584,798 active members*
4,350 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking > MetalWork Discussion > calculating thread depth (single point lathe threading)
Results 1 to 11 of 11
  1. #1
    Join Date
    Nov 2017
    Posts
    591

    calculating thread depth (single point lathe threading)

    Im new to threading so i want to make sure im doing this right. This is on a cnc setup using fusion 360 cam, example of an M6x1mm thread. For starters, heres how im dialing in my threading insert, I start by turning a diameter and checking with a mic, lets say 20mm. I then touch of my threading insert on this known diameter of 20mm. My threading insert has a 2 thou radius on it so after touching off, i back off the tool a calculated amount so the projected sharp point would be right at the turned diameter, in this case backed off .054mm, then enter 20mm for diameter. This would put the projected point of the insert right on the Z axis at X0. Now in fusion for an M6x1 thread, im modeling a 6mm diameter and selecting that surface for the threading op. I specify a 1mm pitch and a thread depth of .866mm (1mm pitch x .866 ratio). After turning to 6mm and then threading, I come back and turn the OD one more time at 5.9mm to deburr. This should result in a zero clearance thread fit right? Well, its giving me a pretty sloppy fit. Im guessing the nut im checking with has some clearance, but this is a much looser fit than just a bit of clearance. Could be that my cheap insert has a larger radius than whats specified, which would put my insert deeper than expected. Is there a better way to dial in the depth for the insert? obviously i could just start shallower and reduce the x offset until its a good fit, but i wanted to see if theres something specific im doing wrong.

  2. #2
    Join Date
    Dec 2013
    Posts
    5717

    Re: calculating thread depth (single point lathe threading)

    I set my tools to the spindle C/L (G54 X0) for all turning operations. Then I let Fusion generate the appropriate G code for threading. Then I run a part and check the result against whatever measuring device is appropriate for the job: Nut, mating part, thread gauge, or thread wires. If the fit is not correct, then I adjust the X cutter comp as needed to dial in the threads.

    Bottom line is you need to dial the machine in as part of the setup procedure. This is true for all production turning.
    Jim Dawson
    Sandy, Oregon, USA

  3. #3
    Join Date
    Nov 2017
    Posts
    591
    Quote Originally Posted by Jim Dawson View Post
    I set my tools to the spindle C/L (G54 X0) for all turning operations. Then I let Fusion generate the appropriate G code for threading. Then I run a part and check the result against whatever measuring device is appropriate for the job: Nut, mating part, thread gauge, or thread wires. If the fit is not correct, then I adjust the X cutter comp as needed to dial in the threads.

    Bottom line is you need to dial the machine in as part of the setup procedure. This is true for all production turning.
    Yep, I realize i need to dial it in, just want to make sure I'm following the right process for setting up the thread insert and setting the proper initial depth in the first place to get as close as possible before dialing in. Fusion doesn't give the depth automatically, it asks for both pitch and depth. Is multiplying pitch by 0.866 to figure depth correct? This is the ratio I found when searching google.

    Also, you mention setting up tools to spindle C/L as g54 X0, as do I with every other tool, but with a threading insert specifically, are you accounting for the radius on the point? If figuring the theoretical projected point of the insert being at X0, the radius edge of the insert will be slightly away from spindle C/L at X0. I'll attach a pic to show what I'm talking about.

  4. #4
    Join Date
    Dec 2013
    Posts
    5717

    Re: calculating thread depth (single point lathe threading)

    Yes, 0.866 is the correct ratio. I just assume a sharp point on the tool when I set it, normally for small pitch threads the tool doesn't have enough radius (or flat) to worry about. Pretty much sharp V threads.
    Jim Dawson
    Sandy, Oregon, USA

  5. #5
    Join Date
    Nov 2017
    Posts
    591

    Re: calculating thread depth (single point lathe threading)

    ok, so it sounds like im doing it right, just expecting a bit too much from calculation alone. Could be some other variables as well, like index pulse triggering and backlash in Z. Any error from one pass to the next will widen the thread a bit, especially on the spring pass since im going twice at the full depth. Maybe ill turn off the spring pass.
    Tolerance on everything else is kind of blowing me away. Once the machine and enclosure stabilize at around 80F, im holding about 4 micron (under 2 tenths) on diameters, no joke. I was hoping for +/- a thou on a home built machine like this lol. I think the vertical X axis really helps with nailing the diameters since any backlash is bottomed out from the weight of the axis. Also having the machine inside an insulated enclosure (mainly for noise), very easy to keep temp consistent.

  6. #6
    Join Date
    Dec 2013
    Posts
    5717

    Re: calculating thread depth (single point lathe threading)

    One thing to note In Fusion you need to plug in 1/2 the calculated thread depth. So in this case the value entered into fusion would be 0.433mm. I forgot to mention that.

    That is awesome! :cheers: Still waiting for some pictures of you machine .
    Jim Dawson
    Sandy, Oregon, USA

  7. #7
    Join Date
    Nov 2017
    Posts
    591
    Quote Originally Posted by Jim Dawson View Post
    One thing to note In Fusion you need to plug in 1/2 the calculated thread depth. So in this case the value entered into fusion would be 0.433mm. I forgot to mention that.

    That is awesome! :cheers: Still waiting for some pictures of you machine .
    Hmmm, 1/2 depth, are you sure? Don't think I could be that far off. The other day I did an m10x1.25, using the full depth (1.25x.866) and it was the same amount of play as the m6 I did. Should have been a lot more slop if I'm going double depth. Actually, I don't think my insert would even go double that depth. That would be about 2.2mm deep into the cut. I'll try again with 1/2 depth just to make sure, but why would it be only 1/2 depth?

