[jtrav]

Hi guys
new to CNC zone
But I am hoping you guys will help me

I have been running (setting, operating, programming) a CNC mill for just under a year
The controller is a A2100 which I think is a really cool conversational programming type.

I have had no problems up to now with tapping holes generally being M25 or under which the machine handles well

However I have a job that requires a 75mm dia hole with a 1.5mm pitch thread 40 mm deep.

Thread milling seams to be the answer, apparently! but I do not have any real access to CNC machining experience as I am a project engineer working for an electronics company and this is our only machine and I am the only one with any prevoius "metal cutting experience"

I think I should be using a bore cycle with the speed and feed set to cut 1.5mm pitch or possibly a helical milling cycle But it is the tooling that is my problem

I have been told that you can get thread milling cutters with indexable carbide tips.

Question: can anyone give me the manufacturer (Kennmetal, Hertel etc) and part number of a thread milling cutter

I am from Great Britain so I will not have access to American suppliers

I would also be greatful for any tips and strategies that I could use to do this job, i.e depth of cut, feeds speeds, tool retraction, orientating the tool etc

Please help I am a little out my depth here !!!

regards
jtrav

[hardmill]

Try Greenfield or SCT(scientific cutting tool)
Both make decent thread mills

[mikewsk2]

i don't know about in gb but advent makes good indexable threadmills, and they will even give you the g-code for the threadmill you/re using. i prefer writing my own because i can get cleaner code than they give me but it helps.
their address is http://www.advent-threadmill.com

[wms]

Jtrav,

I have used Iscar insert thread mills with great success.
They have metric inserts and several different sized tools.
You should have no problem as your hole (75 mm) is almost 3 inchs in diameter. No problem fitting a tool in that.
They will usually help with the program if need be.

[HuFlungDung]

To answer your question Jtrav, No, not anyone can help, but there are a few who can.

I use KBC Tools quite a bit for general tool supply
Toll free Phone (this number works from Canada, anyways):
1-888-522-8665

Page 298 of the current 2003/2004 catalogue.

If you want a replaceable insert type thread mill, there is a good selection of several Vardex thread mill toolholders available.

What would work would be KBC catalogue number
1-289R-220 ($300.80 canadian)
but, the actual Vardex cutter model number is
TMC-100-5

which is 1-inch shank dia, 4.38" overall length, 2.03" working length.

Insert for internal 1.5mm thread pitch is KBC catalogue number
1-2895-230
($82.07 Canadian)

This insert has a cutting edge is about 25.5 mm long, which will give you about 16 or 17 threads per pass.

Write yourself an incremental sub-program to make your milling cycle portable. Just move to the center of the hole for the start (and end positions) and then call the sub. Try to design a spiral lead in to the full depth cut, rather than a radial plunge.
Orbit, then retract to the center, move down an amount equal to some multiple of the thread pitch and cut the bottom half of the threaded hole, since your thread is longer than the insert is.

I found it works best to start low and spiral coming up (one thread pitch per orbit) while cutting. This keeps the cutter in climb mill mode for RH threads.

The feedrate that you would use would likely be .001" to .003" per cutter tooth per revolution, which would be a grand total of one tooth if using an insert threadmill. Just obey the normal speed limits for carbide in the base metal you are using. Use a good air blast to get the chips out of the hole, as you don't want them getting recut by the delicate points of the thread insert. Recutting a chip is like cranking your feedrate up to 200%.

Practise in a piece of MDF first

[EvilScooby]

If it's just a few parts you could get one of those Micro 100 brazed carbide thread mills and program the thread length needed one pitch at a time.

Of course you would have to hone a radius on the thread mill as metric threads have a radius at the root.

Good enough to get you by without spending a lot of dough.

[Fish]

Hello jtrav,

I've done this on a few different machines, but the process is virtually the same. The problem is that now all machines have a code for it. I would scour the manual first, then if you can't find it, call the tech support guys for your machine.

As far as tooling is concerned, maybe pay a visit to various websites like Iscar, Kennametal, Sandvik, etc. You'll probably find what you are looking for, as well as a way to contact your local rep/reseller. These companies also have pretty good technical support, including programming help.

Good luck.

Adam

[CAMmando]

If you dont have a CAM system amd your machine doesnt have a canned cycle for this, you want to make sure your machine supports Helical Interpolation. This is often an option in the controller that may or may not be activated (depending on what option package you purchased),

With Helical interpolation, You use G2 or G3 with a Z value. If the machine accepts 360 degre G2/G3 moves, then each Z is equal to the pitch. If the machine requires you to break the G2/G3 moves into quatrants, the Z is devided accordingly. Use cutter compensation so yopu can sneak up on the size. If the hole is blind it is sometimes desireable to start at teh bottom of the hole and interpolate up. With the size of your hole this probably isnt neccessary. Chatter is usually the result of not enough feed rather than too much. I think that ADVENT link above has some good tech data.

If your machine doesnt have helical interpolation, you need a CAM system to linearize the motion for G01 moves.

As far as what tool to use, there are many so look into what has been suggested so far. If you can find a hungry sales rep, maybe he will come in and get you going on the machine.

[jtrav]

Thanks guys
some quality advise here
I appreciate your help

regards
jtrav

[E-Stop]

Check out the Seco/Caboloy tools at www.carboloy.com Good tools, good company with a good reputation and I know our sales rep will bend over backwards to help out.

They also offer free software for threadmilling. I downloaded it a while back but haven't really got into using it yet but it looks pretty nice. It may help answer some of your questions and give you some cycle times ect. You can download a copy at http://www.carboloy.com/wizard/default.htm

[Kookaburra]

One tip,

If you want to do a right handed thread, don't make the mistake of starting at the top and climb milling the thread as you will find out it will be left handed so starting at the top will require conventional milling or if you want to climb mill you will need to start from the bottom. I would recommend Iscar tools with their IC9028 or IC328 grade inserts as the composition of the carbide and the coating they use is ideal for tip life in thread milling I have also used Seco tools for thread milling, they are not too bad on the big stuff but they are brilliant on the small stuff, M8 etc. Solid carbide thread mills.

[chleborad]

Hey,

Lately I've gotten into writing applications to generate G-Code for specific tasks (such as sphere generating). I was wondering if there might be interest in a software package that could generate helical milling toolpaths built from small linear interpolation moves. This way one could perform helical milling tasks, such as thread milling, on a machine that is not equipped with helical milling cycles.


Would people be interested in such a package???


-Cary

[CAMmando]

I do it in MasterCAM so I would not really have interest in a stand alone program for that specific task.

[HuFlungDung]

Onecnc and Bobcad also have a helix function, perhaps most CADCAMS already do this, plus quite a few tool companies provide little (free) applications to generate cycles for their thread mills. I tell you this just so you could decide if you thought it was worth your while to create another

[kombayotch]

Any place to mail order these at a reasonable price. The local guy is quoting me $160 for the SCT cutters. That seems outrageous.

[moldcore]

That price is not bad, not sure why they are so expensive but they are.
Try page 334 & 335 of the MSC catalog:
http://www1.mscdirect.com/CGI/NNPDFF...=335&PMCTLG=00

[kombayotch]

Hmm...

Has anyone tired creating a threadmill?

I was thinking that something that held lathe tools, like a fly-cutter, but at 90 degrees . Wouldn't be able to bottom out, but a heck of a lot cheaper.

I think I would cry if I broke a $160 cutter that I paid for myself.