C6 Threading.

[ToolMach_Aust]

Hey guys.

Would love to hear from people that are successfully using their C6 for threading and if they can share their tips, settings etc.... This would really help everyone out their that are having trouble getting their C6 to thread correctly.

thanks in advance.

cheers

Frans
Toolmach

[Journey_Man]

Originally Posted by ToolMach_Aust Hey guys. Would love to hear from people that are successfully using their C6 for threading and if they can share their tips, settings etc.... This would really help everyone out their that are having trouble getting their C6 to thread correctly. thanks in advance. cheers Frans Toolmach

hey there;
Here is a zip file...if it made it

I have cut many thds. on the C6 use the wizard in Mach3 Turn and enter the numbers. if you are using inserts(prefered)or a HSS tool make sure every thing is indicated straight. I prefer to "0" Z at the face of the Part and stay .015 away from sholders. Toutch X on the part O.D. enter dia in DRO on Manual Screen>3/8-16 .375 Major dia. "0" part DRO. Zero Z too!

Your Start X dia is .375
Your End X dia is .293
The rest is whatever your Part length is ect.
The Turn wizzard will do the rest.
I have always used 3wire method to measure the thds. and it has always been +/- .001-.003. Works good enough for what it is.
The Threads zip file saves much time. with the numbers. Bob

[PEU]

I made this video showing the C6 in threading action time ago:

http://video.google.com/videoplay?do...05157483&hl=en


Pablo

[ToolMach_Aust]

Journeyman.

Thanks...

A client of ours is having trouble with threading. The threads start fine and then the pitch seems to change further along the thread. Not sure if Mach3 is reading the Spindle Speed correctly?..

Are there any special settings in Mach3 for the spindle. What are your spindle settings.

cheers

Frans

Originally Posted by Journey_Man hey there; Here is a zip file...if it made it I have cut many thds. on the C6 use the wizard in Mach3 Turn and enter the numbers. if you are using inserts(prefered)or a HSS tool make sure every thing is indicated straight. I prefer to "0" Z at the face of the Part and stay .015 away from sholders. Toutch X on the part O.D. enter dia in DRO on Manual Screen>3/8-16 .375 Major dia. "0" part DRO. Zero Z too! Your Start X dia is .375 Your End X dia is .293 The rest is whatever your Part length is ect. The Turn wizzard will do the rest. I have always used 3wire method to measure the thds. and it has always been +/- .001-.003. Works good enough for what it is. The Threads zip file saves much time. with the numbers. Bob

[mayhugh1]

If each succeeding pass is starting in the same place on the workpiece then the index sensor is probably being read properly. This is the most important synchronization required for a typical short thread. - rpm is secondary. If the threads are getting closer together as you go further down the workpiece then the problem may be that you're not starting the tool far enough away from the workpiece to allow it to accelerate up to a constant velocity before it starts cutting. Mach3 should be checking for this and issue a warning before you start, however. If none of this solves the problem and the thread is long or if for some hardware reason the spindle speed is varying too much then you can go to the Config menu ->ports&pins -> spindle setup. There should probably be check in the "Use spindle feedback in Sync Mode' and in "spindle speed averaging.' If this is OK then you might try also placing a check in the 'Closed Loop Spindle Control.' No one really seems to know what to do with the PID parameters and so leave them at their defaults of .3,1,.3. I don't own a C6 but I do own something very similar and threading really does work in MAch3. Run at a very low rpm - I use just over 300 rpm (the bottom end of my spindle motor controller's capability) - so the carriage can keep up with the spindle for your typical range of thread pitches. - Terry

[PEU]

I just made this more detailed video of the C6 threading in action:

http://video.google.com/videoplay?docid=5557473837334990194&hl=en

Pablo

[mayhugh1]

Well, the OP's question turns out to be pretty timely. If you've been reading the discussion on threading over on the Mach forum, it turns out that threading is broken in the current Mach release and has been for sometime -how long is anyone's guess. I'm running version 2.42 and in that version it works fine. Sometime after that release, however, a change was made to the milling side of Mach to improve drilling cycle speeds and this change rippled into Turn and broke the threading functionality. The reported symptoms seem to vary from incorrect pitch to just just really ugly threads. Art claims to have tracked down the problem and believes he has fixed it for a pending release which should be any day now. There hasn't been a development release for several months, which is really unusual for Mach and the developer(s) have been busy cleaning up a number of long standing issues. Hopefully they didn't break anything else of significance along the way. - Terry

[PEU]

can you provide the link to this thread at mach3 forum? Thanks!

[mayhugh1]

Start here for the solution. There is a long thread previous to this describing various user symptoms.

http://groups.yahoo.com/group/mach1m.../message/96103

[deon]

Hi

A drifting pitch in Mach3 is usually a sign of running in demo mode. Make sure your license file is in th Mach3 Directory.

Thanks
Deon