Threading with Acorn lathe Pro

All things related to the Centroid Acorn CNC Controller

Moderator: cnckeith

khancnc
Posts: 9
Joined: Sat Aug 29, 2020 2:30 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 0035FF8A13B8-0729203580
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No

Threading with Acorn lathe Pro

Post by khancnc »

Hi Guys , Need help with threading. I am very new to CNC machining I am a manual lathe & mill machinist, I just got my Lathe Pro Version to do threading I tried cutting a M12x1.75 thread it cut fine but just not deep enough and needed a bit side clearance. So to fix it I went back into the program increased the depth value( didn’t know how to go side clearance) took out another G-Code and run the program again I had to do this like 3 more times till I got it good. What I want to know is a quick and easy way of doing this There has to be another way CNC operator do it. How can you just increase depth of a cut in the same G-Code. I used the Lathe Conversational programming. And also Fusion 360 with Franco’s tool path program.
Thanks everyone in advange
Farrel
tblough
Posts: 3072
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Boston, MA
Contact:

Re: Threading with Acorn lathe Pro

Post by tblough »

In Intercon, select the thread line and edit it. Press F7 for the thread details and adjust the major and minor diameters as needed.

Not sure what you mean by side clearance.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
cnc_smith
Posts: 237
Joined: Mon Nov 20, 2017 10:13 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: Yes
CPU10 or CPU7: Yes
Location: Frenchville, PA

Re: Threading with Acorn lathe Pro

Post by cnc_smith »

Farrel,

You do not increase the depth in the program. You use the Tool Wear - F9 to adjust the thread depth. For an OD thread you go negative for X offset if the thread diameter is to large and for an ID you go positive if it is to small. With threading you almost always have to adjust the diameter to get the correct thread size. It is not that you set up the tool incorrectly for threading. Do not be surprised it is has high as .010" (.25 MM). The easiest why to explain it it the book calculation number for pitch diameter is base on a set nose point for cutting. How the insert nose tip is ground will effect the pitch diameter even with the tool set correctly.
I have been around CNC (NC) machining for over 40 years and you always had to adjust the wear offset to get the correct thread size.
Dana

When requesting support, please ALWAYS post a current report.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
tblough
Posts: 3072
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Boston, MA
Contact:

Re: Threading with Acorn lathe Pro

Post by tblough »

It really depends if you are using a full-form insert or a sharp 60 degree tool.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
vw_chuck
Posts: 194
Joined: Sun Sep 20, 2020 7:34 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 0035FF8FEB5F-0708203490
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No

Re: Threading with Acorn lathe Pro

Post by vw_chuck »

I just drop the minor diameter down a few thou and re-run till the nut threads on nice.
Dana what happens when you forget to zero out the tool wear and use that tool on a different part?
cnc_smith
Posts: 237
Joined: Mon Nov 20, 2017 10:13 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: Yes
CPU10 or CPU7: Yes
Location: Frenchville, PA

Re: Threading with Acorn lathe Pro

Post by cnc_smith »

vw_chuck wrote: Wed Aug 04, 2021 12:31 pm Dana what happens when you forget to zero out the tool wear and use that tool on a different part?
If you are using the same tool to cut a different thread it should cut very close to the correct size. If you change the tool that is your bad for not resetting the wear offset. Using the Tool Wear for adjusting the size of the thread is the easiest way to adjust the thread diameter whether it is a single point threading tool, a partial or full form threading insert. I never like changing the program for adjusting for tool wear or tool adjustment. That is what tool offset is for. Most times your program positions match your drawing dimensions. It makes it easier when you are back checking your program to make sure the dimensions are correct in the program if they are to the drawing dimensions.
Dana

When requesting support, please ALWAYS post a current report.
Need support? READ THIS POST first. http://centroidcncforum.com/viewtopic.php?f=60&t=1043
All Acorn Documentation is located here: viewtopic.php?f=60&t=3397
Answers to common questions: viewforum.php?f=63
and here viewforum.php?f=61
Dave_C
Posts: 669
Joined: Wed Nov 15, 2017 8:25 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: none
DC3IOB: No
CNC11: No
CPU10 or CPU7: No
Location: Springfield, MO. USA
Contact:

Re: Threading with Acorn lathe Pro

Post by Dave_C »

The other issue with lathe threading concerns having the tool cutting at the actual diameter that you think it is. Most of our "hobby" lathes don't have Z or X pulses to home to so we depend on something a little less accurate and then make trial cuts, set the reference and so on.

So programing a .250" cut and the tool cuts .259 is not a tool wear issue, the tool is not referenced properly. Sure you can change tool wear to compensate but in my case I use a electronic touch off tool to set all my tools in a batch and then I reference tool #1 on start up. Then all tools cut what I call out.

Dave C.
Grizzly G0678 Mill ,CNC conversion with Acorn. G4004G Lathe, Mach 3 conversion to Acorn.
khancnc
Posts: 9
Joined: Sat Aug 29, 2020 2:30 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 0035FF8A13B8-0729203580
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No

Re: Threading with Acorn lathe Pro

Post by khancnc »

Thanks heaps guys I will try both ways and see what suits, bump up the minor diameter in intercon and start using tool wear with fusion drawing and see what suits me. Tom I was using a former insert and what I meant about side clearance was that I want it to cut a bit more on the leading surface of my cutter rather fully at the point, hope that makes sense Thanks again All
Cheers
Farrel
tblough
Posts: 3072
Joined: Tue Mar 22, 2016 10:03 am
Acorn CNC Controller: Yes
Allin1DC CNC Controller: Yes
Oak CNC controller: Yes
CNC Control System Serial Number: 100505
100327
102696
103432
7804732B977B-0624192192
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No
Location: Boston, MA
Contact:

Re: Threading with Acorn lathe Pro

Post by tblough »

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.
Cheers,

Tom
Confidence is the feeling you have before you fully understand the situation.
I have CDO. It's like OCD, but the letters are where they should be.
vw_chuck
Posts: 194
Joined: Sun Sep 20, 2020 7:34 pm
Acorn CNC Controller: Yes
Allin1DC CNC Controller: No
Oak CNC controller: No
CNC Control System Serial Number: 0035FF8FEB5F-0708203490
DC3IOB: No
CNC12: Yes
CNC11: No
CPU10 or CPU7: No

Re: Threading with Acorn lathe Pro

Post by vw_chuck »

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.
Post Reply