Please kick-start my first attempt at rigid tapping.

imported_brian_m · Aug 6, 2019

So, I have a new mill with rigid tapping, (Fanuc OiMF control) and a job to do. The job is to drill and tap the end of a number of 0.375 aluminum rods with a 6-32 thread to a depth of 0.375 inch to accept a screw to secure a knob. The flats for the knob are cut in another process because they must be aligned to other features.

I would appreciate advice to make a fast start on the project and reduce my learning time. I am happy with the coding side of things but I need practical advice.

I have built a jig so that two rods at a time can be mounted in a vise. The first process will be to mill the rods to consistent heights which will provide my Z surface. Obviously the next jobs will be to drill and tap which is where my learning curve steepens,

Questions.
The working thread in the rod needs to be 0.375 deep. How deep should I drill to allow bottom clearance for the tap yet still providing a true 0.375 depth of thread? (This will, I imagine depend on the tap).
Which specific type of tap should I use for this job bearing in mind I am tapping into a blind hole? I do not see that I could do the usual hand "taper followed by plug" so how will this effect the tapping depth and hole depth? I suppose I could machine taper tap followed by hand plug tap if I had to.
Should I chip break or peck with a 6-32 tap?

Thanks for any info. you can provide. I am really looking forward to using this new capability.

Brian

Booze Daily · Aug 6, 2019

Given that your hole specs don’t seem that tight, drill as deep as you need to, tap as deep as you need without bottoming out. I’d use a roll tap.

Cole2534 · Aug 6, 2019

I'd be using a bright finish spiral flute bottoming tap. Drill, chamfer, tap, repeat.

doug925 · Aug 6, 2019

6/32 is about the absolute WORST to cut tap. In any material.
The taps (no matter what mfgr) are weak, and will snap....

I STRONGLY recommend a thread forming tap, rather than a cutting tap.
Any plug style will get you the simple 3/8" thread depth, just drill a little deeper than required to tap.
IIRC a Ø.125" hole is the perfect size for thread forming a 6/32.

I would use a 90° spot drill to chamfer to Ø.15",a parabolic flute 1/8" drill to depth, followed up by the forming tap.
Standard, to slightly high ratios are okay, when using soluble oil coolant and thread forming.

Just my $.02

Doug.

Delw · Aug 6, 2019

personally I wouldnt use a vise to locate 3/8 round stock unless they were very short pcs.

I would use a collet, or a 2 3 or 4 multi collet block. due to rigidity and repeatability not to mention speed
for lots of parts I have a few 3 5c collet blocks, and my cycle time from doing 1 part to 9 parts isnt much different maybe 2 mins tops. because your tool change is what eats up your cycle time.

Locate as close to the top of part as possible.
face 1/2" endmill
center drill ( I only use keo style center drills I dont use spot drills cause they suck but hey thats me)
drill
tap
chamfer ( in my case I do this extra operation last but no need to if you dont want too).

spiral bottoming taps work best for cut tapping, roll taps are great also.
you may need to check with your customer on the type of thread Ie cut or rolled some customers have a preference or requirement.not to mention how deep you can go on the drill depth and chamfer size along with what angle for the chamfer.

if the chamfer is not specified I like a 120º gives a cleaner thread on the front end, doesnt give you a burr either.

.375 tap drill depth is not called out .600 works great., if you have specs then pay attention to them,including the minor size which will grow in cut taping.

no need to peck tap either one shot deal.

6-32 cut taps work perfectly fine all day long very rarely have any taps break. and we do thousands of 0-80 2-56 and 4-40 threads.

we do cut to length drill and tap often in both round a square, rectangle parts

imported_brian_m · Aug 6, 2019

Delw said:
personally I wouldnt use a vise to locate 3/8 round stock unless they were very short pcs.

I would use a collet, or a 2 3 or 4 multi collet block. due to rigidity and repeatability not to mention speed
for lots of parts I have a few 3 5c collet blocks, and my cycle time from doing 1 part to 9 parts isnt much different maybe 2 mins tops. because your tool change is what eats up your cycle time.

Locate as close to the top of part as possible.
face 1/2" endmill
center drill ( I only use keo style center drills I dont use spot drills cause they suck but hey thats me)
drill
tap
chamfer ( in my case I do this extra operation last but no need to if you dont want too).

spiral bottoming taps work best for cut tapping, roll taps are great also.
you may need to check with your customer on the type of thread Ie cut or rolled some customers have a preference or requirement.not to mention how deep you can go on the drill depth and chamfer size along with what angle for the chamfer.

if the chamfer is not specified I like a 120º gives a cleaner thread on the front end, doesnt give you a burr either.

.375 tap drill depth is not called out .600 works great., if you have specs then pay attention to them,including the minor size which will grow in cut taping.

no need to peck tap either one shot deal.

