lathe threading single point question

[Mike@Dive Lab Inc.]

Hello and Merry Christmas, can someone clarify or explain this for me, for example to cut a 1/2-20 unf thrdead on my HAAS lathe MCX says the thread minor dia is .4459. after I cut the threadI can tell by looking at it it's not deep enough. It won't fit a standard 1/2-20 nut. to get the nut to thread on I have to go approx. 0.010 deeper, this goes for any thread I try to do. I know there are many variables and classes of fit. I am using a partial profile Iscar 60 deg insert. My offset is correct. What am I missing here? besides experience!!how does the allowances button work? should I be using it?? what about a machine settng?

 

Thanks in advance

 

Mike

[kinglouie V]

tool nose radius??

[Mike@Dive Lab Inc.]

the insert is almost sharp approx. .005 r. It doesn't say on the box or catalogue it is a iscar

 

M type 16 ERM AG 60 ?

[Tim Simmermon]

Check to see that you are using Equal area cuts, not equal depths. Also set your last cut for .001 - .002. Also set for 1 spring pass to get rid of any deflection. Check in your insert catalog to get the recommended # of cuts. Also check your tool nose radius.

 

HTH

[Guest]

According to the Machinery's Handbook thread info, the minor should be .4392". I fiddled with the computer thread depth thingy, and although I know the basic major should be .5", you don't machine to that... usually it's .005 - .007 undersize (or something like that). So, if you change the .5 to .494, you get the chart minor diameter....

 

I know you shouldn't have to do this, but, what ya gonna do? Maybe you can modify the thread tables to make it correct... or the guys from CNC make it correct in a revision?

[Mike@Dive Lab Inc.]

I'll try that, I have been using equal depths not area I'll go play with ir right now

 

Thanks Much

 

Mike

[Mike@Dive Lab Inc.]

I just tried the compute from formula

 

I entered .493 for major and it gave me

.43887 for the minor

 

that seems pretty close to what I think it needs to be

 

Thanks.

Mike

[smokey_44]

check the minor dia by using the 3 wire method , that will tell you if your right or not (at the correct size)

 

 

Dave

[crazy^millman]

I would rather use my Anvil Thread Mic to check the Pitch Diameter. Unless you have a call out on the print to hit a Minor I always make my Class of threads to the pithc dia and if using a full profile insert everything else will be perfect.

 

HTH

[Mike@Dive Lab Inc.]

Thanks guys, I got it figured out

 

have a great weekend

 

Mike w.

[heavychevy2155]

I like to use equal area, cut the threads and measure with thread mics then just recut the thread most of the time i seem to have to move about -.015 to-.02 in my offset then everythings aok. Are you using canned or longhand.

[Andy]

Ditto with heavy. Equal area, canned, full profile tool, and thread mic (Calibrated on a known good thread), and adjust at machine till perfect.