10-24 thread milling

[Quickmike]

Looking for some help with thread milling 152 holes in 304 stainless. tap drill .300 deep max. 10-24 unc 2B .17 deep min. I have done some thread milling before. But not with anything this small. We only have one thread mill. So I am hoping to get it right from the start. The cutter is tiny and I am afraid of breaking it.Especially with it being 304. Wondering how many radial passes to make and what depths for each.

[Matthew Hajicek - Singularity]

Working backward, I do two passes at nominal, one 20% of the material away, and another an additional 30% of the material away.  The material is figured as the radial distance from the pilot hole to the major diameter of the thread.  Also, the larger the pilot hole is the better; I tend to use 50% thread in steels unless otherwise specified.

 

[djstedman]

Well first off, the configuration of your threadmill will make a lot of difference on how this approached / speeds feeds etc. - You said the threadmill is tiny, I would expect it to be around a .140 diameter, if its smaller you probably want to go slower than what I will be suggesting.

 

You could have a threadmill with only a couple of teeth on it, or with teeth on the entire depth, given the short thread depth I will assume its going to have full engagement.

 

Another question would be number of flutes, given I don't know I will attempt to give you an idea for ipt and you will have to calculate from there.

 

I would start with 330SFM and .0011 per flute, 85% engagement on first pass and 15% on finish, best bet is to helical arc in and out of the cut with a slower federate used when arcing into the cut. You may find that adding a third pass as a spring pass will make a more reliable hole.

 

I would expect to have to comp the tool a bit when you start until it wears in a bit, and wouldn't be surprised if you end up having to comp it more as it wears, although I don't think 152 holes is asking too much of it, we have done over 1000 2-56 holes in 15-5 with one threadmill.

 

If the holes are a few each in a lot of parts this is no big deal but if they are all in one part.. well .. good luck with that .. since you will have to figure a way to check each hole (or every few holes)  as its done to make offsets to your comp value.

 

Anyhow good luck, although to be honest I don't think it should be that hard.. and for future attempts I would seriously look at Vardex, and thier TMGen software, its free and will recommend threadmill / feed speed based on material choice and depth etc.. It only recommends Vardex tools but theres always a catch I guess.

[gms1]

I threadmill a lot with tools smaller in diameter than that. I use the toolpath program from vardex to figure out my feed rates for all my materials. We almost exclusively purchase their tools so your tooling may require something different.

 

http://www.vargus.com/vardex/template/default.aspx?pCatId=9&pageId=75

[Quickmike]

Thanks for the help. We "had" a tool from Harvey in the multi form. Had 9 threads. Now we have a single form style and it is working pretty good.

[GIZMO 21]

Go into the harvey website.under the threadmill section theres some really good info

About feeds and speeds, depth of cuts for different materials,even a formula to figure out

Radial feedrate.good info. Just to check out. i recommend it.

[gms1]

Harvey does have some good stuff but I am just partial to Vardex. They have some really nice 3 flute threadmills that use 1-64, 6-32, 10-32, 1/4-28 on daily in 7050 alum and 15-5ph ss. Its the millipro style threadmill

[cncchipmaker]

Looking for some help with thread milling 152 holes in 304 stainless. tap drill .300 deep max. 10-24 unc 2B .17 deep min. I have done some thread milling before. But not with anything this small. We only have one thread mill. So I am hoping to get it right from the start. The cutter is tiny and I am afraid of breaking it.Especially with it being 304. Wondering how many radial passes to make and what depths for each.

Roll tapping would be much more efficient than thread milling. We have had great luck in 304, must use oil though and make sure the minor diameter is free of coolant before tapping