Breaking thread mills

[jeff]

What speeds and feeds do you guys use for tiny thread mills in A2?

Using a single point thread mill for an M6x1 thread, about 1/2" deep.

The first one did about 20-25 holes, broke at the shank, the 2nd did 2 holes, broke at the same spot.

This is the thread mill I'm using http://www.lakeshorecarbide.com/12singleprofilethreadmill58loc160cutdiaaltinctd24-56range.aspx

Material is A2 (not hardened), drilled hole is about 1/4" deeper than the thread goes.

200-250spfm, 6-8ipm. (4 flute)

 

I think it must be my cut depths, I'm taking 1 pass leaving .005, and then 1 finish pass.

Any suggestions?

Thanks.

[nickbe10]

25 minutes ago, jeff said:

I think it must be my cut depths, I'm taking 1 pass leaving .005, and then 1 finish pass.

Looks like about .02 - .025 thread depth (no calculator for exact numbers just in my head) so you might want to add a roughing pass or two, that's a pretty fragile cutter.......Also you are only driving a final arc of ,035R, not much motion there. What entry are you using? You really want the tool arcing on material engagement, but there is not much room to maneuver, perpendicular entry picking up .015 - 0.02 might be a bit much . S & F look like a reasonable starting point.

 

[jeff]

4 minutes ago, nickbe10 said:

 What entry are you using? You really want the tool arcing on material engagement, 

 

Yes, I have it entering on an arc.  1st a straight line (for wear comp), then an arc. 

I'll have to do more roughing passes I guess. 

Thanks!

[nickbe10]

1 minute ago, jeff said:

I'll have to do more roughing passes I guess. 

This is one of those balancing acts, room to do what you want vs. tool strength. I would be tempted to try the next size down if it gives you the reach you need.

Now you can complete the straight line move in "air" before starting the arc for engagement. You might not sacrifice much in time either with increased RPM even with lighter cuts, think High Feed Strategy...

[gcode]

This is what Carmex came up with ( note these are metric feeds and speeds)

I cannot recommend the Carmex line of HardCut thread mills highly enough.

You can also buy knockoffs from Harvey Tool

Try this software and select the Hardcut line.. I guarantee you will at least double

your tool life and cut your cycle time in half.

 

Note that they run G04 and G42 climb cutting from the top down

http://www.carmex.com/

%
O202
( FANUC I&J, RH, CLIMB, INTERNAL THREAD MILLING )
( TOOL - MTSH06047C14 1.0ISO )
( THREAD - PITCH :1.00 MM, DIAMETER 6 MM, DEPTH 0.25 INCH )
( TOOL RADIUS COMPENSATION - D1=0 )
N1 T1 M6
G90 G00 G54 G40 G17 G94 X0.000 Y0.000 S4450 M04
G43 H1 Z15.000 M08
( PASS NUMBER - 1 )
G90 G01 Z0.775 F2000
G91 G42 D1 X0.337 Y0.337 Z0.000 F162
G02 X0.337 Y-0.337 Z-0.125 I0.000 J-0.337 F162
G02 X0.000 Y0.000 Z-1.000 I-0.675 J0.000
G02 X0.000 Y0.000 Z-1.000 I-0.675 J0.000
G02 X0.000 Y0.000 Z-1.000 I-0.675 J0.000
G02 X0.000 Y0.000 Z-1.000 I-0.675 J0.000
G02 X0.000 Y0.000 Z-1.000 I-0.675 J0.000

[jeff]

Is top down the way to go for single profile thread mills? I'm used to using full profile thread mills from the bottom up

[gcode]

29 minutes ago, jeff said:

Is top down the way to go for single profile thread mills? I'm used to using full profile thread mills from the bottom up

with a regular thread mill spinning G03, a top down right hand thread is conventional milling... not ideal for tough materials

That's why the Hardcuts work so well

You cut top down G04 and you are climb milling

You toolpath it like a single profile cutter, but the  tool has three threads worth of flute so you get

a cutting pass followed by 2 spring passes all in the same toolpath

If you can go 2 or 3 pitches deeper than B/P spec,  you'll still get a good thread, even when the first set of teeth is badly worn.  

[nickc]

On 4/18/2018 at 8:58 AM, jeff said:

What speeds and feeds do you guys use for tiny thread mills in A2?

Using a single point thread mill for an M6x1 thread, about 1/2" deep.

The first one did about 20-25 holes, broke at the shank, the 2nd did 2 holes, broke at the same spot.

This is the thread mill I'm using http://www.lakeshorecarbide.com/12singleprofilethreadmill58loc160cutdiaaltinctd24-56range.aspx

Material is A2 (not hardened), drilled hole is about 1/4" deeper than the thread goes.

200-250spfm, 6-8ipm. (4 flute)

 

I think it must be my cut depths, I'm taking 1 pass leaving .005, and then 1 finish pass.

Any suggestions?

Thanks.

Make  sure you compensate for the actual arc size youre cutting

i use this formula

((hole diameter-cutter diameter)/hole diameter)* linear feed=feedrate at center of tool

 

example   3/8-16     with a 3 flute tool at .28 dia

(.313-.28)=.033

.033/.313=.105

 

linear feedrate example   .0013 fpt 

sfm 200

3.82*200=764

764*3*.0013=2.979   this is your linear feedrate

2.979*.105=.312    this your actual feedrate at tool center ---use this as you programmed feed

 

also slow feed by 30% or more at the first entry of the cut for at least a half revolution of the thread

[Pilot Plant Supervisor]

We have always used Micro 100 single point thread mills in infiltrated Tungsten, and Titanium, cutting top down G03 (conventional cut) with no problems. We cut right to size, but usually take a spring pass or two. I can't remember offhand, but I think SFPM is around 150 and only around .0002" chip per tooth.