DOC and Holding Tight Tolerances
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 24
  1. #1
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    68
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    17

    Default DOC and Holding Tight Tolerances

    Right,

    Im working on a jb at the moment where I have a cast iron impeller with a 30mm bore +/- 0.01mm, Im wanting to program the part efficiently and not use necessary tools if need be as this is a production part.

    So my intention to machine the bore was to use a 28mm u-drill, offset the u-drill to drill 29mm, then take the bore to size with 1 finish pass, however im cautious that leaving 1mm in the bore might make it tricky to hold the +/- 0.01mm tolerance. Do you think this is a no go?

    Typically my colleagues would drill to 28mm and then rough the bore 29.7mm then take a finish pass, leaving little in the bore to help hold size.

    However the problem with this is that the bore is 70mm long and because we use standard tooling in our factory this means that I would need to use an 20mm boring bar stuck out 75mm th a 0.8mm nose rad. This is where i have had issues occur before because taking such a small cut with 0.8mm rad, the material acts as a wedge between the part and boring bar and causes vibration.

    What would you do?

    And unfortunately I cannot purchase new tooling for this job.

    Also, i am reluctant to put a smaller u-drill in and then to take a bigger cut with my rough boring bar as I am trying to cut time and the No tools.

    Opinions please!

  2. #2
    Join Date
    Jun 2006
    Country
    UNITED STATES
    State/Province
    Alabama
    Posts
    1,849
    Post Thanks / Like
    Likes (Given)
    1063
    Likes (Received)
    720

    Default

    If you can't buy tools and you don't want to scrap any parts, Drill and Bore....

  3. Likes NAST555 liked this post
  4. #3
    Join Date
    Jan 2006
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    1,510
    Post Thanks / Like
    Likes (Given)
    566
    Likes (Received)
    689

    Default

    Curious as to why you cannot purchase proper tooling.

    If time saved (and potential for scrap reduced) will pay for it, it's a no brainer.

  5. Likes Bobw, AMEC1941 liked this post
  6. #4
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,476
    Post Thanks / Like
    Likes (Given)
    1058
    Likes (Received)
    607

    Default

    Punch the hole with your 28mm drill. Then use the same drill to take a small bore cut to 28.5mm or hell even 29mm to make sure the bore is nice and round. Then tell your boss to seriously realise that buying a few 0.4mm rad inserts is a no brainer.
    Put your bar in and play with feeds and speeds to get rid of the chatter. 70mm is not long for a 25mm bar with the correct insert. I hope your machine is in decent condition, if so you should hold that tolerance no problem.

  7. #5
    Join Date
    Oct 2010
    Location
    Dewees Texas
    Posts
    1,950
    Post Thanks / Like
    Likes (Given)
    24
    Likes (Received)
    493

    Default

    We sometimes reshape inserts for specific needs. If you have a grinder with a diamond wheel and the insert will allow reshaping, have at it.

  8. #6
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,214
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    Quote Originally Posted by KristianSilva View Post
    Right,

    Im working on a jb at the moment where I have a cast iron impeller with a 30mm bore +/- 0.01mm, Im wanting to program the part efficiently and not use necessary tools if need be as this is a production part.

    So my intention to machine the bore was to use a 28mm u-drill, offset the u-drill to drill 29mm, then take the bore to size with 1 finish pass, however im cautious that leaving 1mm in the bore might make it tricky to hold the +/- 0.01mm tolerance. Do you think this is a no go?

    Typically my colleagues would drill to 28mm and then rough the bore 29.7mm then take a finish pass, leaving little in the bore to help hold size.

    However the problem with this is that the bore is 70mm long and because we use standard tooling in our factory this means that I would need to use an 20mm boring bar stuck out 75mm th a 0.8mm nose rad. This is where i have had issues occur before because taking such a small cut with 0.8mm rad, the material acts as a wedge between the part and boring bar and causes vibration.

    What would you do?

    And unfortunately I cannot purchase new tooling for this job.

