Page 2 of 3
Re: Threading with Acorn lathe Pro
Posted: Thu Aug 05, 2021 9:50 am
by cnc_smith
vw_chuck wrote: ↑Thu Aug 05, 2021 9:29 am
Dave C I have all my tool offsets set correctly to and if I use the built in dimensions for a thread a nut will not thread on.
Also use 29.5 as the infeed angle and save yourself a massive chatter headache. I can see 55 or 65 working in aluminum or brass but no way in steel.
29.5 is the standard angle. For Centroid you need to double that to 59 for the infeed (thread angle in Intercon)
Re: Threading with Acorn lathe Pro
Posted: Thu Aug 05, 2021 11:51 am
by Dave_C
vw_chuck wrote: ↑Thu Aug 05, 2021 9:29 am
Dave C I have all my tool offsets set correctly to and if I use the built in dimensions for a thread a nut will not thread on.
Also use 29.5 as the infeed angle and save yourself a massive chatter headache. I can see 55 or 65 working in aluminum or brass but no way in steel.
You can have your tool offsets all correct but if the lathe does not home to the exact same dimension on startup they are all off by the same amount!
I have to take a test cut with the master tool and set the reference for the day each time I boot up. I don't have an x or z pulses to do that for me.
Dave C.
Re: Threading with Acorn lathe Pro
Posted: Thu Aug 05, 2021 1:40 pm
by vw_chuck
Dave C yes everyone using Acorn that has a shitty home switches does it your way finding X zero with tool number 1. I always said Acorn needs memory so that it remembers where it was when shut down and then you wouldn't need to reset the X zero everytime.
Dana that is good to know as I never read anywhere that the angle in centroid is double of what you want it to be. What happens if you put in 29.5 in Acorn then? It will try to cut at 15 degrees?
Re: Threading with Acorn lathe Pro
Posted: Thu Aug 05, 2021 2:10 pm
by Dave_C
Dave C yes everyone using Acorn that has a shitty home switches does it your way finding X zero with tool number 1.
Even with a memory function of the last know coordinates, steppers will twitch on powerup so they would not be at the last know location anyway!
No motor encoders (actually mine do have encoders, hybrid steppers) and Acorn could not read them anyway to keep position.
So I don't any other way to do it. After all that, my threads fit!
Dave C.
Re: Threading with Acorn lathe Pro
Posted: Thu Aug 05, 2021 2:11 pm
by cnc_smith
vw_chuck wrote: ↑Thu Aug 05, 2021 1:40 pm
Dana that is good to know as I never read anywhere that the angle in centroid is double of what you want it to be. What happens if you put in 29.5 in Acorn then? It will try to cut at 15 degrees?
Yes it would cut at 14.75.
tblough wrote: ↑Thu Aug 05, 2021 7:26 am
On the thread details screen (F7) the "thread angle" setting controls how much of the cut is on the flank of the tool. Entering 60° will cut with the tip (evenly on both flanks). I usually use 55°, or 65° depending on which way I want the chips to curl.
This is why tblough is using 55 or 65.
Re: Threading with Acorn lathe Pro
Posted: Thu Aug 05, 2021 7:35 pm
by tblough
Just to note, most of my threading is in 17-4 PH stainless around 35Rc, not aluminum.
Re: Threading with Acorn lathe Pro
Posted: Mon May 06, 2024 5:31 pm
by glbreil
Hello, I know this is an old thread, but I found it while searching for information on thread angle.
Is it accurate that the thread angle needs to be doubled to get actual entry angle that you want?
If I am reading the thread right then 59 degrees setting a manual compound slide at 29.5 and if you want to cut straight in you would need to set the tread angle in Enercon at 120 degrees or 0 according to the manual.
I also noticed in the manual that 55 degrees is a standard number? If it is doubled that would be 27.5 degrees. Why 27.5 instead of 29.5.
Thanks Gary
Re: Threading with Acorn lathe Pro
Posted: Mon May 06, 2024 7:09 pm
by tblough
It's an old thread, but the information is still correct.
tblough wrote: ↑Thu Aug 05, 2021 7:26 am
On the thread details screen (F7) the "thread angle" setting controls how much of the cut is on the flank of the tool. Entering 60° will cut with the tip (evenly on both flanks). I usually use 55°, or 65° depending on which way I want the chips to curl.
Re: Threading with Acorn lathe Pro
Posted: Tue May 07, 2024 8:20 am
by cnc_smith
The Thread angle is the compound angle, not the angle of the insert. Compound angle controls the angle that the control adjust how the cutting on the insert is done. 59 (29 1/2) adjusts the cut so most of the cut is done on the leading side of the insert. With compound angle of 0.0 the insert will cut the same on the leading edge and trailing edge. 0.0 cause more tool pressure. No mater what the compound angle is with a 60 degree insert it will cut the correct thread because insert determines the thread angle. Centroid using the wording of Thread angle instead of Thread Compound has created confusion for years.
Re: Threading with Acorn lathe Pro
Posted: Tue May 07, 2024 4:19 pm
by cnckeith
cnc_smith wrote: ↑Tue May 07, 2024 8:20 am
The Thread angle is the compound angle, not the angle of the insert. Compound angle controls the angle that the control adjust how the cutting on the insert is done. 59 (29 1/2) adjusts the cut so most of the cut is done on the leading side of the insert. With compound angle of 0.0 the insert will cut the same on the leading edge and trailing edge. 0.0 cause more tool pressure. No mater what the compound angle is with a 60 degree insert it will cut the correct thread because insert determines the thread angle. Centroid using the wording of Thread angle instead of Thread Compound has created confusion for years.
thanks Dana!