Hello Guest it is May 09, 2021, 06:11:34 AM

Author Topic: Threading on the lathe  (Read 5791 times)

0 Members and 1 Guest are viewing this topic.

Threading on the lathe
« on: September 17, 2011, 06:30:09 PM »
I have had some limited success using Poppabears Quick Threading Wizard.

but a few issues have arisen..

1.  I can't get it working on later than Mach 2.63 (caused a few headaches)

2.  With an M60 x 5mm 55 degree internal thread, whatever setting I use in the wizard, the tool is taking a big chunk of metal out at a time..
as it nears the bottom of the thread, the contact is over 5mm wide at best..

My lathe is not a toy, but thats asking a bit much, the internal threading tool is not as well supported as an outside tool and chatters.. 

is there either a newer wizard

and or

a means of generating G32 or G76 to take several cuts with a small z offset between each. (not from what I have found out so far)

will I have to write it by hand  ?

sounds like I will use up a lot of machinable wax getting it right..

ideas ?

or do I just give up and mill the thread   :-(

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Threading on the lathe
« Reply #1 on: September 17, 2011, 06:45:33 PM »
Not used Scotts wizard but the simple threading one seems to work fine, not used it for a while as I do it mostly in CAM but just tried it just now and the code looked fine. Did you know you can set some of the parameters by using the Settings button on the simple threading page? May be where you are having issues?
Hood
Re: Threading on the lathe
« Reply #2 on: September 17, 2011, 07:26:41 PM »
Hood,

Its not the depth of cut but the width of cut when cutting the large thread.. 
using either of the wizards the whole of one side of the tool is in contact with the work for the whole depth of the thread.
Alternating flank infeed might help, but does Mach3 support the  G76 alternate flank feed?  I've not found it in the documantation.
It seems to be the "P" parameter where I've found it on the net,  but Mach documentation says this is a pitch

Chris

Offline DAlgie

*
  •  314 314
    • View Profile
    • Algie Composite Aircraft
Re: Threading on the lathe
« Reply #3 on: September 18, 2011, 12:27:40 AM »
The simple threading wizard uses the G76 flank type feed yes. Sounds to me like you are either; using too long of a threading bar, too small for the thread pitch and as the depth gets deeper it has higher tool contact and starts to chatter, and/or you have the starting thread cut depth set too deep. Also, a lot of guys on here try to thread at stupid RPMs, I dont know all you are doing but keep the RPM to maybe 250 for that thread?
DaveA.

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Threading on the lathe
« Reply #4 on: September 18, 2011, 03:54:18 AM »
I think you will always have that final width of contact no matter what method you use. Rigid setup is the only way to do a large thread as Dave has said. I have never used Alternate flank but it is supposedly available by setting the Cut Type to 1 for alternate flank, its on the Turn Options page (From Config Menu then Ports and Pins)
Hood

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Threading on the lathe
« Reply #5 on: September 18, 2011, 04:46:12 AM »
Just got the wizard to produce code with both flank and alternate flank and it seems like it is working.
I used the Test=true option in the macro so that the code spat out is G32 so it can be read, see attached screenshot.
Hood
Re: Threading on the lathe
« Reply #6 on: September 18, 2011, 06:43:54 AM »
Thanks Hood,

I get the alternate flank code correctly on my office machine

I missed that Cut Type setting on the ports and pins page completely..  

I've gone back to 2.63 on the machine so I will try that today,

appreciate the help

Chris

Offline Hood

*
  •  25,838 25,838
  • Carnoustie, Scotland
    • View Profile
Re: Threading on the lathe
« Reply #7 on: September 18, 2011, 06:47:44 AM »
Art found a problem with threading in the driver a while back so it may be an idea to use the latest version if you are using the parallel port, then again if earlier versions didnt pose a problem for you before (never did for me) you may as well stick with what you know :)
I think it all depended on how steady your spindle was under speed, my lathes fairly big so I never had problems, use the SmoothStepper now anyway.
Hood
Re: Threading on the lathe
« Reply #8 on: September 18, 2011, 07:00:20 AM »
yes, parallel port...

simple turning operations worked fine with the latest version, but when using the wizards for threading all hell broke loose..
the predicted toolpath looked OK but the actual toolpath and the screen toolpath trace were all over the place.. seemingly random !
I couldn't fix it so I went back to the last known good setup, which was 2.63, things settled down right away..
as a beginner, I don't know enough to know if it was the driver or something else so I reinstalled everything...

as long as it holds together.. I don't mind which version it is !

My lathe is a retrofit I started working on this summer..  its 48 inches beween centres will swing 19 inches diameter over the gap and has a 3hp motor with a VFD..  still using steppers as thats what I'm familiar with..

These threads are the internal threads on the faceplates to match the spindle nose..  hence the extra care I am taking..

At least I make my own machinable wax, so I can test as much as I want !

thanks again for your help

Chris

Offline RICH

*
  • *
  •  7,419 7,419
    • View Profile
Re: Threading on the lathe
« Reply #9 on: September 18, 2011, 07:21:50 AM »
SPIYDA,
Suggest you have a look at "Threading on The Lathe - Mach3 Turn" write up as it  has a lot of info on threading.
On page 44 you will find how to set and what settings are used for Cut Type and Infeed Type ( it's the only place you will find
that info documented).
All the cut types do work, G32 and G76 work, and also the wizards.

For deep threads i would suggest the alternate flank cutting. Note that spring passes will be full cutting of the profile.
One of the interesting things about using alternate flank cutting  is that you can cut an acme type thread with a sharp v type
cutter. You just restrict the depth of the full depth.

I would strongly suggest that anyone doing threading test out their lathe before cutting  an actual piece.
You really need to know just what to expect. Alternate flank works great ....but .....if your late system is not accurate
the results can be bad IE; won't be able to  hold the tolerance, spring passes may be far to deep etc. Be attentive to
the formed chip as it tells you a lot.

User should always run the "calc number of passes" since that will warn you if velocity settings are exceeded.
Take into consideration motor torque available to velocity.

Hope the above helps you out,
RICH
  
 REF TO THE WRITE UP:
- Support>Documentation
- Members Docs> http://www.machsupport.com/forum/index.php/topic,13017.msg85313.html#msg85313
« Last Edit: September 18, 2011, 08:02:57 AM by RICH »