threadmilling depths

skywalker4 · Jun 19, 2018

Hi,

I am working on threadmilling a 3/4-14 npt hole, my threadmill has one insert 14 pitch .790 dia. .550" long
I the major dia. at 1.035. i had to comp it .050" to get the gauge to fit correctly?

any ideas on where that .050" comes from??

Thanks........

DMF_TomB · Jun 19, 2018

skywalker4 said:
Hi,

I am working on threadmilling a 3/4-14 npt hole, my threadmill has one insert 14 pitch .790 dia. .550" long
I the major dia. at 1.035. i had to comp it .050" to get the gauge to fit correctly?

any ideas on where that .050" comes from??

Thanks........

.
tool dia comp, almost always need to take a few test cuts to get close. i usually record tool comp number when new and when dull like
1.0000 new
1.0050 dull
obviously can always recut more, but hard to put material back. usually safer to take test cut ALSO many times its best to rough out most of threads and take another finish cut of .005 or less to reduce tool deflection
.
i have had parts move in vise trying to take too much thread milling all in one pass. usually better to take a roughing then a finish pass
.
also if you got vise really tight many parts when vise loosened the thread milled holes will go out of round. just saying best to check threads again when part out of the vise or when vise is loosened

litlerob1 · Jun 19, 2018

Post a part number and manufacturer of the Threadmill. How is the Tool being held, how is the part being held, what Machine is it on, how many RPM? There is a lot to be guessing here.

R

DMF_TomB · Jun 19, 2018

skywalker4 said:
Hi,

I am working on threadmilling a 3/4-14 npt hole, my threadmill has one insert 14 pitch .790 dia. .550" long
I the major dia. at 1.035. i had to comp it .050" to get the gauge to fit correctly?

any ideas on where that .050" comes from??

Thanks........

.
had a guy use thread milling program so it came out you had to use 1.0000 for tool dia comp even though it was not a 1.0000 dia tool..... why?
.
cause somebody wanted tool dia comp to start out as a nice easy number to remember like 1.0000 rather than .8467 or other odd size. also tool was not easy to measure.
.
it did make things easier 1.0000 when new and 1.0050 tool dia comp when it was getting dull. change insert and it usually started back at 1.0000 tool dia comp again. when he made thread milling program he adjusted it so things came out that way on purpose

gregormarwick · Jun 19, 2018

skywalker4 said:
Hi,

I am working on threadmilling a 3/4-14 npt hole, my threadmill has one insert 14 pitch .790 dia. .550" long
I the major dia. at 1.035. i had to comp it .050" to get the gauge to fit correctly?

any ideas on where that .050" comes from??

Thanks........

Probably you did a simple circular helix rather than the spiral helix that is required for taper threadmillling. Doing a circular helix with a tapered threadmill leaves an axial step on the wall of the thread which will prevent the gauge from fitting, so you had to overcut it to get the gauge to go in.

If this is the case, then you have made a defective thread.

Alternatively, if you did all that properly, then you just had to tweak it to get the right size, which isn't uncommon with threadmills. However, .050" is a lot, so I'm inclined to stick with my first guess.

SIM · Jun 19, 2018

Could also be where your starting the thread. With a tapered helix, you might be engaging full depth a thread higher then your wanting to.

I found threadmills as in solid mills to be really pretty close to the given numbers. My indexable threadmills not so much.

skywalker4 · Jun 19, 2018

litlerob1 said:
Post a part number and manufacturer of the Threadmill. How is the Tool being held, how is the part being held, what Machine is it on, how many RPM? There is a lot to be guessing here.

R

its kennametal .790" mill, cant see the part number, in a endmill holder, test pc in a vise

here is the program. for a fadal 3016

T03M06
M01
M08
G54G00X0.0Y0.0S2901M03
G43H03Z1.0
G80
Z0.15
G01Z-0.5589F4.3
G41D03X0.0334Y-0.0334F8.5
G03X0.0925Y0.0Z-0.55I0.0201J0.0334
G01Y0.0003
G03X0.0947Y0.0Z-0.4786I-0.0925J-0.0003
G03X0.035Y0.035Z-0.4696I-0.0401J0.0
G40D03G01X0.0Y0.0
G00
G43H03Z1.0S2901M03
X0.0Y0.0
Z0.15
G01Z-0.5589F4.3
G41D03X0.0334Y-0.0334F8.5
G03X0.1038Y0.0Z-0.55I0.0273J0.0334
G01Y0.0003
G03X0.106Y0.0Z-0.4786I-0.1038J-0.0003
G03X0.035Y0.035Z-0.4696I-0.0441J0.0
G40D03G01X0.0Y0.0
G00
G43H03Z1.0S2901M03
M05M09
G28H00Z0.0
G53Y8.0
G54M30

litlerob1 · Jun 19, 2018

It appears that in the code you posted the largest diameter that the Tool is cutting is .9976" but need to be 1.0596".

Based on .9105"(Basic Minor diameter)+.0349"(Taper amount in .5589")=.9454+.0571(Thread Height)*2=1.0596.

R

Bobw · Jun 19, 2018

Its a Fadal.. There is probably fifty thou of backlash... :eek:

skywalker4 · Jun 20, 2018

no i was doing a helix.

gregormarwick · Jun 20, 2018

skywalker4 said:
no i was doing a helix.

Helix yes, but circular or spiral? Taper threadmilling requires a spiral helix.

I am not a Fadal user, but your code seems messed up.

Usually a spiral helix is approximated by splitting it into multiple circular helices with different centre points.

It seems that your code (I'm guessing cam generated) is attempting to do that, but is only outputting a single move instead of splitting into quadrants for example. That would explain the .0003" linear step between the ramp on and the cut, and the fact that the centre point is offset by the same amount.

Search

Largest Manufacturing Technology Community on the Web

Search

threadmilling depths

skywalker4

Guest

DMF_TomB

Diamond

litlerob1

Diamond

DMF_TomB

Diamond

gregormarwick

Diamond

SIM

Titanium

skywalker4

Guest

litlerob1

Diamond

Bobw

Diamond

skywalker4

Guest

gregormarwick

Diamond

Similar threads