    Also, i am reluctant to put a smaller u-drill in and then to take a bigger cut with my rough boring bar as I am trying to cut time and the No tools.

    Opinions please!
    .
    .
    for high precision normally
    .
    1st pass leave 0.12 mm (evens bore out reduces cutter deflection following passes)
    .
    2nd pass leave .025 to .075 mm (there is a minimum that will reliably cut and a max where deflection becomes a problem)
    .
    3rd final pass normally take shallow test cut to confirm bore size before boring full depth
    .
    each standard tool setup has precise tolerances on length, width stickout amount thus the tool history accumulated from 1000's of previous bored holes can predict what kind of tolerances you can expect to hold.
    .
    cutting dry and heat buildup and cutting with cold coolant can easily effect bore taper. normally use a work log to record previous job runs and have a warning like often bores .0003" smaller at back of bore if coolant is cold. so if you use a history log of last 1000 bored holes you got a much better ideal what will happen on the next 1000 holes

  9. #7
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,476
    Post Thanks / Like
    Likes (Given)
    1058
    Likes (Received)
    607

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    .

    .
    2nd pass leave .025 to .075 mm (there is a minimum that will reliably cut and a max where deflection becomes a problem)
    .
    Do you guys seriously take such small DOC on a production job with a boring bar? I'd be scared that such a tiny chip would cause crap. For +-0.01mm you should be able to take a lot bigger on a decent machine.

  10. #8
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,992
    Post Thanks / Like
    Likes (Given)
    4390
    Likes (Received)
    1496

    Default

    You may get away with just 2 stabs at it but for the best consistency I'd drill, rough bore then finish cut. What material?

    Brent

  11. #9
    Join Date
    Feb 2005
    Location
    Hatch, NM Chile capital of the WORLD
    Posts
    8,846
    Post Thanks / Like
    Likes (Given)
    12831
    Likes (Received)
    10136

    Default

    then rough the bore 29.7mm then take a finish pass, leaving little in the bore to help hold size.
    Why does having less material in the bore help hold size???

    I screwed up more tight tolerances early in my career "sneaking up on it" and taking small cuts..

    And who cares if the bar deflects, as long as it deflects the same amount on every single part
    and is repeatable.... And you aren't tearing your tools up...


    Since Tom posted his method... MY method of tight tolerance lathe stuff.. I take 2 identical
    cuts.. Say my bore has to be 2.000" ±.001.... I'll rough to say 1.900, then take my first finish/test
    cut at 1.950.. Measure, offset if necessary, then run the finish at 2"... Nail it every time.

    Same DOC, same feed, same speed.. The final finish cut is going to do the exact same thing the test
    cut did 30 seconds ago...

    If its some cheap small material, I don't bother.. If its moderately expensive material, I'll set
    up this way, and then let it run, making adjustments as needed.. If its REALLY expensive material
    or I only have 'Just Enough'.. I'll do the test cut and measure on every part.

    And I would definitely go with the smaller nose radius... If your nose R is NOT buried, you have
    essentially only force trying to deflect your bar.. Bury the nose, and some of those cutting
    forces are being directed directly back down the bar.. Seems to help stabalize things also.

    Too small of a DOC can lead to chatter on some occasions. Seems to let things bounce around too
    much.

  12. #10
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,214
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2389

    Default

    Quote Originally Posted by NAST555 View Post
    Do you guys seriously take such small DOC on a production job with a boring bar? I'd be scared that such a tiny chip would cause crap. For +-0.01mm you should be able to take a lot bigger on a decent machine.
    .
    my normal tolerances are
    1/3 of parts +/-.0025 mm or .0001"
    1/3 of parts +/.005 mm or .0002"
    1/3 of parts +/-.025 mm or .001" usually when length to dia ratio prevents tighter tolerances
    .
    last 10,000 parts (most are 20 to 10,000 lbs and $100. to $20,000.) and easily over 1000 bored holes.
    .
    point is when you got a history log on standardized setup tools and every different cutting parameters tried and you record what works best, reliable and what doesnt work too well and why you can quickly determine best settings to try for high reliability
    .
    it is rare to get even .0025 mm or .0001" different that the target dimensions and most of that is from temperature effects
    .
    i use a work log and record total time to do jobs including rework or remaking parts. auto calculation of time average is used with recording what takes more than average time. a considerable source of extra time used is somebody trying to save a few minutes of time and causing 1 to 100 hours of added rework time. its quite easy to see what is actually faster not what might appear to be faster

