[dlenardu]

I have a Centurion V. Is there a way to do single point thread milling in conversational programming? My cam program creates such a large file that I have to DNC the file and it seems to limit the feed to 8.5 ipm even though I have it set at 30 ipm

[Brian L]

Mine doesn't have that option but I believe there are some software versions that do (mine is old, 1992). Regardless, hand writing code for a threadmilling operation is pretty easy... with a single thread form per circle you don't even need to helical into the cut, start at the bottom, centered in the hole, move out X plus, then do helical circles until you are out of the hole. Code looks something like this:

......
G00 X0 Y0 (move to hole location)
G01 Z-.5 F20 (go to maximum depth of thread)
X.200 (move out amount required to get to major diameter minus half the cutter diameter)
M98 P1000 L11 (Call subroutine and loop it enough times to thread your way out of the hole)
G90 X0 (set the control back to absolute programming and move back to centerline)
G00 Z.1 (pull up in Z to safe level)
...... (continue on to next hole, or end tool)

And your subroutine:

O1000 (program name has to match P call in the above section)
G91 (change machine to incremental movement)
G03 I-.200 Z.05 F30 (perform CCW circle with Z positive amount that equals pitch of the thread)
M99 (end subroutine)

That is about all there is to it. You have to get the amount to move off centerline by figuring out half the major diameter- half the cutter diameter and that should be the amount to move in X positive. The Z value in the subroutine is the pitch, I did this one at 20 TPI for example. So, what, maybe 10 lines of code, you won't have to DNC or any such thing with that. Once you figure out your exact amount of move offset, as long as you use the same cutter and same thread size, this will work for that thread in any part.

Something that might explain your decreased feed rate, a lot of CAM systems take into account the diameter of the cutter and program the actual path slower because the feed rate increases based on the cutter diameter. So, your actual feedrate at the cutting edges might be 30ipm and yet the CAM software programed the tools "center path" at 8.5ipm.

[allen mullis]

your cad/cam may also have an option to output the code in arcs or lines, the lines option will generally give you roughly 1000 times the program length because it breaks it down into line movements, and if your control doesn't have the look ahead to support the code whizzing by, then the control will slow the feedrate to allow for buffer, regardless of what you want it to do. I would suggest a single board computer upgrade from the manufacturer or sportybob, that should give you around 32 MB program cap and 256 MG storage, and the ability to drip feed a 2 GIG program from a compact flash card or SD card if you added it. I despise 3-1/2 floppies and have upgraded 5 of my milltronics to CF.

[dlenardu]

Brian L Thanks for the info. I will give that a try and see if I can get it working. I think allenmullis is correct in the "look ahead" causing it to slow down because the feedrate being outputted is correct but it is like the control is having to slow it down in order to keep up. The cam system is outputting the code in linear coordinates so each XYZ coordinate, not arcs. I need to also look into the cam software to see if there is an option for arcs, but right now I will give Brian L's advice a try. Thanks again for all the info.

[Brian L]

With these older machines that don't have much of a look ahead buffer, this is where writing some code by hand really shines. Like Allen said, the CAM system might turn one helical circle into a thousand lines of code, really putting the whammo on the control. If you program using g02/g03 (arcs) your program gets small and the computer can process without any slowdown at all.

Just remember that your programmed feedrate is at the centerline of the cutter. If your thread mill is say .450 in diameter and you are only swinging a .150" arc radius or so, your peripheral feedrate is going to be almost twice the centerline feedrate.

[dholby]

Can't recall if Centurion 5 has dnc fast, it may only be on centurion 6. the dnc fast has a look ahead which allows higher feeds.
Cam programs made point to point on thread milling, its really 3d, large file.
If you understand the loop program it will be shorter. It to is point to point. So if you need a better finish you will need to made smaller increments ( more loops )

Cam or manual programing think of chordal segment of a circle this is what the curve tolerance is on cam systems. Its the height of the segment not the width, with controls the width.

[allen mullis]

Be careful jumping in to Fast DNC, I would hold my finger over the feed hold. It has been my experience that in fast DNC the control will ignore some parts of the code and cause a crash or at least result in a broken tool. I think "Fast DNC" was intended for single tool programs, like for example sweeping a cavity with a copy mill where the program is simple lines and arcs without tool changes. I had the same issue once upon a time with one of my mills (before the control upgrade) and did as you are thinking of doing and tried to run it in fast dnc, if I remember correctly, when commanded to change tools, it went to Z clearance, and went on with the program as if it had changed tools when it hadn't , resulting in a buried tool and a nice purple color around the area where the collet nut was friction welded to the dead part. All I'm saying is be careful when you turn it loose.

Can't recall if Centurion 5 has dnc fast, it may only be on centurion 6. the dnc fast has a look ahead which allows higher feeds.
Cam programs made point to point on thread milling, its really 3d, large file.
If you understand the loop program it will be shorter. It to is point to point. So if you need a better finish you will need to made smaller increments ( more loops )

Cam or manual programing think of chordal segment of a circle this is what the curve tolerance is on cam systems. Its the height of the segment not the width, with controls the width.