    Here's a couple pics, just what I have on my phone, at work right now. The mill turn spindle, few pics of gang tooling set up, couple parts i turned, a brass m10 bolt and the piston for the spindle brake. All parts for the mill turn and gang tooling were done on this machine. The center portion of the gang tooling is the biggest part I've milled. Started as a 13 pound block of 6061, I think it was 6 pounds finished. The 80mm diameter, 125mm deep bore for spindle was tricky. Had to come at it from both ends with a maritool 3/8 reduced shank endmill. Managed to get the bore to meet perfect in the middle, maybe a 1 thou step.

    First couple pics got flipped 90. That first pic is the horizontal servo driven spindle. Dunham spindle and closer, dmm 1.8kw at the back next to closer which you can't really see, just the plugs sticking up. pneumatic brake on the rotor, piston inside of it is pic 3

  8. #8
    Join Date
    Dec 2013
    Posts
    5717

    Re: calculating thread depth (single point lathe threading)

    Very nice work!

    Maybe I should say for my machine I have to plug in the Single Depth of the thread for it to cut correctly. That would be ''T'' dimension in the Fusion illustration when you hover over the Thread Depth text box.

    Let's take the example of M6x1 for a tapped hole (from a thread chart and neglecting the ratio), Major Dia = 6mm, Minor Dia = 5mm (drill size), 6mm-5mm = Double depth = 1mm, and Single Depth = 1mm/2 or 0.5mm which is what I would have to enter into the text box for my machine to cut correctly. Maybe Mach3 interprets the thread depth differently than my software does. In my case, Fusion outputs everything in diameter, at least for turning, and my X DRO displays diameter, but internally the machine is actually positioning for the radius. I've never studied the G code to try to figure out what it is actually doing when threading because it has always worked when I plugged in the single depth.

    Interestingly, on my Haas mill, I also have to enter the single depth when thread milling.
    Jim Dawson
    Sandy, Oregon, USA

  9. #9
    Join Date
    Nov 2017
    Posts
    591
    Quote Originally Posted by Jim Dawson View Post
    Very nice work!

    Maybe I should say for my machine I have to plug in the Single Depth of the thread for it to cut correctly. That would be ''T'' dimension in the Fusion illustration when you hover over the Thread Depth text box.

    Let's take the example of M6x1 for a tapped hole (from a thread chart and neglecting the ratio), Major Dia = 6mm, Minor Dia = 5mm (drill size), 6mm-5mm = Double depth = 1mm, and Single Depth = 1mm/2 or 0.5mm which is what I would have to enter into the text box for my machine to cut correctly. Maybe Mach3 interprets the thread depth differently than my software does. In my case, Fusion outputs everything in diameter, at least for turning, and my X DRO displays diameter, but internally the machine is actually positioning for the radius. I've never studied the G code to try to figure out what it is actually doing when threading because it has always worked when I plugged in the single depth.

    Interestingly, on my Haas mill, I also have to enter the single depth when thread milling.
    I thought pitch x .86 was for single thread depth? On my machine, single depth is what I want. Since I'm using mach3 mill for both turning and milling, all my turning moves are output 1 to 1 and that's also what my dro shows. With x at 10mm in dro, I'm turning at 20mm diameter. To make this work with fusion cam, I had to modify post to remove the scale factor of 2.

    Looking at a metric thread diagram, there's definitely something I don't have quite right. I assumed that with a male thread, the outside point, or at least projected point was supposed to land right on the major diameter. In the diagram I'm looking at, that's not the case. It shows the finished diameter of an m6 at 6mm with a specified flat on the outer tip of the thread. I knew there was supposed to be a small flat, but i assumed you just cleaned up at a bit less than major diameter to get that flat. That was an incorrect assumption. 0.866 is the correct ratio for a single thread, (ratio of base to height of 60deg triangle) but where im going wrong is figuring the sharp point of thread being right at major diameter. I'm gonna watch a couple videos on fusion threading and lathe threading in general. I'm sure I'll figure it out. At least now I know it is indeed a calculation problem and not a machine tolerance problem.

  10. #10
    Join Date
    Nov 2017
    Posts
    591

    Re: calculating thread depth (single point lathe threading)

    Ok, looked through some videos and charts. Looks like I need to just forget about that .866 ratio and instead go to a thread chart, subtract specified minor D from major D, divide by 2, that's my thread depth. Doing so results in significantly less depth than I figured from the ratio. So that explains my loose threads.

  11. #11
    Join Date
    Dec 2013
    Posts
    5717

    Re: calculating thread depth (single point lathe threading)

    Quote Originally Posted by QuinnSjoblom View Post
    Ok, looked through some videos and charts. Looks like I need to just forget about that .866 ratio and instead go to a thread chart, subtract specified minor D from major D, divide by 2, that's my thread depth. Doing so results in significantly less depth than I figured from the ratio. So that explains my loose threads.
    Yup, that's what I've been doing. Then make a final adjustment with the cutter comp to dial in the fit.
    Jim Dawson
    Sandy, Oregon, USA

Similar Threads

  1. CNC hobby lathe single point threading
    By ChrisW in forum Uncategorised MetalWorking Machines
    Replies: 1
    Last Post: 07-08-2013, 09:03 PM
  2. Single point threading (lathe) with EMC
    By chafik in forum LinuxCNC (formerly EMC2)
    Replies: 2
    Last Post: 06-08-2008, 12:04 AM
  3. Replies: 10
    Last Post: 02-07-2008, 08:28 PM
  4. Single point threading
    By DragnsBane in forum MetalWork Discussion
    Replies: 2
    Last Post: 10-06-2007, 05:25 AM
  5. Single point threading
    By kdoney in forum Mach Mill
    Replies: 8
    Last Post: 02-09-2006, 06:13 AM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •