Weird offset experience - any thoughts?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 21
  1. #1
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default Weird offset experience - any thoughts?

    Made up a test part last night for a customer to prove out a concept. Short version of the story - I made a bolt and mating nut.

    I ran the bolt first, it’s an ACME thread, mic’d with a wire, near perfect, no offset.

    I ran the nut second, same tooling, same everything, but had to compensate the thread mill -.0087 to get the part to thread how I wanted. They mate near perfect, with no perceptible slop.

    I am perplexed by the -.0087 comp?

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,131
    Post Thanks / Like
    Likes (Given)
    1620
    Likes (Received)
    1941

    Default

    Quote Originally Posted by Fal Grunt View Post
    Made up a test part last night for a customer to prove out a concept. Short version of the story - I made a bolt and mating nut.

    I ran the bolt first, it’s an ACME thread, mic’d with a wire, near perfect, no offset.

    I ran the nut second, same tooling, same everything, but had to compensate the thread mill -.0087 to get the part to thread how I wanted. They mate near perfect, with no perceptible slop.

    I am perplexed by the -.0087 comp?
    The nut had to be larger for the bolt to go in, otherwise they would be size for size (no running clearance at all)...?

  3. #3
    Join Date
    Sep 2007
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,333
    Post Thanks / Like
    Likes (Given)
    209
    Likes (Received)
    1639

    Default

    Threadmills aren't necessarily "perfect" in that you can simply program the desired diameter, plug in the tool's measured OD, and you're done. Every threadmill I've used, from multiple vendors, needed some offset to get the right PD.

    Regards.

    Mike

  4. Likes coffeetek liked this post
  5. #4
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    447
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    159

    Default

    I think for the most part the two Mike's have it. The only other things I can think of are:

    Old and potentially incorrect backlash settings in control
    Backlash settings causing equal but opposite error working from an OD feature to an ID one. With the combination of the two being addressed numbers wise during creation of the mating part or nut. (Because the awareness of the error wasn't yet evident during the production of the screw. In effect... you got lucky.)
    Feed rate differences between an ID and OD feature of equal size would be quite drastic. If not comped correctly you could add a little more say, following error?

    But again mostly what the Mike's said.

    Dave
    Last edited by 13engines; 12-30-2019 at 11:05 AM. Reason: added "differences"

  6. #5
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Quote Originally Posted by Mike1974 View Post
    The nut had to be larger for the bolt to go in, otherwise they would be size for size (no running clearance at all)...?
    Yes, there has to be clearance, but have you ever cut a thread with .008 clearance? I meant to put in my first post, I don't have a LOT of experience with ACME... but .008"? That seems... well crazy given the feel of the thread. If you cut a 60* thread with .008" clearance it'd be loose and wobbly. This is a pretty snug fit, the kind where you start to thread it in and it binds, you comp .0002 and it threads in with slight effort.

    Quote Originally Posted by Finegrain View Post
    Threadmills aren't necessarily "perfect" in that you can simply program the desired diameter, plug in the tool's measured OD, and you're done. Every threadmill I've used, from multiple vendors, needed some offset to get the right PD.

    Regards.

    Mike
    Sure, that has been my experience as well. Usually you have to comp a little to dial in size. BUT... say I measured with my mic wrong... say 5 tenths, and say my wire was wrong, let's say another 5 tenths, then let's say just because shit happens and I can be dumb, a thousandth. So when I read my mic measuring over the wire, I was .002" off. That still leaves me comping the other side .006".

    Take into consideration Mike (1) comment about thread clearance, because, yes, thread does have to have clearance, .006" clearance? I don't think so...

    Quote Originally Posted by 13engines View Post
    I think for the most part the two Mike's have it. The only other things I can think of are:

    Old and potentially incorrect backlash settings in control
    Backlash settings causing equal but opposite error working from an OD feature to an ID one. With the combination of the two being addressed numbers wise during creation of the mating part or nut. (Because the awareness of the error wasn't yet evident during the production of the screw. In effect... you got lucky.)
    Feed rates between an ID and OD feature of equal size would be quite drastic. If not comped correctly you could add a little more say, following error?

    But again mostly what the Mike's said.

    Dave
    I'd throw out the first two... hopefully... it's a machine less than a year old.

    I thought about feed rates when I was cutting it and I first started comping more than what I would consider normal. I don't remember the feed rates, and I didn't do any real math, but ran the OD at something like 54ipm and the id at something around half that. Maybe that was still too quick?

    I think what is bothering me so much is the fact that I measured the first side mic'd with a wire... I couldn't have been very far off...

  7. #6
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    842
    Post Thanks / Like
    Likes (Given)
    149
    Likes (Received)
    455

    Default

    I did work on a proprietary ACME thread with a 15deg included angle and we used 0.010" clearance per side on the OD and the angles got 0.005" a side (0.010" total).

    Not sure if that is clear but I can't show you a drawing of it due to NDA.

  8. #7
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    4,131
    Post Thanks / Like
    Likes (Given)
    1620
    Likes (Received)
    1941

    Default

    Quote Originally Posted by Fal Grunt View Post
    Yes, there has to be clearance, but have you ever cut a thread with .008 clearance? I meant to put in my first post, I don't have a LOT of experience with ACME... but .008"? That seems... well crazy given the feel of the thread. If you cut a 60* thread with .008" clearance it'd be loose and wobbly. This is a pretty snug fit, the kind where you start to thread it in and it binds, you comp .0002 and it threads in with slight effort.



    Sure, that has been my experience as well. Usually you have to comp a little to dial in size. BUT... say I measured with my mic wrong... say 5 tenths, and say my wire was wrong, let's say another 5 tenths, then let's say just because shit happens and I can be dumb, a thousandth. So when I read my mic measuring over the wire, I was .002" off. That still leaves me comping the other side .006".

    Take into consideration Mike (1) comment about thread clearance, because, yes, thread does have to have clearance, .006" clearance? I don't think so...



    I'd throw out the first two... hopefully... it's a machine less than a year old.

    I thought about feed rates when I was cutting it and I first started comping more than what I would consider normal. I don't remember the feed rates, and I didn't do any real math, but ran the OD at something like 54ipm and the id at something around half that. Maybe that was still too quick?

    I think what is bothering me so much is the fact that I measured the first side mic'd with a wire... I couldn't have been very far off...
    Are you sure on that .006" ?

    I don't know it to be true or not, but checking a 'commercial' grade 4-40 shcs (we don't use much of anything larger than that) with a nut screwed up to within one revolution of the head, I measure .002" movement. Ass-u-ming the larger the thread the more clearance...? I didn't see what size your acme thread is, but maybe 1/2"-3/4"? I wouldn't think .006" total clearance to be unreasonable, but I don't do enough threading to know for sure...

  9. #8
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Quote Originally Posted by Rick Finsta View Post
    I did work on a proprietary ACME thread with a 15deg included angle and we used 0.010" clearance per side on the OD and the angles got 0.005" a side (0.010" total).

    Not sure if that is clear but I can't show you a drawing of it due to NDA.
    Quote Originally Posted by Mike1974 View Post
    Are you sure on that .006" ?

    I don't know it to be true or not, but checking a 'commercial' grade 4-40 shcs (we don't use much of anything larger than that) with a nut screwed up to within one revolution of the head, I measure .002" movement. Ass-u-ming the larger the thread the more clearance...? I didn't see what size your acme thread is, but maybe 1/2"-3/4"? I wouldn't think .006" total clearance to be unreasonable, but I don't do enough threading to know for sure...
    This is why I never finished my engineering degree... among many other reasons! Guess if I really want to know the answer I will have to draw up the thread and do some calculations.

    It's a bastard thread, which is proving to be quite challenging in itself. I basically made it up as I went. I poured through some NIST documents and Machinery's handbook to get a good idea, but everything I found had HUGE (in my opinion) variances that frankly didn't make sense. It is a 1 1/16 - 10 ACME. Based on some other design considerations, it may get bumped up to a 1 1/8, but I have to see how this one works out.

    If I have some time this afternoon I will chuck it in the lathe and see what kind of wobble it has.

    I guess if you break it down, say I was .002" off (doubt it) I'd have .003" per side clearance, which based on what Rick Finsta said, .003" per side on the thread wouldn't be outrageous.

  10. #9
    Join Date
    Dec 2013
    Country
    UNITED STATES
    State/Province
    California
    Posts
    777
    Post Thanks / Like
    Likes (Given)
    239
    Likes (Received)
    456

    Default

    Simple formula to compensate feedrate when machining inside arcs or bores:

    Fcompensated = Fstraightline x (Dia.Work - Dia.Cutter/Dia.Work)

    This becomes more critical the closer the tool Dia. Is to the work Dia. You can also plug in Radius values instead of D. Outside arcs you add Dwork and Dcutter so outside arcs you actually compensate faster than straight line.
    Assuming you were using a 1/2 thread mill on the 1.0625 D work piece, your actual feedrate at the cut on the OD was 36.7 IPM (54/1.47), ID Feedrate should be about 19.4 IPM for the same chipload.

  11. #10
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Fcompensated = Fstraightline x (Dia.Work - Dia.Cutter/Dia.Work)

    OD
    Fcompensated = 54 x (1.0625 - .327/1.0625)
    Fcompensated = 40.7

    ID
    Fcompensated = 27 x (.952 - .327/.952)
    Fcompensated = 16.4

    Thanks Frank!

  12. #11
    Join Date
    Jun 2002
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    2,672
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2212

    Default

    Good morning Fal Grunt:
    There is a little appreciated basic geometric problem with threadmilling having to do with the fact that the cutter is not aligned to the helix angle of the thread except when the milling is done on a 5 axis machine or a dedicated thread milling machine that tilts the cutter.

    That mismatch between the plane of cutter rotation and the helix angle of the thread affects the threadform to varying degrees depending on a few factors.
    1) Coarse pitches are worse than fine ones.
    2) Bigger cutters are worse than smaller ones
    3) Square threads are worse than 60 degree vee threads and Acme threads fall between the extremes.
    4) Internal threads are worse than external threads
    5) Smaller diameters are worse than bigger ones for a given pitch.

    The issue is clearance between the flanks of the thread and the sides of the cutter.
    To visualize the extreme case, imagine a coarse pitch square thread such as might be used on a woodworker's vise.
    If you slip a disc that simulates the cutter into the thread, you will see that it cannot align to the threadform without being tilted at the helix angle of the thread, and for very coarse pitches it cannot be inserted at all, unless it is very small in diameter compared to the diameter of the thread.
    When you cut such a thread on a VMC the flanks will not be correct.

    As you go from a square thread to a 60 degree Vee profile, the error becomes less because the cutter can clear the flanks of the thread better.
    Get the combination of pitch, thread diameter and cutter diameter correct, and a 60 degree Vee profile will clear the flanks as it's driven around the developing thread and the form will be good.
    The window is narrower for an Acme at 14 1/2 degree flank angle and hopeless for a square thread at zero degree flank angle.
    Internal threads are worse than external threads because the thread form curves toward the periphery of the cutter.
    With external threads, of course, the thread flanks curve away from the cutter so there is more clearance.
    Smaller cutters curve away from the developing thread flanks more than large cutters do...so the rule of thumb is to use the smallest cutter you can, especially for internal threads.

    So if I'm understanding correctly, the offset you had to input was a negative one...ie you had to program a smaller internal thread than you expected in order to get the fit correct.
    If that's the case then my babble above explains your experience...if not, then I have no frickin' idea what might have gone wrong!!

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining

  13. Likes 706jim, DrHook liked this post
  14. #12
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Quote Originally Posted by implmex View Post
    Good morning Fal Grunt:
    There is a little appreciated basic geometric problem with threadmilling having to do with the fact that the cutter is not aligned to the helix angle of the thread except when the milling is done on a 5 axis machine or a dedicated thread milling machine that tilts the cutter.

    That mismatch between the plane of cutter rotation and the helix angle of the thread affects the threadform to varying degrees depending on a few factors.
    1) Coarse pitches are worse than fine ones.
    2) Bigger cutters are worse than smaller ones
    3) Square threads are worse than 60 degree vee threads and Acme threads fall between the extremes.
    4) Internal threads are worse than external threads
    5) Smaller diameters are worse than bigger ones for a given pitch.

    The issue is clearance between the flanks of the thread and the sides of the cutter.
    To visualize the extreme case, imagine a coarse pitch square thread such as might be used on a woodworker's vise.
    If you slip a disc that simulates the cutter into the thread, you will see that it cannot align to the threadform without being tilted at the helix angle of the thread, and for very coarse pitches it cannot be inserted at all, unless it is very small in diameter compared to the diameter of the thread.
    When you cut such a thread on a VMC the flanks will not be correct.