  13. #11
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    68
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    17

    Default

    I forgot to mention, where I said I wanted to drill to 29mm then finish bore in 1 pass, I would be doing this with a 0.4 insert.

    Quote Originally Posted by Rstewart View Post
    If you can't buy tools and you don't want to scrap any parts, Drill and Bore....
    Do you mean drill and then finish bore, or drill, rough bore then finish bore?

    Quote Originally Posted by chip_maker View Post
    Curious as to why you cannot purchase proper tooling.

    If time saved (and potential for scrap reduced) will pay for it, it's a no brainer.
    Since we have a 28mm u dril that can be offset to drill a 29mm hole, I would have a hard time justifying buying a £300 u-drill to take an extra 0.5mm out of the bore.

    Quote Originally Posted by DMF_TomB View Post
    .
    .
    for high precision normally
    .
    1st pass leave 0.12 mm (evens bore out reduces cutter deflection following passes)
    .
    2nd pass leave .025 to .075 mm (there is a minimum that will reliably cut and a max where deflection becomes a problem)
    .
    3rd final pass normally take shallow test cut to confirm bore size before boring full depth
    .
    each standard tool setup has precise tolerances on length, width stickout amount thus the tool history accumulated from 1000's of previous bored holes can predict what kind of tolerances you can expect to hold.
    .
    cutting dry and heat buildup and cutting with cold coolant can easily effect bore taper. normally use a work log to record previous job runs and have a warning like often bores .0003" smaller at back of bore if coolant is cold. so if you use a history log of last 1000 bored holes you got a much better ideal what will happen on the next 1000 holes
    Unfortunatley we dont have a log, but what my colleagues are saying is they know that their method works. This alos seems like quite an involved process, since we have unskilled operators this may not be the best solution for us.

    Quote Originally Posted by yardbird View Post
    You may get away with just 2 stabs at it but for the best consistency I'd drill, rough bore then finish cut. What material?

    Brent
    The material is EN-GJS-450 cast iron. One option i was considering was drilling to 28mm, rough boring to 29.7mm with a 0.4 ccmt and then finish boring to size with a dnmg 0.4. What do you think? Does this sound like a better idea than just drilling to 29mm then taking 1 finish pass with a 0.4 insert?

    Quote Originally Posted by Bobw View Post
    Why does having less material in the bore help hold size???

    I screwed up more tight tolerances early in my career "sneaking up on it" and taking small cuts..

    And who cares if the bar deflects, as long as it deflects the same amount on every single part
    and is repeatable.... And you aren't tearing your tools up...


    Since Tom posted his method... MY method of tight tolerance lathe stuff.. I take 2 identical
    cuts.. Say my bore has to be 2.000" ±.001.... I'll rough to say 1.900, then take my first finish/test
    cut at 1.950.. Measure, offset if necessary, then run the finish at 2"... Nail it every time.

    Same DOC, same feed, same speed.. The final finish cut is going to do the exact same thing the test
    cut did 30 seconds ago...

    If its some cheap small material, I don't bother.. If its moderately expensive material, I'll set
    up this way, and then let it run, making adjustments as needed.. If its REALLY expensive material
    or I only have 'Just Enough'.. I'll do the test cut and measure on every part.

    And I would definitely go with the smaller nose radius... If your nose R is NOT buried, you have
    essentially only force trying to deflect your bar.. Bury the nose, and some of those cutting
    forces are being directed directly back down the bar.. Seems to help stabalize things also.

