Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: spiyda 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 :-(
-
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
-
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
-
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.
-
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
-
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
-
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
-
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
-
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
-
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
-
with a VFD.. still using steppers as that's what I'm familiar with..
Set the speed manually on the VFD. Having a variable speed will screw up the thread cycle.
These threads are the internal threads on the faceplates to match the spindle nose.
Try cutting an external thread and see what class thread you are achieving. The spindle nose threads are usually
ground and yes you want a matching tolerance. A shop would chase them.
RICH
-
Cheers Rich and hood,
I figured out the manual speed part..
Internal and external threads are now perfect when cut in machinable wax.
The size of the swarf is now well within the machine's capability
I have to do a bit of fettling on the machine before I cut the final version in steel..
I have a grub screw that keeps wanting to undo itself right at the critical moment!
No point in rushing when I am tired...Fingers crossed for tomorrow !
The accuracy required and difficulty of machining this particular thread is as hard as I want to go.
I'd much rather machine a nice easy fine thread.. but no choice.. I can't get anything ready made with the correct thread.
It seems to be a bit of a hybrid, all metric apart from the thread angle of 55 degrees.
At least i know a lot more about the workings of Mach, and the capabilities of my lathe now !
-
Well,
to round this thread off. ;)
success !
I managed to cut a well matched thread to fit the spindle nose.. first attempt in steel.
It can be taken off and replaced with no detectable runout.. yippee !
I broke the threading tool after I had cut the thread to size, attempting to really get a good finish.... my stupidity, I was tired by then
but it was only a few quid and well worth sacrificing to be able to mount my 25Kg 3 jaw chuck.
Now I understand the wizards a little better, the task seems less daunting.. and I will make a couple more..
thanks again for the help
-
Happy it turned out well.
RICH