Centroid Community CNC Support Forum

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

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.

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.

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

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?

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.

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.

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

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.

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.