    Too small of a DOC can lead to chatter on some occasions. Seems to let things bounce around too
    much.
    What they tell me is in their experience they find that it is easier to hold size consistently when only leaving 0.3mm in the bore because the inserts last longer, therefore you are not chasing the the tolerance with the offset page constantly. This is machining on a haas st30 btw.

    Quote Originally Posted by NAST555 View Post
    Punch the hole with your 28mm drill. Then use the same drill to take a small bore cut to 28.5mm or hell even 29mm to make sure the bore is nice and round. Then tell your boss to seriously realise that buying a few 0.4mm rad inserts is a no brainer.
    Put your bar in and play with feeds and speeds to get rid of the chatter. 70mm is not long for a 25mm bar with the correct insert. I hope your machine is in decent condition, if so you should hold that tolerance no problem.
    The 28mm udril we have can be offset by 0.5mm therefore drilling a 29mm hole, I have thought about drilling straight to 29mm and then taking 1 finish pass with (we have 0.4 inserts) a 0.4 insert to take to final size. Also, the finish boring bar will be a 20mm bar. Our 25mm bars require a minimum bore dia of 32mm.

  14. #12
    Join Date
    May 2009
    Location
    Canandaigua, NY, USA
    Posts
    2,642
    Post Thanks / Like
    Likes (Given)
    121
    Likes (Received)
    1072

    Default

    How about finishing it with a 30 mm reamer?

  15. #13
    Join Date
    Jan 2006
    Country
    UNITED STATES
    State/Province
    Connecticut
    Posts
    1,510
    Post Thanks / Like
    Likes (Given)
    566
    Likes (Received)
    689

    Default

    I can understand not springing for a drill, but what about a smaller diameter boring bar, preferably carbide shank for rigidity.

    I have various sized carbide shank bars here. They make high l/d ratio holes so much easier,accurate & chatter free.

  16. #14
    Join Date
    Jun 2018
    Location
    Posts
    31
    Post Thanks / Like
    Likes (Given)
    87
    Likes (Received)
    14

    Default

    Quote Originally Posted by Bobw View Post
    Why does having less material in the bore help hold size???

    I screwed up more tight tolerances early in my career "sneaking up on it" and taking small cuts..

    And who cares if the bar deflects, as long as it deflects the same amount on every single part
    and is repeatable.... And you aren't tearing your tools up...


    Since Tom posted his method... MY method of tight tolerance lathe stuff.. I take 2 identical
    cuts.. Say my bore has to be 2.000" ±.001.... I'll rough to say 1.900, then take my first finish/test
    cut at 1.950.. Measure, offset if necessary, then run the finish at 2"... Nail it every time.

    Same DOC, same feed, same speed.. The final finish cut is going to do the exact same thing the test
    cut did 30 seconds ago...

    If its some cheap small material, I don't bother.. If its moderately expensive material, I'll set
    up this way, and then let it run, making adjustments as needed.. If its REALLY expensive material
    or I only have 'Just Enough'.. I'll do the test cut and measure on every part.

    And I would definitely go with the smaller nose radius... If your nose R is NOT buried, you have
    essentially only force trying to deflect your bar.. Bury the nose, and some of those cutting
    forces are being directed directly back down the bar.. Seems to help stabalize things also.

    Too small of a DOC can lead to chatter on some occasions. Seems to let things bounce around too
    much.
    Seconded, there have been times where I've left .03-.06 DOC to finish with a .008r insert in 1018 and 12L14 to get a consistent size and good finish(part had max radius call outs and required 12ra finish). I also hate leaving that small an amount to finish because the cut doesn't form a chip properly and leads to excessive tool wear.

