One clean up pass after threading…T32B
After single point external threading some 6061 M10x1.5 pieces I was taking one pass with a OD tool to clean up the OD and then wanting to take one more pass with the threading tool to clean up the remaining burrs from the threaded area.
Added another threading process with the start and finish X .001” above the root diameter and set thread height to .0005”. The least amount of passes it would take was 5 regardless of any combination of start height or thread height.
On another control it has a feature to run one pass at the finish depth after the OD clean up. Is there a simple way in Mazatrol to set up one pass at the finish depth or if I use a manual program using IPR will it pick up the thread start point?
I Have a T2 control that I do what you are wanting to do. I just copy the above threading process and change the number of passes at 3. The 3 passes allow the insert to take out any tool deflection instead of pushing it back out.
Insetad of going through all that trouble, I suggest you get yourself a "Topping Insert," this will do everything you want it to do in one process, NICE SMOOTH THREADS, "BURR FREE"
It does improve things but I usually still add the turning pass and a threading pass to clean up the burr at the start (and end with undercut) of the thread. A topping insert won't touch those.
Originally Posted by SteelCutter
I'm using a partial profile insert as you mentioned, as they cover a wide range of pitches. If I ever get into a large run of a single pitch I'll pick up some full profile (I assume that what you mean by topping insert) inserts for that job.
I haven't got the manual in front of me but try coping the threading unit into another unit and make the second unit full depth. It will pick up the same entry point as long as you don't change the speed and should take only one pass unless the parameters aren't set correctly. There is also block cycle G32 in manual programming. Good luck
In all my years making chips, and they go back to the late 60's ( to date ,) I've never seen a "Machined Thread" come off a lathe, manual or cnc, without some type of sharp edge, burr or at the very least a feather edge!
( even with a topping insert ) <==== this is what in my experience will give you the least ammount of sharp edges, burrs or feather edges!
*Hence, any one that has a customer or customers requiring a completely smooth thread, 100%, needs to be adding cost for either manual buffing, polishing, filing, de-burring or tumble de-burring! else, you will loose your ARSES in the process because all you will be doing is wrapping each piece with a 20 dollar bill before sending it to the customer!
With all due respect!
You sound (read) annoyed. With the "Personal experience", multiple colors, and "With all due respect". I could be wrong but if you are, why?
Not annoyed at all, Chris!
If you look at any of my posts, I use different fonts/colors simply to highlight my different views, the Image Capture is basically one that I like using as my signature, if you will, and the "With all due respect" I use to make sure that people don't take offense, AS THEY HAVE IN THE PAST, with some of my other posts/replies!
I've been around to long to let myself be ANNOYED <==== just so you know, this color font doesn't mean I'm annoyed
neither does the image capture below
The best thread I have ever seen came from the old school geometric die heads. I still use them exclusively on gang tool machines when doing chucker work, perfect threads every time with one pass and never have to stop or reverse the spindle!
Burr free threads!
I agree with the preivous post, copy the threading line and have your threading pass exceed your thread depth, you should get one cleanup pass out of that.
Leave a little material on your lead in champher ( physical) and after your first threading cycle go back to your groove tool or finish turning tool and recut the champher from the thread side on the champher (G41) and then do a finish pass on the thread. The previous post was also right, a full form or cresting insert is no help in this area.
Be sure not to go the same direction as your first cut or you are just going to move the burr, not remove it.
You need to play with it, different material react differently, some need more materal left on it and some need less. Some you need to run two different angles.
This process should get you past a 10 power inspection magnfication, but I think it will just be a little plastic deformation which is not a probem for most applications.
Here's what I do to keep the threads lookin' pretty. K.I.S.S. method applies here, I'm discouraged from using manual processes in my programs so that the operators don't become confused.
Rough O.D. Then, thread using a regular threader (not a full-profile 'topper') Finish O.D. and and groove relief (if needed), then using the canned #1 thread process set some obscure depth (such as 1") and the threader will make just two passes over the thread to clean it up. Also changing the angle can help push the burr one way or another.
The resulting thread is smooth enough so that one can't shave with it, and (to the naked eye) is burr-free and suits most of our customers. One also gets the benefit of using a universal threader so that the operators don't have to determine what threader to use when changing inserts.