Presume I can use either cutter type, and presume I have a Brother Speedio with synchronized tapping, and assume all other things being equal such that the hole size is accessible for either process. Which cutter is preferred or is it a wash either way?
Follow along with the video below to see how to install our site as a web app on your home screen.
Note: This feature may not be available in some browsers.
Largest Manufacturing Technology Community on the Web
Stay Connected:
Tapping versus Thread Milling
- Thread starter drcoelho
- Start date
- Replies 50
- Views 3,600
crossthread82
Hot Rolled
- Joined
- Apr 1, 2022
- Location
- Maryland
What size thread? What material? How many holes/parts? How deep are they threaded? Need more info.
BALNH
Cast Iron
- Joined
- Oct 27, 2006
- Location
- New Hampshire
Even in titanium they’re are some nice Ti specific taps. As with anything context matters.
mhajicek
Diamond
- Joined
- May 11, 2017
- Location
- Maple Grove, MN, USA
I've used form taps in Ti6Al4V-ELI on short run production of 000-120 threads. I tried threadmilling first, and while it worked, it was slow, required constant offset adjustments as the tool dulled, and frequent tool replacements. After switching, the one form tap lasted over 100 holes (the rest of the run) with no adjustment, and was much faster.
Course or Fine Pitch? Tapping would be faster for sure! Imo with given parameters... Thread Mill.... It is a one off part anyways. Not sure how stout the speedio is but 20x holes at that dia x 1.0depth and course pitch is asking to scrap a part. If it's fine pitch you should be fine to tap it. Use a good tap though.
Last edited:
How do you figure? You're saying that a new tap, in mild steel can't tap 20 thru holes 1" deep without failing?
Your tooling bill must be thru the roof!
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
As can tapped holes when the machine has Rigid Tapping, as it was said to be assumed by the OP. Simply adjust the Z Start position to get the required orientation.
With Thread Milling, its preferable to start at the bottom of the hole so that the cutter is Climb Milling. In the OP's example of a through hole, the orientation can be adjusted also by varying the Z Start Point, but if the Thread had to finish at a particular hole depth, then a Start Angle at the bottom would have to be calculated to get the correct orientation.
Regards,
Bill
Last edited:
If this is a one-off part, it could go either way. Both tools will get the job done, but the threadmill will undoubtedly take longer in the mill. However, then you'll have a threadmill on hand that can be used for a wide variety of tapped features in the future. If you opt for the tap, you'll likely finish your part faster but will be limited by on-hand tooling in the future. Personally, I'd get a tap and call it a day, but I already have threadmills on hand so I'm only looking to keep cycle time down.
With a threadmill I generally do a could finish passes to ensure I've cut everything I need to without deflection, but I only ever need to do one or two features on a part, so the time spent re-running a toolpath isn't a problem. If you are running 20 threaded holes your cycle time is going to go up, up, and away.
RJT
Titanium
- Joined
- Aug 24, 2006
- Location
- greensboro,northcarolina
For larger holes (over 5/8") or high nickel alloys we thread mill, or if you need to get really close to the bottom of a hole. Might depend on the horsepower of your machine. Left hand thread mills are readily available to climb mill from the top of the hole. If it's easy to tap, that's our preferred method. Really oddball low quantity threads can be done with a single point thread mill, so it's like a universal tap.
angelw
Diamond
- Joined
- Sep 10, 2010
- Location
- Victoria Australia
Finegrain
Diamond
- Joined
- Sep 6, 2007
- Location
- Seattle, Washington
That's definitely a threadmill job if I were doing it, but only because I have a 30-taper mill.
Regards.
Mike
To me, especially with a Brother, if you can tap it, do. Nothing in the world makes a Brother happier than tapping. So, to my thinking, this is an obvious question. If you can go either way, why would you ever pick the one that is 10x slower and uses the more expensive tool?
Tap when you can, thread mill when you can't. Hardened steel, blind holes with threads all the way down, really oddball stuff like 1.5"-40, etc. Maybe if you need some unusual thread fit. If you have three holes to do, the job isn't going to repeat and you don't own the tap.
But if it is truly an "I could use either happily" then why would you ever not tap?
Tap when you can, thread mill when you can't. Hardened steel, blind holes with threads all the way down, really oddball stuff like 1.5"-40, etc. Maybe if you need some unusual thread fit. If you have three holes to do, the job isn't going to repeat and you don't own the tap.
But if it is truly an "I could use either happily" then why would you ever not tap?
crossthread82
Hot Rolled
- Joined
- Apr 1, 2022
- Location
- Maryland
Tapping is almost always faster especially for that. The only time threadmilling makes sense IMO is when doing titanium/inconel where tap breakage is more probable or doing a huge thread your machine can't tap, or a custom that a tap doesn't exist for.
But a M16 is a piece of cake for a speedio, spiral point gun tap from OSG, Balax, or Emuge will punch those in probably 10 times faster than threadmilling.
implmex
Diamond
- Joined
- Jun 23, 2002
- Location
- Vancouver BC Canada
Hi mhajicek:
You wrote in post #7:
"I've used form taps in Ti6Al4V-ELI on short run production of 000-120 threads."
You are one brave dude if I do say so myself.
Form tapping 000:120 in Ti6Al4V?...you have my undying respect for making that happen.
And I thought I did some crazy shit.
Just goes to show yet again, that nobody knows it all and we can all learn something from one another.
I just learned something new and very cool from you today, so thank you for that!
If you'd pitched it to me, I'd have sworn you'd never get away with it.
Of course I'd have sworn thread milling it was going to be the Devil's very own too.
Cheers
Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
You wrote in post #7:
"I've used form taps in Ti6Al4V-ELI on short run production of 000-120 threads."
You are one brave dude if I do say so myself.
Form tapping 000:120 in Ti6Al4V?...you have my undying respect for making that happen.
And I thought I did some crazy shit.
Just goes to show yet again, that nobody knows it all and we can all learn something from one another.
I just learned something new and very cool from you today, so thank you for that!
If you'd pitched it to me, I'd have sworn you'd never get away with it.
Of course I'd have sworn thread milling it was going to be the Devil's very own too.
Cheers
Marcus
www.implant-mechanix.com
www.vancouverwireedm.com
Last edited:
Such a general description of the application you got there. Instead of explaining my thoughts further... Let's just take bets and see how it goes... I say tap failure is likely. Ofc as previously stated idk how stout a speedio is. Other people say 16mm is a cake walk for it. We shall see! Wish the op success for sure either way!
triumph406
Diamond
- Joined
- Sep 14, 2008
- Location
- ca
16mm thru hole, tap failure is highly unlikely in the general course of things. I'd expect in MS, hundreds if not thousands of holes before I even looked at the tap. Based on experiance I'd use a coated tap, TiCn has worked well for me (ymmv)
I tapped 10-32 into MS right up to last thread on spiral point tap a while ago, would change the tap every 400 holes, not because I had too, but because a broken tap would be a lot more expensive then a replacement tap so didn't want to take a chance. With TiCN coating there was no visible wear at all.
