[Dadeslot]

I am trying to program a 1/4-18 not with a single point tool on my Haas mill unfortunately. All the software I use wants to use a single pass tool. Any help would be great.



Thanks,
Dadeslot

[I_flungdung]

Using a thread mill style tool?

[dcoupar]

I believe his post says "single point tool".

Out of curiosity, Dadeslot, why not tap the hole?

One more question, does your machine have the User Macro option turned on?

[tobyaxis]

I am trying to program a 1/4-18 not with a single point tool on my Haas mill unfortunately. All the software I use wants to use a single pass tool. Any help would be great.

Thanks,
Dadeslot

Right Hand Thread
Start the tool at the bottom about 1 or 2 threads past the bore.
Lead into the Pitch Diameter and call your cutter compensation so you can adjust the PD.

Helically CCW Interpolate two passes up.

Cancel your tool compensation then move to the next bore.

ex. Using tool centerline single hob thread mill with a diameter of .65D

N3
T3M6
G90G54G40G0X2.04Y-1.875S7000M3
G43Z1.H3
Z.1M8
G1Z-.6F50.
G41G1D3Y-2.331F20.
G3X2.04Y-2.331Z-.5167J.456
X2.04Y-2.331Z-.443J.456
G40G1Y-1.875F50.
G80G0Z.1M9
Z1.M5
G91G30Z0M19
M1

[dcoupar]

This one may get you close. It's programmed with a 3/8" single-point thread tool. No guarantees.

[Dadeslot]

Thanks that looks like what I came up with. I am using a Haas tool room mill so a pipe tap stalls my spindle + I have over 200 holes to tap in hastaloy I have tried the hob mills they do great for 2 or 3 parts but don't hold up well and at 150. a pop not cost effective. I have have good luck thread mill std threads in the past so hopefully this will work.

Thanks for the replies

Dadeslot

[tobyaxis]

Thanks that looks like what I came up with. I am using a Haas tool room mill so a pipe tap stalls my spindle + I have over 200 holes to tap in hastaloy I have tried the hob mills they do great for 2 or 3 parts but don't hold up well and at 150. a pop not cost effective. I have have good luck thread mill std threads in the past so hopefully this will work.

Thanks for the replies

Dadeslot

Hastalloy, yummy stuff. Use two cutters. First cutter take a few roughing passes, then the final pass with the second tool. Your tool life will improve and you will be able to get through more parts. Hasalloy is gummy and hard so light cuts are not a good idea. Use a cutter that has a Titanium Aluminum Nitride Coating.

Try Harvey Tool fair prices for micro grain carbide thread mills.

[cinomarra]

seco tools offers thread mills that will suit your application.
they are a bit pricey but they work great.we thread mill heat treated inconel 718 all day long, no problems.also if you go on their website they offer a downloadable interactive program called "thread milling wizzard" .just answer questions as you go along and it will give the g-code for any threading application.hope this helps

[Dado]

How thick is the work piece ? If it's less than an inch, use a high spiral cobalt tap. Also use a thicker mix of coolant, or tap heavy. Use a rigid taping method as well.

It's all what works. Threadmills are great time savers. I always use them on larger threaded holes. They are great for blind holes. When all else fails, use a tap and heavy lube.

You probable knew this all ready. But, I never know who I'm talking to. Brginner or otherwise.

Good luck

[DareBee]

Vardex has great coated threadmills as well.
They also have a free program (download) to generate the threadmill code.
Much easier to use than Seco's and isn't a massive download.

[Daleb]

we use Advent thread mills. On a recent job we made a 1/2"-14 NPT took two passes ran 750 pieces in 316 st. st. and only made one adjust.