small thread close to shoulder

[hacdlux]

im trying to cut a m3x.5 thread in 303s stainless and keep running into a torn/smeared finish,

ive tried carmex full profile inserts, and applitec 766 2.0

the carmex inserts i get smearing until 3000 rpm then i cant get close enough to the shoulder.

the appitecs kept blowing the tips off

both inserts are having to be ground to clear the shoulder

running g92 between 600 and 2500 rpm .003 passes

we had one edge work out for a couple hundred pcs till it eventuallly wore out
but most of the time i cant get a run started

[MCImes]

I was just making some m3 threads on a 303 part. I used a g76. Im pretty sure this is the code I used:

G76 P031060 Q0010 R.001
G76 X.096 Z1.600 P0110 Q0050 F.01968 R-.002

In my experience when I get torn threads my initial cut has been too deep so try going with a smaller first cut.

Also one thing to look for, if your starting point in X is too close to the major diameter the threading tool wont clear the threads upon rapid retract and it will buzz over the top of the threads which looks like tearing unless you look very closely. So if a smaller initial DOC doesnt help try raising up the start point in X.

I usually do OD threading <.375" at 1000 rpm regardless of size and it always works for me.

Lastly, Ive noticed my threads are a lot nicer if I leave .001-.002 on the major and program a deburr pass to take off a couple thousandths after threading then give the threads another 2 or so passes at minor,

so, turn major .002 over, thread normally, turn major again to final size, thread again at minor dia 2 passes

[micky316]

If I was running G92 I would be at 1500ish rpm and start and do it in 10 or 12 passes the first 4 at about .1mm deep then gradually down to the last 2 passes at at .01mm two finishing passes at the finished depth,I would however normally use G76 and cut the thread in 10 or 12 passes same revs as before first cut at .1 to .15mm last cuts .02mm something like this

DIMN IN MM

X START AT 4.5MM, S 1500 RPM

G76 P020000 Q50 R.02 (you can change the P to P020060 if you prefer )
G76 X( FIN DIMN) ,Z( FIN DIMN), P=DEPTH,Q100, F=FEED

I presume you using neat oil ? to be honest any coated insert should have no problems getting a great finish and 1 edge should do hundreds of parts
Mick

[minardsanders]

I"m curious are you feeding straight in or are you leading the tool with a 29.5 or 30 deg. lead, this will help from loading and pulling the tool in which tears the threads. You might also try running your rpm down a little, try playing with this and see if it works.

[SirDenisNayland]

Add a spring pass and exponentially decrease the depth of cut. I never thread with constant DOCs, as the tool gets closer to the final pitch diameter more of the threading edge is used, thus more load, which is why you want to decrease the DOC as you appraoch final diameter.

Also check your tool center as I know threading tools can be a little trickier in part because you can't just face off the material until there is no pip. Tools are never plug and play, no matter what the manufacturer may claim.

Edit: also its my preference, but I generally don't thread any faster than 2000 rpm as your lead drastically increases and you run into more issues. Remember it may thread a second slower, but you'll be fiddling with it less, get it running quicker, better tool life and sometimes you just can't get the required lead without pulling out of the guide. I know a lot of people overlook giving yourself a proper lead, many think just give a pitch or two lead but fail to realize that as you up those rpms you also need to up your lead.

[hacdlux]

got it down now,
changed over to a g76 with a 30 infeed

on the g92
i was running .003 cuts to within .005 then .001 to minor with 1 spring
then ran the ood turn over
then 1 more spring

the galling was down in the flanks not on top of the threads

im not sure what was going on with the applitecs, they are normally my fall back insert(cuts any thing as long as im not doing long threads

[SirDenisNayland]

You never did mention if it was a thread on the front of the part or mid part. The only diference between g76 has over g92 is its angle in and angle out options, both will in effect create the same thread, except for g76 allowing you to control the way the thread ends, but since you were up against a shoulder you are straight pulling out anyway, which is why I ask if it was a thread on the end of the part or not. The only real time I've found to need g76 is for entering where a thread may have a shoulder on both ends, making it imposible to do a standard g92 straight feed.

Id be willing to bet its somethibg else you changed, or that you inadvertantly allowed yourself the proper lead with g76 glad you got it going.

Cheers