    Edit: Hell with that open of a tolerance I'd try to just take it straight from your drill size to finish with a 1/64r insert
    Last edited by TheTalman1; 07-11-2018 at 03:26 PM. Reason: I felt like it

  17. #15
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,476
    Post Thanks / Like
    Likes (Given)
    1058
    Likes (Received)
    607

    Default

    Quote Originally Posted by DMF_TomB View Post
    .
    my normal tolerances are
    1/3 of parts +/-.0025 mm or .0001"
    1/3 of parts +/.005 mm or .0002"
    1/3 of parts +/-.025 mm or .001" usually when length to dia ratio prevents tighter tolerances
    .
    last 10,000 parts (most are 20 to 10,000 lbs and $100. to $20,000.) and easily over 1000 bored holes.
    .
    point is when you got a history log on standardized setup tools and every different cutting parameters tried and you record what works best, reliable and what doesnt work too well and why you can quickly determine best settings to try for high reliability
    .
    it is rare to get even .0025 mm or .0001" different that the target dimensions and most of that is from temperature effects
    .
    i use a work log and record total time to do jobs including rework or remaking parts. auto calculation of time average is used with recording what takes more than average time. a considerable source of extra time used is somebody trying to save a few minutes of time and causing 1 to 100 hours of added rework time. its quite easy to see what is actually faster not what might appear to be faster

    Yeah ok... 0.0025 is the same as 0.01. I'll hit +-0.01 on my damn Colchester student all day long. I don't see how taking a 1mm or 1.5mm dia cut is going to give you weird erratic results on a bar that is probably rated to be able to take at LEAST 2 or 2.5mm/side.

    On a side note, just for you Tom, last part I made was a drilled and tapped block, 2 holes, tapped M8 15mm deep,mild steel,Emuge spiral flute tap,Titex 6.8mm drill 20mm deep,12mm chamfer tool, checked each hole with a capscrew, 1 off, cost the customer a chocolate bar, I ate it during a tea break. T e hole depth was unfortunately 0.00005mm too deep but the customer didn't mind because his wife didn't mind that the block that held her washing line bracket up was that tiny bit lighter. NOW I am sure that really helped the OP a lot.

    All I know is that Bob is spot on for a general rule of thumb on DOC. You don't, generally, want to be taking less than your nose radius/side. I also agree with his last 2 passes being the same or pretty close to the same to get the deflection,vibration and so on constant between the cuts on a manual lathe when you are dialing it in. It is the only sure way that I do it.

    On a production run,like the OP said he is setting up for in his first post, you dial it in on your cnc and run with it with obviously the correct gauges to check the tolerance. Then check what tool life is and put that into your knowledge base to know when to flip inserts. When an insert is flipped dial it in again, for that tolerance I would, and go to the next insert change counter.

    +-0.01mm is SERIOUSLY NOT ROCKET SCIENCE. Guys have been hitting those tolerance for many many years, long before cnc's or indexable tipped tools were even around.

    OP the only reason why I suggested taking a cut with the side of your drill to 28.5mm or 29mm AFTER drilling is so that the finish inside the bore is constant on each part before the finishing part. You want the finishing pass to be as consistent as possible every time it runs.

  18. Likes Mtndew, TheTalman1 liked this post
  19. #16
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    68
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    17

    Default

    Quote Originally Posted by NAST555 View Post
    Yeah ok... 0.0025 is the same as 0.01. I'll hit +-0.01 on my damn Colchester student all day long. I don't see how taking a 1mm or 1.5mm dia cut is going to give you weird erratic results on a bar that is probably rated to be able to take at LEAST 2 or 2.5mm/side.

    On a side note, just for you Tom, last part I made was a drilled and tapped block, 2 holes, tapped M8 15mm deep,mild steel,Emuge spiral flute tap,Titex 6.8mm drill 20mm deep,12mm chamfer tool, checked each hole with a capscrew, 1 off, cost the customer a chocolate bar, I ate it during a tea break. T e hole depth was unfortunately 0.00005mm too deep but the customer didn't mind because his wife didn't mind that the block that held her washing line bracket up was that tiny bit lighter. NOW I am sure that really helped the OP a lot.

