Default

    Alright, I'm going to side with cgrim3 on some of this - if it's "so simple" how come it often produces bizarre results? (Holes physically smaller than the tool that just went through them....)

    Also, reamers are long, on purpose, to give them flex - they're suppose to follow the hole and correct it's size and roundness. When folks say to manage the TIR, that makes some sense, but the whole point of the long shaft is let the reamer float to where the hole actually is. Whatever works.

  28. Likes primeholy liked this post
  29. #37
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    530

    Default

    Quote Originally Posted by Rapid_Tech View Post
    So much hypothesizing for a relatively simple hole .

    Drill with a 6mm or 15/64" stub carbide drill, chamfer, followed by a stub .2496/.2497 carbide reamer. Since you're cutting aluminum, I'd start around 1000rpm/10ipm and play around from there depending how fast you want to get the job done.
    You don't need a carbide reamer for aluminum.

  30. #38
    Join Date
    Oct 2014
    Country
    CANADA
    State/Province
    Ontario
    Posts
    175
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    95

    Default

    Quote Originally Posted by Shawnrs View Post
    You don't need a carbide reamer for aluminum.
    Damn, I've been doing it wrong all this time! I though high speed steel was only for ferrous and carbide for non-ferrous materials. Can you tell me if this is wrong?

  31. #39
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    530

    Default

    Quote Originally Posted by Rapid_Tech View Post
    Damn, I've been doing it wrong all this time! I though high speed steel was only for ferrous and carbide for non-ferrous materials. Can you tell me if this is wrong?
    I would not say you are doing it wrong, I just said you don’t need a carbide reamer for aluminum. I have used carbide reamers, endmills for reaming aluminum. I have spiral cut .250 press fit and slip fit holes with 3/16 endmills. I circular interpolated holes with endmills and even use G13 in a haas for a tight tolerance in the past. in this application I find that using a high speed reamer work fine. It is much cheaper than the carbide tooling for the application the OP was mentioning. I thought I read he was reaming 4 holes originally.

  32. #40
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    928
    Post Thanks / Like
    Likes (Given)
    176
    Likes (Received)
    530

    Default

    N
    Quote Originally Posted by cgrim3 View Post
    After doing a lot of research, I found a lot of answers to my questions. I hope other people find this helpful. They are the following:

    1. Always indicate the reamer in. If the reamer is indicated in good enough to where it is concentric with the spindle, you probably don't need to use a floating holder in a mill. Sometimes a reamer will squeal a little bit at the top of a hole with a floating reamer holder because it is finding center. ALWAYS INDICATE IT IN. If your spindle runs out or you are reaming in a lathe and you cannot get the reamer indicated in, use a floating holder so the reamer can find center. If you are not using a floating holder, try to use a collet that runs true instead of a drill chuck. It depends on your tooling, but typically collets will run truer then your drill chuck.

    2. You can use coolant or oil or viscous tapping fluid. Opinions do vary on this matter and is a debated subject. Make sure your coolant is concentrated enough though and that you keep the part and reamer cool to get consistent hole sizes. Some reamers are made to accept thru coolant. Again, this is a debated issue between oil vs coolant vs viscous tapping fluid and which one produces finer holes when reaming. Try doing all three and see what works for you. Me, personally, I see better results using oil with other things (such as using a boring bar on a close ID). Again, try both oil and coolant to see which works best for you.

    3. On the mill, use a G86 drilling cycle (opinions vary), but the majority of people seem to have the best luck with a G86 cycle. This cycle feeds to the bottom of the hole, turns the spindle off, and rapids out. Other people like to use G81 (standard drilling cycle), G85 (feed into the hole and feed out of the hole at same speed, and G76 (feed to bottom of hole, oriented stop, and rapid out of hole) but it seems like G86 gives the best results for hole size and surface finish and is the most popular.

    4. The rule is to leave 2%-3% to be reamed. For example, if I want to ream a .500" hole, leave .010"-.015" for the reamer to remove. A .250 reamed hole would leave .005 - .0075". Don't leave too much material as this will overload the reamer and break it/cause premature wear. Also don't leave too little material as this will burnish and scar the hole somewhat. 2-3% material left is the rule according to the guide I attached and other sources.

    5. If you have a thru hole, a left spiral reamer will push the chips out of the hole and will leave the best finish out of all the machine/chucking reamers. For a blind hole, use a right spiral reamer and/or straight fluted reamer to pull the chips up out of the hole. DO NOT USE A LEFT SPIRAL REAMER FOR A BLIND HOLE. A straight fluted reamer is ideal for short chipping materials like brass, cast iron, etc. Flutes for reamers are similar to flutes of taps (i.e. spiral flute tap pulls chips out of hole, gun tap pushes chips through the hole, straight flutes taps is for short chipping material). You want to have the best chip evacuation possible so you do not oversize the hole, overload the reamer, and leave the best surface finish possible.
    Note: spiral reamers should also be used if the hole your cutting has some kind of interrupted cut (such as a keyway in the hole). DO NOT use a straight flute reamer for a hole that has an interrupted cut and/or keyway.

    6. To start the job, do what you always do when drilling: spot/center drill, & drill. If you want a reamer to run dead nut, run an endmill through the hole to straighten it out before running a reamer through the hole, since a reamer follows whatever hole is already there. A reamer will follow a straight hole and/or a crooked hole. Make sure the hole is straight before running the reamer through. If you don't want to run an endmill through before the reamer, try indicating your drill in so the drill creates a straight hole that the reamer can follow. Remember, a carbide drill/reamer will cut straighter and leave a more precise hole than a hss/cobalt drill/reamer so try using carbide before reaming (since carbide is so much stiffer since it has a much higher Young's modulus than HSS/cobalt).

    7. Always countersink your hole before reaming. This helps start the reamer and removes any burr at the top of the hole that may deflect the reamer and/or cause a bell mouthed hole and cause poor surface finish.

    8. DO NOT PECK THE REAMER

    9. Always get speeds and feeds for your reamer from the manufacture's website. Speeds and feeds do depend on the material you are cutting, whether the reamer is made of carbide or HSS/cobalt, the number of flutes of the reamer, and the depth of the hole. Manufacturers do seem to overestimate their speeds and feeds, so always start at the low end of their recommendations. Having the incorrect speeds and feeds will leave poor surface finish and can oversize your hole.

    10. If you have a hole with a tolerance (such as .2496 -.0001 +.0004), buy the .2495 reamer so it gives as much room as possible in case the reamer cuts oversized.

    11. Try to pay close attention to the manufacture's reamer tolerance. Some manufacturers have a closer tolerance on reamers than others. Pay attention to this. Which one you buy depends on how close your hole has to be and your own budget.

    12. If your setup is good and your doing everything right and your hole is oversize, try stoning the cutting edges of your reamer. Sometimes the reamer is too sharp from the factory and there can be a little bit of "fuzz" on the reamer from the manufacturing process.

    13. Use the shortest reamer possible. Runout multiplies rapidly as the distance from the spindle increases.

    14. When buying a reamer, try to get the most flutes possible within your budget.

    This is the kind of info I was really looking for. If you have something I missed, please let me know.

    Thanks,

    Chris

    Just curious, for a person that does not have a lot of experience in reaming holes you seem to put a lot of information in this thread 1 day later on reaming holes. Did you try everything you listed?


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
  •