    As you go from a square thread to a 60 degree Vee profile, the error becomes less because the cutter can clear the flanks of the thread better.
    Get the combination of pitch, thread diameter and cutter diameter correct, and a 60 degree Vee profile will clear the flanks as it's driven around the developing thread and the form will be good.
    The window is narrower for an Acme at 14 1/2 degree flank angle and hopeless for a square thread at zero degree flank angle.
    Internal threads are worse than external threads because the thread form curves toward the periphery of the cutter.
    With external threads, of course, the thread flanks curve away from the cutter so there is more clearance.
    Smaller cutters curve away from the developing thread flanks more than large cutters do...so the rule of thumb is to use the smallest cutter you can, especially for internal threads.

    So if I'm understanding correctly, the offset you had to input was a negative one...ie you had to program a smaller internal thread than you expected in order to get the fit correct.
    If that's the case then my babble above explains your experience...if not, then I have no frickin' idea what might have gone wrong!!

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining
    Great summary Marcus! Yes I am familiar with this, I am currently machining a square thread part that *SHOULD* be cut at minimum on a 4th offset for the correct pitch angle. Going from a 1/4" thread mill to a 3/8" thread mill increases the width of the thread by .003"! This is as you said the cutter wiping (my terminology) the back of the thread as it follows the lead.

    In this case the helix angle is 1.8*.

    I would cut it on my horizontal, which is a universal and I can offset for this very purpose, but I do not have a low lead for it, and cannot get a fine enough lead.

    I hadn't thought of this last night, as I had in my head it wasn't an issue with the ACME like it was for the square or buttress threads I have cut in the past.

    Another excellent point that likely contributed part of it!

  15. #13
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    447
    Post Thanks / Like
    Likes (Given)
    8
    Likes (Received)
    159

    Default

    Quote Originally Posted by Fal Grunt View Post
    Fcompensated = Fstraightline x (Dia.Work - Dia.Cutter/Dia.Work)

    OD
    Fcompensated = 54 x (1.0625 - .327/1.0625)
    Fcompensated = 40.7

    ID
    Fcompensated = 27 x (.952 - .327/.952)
    Fcompensated = 16.4

    Thanks Frank!

    Hi Fal Grunt,

    I think you've gotten some of the best info so far from Marcus. Most of that knowledge is past my pay grade. But the math above not so much.

    The Fstraightline will be the same for both OD and ID.

    The OD feed rate will always be higher then straight line feed. Of course the opposite being true for ID. If your answers aren't coming out that way you know something is wrong.

    With 54ipm straight feed and 0.952 ID/1.0625OD and 0.327cutter I get - F35.5 for ID and F70.6 OD.

    If you re-read brotherfrank's post you'll notice the mistake. (Plus not minus on OD)

    I use a super nice little app on my iPhone 3GS that I got years ago. (Meaning the app and the phone still in use.) App is called iMachine. Sure there are many others,

    Anyway... As I see you've noticed, the Marcus stuff was a good read. The feed formulas above will shake out soon enough.

    Dave

  16. #14
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Quote Originally Posted by 13engines View Post
    The feed formulas above will shake out soon enough.

    Dave
    Ha! That is what happens when I try to do three things during lunch.

  17. #15
    Join Date
    Jun 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    125
    Likes (Received)
    146

    Default

    Quote Originally Posted by implmex View Post
    Good morning Fal Grunt:
    There is a little appreciated basic geometric problem with threadmilling having to do with the fact that the cutter is not aligned to the helix angle of the thread except when the milling is done on a 5 axis machine or a dedicated thread milling machine that tilts the cutter.

    That mismatch between the plane of cutter rotation and the helix angle of the thread affects the threadform to varying degrees depending on a few factors.
    1) Coarse pitches are worse than fine ones.
    2) Bigger cutters are worse than smaller ones
    3) Square threads are worse than 60 degree vee threads and Acme threads fall between the extremes.
    4) Internal threads are worse than external threads
    5) Smaller diameters are worse than bigger ones for a given pitch.