    All I know is that Bob is spot on for a general rule of thumb on DOC. You don't, generally, want to be taking less than your nose radius/side. I also agree with his last 2 passes being the same or pretty close to the same to get the deflection,vibration and so on constant between the cuts on a manual lathe when you are dialing it in. It is the only sure way that I do it.

    On a production run,like the OP said he is setting up for in his first post, you dial it in on your cnc and run with it with obviously the correct gauges to check the tolerance. Then check what tool life is and put that into your knowledge base to know when to flip inserts. When an insert is flipped dial it in again, for that tolerance I would, and go to the next insert change counter.

    +-0.01mm is SERIOUSLY NOT ROCKET SCIENCE. Guys have been hitting those tolerance for many many years, long before cnc's or indexable tipped tools were even around.

    OP the only reason why I suggested taking a cut with the side of your drill to 28.5mm or 29mm AFTER drilling is so that the finish inside the bore is constant on each part before the finishing part. You want the finishing pass to be as consistent as possible every time it runs.
    Thank you for your reply!!

    I wasnt worried about taking a big depth of cut with regards to whether the boring bar could handle it or not, because as you say it is more than capable or 2-3mm a side, it was because the people I work with had said that by leaving 0.3 in the bore It would be easier to maintain size because the insert would wear less. This brings me on to the reason I started this post, I wanted to see if people on this forum agreed with my colleagues as what they said goes against what the tooling manufacturers recommend, which is like you say, minimum DOC = nose radius. Not being as experienced as them I thought I would post on here for advice.

    Thank you for explaining the reasons behind wanting to take a roughing pass with the boring bar/u-drill, so will drilling straight to 29mm not produce a consistent enough size and roundness? could you quantify what you would class as consistent enough size and roundness?

    If thats the case, I think I will drill 28mm, take a roughing pass to 29mm with the u-drill/rough boring bar with a 0.4 insert, then come in with a finish boring bar 0.4 an take to 30mm finish size - this way my finisher is only doing the finishing so should last longer.

    How does that sound?

  20. #17
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    526
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    267

    Default

    16 posts and nobody asked what the material is ?

    On 8620 or similar gooey stuff I'd want a good .015" finish stock. But on 9310 or some heat-treated materials, I'd go for about a thou, so the long stringy cut-your-hands-to-ribbons chip doesn't scar the surface.

    A lot depends on the material, then the insert.

  21. #18
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    68
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    17

    Default

    Quote Originally Posted by KristianSilva View Post
    Right,

    Im working on a job at the moment where I have a cast iron impeller with a 30mm bore +/- 0.01mm, Im wanting to program the part efficiently and not use necessary tools if need be as this is a production part.

    The material is EN-GJS-450 cast iron. One option i was considering was drilling...


    Quote Originally Posted by EmanuelGoldstein View Post
    16 posts and nobody asked what the material is ?

    On 8620 or similar gooey stuff I'd want a good .015" finish stock. But on 9310 or some heat-treated materials, I'd go for about a thou, so the long stringy cut-your-hands-to-ribbons chip doesn't scar the surface.

    A lot depends on the material, then the insert.
    Alright wise guy, I said the material in the opening post and then again a few posts later. Try reading all 16 posts before start giving your superior opinion...

  22. Likes chip_maker, [email protected] liked this post
  23. #19
    Join Date
    Apr 2018
    Country
    UNITED KINGDOM
    Posts
    526
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    267

    Default

    Quote Originally Posted by KristianSilva View Post
    Alright wise guy, I said the material in the opening post...
    Blew that one ! And I looked, too.

    Better have the eyes checked tomorrow ... the big print helps, thanks

    Trying to hold a half in cast iron sucks. I'd hone it. I s'pose you don't have a hone, either. Ick

  24. Likes Bobw, [email protected], TheTalman1 liked this post
  25. #20
    Join Date
    Nov 2016
    Country
    UNITED KINGDOM
    Posts
    68
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    17

    Default

    Cant hone or ream as the bore has some formed features


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
  •  
2