Nerdlinger
Stainless
- Joined
- Aug 10, 2013
- Location
- Chicago, IL
Just like the title says...any reason NOT to?
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:
Any reason to NOT max out rapid tap return?
- Thread starter Nerdlinger
- Start date
- Replies 14
- Views 2,803
BROTHERFRANK
Stainless
- Joined
- Dec 20, 2013
- Location
- SoCal
Depending upon the material being tapped, I think if you are using roll or forming taps there may be quite a bit of friction on the way out since the thread is formed and trying to spring back some. Of course you will need to look at the number of tapped holes you are doing and decide if any decreased tool life is worth the time you are saving by exiting faster. With cut taps I don't think friction on the way out is as much of an issue.
Atomkinder
Titanium
- Joined
- May 8, 2012
- Location
- Mid-Iowa, USA
Many machines never make it to max RPM anyway.
solidworkscadman
Hot Rolled
- Joined
- Mar 10, 2011
- Location
- MASS
For me it burns the taps up in 300 series stainless
Mike1974
Diamond
- Joined
- Nov 5, 2014
- Location
- Tampa area
That and the depth you are tapping should be a factor. Most of my taps are very short depths .3-.5". I have tried feeding some of these at 30ipm compared to 15ipm and I can't see a difference (4-8 holes typically). I have my tap retract set to 2x. I would be suspect of the controls ability to keep up after 3 or 4x anyways, unless you are using a drilltap machine to begin with...
Nerdlinger
Stainless
- Joined
- Aug 10, 2013
- Location
- Chicago, IL
It's a two year old Brother so I don't think the machine should be the weak point. I'm going in at S500. I tried retracting at max (S6000) but broke the 5-40 spiral tap X .550 deep after a few holes. I backed it down to S3000 (L3000, actually, for the retract word) and have made maybe 100 holes since so maybe I'll just keep it at that. Thanks for the help! 
Matt@RFR
Titanium
- Joined
- May 26, 2004
- Location
- Paradise, Ca
Are you tapping inconel? 16SFM is mighty slow. If you're in aluminum or even mild steel and it's a coated tap, why not go to 3000 RPM in AND out?
DMF_TomB
Diamond
- Joined
- Dec 13, 2008
- Location
- Rochester, NY, USA
depends on if little cheap part and if tap breaks you can just throw the part away and make another.
.
some metals break taps easier especially at higher rpm and if not enough coolant and or tapping fluid. after often spending a hour getting most of a tap out and still having little chucks in hole not allowing tapping without breaking another tap i usually find it is faster to go slower
.
some metals break taps easier especially at higher rpm and if not enough coolant and or tapping fluid. after often spending a hour getting most of a tap out and still having little chucks in hole not allowing tapping without breaking another tap i usually find it is faster to go slower
Nerdlinger
Stainless
- Joined
- Aug 10, 2013
- Location
- Chicago, IL
Ha! Nope, ANN4140. I'm using a Widia VariTap. Says 15-40SFM. I had poor life at higher feeds and it's better at S500 but now that you mention it I'm still not sold...maybe 500 holes MAX. Does that sound like good life for a 5-40 spiral tap .550" deep in 4140? I'm pre drilling with a 2.65mm ghuring.
Matt@RFR
Titanium
- Joined
- May 26, 2004
- Location
- Paradise, Ca
Not the same thing, but for you to reference, we tap 4140A thru 1/2" with a 1/4-20 Balax Tin coated form tap. Just happens to be 40 SFM and coolant at 8-10%, nothing special. Can't remember how long it's been since we replaced one of those taps... I'm guessing at least 900 holes ago. We're at 4x tap retract speed, but it's a thru hole too.
dstryr
Diamond
- Joined
- Jan 22, 2010
- Location
- Nampa Idaho
Form tap my friend... Control the minor diameter with a carbide drill to perfect size and your taps will last a lot longer.
Plenty of reasons such as tap length, tap size, thread size, material,tap type (roll, cut, spiral, etc). Larger diameter taps its prolly a non issue but with smaller ones it may cause pre-mature wear or breakage depending on the material or pilot hole size, depth, etc. Something else to consider is how much time you're actually saving. Is it really worth it to save a few seconds? For some jobs sure but for most I really doubt it.
I look at the increased tap retract speed as a productivity recovery tool as opposed to a productivity enhancement. I only use it when I think I'm tapping slower than I should be (poor setup, difficult workholding) and it helps to recover the loss. When things are going well I'm already pushing the tap close to the max and although it may not be cutting on the way out it's still generating heat. I've always looked at this function in this way but no one has ever explained it to me, it's just what made sense to me when I first encountered the setting.
If I double or triple the retract feed (also doubling or 3x the SFM), am I exceeding the manufacturer recommendations or do I get a pass because I'm not cutting?
If I double or triple the retract feed (also doubling or 3x the SFM), am I exceeding the manufacturer recommendations or do I get a pass because I'm not cutting?