6-32 cut taps work perfectly fine all day long very rarely have any taps break. and we do thousands of 0-80 2-56 and 4-40 threads.

we do cut to length drill and tap often in both round a square, rectangle parts

Thanks for the suggestions guys. All valuable and I will work through them to find the best fit for my mill. DELW, I was not clear on my use of the vise. I actually made a pair of floating jaws that locate and clamp into my vise. These jaws are drilled and reamed to take the rod vertically and hold it firmly.

There is a groove around the rod but I still have plenty of room to drill to the suggested 0.6 depth. I need to order some of the taps suggested - you can't have too many taps.

This is not a commercial project, I use the machines to support my real business so thankfully I am under no pressure to produce in a hurry which gives me a chance to do things right.

Brian

G00 Proto · Aug 6, 2019

I didn't read everything so sorry if repetitive.

Drill .625 deep using a 3.2mm Guhring 2 Flute stub drill. 6000 RPM and 18 IPM, one shot no pecks.

Tap with a 6-32 Roll Tap .450 Inches deep at 1000 RPM, 31.25 IPM.

Feeds and speeds are conservative to accommodate most machines. I double them on my quicker machines. I'm guessing I run these specs ~10k per year, haven't found a need to change.

blkaplan · Aug 6, 2019

I'd also recommend a forming tap. Guhring makes great ones!!!

Sent from my Pixel 2 using Tapatalk

Mike1974 · Aug 7, 2019

G00 Proto said:
I didn't read everything so sorry if repetitive.

Drill .625 deep using a 3.2mm Guhring 2 Flute stub drill. 6000 RPM and 18 IPM, one shot no pecks.

Tap with a 6-32 Roll Tap .450 Inches deep at 1000 RPM, 31.25 IPM.

Feeds and speeds are conservative to accommodate most machines. I double them on my quicker machines. I'm guessing I run these specs ~10k per year, haven't found a need to change.

Nothing wrong with drilling a little extra deep, but it is not needed for a form tap.

We tap 4-40 and 2-56 all day every day in 6061 alum. The 4-40 tap drill (.0995") I drill .03" deeper than the tap, and the 2-56 tap drill (.0781") I drill .025" deeper than the tap. Your point, for 118deg is roughly .3xdia so for a 6-32 tap drill (.125") you would need to drill about .49" deep to tap to .45" deep.

This all assuming form/roll taps and rigid tapping in a solid (not compression/ext) holder like a collet.

edit: wanted to add this is for our own product so we don't have to meet any thread specs, if you are doing aerospace or gubmint, sometimes you can't use a form tap and need to cut tap to meet specs

G00 Proto · Aug 7, 2019

Mike1974 said:
Nothing wrong with drilling a little extra deep, but it is not needed for a form tap.

We tap 4-40 and 2-56 all day every day in 6061 alum. The 4-40 tap drill (.0995") I drill .03" deeper than the tap, and the 2-56 tap drill (.0781") I drill .025" deeper than the tap. Your point, for 118deg is roughly .3xdia so for a 6-32 tap drill (.125") you would need to drill about .49" deep to tap to .45" deep.

This all assuming form/roll taps and rigid tapping in a solid (not compression/ext) holder like a collet.

edit: wanted to add this is for our own product so we don't have to meet any thread specs, if you are doing aerospace or gubmint, sometimes you can't use a form tap and need to cut tap to meet specs

You’re a little braver than me on blind tapped holes even with a form taps, but what I called out is a bit excessive. Just happened to be the specs for the part I just ran.

Good point on form taps not working with some prints and inspection methods. Also worth mentioning they don’t work real well if you are very near to a part edge.

Mike1974 · Aug 7, 2019

G00 Proto said:
You’re a little braver than me on blind tapped holes even with a form taps, but what I called out is a bit excessive. Just happened to be the specs for the part I just ran.

Good point on form taps not working with some prints and inspection methods. Also worth mentioning they don’t work real well if you are very near to a part edge.

LoL not brave, just a necessity for us. If you inspect a form tap (modified bottoming) the first 2-3 threads or so are tapered, almost like wood screw but not to a sharp point. This gives you a tad extra clearance at the bottom of the hole.

Mike1974 · Aug 7, 2019

G00 Proto said:
You’re a little braver than me on blind tapped holes even with a form taps, but what I called out is a bit excessive. Just happened to be the specs for the part I just ran.

Good point on form taps not working with some prints and inspection methods. Also worth mentioning they don’t work real well if you are very near to a part edge.

Yes good point. We actually do some parts with holes near edge (not at work so not sure how close) that actually bulge the mat'l out a few tenths. We have to run the endmill back around them after they are tapped to hit our tolerance.

Search

Largest Manufacturing Technology Community on the Web

Search

Please kick-start my first attempt at rigid tapping.

imported_brian_m

Cast Iron

Booze Daily

Titanium

Cole2534

Diamond

doug925

Titanium

Delw

Stainless

imported_brian_m

Cast Iron

G00 Proto

Hot Rolled

blkaplan

Cast Iron

Mike1974

Diamond

G00 Proto

Hot Rolled

Mike1974

Diamond

Mike1974

Diamond

Similar threads