Turning a custom thread w/G33?

[SRT Mike]

My last question for a little while, I promise.

I have a part that is 1.9" ID made from 6061 AL - just a cylinder basically. I have a "lens" that will screw in the front, just a clear piece of acrylic. I am making both parts so I can choose whatever thread I like.

I only have a MAX of about 0.75" worth of thread I can turn in the cylinder (because there is a shoulder at that depth), so I was planning to use a somewhat fine thread. I was thinking something like 1.9" 32TPI. It certainly won't be a standard size.

I am using a 16IRM AG60 threading insert which can do 8 to 48tpi threads. And here's whats confusing me

1) I've read the problem with the AG bits is the nose radius doesn't match the specific base of the thread groove, so you need to go deeper than usual to make sure you have clearance at the base (this is probably not a problem for me since I am making the mating part also). But how much deeper do you need to go then? Or would I just skim off the peaks of the threads on the mating part and make this a non issue?

2) The insert technical doc says to reduce the infeed amount with each pass (make each pass take less and less material). OK fine - I can find specs on what the thread depth of a standard thread would be, but how do I determine the thread depth (i.e. minor diameter) for a custom thread like this? Isnt thread depth going to be controlled by the pitch anyway since it's a 60-degree insert?

3) Iscar says "a finishing pass will be needed for partial profile cutters". OK, so what do I do, take a thou or two off with my straight turning but after I do the thread? How deep am I supposed to skim down? Just knock off the peaks? Match the major diameter?

4) How do you know how many passes to do? Iscar just says "several" - seems kinds hokey... I've read 4 passes would be OK in 6061AL with that light a cut, but the machinist in the company next door thought it should be more like 6 or 8, maybe more.

If anyone has a suggestion for the G33 command to cut a 1.90" (starting diameter) thread with a 32TPI thread, that would be good. I'm just not totally sure on how much to adjust my X values on each pass and what end X value I should be shooting for (especially given the nose radius issue).

Sorry for the length, my first time trying threading on the late if you couldn't tell

[Geof]

The multi-thread insert has a nose radius small enough for the finest thread it is suitable for; no choice...it has to be that small. This means of course that it is too small, i.e. the cutting depth will be deeper than a normal full profile insert for any thread coarser than the finest thread.

I have done a lot of custom 16tpi threads with this type of insert and I 'calibrated' the depth of cut.

The diametral difference between the OD and ID needed to be 0.065": in other words if I needed a 2.000" OD thread I would bore 1.935" for the ID.

The cut depth in both cases was 0.085" again on the diameter. On the OD the final cutting pass was around 1.815" and similarly on the ID the final pass was 2.020"

These figures do need a little playing around by a few thou depending on how loose you want the thread but I was able to thread mating pieces from scratch and have them fit very well.

Theoretically for 32 tpi you should be able to use 0.0325" and 0.0425".

I used G92 because I find it easier; just set the Z length, tpi and first cut in the G92 line then follow with multiple X values. I normally end with two or three passes at the same X for cleanup. The reason I like G92 is that it is dead simple to add smaller (or larger depending on OD or ID) X values to skim a little more off; normally I go three or five thou shallow at first so I don't overshoot. Never did figure out how to have the tool put metal back on.

EDIT:

My method to estimate the thread depth for any pitch is to just look a a tap drill chart; for instance 3/8"-16 uses 5/16" for a 75% thread so 0.065" diameter measure for the thread depth is a good start. I know someone is going to suggest going to the machinist's bible but my way works for me.

[SRT Mike]

Thanks Geof as usual

Here's what I did that seems to have helped...

First I changed go G71

I changed to 16tpi, because at 48tpi it was just too small and I was getting burrs like crazy. At 16tpi it is deep enough to be able to bite in and the thread looks pretty much perfect

I calculated the major and minor diameter in CAD knowing the teeth are 60 degrees and pitch of 1/16th". I came up with something of a diameter difference of 0.100 between major/minor. The threads were still sort of crappy until I switched to a 5-degree reflief away from the thread-in angle and just took 5-thou per pass. It is doing it in about 10 passes and I am sure I can speed it up, but at least it looks good for a starting point.

Now for the other side (mating part)

[Geof]

Originally Posted by SRT Mike ...I calculated the major and minor diameter in CAD knowing the teeth are 60 degrees and pitch of 1/16th". I came up with something of a diameter difference of 0.100 between major/minor. The threads were still sort of crappy until I switched to a 5-degree reflief away from the thread-in angle and just took 5-thou per pass. It is doing it in about 10 passes and I am sure I can speed it up, but at least it looks good for a starting point. Now for the other side (mating part)

Your 0.100 between major/minor is to a sharp point so your numbers correspond with mine.

What is your rpm? I find going fast and lots of coolant is the answer for a good finish. With threading many times the limiting factor is the maximum feedrate the machine can handle but remember to leave a bit of Z distance for the spindle to accelerate and get things synchronized.