Form taps or spiral.

[lwells]

After using floating tap heads for ever I finally have a nice new mori with a fifty tapper and ridged tapping. I want to get away from drilling holes deeper for chip clearence and eliminate picking chips out of the holes when done, and with my coolant flow I can't see if chips are clinging to the tap. I hear alot abought form taps but have never used them. I do a lot of cast and a fair amount of mild tool steels. Not looking for high volume production but would like to explore higher feed rates and more consistent thread depths. Assembly will thank me later.

[chris m]

Form tapping blind holes in steels is the only way to fly; we use OSG Hy-Pro NRT for simple applications and OSG ExoTap NRT for the harder stuff. If the 'cast' you're talking about is cast iron I think you're SOL with form taps; typically not recommended for those materials. We have used slow-spiral fluted cut taps in ductile iron with pretty good succes; fast spiral taps suck a$$, in my opinion, for anything except wrought aluminum.

 

C

[Guest CNC Apps Guy 1]

Threadmill the cast iron for sure. If I'm going to tap, I prefer roll taps. The OSG solid carbide form taps are awesome and if possible, go with High Pressure coolant thru spindle.

 

JM2C

[Norbert @ Shopware]

I worked with D2, CPM10V and A2 for 15 years and broke a ton of taps. Until I started to use the OSG roll taps. After I discovered these babies, there was no going back, especially on blind holes.

 

So, I second the posts above.

[Cad-Camr]

We tap around 1500 Rpm in our 50 taper Mori Horizontal in AL. It could probably handle 2,000 to 3000 Rpm in specific applications. Using form taps where you can will eliminate a lot of headaches. Thread-milling is also a great way to get close the the bottom of a hole when the part geometry wont allow you to drill deeper. We use mostly OSG Spiral Point Taps. Some Spiral Flute Taps in the larger sizes. Have fun with your new Mori.

[Tim Johnson]

While using a roll tap is highly preferred the cost of the part also needs to be considered. A broken roll tap is very hard to remove and usually results in causing a scrap part. If the cost of the material/part is low then the roll tap is the way to go. If the possibility of scrapping the part is going to cause hardship then thread milling or cut tapping may be the better choice.

 

We do roll tap 1/4" and smaller in alum at 4000 rpm all the time here.

[Bruce Caulley]

Just make sure you only rolltap materials within the correct ductile limits, otherwise the thread will be weak as xxxx.

 

Bruce

[Tinhman]

Well, i would like to go a little bit more details about this because a get one coming next week.

material is A36 bar stock 1/2 thickness x 1 wide and we have to tap 3/8-16 thru. 10 holes for each part and 500 holes total for this job.

We plan to drill it thru. with solid CB drill (3600rpm, 40-50 Ipm, one shot) then roll tap about 400 rpm.

My question is with this particular job, thread milling is a better choice? and if it is the case, what kind of tool, speed and feed i have to look for? Please advice

Thanks and have nice weekend

[somename75]

For what you just stated, I would have to vote roll tap all day long, it will be faster and cheaper than threadmilling, but if you don't feel like trying form taps, I've had great luck with osg hypro taps spiral flute, you can run them just as fast as a form tap in that aplication hth

[chris m]

In steel like you are going to machine you would have no problem with a Hy-Pro form tap, TiN coated. The RPM listed may be a shade on the high side, but I am always very conservative with speed in tapping, so you may be fine. I am only saying this because you said you don't use forming taps: remember that the prep hole is considerably larger for a roll tap than a cut tap.

 

C

[lwells]

I assume roll and form taps are the same thing. Almost all my jobs are one off. 1-4 parts. Mild tool steels and cast iron parts. I'm definetly looking into form taps,but would like to find somthing that works in cast iron as well. Set up my tool changer and leave em sit. Tool guy is trying to sell us some new stuff and i'm trying to get educated. Shop is slow so I get some play time. Thanks for the input.

[Quickmike]

The size of the hole before roll or form taps is critical. You may want to do a test piece to get the hole size dialed in. I have seen if the hole is to big before form tapping it will look like a double lead thread. It also is sometimes easier to crossthread a screw in a formed thread than a cut one.

[JMWorks]

We machine alot of cast iron also and for that I choose an emuge spiral flute cut tap. We have also had good luck with Dormer spiral flute cut taps and they are considerably cheaper. But for the steels and stainless steels I would agree with the rest, roll taps are the way to go and we also use the OSG roll taps 1/2 and under usually(have used the emuges with very similar performance). With a roll tap speed and coolant is critical as a lot of heat is formed and the faster you can get in and out safely and consistently-the better. Some experimenting must be done with roll taps in relation to tap drill size if you have a very critical tolerance. If its not an "aerospace" part the recomendations from the manufacturer are very close but that also varies ever so slightly with material and conditions of the system. Also important when roll tapping is to countersink the top of the thread, when it forms the first thread some of the material is displaced above the surface of the part. I am a big fan of roll taps especially since they are generally stronger than a standard cut thread.

[Tinhman]

I just wonder that Is it thread Milling will be faster process than roll tap in this case???

The tolerance of thread is not really critical and forget to mention we have thru. collant spindle.

Thanks and have a good day

[lwells]

Can you tread mill a 1/4-20?

[Guest CNC Apps Guy 1]

quote:

---

Can you tread mill a 1/4-20?

---

Is the Pope Catholic???

 

I've threadmilled 2-56 blind holes at .201 deep in Titanium. No problems whtsoever.

 

1/4-20... walk in the park.

[DavidSV]

I thread milled a 00-90 on some plastic... that carbon plastic all the new military stuff is molded from....

[moeh]

I could be wrong here, but the way I understand it is the tolerance of the tap determines the process to a point. For examole, we had some parts recently that had a 4H5H on a threaded hole. Our only option was to use a form tap.

[Guest CNC Apps Guy 1]

That's thread class right?

 

You can hold .0002 on pitch diameter with a threadmill. On a tap, the form is what it is. You can't change anything about it.