thread milling
thread milling
(OP)
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.
INTELLIGENT WORK FORUMS
FOR ENGINEERING PROFESSIONALS Come Join Us!Are you an
Engineering professional? Join Eng-Tips Forums!
*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail. Posting GuidelinesJobs |
|
RE: thread milling
P@
RE: thread milling
RE: thread milling
RE: thread milling
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.
RE: thread milling
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.