thread milling 2

[debri800]

Could anyone give me advice on thread milling , want to try milling 1/4-20 threads in stainless steel. Feeds and speeds along with depth of cut would be a great help.

 

[Yahnozha]

depends on if your using a single point tool or a multi point tool. Since the cut depth is pretty small (thread height) and (if single point threading) you can go pretty fast since your not removing that much material. Think of milling with a small end mill, taking a shallow cut. If your using a multi point tool go a little slower...Sorry I dont have any feeds/speeds. I learned by trial and error.

P@

 

[fagantj]

What material the tap is used is also an issue. What is the material of tap is it?

 

[debri800]

Am using solid carbide multi point thread mill in 316 stainless steel.If this does not work will try form tap,any info on this would also be helpful.Thanks

 

[WIPLASH]

The speeds and feeds you want are not able to be calculated from the info. you've given.The correct speed is calculated from the diameter of the cutter and the feed is calculated by the number of flutes on the cutter.although the way to calculate feeds and speeds is as follows.3.82*surface feed /dia. of cutter= R.P.M. and for feed the calculation is R.P.M.*chipload*# of flutes=feed
an example calculation for 316 stainless,using a 4 fluted .5 Dia. cutter is as follows:

3.82(this is constant )*100(surface feet for uncoated carbide on 316 stainless)/.5(Dia. of cutter)=764R.P.M.
764R.P.M.*.002(chipload)*4(# of flutes)=6.112I.P.M.


These are approximate I would have to know what the diameter of the cutter is and the number of flutes on the cutter to give precise feeds and speeds.Also this calculation works for milling, drilling, boring, reaming and turning.This is with out a doubt the most accepted way of calculating feeds and speeds in machine practice.Though you must remember that machining is an art not a science so any calculation is approximate.Also alot of people round the constant to 4.from 3.819718634 I round it to 3.82 because over the last 12 years I have came to believe it calculates feeds and speeds more accuratley.

 

[scottmaha]

thread milling will work well in your application. however, i feel that form tapping would be your best route. form tapping works extremely well in ductile materials such as austenitic stainless steel - which is what class stainless 316 falls into to. you will want to use a good lubricating oil instead of conventional coolant for this to work well. form tapping requires more torque as you are displacing the material instead of cutting it.

you mentioned that you are looking for a 1/4-20 thread. i assume that this is a class 2B thread. if you you want to have 55 percent effective threads then use a .2312" drill. 65 percent effective threads require a .228"(#1) drill. if you require 75 percent effective threads then use a .225" drill. you will notice that the drill size for a form tap is some what bigger than for a cut tap. the reason is because the minor diameter of the thread is produced by the inward displacement of the material being tapped. also, i would recommend using a form tap with a TiN coating to increase lubricity.

the speed for a form tap is normally double of that of a cut tap. therefore, i would suggest starting with 35-40 SFM in 316 stainless using a TiN coated HSS cobalt tap. the feed rate will equal the pitch of the tap of course.

if you would rather take the thread milling approach, then try the following. you said that you were using a solid carbide thread mill. i would suggest a speed of 150-200 SFM. the feed rate should start at .0005 per flute. for example:

RPM = 175 * 3.82 / .25
= 2,764 rpm

FEED RATE(if using a three flute thread mill)

=.0005 * 3
=.0015 IPR(inch per revolution)
=2,764 * .0015
=4 IPM(inches per minute)

since you are thread milling such a small thread i would also suggest using the 60/40 thread milling approach. that is, take 60 percent of the radial depth of cut during the first pass and the remaining 40 percent of the radial depth of cut during the second pass. this will help reduce the chance of tool breakage. the diameter of a thread mill that can fit in a hole small enough to produce a 1/4-20 thread is around 3/16". so you see, that small of a diameter coupled with the fact that it is solid carbide makes it very susceptible to breakage.

another consideration will be the type of milling approach you will take. there are several types, but a couple of the preferred methods is the radial and tangential approach. in your case the tangential approach is the best method to use. this puts let stress on the cutter as you are programming the cutter to slowly arc into the material. the radial approach puts the cutter at the center of the hole and then feeding it radially into the material until you have reached the specified depth of cut. this causes chatter sometimes and could be detrimental to the life of that small of a cutter.

i could go into great detail in explaining this. however, i picked up a lot of this information from Kennametal's holemaking catalog. it is catalog number 0070. the information can be found in the technical section.