Ya, it's 4140ph. I'll drop the SFM and see what happens.
Programmed via Mazatrol
I'd actually do the opposite...
KC5010 is a hard subtrate PVD coated insert. It needs a bit of heat to perform and prevent chipping. For KC5010 in 4140 in the mid 30's RC I'd be running a minimum of 230 SFM, but should be able to do ok up to about 500. Heat will help the chip flow better. But no amount of feeds and speeds will solve a rigidity issue in the setup.
Two things about the application you are doing.
1) When you cut your test piece it worked out, correct? Likely you had a short part in the chuck, with no rigidity issues...
2) You transferred over to the long part and now you have issues. This is because of tool pressure. No way around it with standard threading cycles so to speak. You have an .087 wide tool and as you get deeper the amount of tool engaged is .087" + the depth into the thread divided by the cosine of 14.5 degrees. So no less than a .087 depth of cut worth of tool pressure, but as you get to the depth of the thread, you are now talking almost a .quarter of an inch of tool engagement with the part assuming you are only cutting on the front edge of the insert, which if chattering is not the case....... That is a shit-ton of tool pressure.
So anyway, you have learned your machine is rigid enough, but the part isn't right? How do we fix this you say?
Two things:
1) Switch to KCU25 or KC5025 grade. These are a bit softer and will handle the deflection and lack of rigidity better. You are still going to want to be running somewhere 230-350 SFM.
2) You need to get creative on how you program this in order to minimize the amount of cutting edge engaging the part at a time. You can try a zig-zag/alternating flank cycle, not sure if you can do that on a Mazatrol, but my experience is it will still create too much tool pressure with an Acme due to the width of the land on the end of the insert. What you need to do is manually calculate out all of the thread starts and end points, for each diameter of depth of cut to go down the center, then front flank, then rear flank, repeat for each depth. You should be able to take about .010" to .015" per depth, but any more than that will likely get a bit greedy. As you calculate these, I would leave about .002-.003 on each flank for finishing, and before you get to the bottom you will want to flank the front and back at finish dimension, cheating off the bottom by about .005"-.010" this allows you to cut only with the flanks of the tool, with no end pressure, then take two final passes down the middle to final depth, leaving about .002" for the last pass, cheating the minor diameter a little if you can, but understand you will need to cut the flanks again to "dig out" the corners.
If it still chatters while doing this:
1) You can use a 5 pitch insert, but you may need to grind a little relief in it to get the depth. But it will have less tool pressure as the end is only .0689" wide or 20% or so less.
2) You can use a narrow grooving tool and pick out the thread bit by bit, then surface the thread using the radiused corners of the inserts. Very time consuming, very tedious, but will get it done guaranteed. I have a friend who has done this before on a manual lathe..... When you look at the thread you would never know that's how he did it. I think that was a 4" - 2 pitch ACME thread for a mobile track pin press, might even have been a larger pitch than that.
Best of luck. There is rarely an easy button when it comes to acme threading in the large pitch arena.
