Single Point Threading

[Toolfab]

I have never done this in a mill before. I guess I have a multiple point question. 1) Is there a tool somewhere in a default .TL9 file that I can use? 2) Does the "threadmilling" in MC utilize a single point tool well? 3) Why the hell would anyone single point in a mill rather than using a threadmill?

 

I would really appreciate some imput on this. Thanks all.

[Eric S.]

hello

 

 

the thread milling tool path does allow for a single poing tool. On the thread mill page at the top LH corner it asks you for the number of acive teeth change it to 1.

 

Eric

[Toolfab]

Thanks Eric!

 

What is the advantage to "single pointing" rather than using a multi flute solid carbide thread mill? To me, it does not make sense/

[Fig sign]

quote:

---

What is the advantage to "single pointing" rather than using a multi flute solid carbide thread mill? To me, it does not make sense/

---

4 me ,it has a lot of sense ...---... Custom thread pitches !

U can do any pitch U like like metric 2.02 (It is mostly needed for moldmaking where plastic expansion must be taking into account when doing mold )

 

Iskander teh custom thread cutter

[Eric S.]

I'd rather use a multi point tool if I have one. But a single point tool is much easier to make yourself in a pinch. Another reason maybe that there are less teeth engaged in the cut so the tool will not deflect as much? Even if you have a multi tooth tool I sometimes lie about the # of teeth so that the tool will do more passes and reduce the springing. Hope this helps!

 

Eric

[Toolfab]

I never really thought about that Iskander. That is a valid point. Wouldn't the time saved on the machine justify haveing a couple different thread mill's rather than a single point? My understanding is that thread milling is faster than using a single insert?

 

Again, just trying to understand!

 

[Eric S.]

Very good point Iskander I forgot about that one!

[Smit]

Single point tools are cheaper, much cheaper. That's important in my shop. You can use one single point for a number of different thread types, so not as many tools to track in inventory. So if you use them only occasionally, and don't run a large quantity of parts, they do make sense.

[Eric S.]

Paul you are right to think multi point is faster. It has always been the case when I have done it. I think it come down to the question of is it worth buying the thead mill for the job that you are going to run?

[Fig sign]

Paul !

 

Every year I make 50-70 different threads ,different thread profile ,angles and pitch on inserts and electrodes .

None of this threads are standart

Or too big to buy a tool for one thread .

So at my place rules thread cutting with a lathe thread cutter or smthn similar .

And self-made cutters for non-standart profiles .

 

[ 12-03-2003, 11:33 AM: Message edited by: Iskander teh Lazy ]

[Toolfab]

quote:

---

50-70 different threads

---

YIKES that would be alot of tooling if it were not a single point. It is nice to see some pro's and con's. We make thread mills here, so I have a one sided bias that I am proud to show...

 

I have always wondered why people would single point, in your case Iskander, I can now understand. Have you weighed the cost of resharping a thread mill rather than buying new inserts? In the long run, are YOU still better off with single point?

 

The amount of time spent in the hole is an incredible difference. If you are making a 12 pitch 1in deep, set your active teeth to 1 and not the time in backplot, then set it to 48 over a 1 LOC threadmill. That to me makes it worth it. Machine burden rate is more than the cost of the thredmill. If this is something you do all the time, it might be worth it.

 

Thank you for helping me understand the reason behind the single point!

 

to all that posted

[Fig sign]

Consider how much will cost and time of delivering a thread cutter for not standart pitch and who will guarantee I`ll use it ever even one more time .

Every plastic has it`s own expansion (regression ) .

In my case when my boss says do this thread my reaction time is 2 minutes to set tool and 15-20 min to start working max .

[crazy^millman]

Another point is that you can also do the odd ball lengths where as most thread mills will only do a certain depth acarbide single point tool if used the right way can do a dpth of over 2". The good point expressed above like many different pitchs is a great one also. I also like them for the low profie also in place where speace is tight. It is great where you have the chance to use inserted tools but where in the place you have one part most times to make threads on the inserted tools could end up cosing more than the whole job. I also use the single point tool id and od like on pipe threads where as on a inserted I think you would need 2 inserts. I also like the single point tool if doing different thread pitchs on the same part makes one tool go pretty quick and cheap.

 

Crazy Millman teh Micro-100 make a great tool for this as well as Internal Tool

[robk]

After I'm done thread milling a through hole with a single point cutter, I could go back in thru the tapped hole and chamfer the opposite side without flipping the plate. 2 birds with one stone.

 

Rob

[Kenneth Potter]

In pipe (NPT)tapping holes that the print calls for the tap hole to be flat bottom & shallow( CLOSE TO THE BOTTOM THREAT )I use the powdered carb tread mills 80.-350$

OR A SINGLE point.....this allows room for the bottom tread (TIGHT) to get close to the floor of the blind hole..comp out the size

[Mgrenier]

Well Paul,

 

Here, we make custom parts that are one shot deals. So, for us it makes more sense to buy a single point thread mill bar on which we can put a wide variety of inserts. Plus, we make big parts, where can you find a thread mill tool that can do a M90*5 hole with a 120MM depth of threads?

 

Just my opinion,

 

Have a nice day,

[jimp]

All we cut here is Quartz so our tools are Diamond formed tools. The problem I have with Thread mill is that I need to take multi cuts which means having to draw numerous arc at diferent step sizes is there a C hook that allows Multi thread cutting?

[jimp]

All we cut here is Quartz so our tools are Diamond formed tools. The problem I have with Thread mill is that I need to take multi cuts which means having to draw numerous arc at diferent step sizes is there a C hook that allows Multi thread cutting?