    The issue is clearance between the flanks of the thread and the sides of the cutter.
    To visualize the extreme case, imagine a coarse pitch square thread such as might be used on a woodworker's vise.
    If you slip a disc that simulates the cutter into the thread, you will see that it cannot align to the threadform without being tilted at the helix angle of the thread, and for very coarse pitches it cannot be inserted at all, unless it is very small in diameter compared to the diameter of the thread.
    When you cut such a thread on a VMC the flanks will not be correct.

    As you go from a square thread to a 60 degree Vee profile, the error becomes less because the cutter can clear the flanks of the thread better.
    Get the combination of pitch, thread diameter and cutter diameter correct, and a 60 degree Vee profile will clear the flanks as it's driven around the developing thread and the form will be good.
    The window is narrower for an Acme at 14 1/2 degree flank angle and hopeless for a square thread at zero degree flank angle.
    Internal threads are worse than external threads because the thread form curves toward the periphery of the cutter.
    With external threads, of course, the thread flanks curve away from the cutter so there is more clearance.
    Smaller cutters curve away from the developing thread flanks more than large cutters do...so the rule of thumb is to use the smallest cutter you can, especially for internal threads.

    So if I'm understanding correctly, the offset you had to input was a negative one...ie you had to program a smaller internal thread than you expected in order to get the fit correct.
    If that's the case then my babble above explains your experience...if not, then I have no frickin' idea what might have gone wrong!!

    Cheers

    Marcus
    Implant Mechanix • Design & Innovation > HOME
    Vancouver Wire EDM -- Wire EDM Machining
    Probably this. I have thread milled Acme and Stub Acme, every time I can remember I have had to take PD to near high to get the mating part to go. Acme threads are very loose by design. On a 1.062-10 2G Acme the PD tolerance is .0157" Thats an awful lot of slop, not even counting built in clearance.

  18. #16
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    Kansas
    Posts
    347
    Post Thanks / Like
    Likes (Given)
    79
    Likes (Received)
    160

    Default

    Wild ass guess based on something I glance over a few moons ago.. measuring acme with wires can give poor results because of the forces applied to the wire during measuring cause them to wedge into the thread, then the Male is to big.

  19. #17
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Quote Originally Posted by pgmrmike View Post
    Probably this. I have thread milled Acme and Stub Acme, every time I can remember I have had to take PD to near high to get the mating part to go. Acme threads are very loose by design. On a 1.062-10 2G Acme the PD tolerance is .0157" Thats an awful lot of slop, not even counting built in clearance.
    I'm curious where you found that spec? I found a NIST document on ACME but they did not list that size. Using their listed 10 pitch with the high tolerance spec (forget what it was called) I still had a widely varying pitch measurements that in some regards simply wouldn't work.

  20. #18
    Join Date
    Jan 2012
    Location
    indiana, usa
    Posts
    174
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    44

    Default

    I just put it into my thread software.
    1-1/16"-10 2G acme thread

    External P.D 1.0125-1.0285
    Internal P.D. .9888-1.0045

  21. #19
    Join Date
    Jun 2010
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    125
    Likes (Received)
    146

    Default

    Quote Originally Posted by Fal Grunt View Post
    I'm curious where you found that spec? I found a NIST document on ACME but they did not list that size. Using their listed 10 pitch with the high tolerance spec (forget what it was called) I still had a widely varying pitch measurements that in some regards simply wouldn't work.
    Gagemaker Thread Disk. It does the math. The companies I do work for use every size imaginable, ( Oil field ) Rarely the common sizes. Example 4.454-4 Acme 2G RH

  22. #20
    Join Date
    Aug 2010
    Location
    Medina OH
    Posts
    2,083
    Post Thanks / Like
    Likes (Given)
    211
    Likes (Received)
    1009

    Default

    Quote Originally Posted by chad883 View Post
    I just put it into my thread software.
    1-1/16"-10 2G acme thread

    External P.D 1.0125-1.0285
    Internal P.D. .9888-1.0045
    Thanks for that! Would you mind running 1-1/8"-10 for me as well?

    Quote Originally Posted by pgmrmike View Post
    Gagemaker Thread Disk. It does the math. The companies I do work for use every size imaginable, ( Oil field ) Rarely the common sizes. Example 4.454-4 Acme 2G RH
    Good to know! Wish I had a program like that... but I'd only need to use it every few years...


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
  •