# Mach3 Turn



## Blackhawk (May 15, 2015)

My attempt at threading using mach3 turn. The threads look worse than they are. I believe I got to take a smaller depth of cut. Anyone care to comment if my formulas I'm using are correct I would appreciate it. I used demensions from machinist handbook

Lanham


----------



## jumps4 (May 15, 2015)

rigidity and depth per pass seem to be the problem, try to keep the part as close to the chuck as safely possible.
reduce the amount the tool is sticking out of the holder.
your carbide sounded like it chipped on one of the last passes, look close at the point
I can't get carbide to cut mild steel very well I have gone to HSS tools with a lot better results
mild steel is really gummy so make the depth per pass .002 or less and try running 5 spring passes
in settings on the wizard try setting the min pass depth to .002 or less and the last pass to .0001 also set angle to 29.5 or 30 to reduce load on tip.
try threading at 300 rpm.
run in the lowest gear ration (belt ratio) you have for the most torgue.
the lathe seems to be operating fine and starting in the correct location each pass, finding the setting you need for your lathe rigidity seem to be all you need.
Steve


----------



## Blackhawk (May 15, 2015)

Thanks Steve
I tried again before I read your post, I changed the pass to .001 and ran it. A tad better but still to much chatter. 
I will lower the rpm and make additional changes you suggested and try again. I'm actually using hss inserts, I couldn't get carbide to work either

Lanham


----------



## awander (May 15, 2015)

You're in Diameter Mode; you don't want to divide the work diameter by 2 to arrive at your X coordinate setting. Enter the diameter directly in the X DRO after touching off on diameter.

Something is also very wrong with the program-you have an X start diameter of .247, and an X end diameter of .216. That means you are going into the part by (.247-.216) or .031, but that's on the diameter. The actual amount the tool should be going into the work(on the radius) is half of that or .0155. With a first pass depth of .009, the program should only do 2 passes. It's doing quite a few more than that.....

The number you figured for depth of cut is actually H, or the height of a sharp V thread, which is no longer used(for at least a hundred years). A UNF thread(See the figure below, from Machinery's Handbook 26)) needs to have different-sized flats at the root and the crest, equal in height to (1/4H + 1/8H) or 3/8H. So the depth of cut is 5/8H, which would come to .019375.




Also, the number for depth of cut is, again, on the radius. You need to double it for the diameter when you enter it into the wizard screen. This would give you 2 x .019375 or .03875 depth on the diameter. So your Xend dimension should be (.247-.03875) or .20825.

All those calculations, of course, assume that you are using a tool with the proper-sized flat on the end, which for a 28TPI thread would be about .009 wide and .008 high. If you use a sharp tool, or a tool with a different flat, or a rounded tool, the calcs will change. Not to mention that your tool, if it starts out sarp, will wear at the tip as you use it.

I usually start a thread with a sharp tool, touched off against the work, and if it wears, it just means my threads will be closer to correct(they will not have the sharp root)

I was trying to use Mach3 for threading last week, and I discovered that on my machine, at least, G76 is acting very strange. I got my threads cut (30TPI) but I really had to fight the machine for a while. I use a Smoothstepper, so that may have something to do with the problems I had. But I don't know what's up with yours......


----------

