Left Hand Thread Mill Cutter Confusion

[CNC CHRIS]

First Time Thread Milling with a left hand cutter. i was told to use a left handed cutter because it was best suited for the type of material (titanium)

The call out for the thread is 1/4-28 UNJF - 3B

i Define my tool correctly and chose the spindle direction CCW.

On my cut parameters, i chose "ID Thread". 

when its asking "right hand thread" or "left Hand Thread", is that asking for the thread on the blueprint call out or the type of cutter you're using?

I pressed the "help" button, and it says its the "thread you are cutting"

so i chose "right hand thread" since thats the call out on the BP.

then i chose "top to bottom" for the machining direction. and it says its going to be "conventional milling" but when i run backplot, i believe its climb cutting.

am i missing something?\

i have attached a file.

i am using MC2022

 

 

trial.mcam

[gcode]

you want to choose right hand thread and top down

 

[CNC CHRIS]

but when i do, why does it say its going to cut "conventional milling"

if you run backplot, isnt that showing "climb cutting"

[Matthew Hajicek - Singularity]

Just for future reference, I cut both right and left hand threads in Ti and 17-4 H900 with standard right hand threadmills.  Just need a slow entry feed if you're entering at the bottom.  Also, three passes with approximately equal material cross-section, plus a skim pass.

[gcode]

28 minutes ago, CNC CHRIS said:

but when i do, why does it say its going to cut "conventional milling"

that is a bug

 

[gcode]

go the the online Carmex threading wizard   Carmex Tool Wizard - Welcome

work your way through it selecting the correct material and a thread mill from the "HARDCUT" line

keep working through the wizard and use it to post gcode... that will show you what your code should look like

you should be getting a G04 , a G42 CDC callout and a top down toolpath

when using these cutters I lie to Mastercam and define the cutter as a single point tool so that I get a single toolpath from top to bottom

These cutters have 3 teeth and doing that gives you one finish pass and 2 spring passes all in one pass.

If you can, run the tool 3 teeth deeper than your depth callout.. as the leading teeth break down, the next two are still

making good spring passes and your thread will gage properly to the required depth

You get a safe repeatable toolpath that makes good threads for a long time.