What's new
What's new

Breaking Taps- Blind Holes- Brother TC-S2C

biglord4ever

Aluminum
Joined
Feb 11, 2015
I'm tapping 1/4-20 blind holes in 6061- predrill .201" clearance hole 1.43" deep, tapping .85" deep. I've tried running both OSG and MariTool taps- spiral, semi bottoming. Originally pecking every .2", then reduced to every .1". 200RPM, 10F

The taps make it about 5 parts and then blow. I'm new to this, so what am I doing wrong?

Thanks in advance.
 
200 rpm????

I usually run 75 SFM (1146 rpm) for btm tapping in 6061, with a 1/4-20 spiral flute (any brand) cnc tap.
Also, try bumping the drill to 13/64" (.2031) as a minimum.
You have from Ø.1960 - Ø.207 to meet the minor diameter spec for a 2B thread.
Use a larger tap drill.

Also, are the shavings getting jammed in between the tap shank, and clearance hole? What diameter clearance hole is above the thread?
A depth of 1.43" before getting to the threads requires a longer tap (possibly DIN length??) and that too could be causing you problems.

For a full depth of .85" I would peck 2X (maybe 3, max) to get there.

What type of coolant?

Is the concentration enough?

My apologies for the rambling/ unorganized post. My ADHD med's must be wearing off.:D
 
Let me restate, I am predrilling to 1.43" deep and tapping .85" of that.

I was taught to tap at an RPM of 10x pitch and a feed of 10. But it sounds like that's a "bit" more conservative than you're running. ;)

Wallover 880 coolant. Define "enough concentration" for me.
 
...I was taught to tap at an RPM of 10x pitch and a feed of 10.
Whoever told you that sure as hell wasn't doing you any favors.

You would run a 1/4-28 slower than a 1/4-20 because it has less pitch???

RPM is material dependent. Feedrate is pitch dependent. 200 RPM is waaaay too slow for tapping 1/4" in aluminum.

My goto cutting tap for that hole is a Hy-Pro 298 series. No pecking, one shot to depth. 1000 RPM, feedrate 50 IPM. #7 tap drill. You should get in excess of 1000 holes in 6061 with that tap.

You can form tap too, no chips to worry about...

edit to add: I don't know what your clearance plane is, but I run more than .100" above the part when rigid tapping. Reason is I like to give the spindle a chance to get up to speed before I hit the material. .100" clearance means you are expecting the spindle to be at speed in 2 revolutions.

I usually start the tap at .500" above the part. That gives the spindle 10 revolutions to get up to speed.
 
"A feed of 10"

IDK what that is, but just the mention of anything other than "Thread pitch" scares me! :eek:



------------------------

Think Snow Eh!
Ox
 
Take some scrap aluminium. Bump that to at least 800-1000rpm, fill the hole with WD-40 or A9 and see if it'll bang it in 1 shot no pecking, use a good OSG spiral flute tap for AL. Then inspect the thread to see if its actually right, maybe something else is wrong with your code or whatever else. If it looks all good, then try it with your coolant, if it goes to hell, well I guess its your coolant.
Maybe also consider form tapping.

I go .70" deep in 304 stainless in one shot with 1/4-20's and cutting oil, 600rpm, rich coolant won't quite "cut it". AL likes a lot of lubricity too. Make sure the chips make it out of the hole and don't stick to the tap before it enters the next hole. When worried I call each hole as its own thing and M0, clean tap, fill hole, tap it, next. Yeah its a bit slower but nobody wins the race to making scrap parts either, 1000's oh holes would be a different story though.
I program in IPM for my rigid tapping, cad/cam thing, works fine, not sure what a Brother wants to eat for code though.
I too start about 1/2" away from the part.
 
Just toss the SF taps back in the toy box and get some form taps (prolly just one actually) and be done with it.

I waved the flag for form taps back in the 90's, but not as much these days with the new (?) SF/MB type taps. But 1/4" doesn't leave much gullet to git'cher chips out.

6061 forms up so nice - there's just no reason not to. You can roll right up to 100% thread and look like a champ and run forever - just so's you don't try for that 101%, which will overfill the tap and blow it....


---------------------

Think Snow Eh!
Ox
 
Just threadmill it and call it a day! I hate tapping! Lol! I avoid it as much as possible especially in blind holes, lol! You can threadmill any size thread, get em at Harvey Tool. [emoji6] That company has some really sexy tools. Good luck man.

Sent from my Pixel 2 using Tapatalk
 
what does your tap code look like? Should be:
G77 Z-.85 R.1 J20 S6000 ;

6061 you can tap up to 3/8" Dia at 6000 rpm with your brother easily. I prefer roll (forming) taps if possible. Tap drill should be .225" if using form tap. Make sure tap is held very well and can't slip in the holder (ER or SK). Make sure your coolant is rich (good lube). Also verify that your tap drill actually is going as deep as you think it is. You have a tapping hot rod.

Brother Synchronous Tapping - YouTube
 
I'm with Ox on the form taps. We have one job that repeats every few months with four 6-32 holes in each piece in 6061. Two thru, two blind. Last time I ran the job I form tapped 1400 pieces (that's 5600 holes) on a single tap. If you go that route, make sure you get the right tap for the right material and use the correct drill size.
 
What BrotherFrank said.....
also if you want to have some real fun, get a MA Ford 229 tap drill, run 10K rpm and 80 inches per minute.
Form tapping you won't need to drill as deep, and won't have to pluck chips out of the holes.
 
Is the idea behind using a faster speed that the inertia of the spindle will carry the tap in and require less force for the tap to cut- thereby reducing the amount of pressure on the tap flutes?
 
Is the idea behind using a faster speed that the inertia of the spindle will carry the tap in and require less force for the tap to cut- thereby reducing the amount of pressure on the tap flutes?

At 200RPM, you are not in the torque curve (Brother asks for a specific M Code when going that slow) and you are just rubbing the tap, adding pressure on the tool and material. It is just bad machining practice.

If 6,000 scares you , bump to at least 2,000 and add a peck in the middle.
 
Is the idea behind using a faster speed that the inertia of the spindle will carry the tap in and require less force for the tap to cut- thereby reducing the amount of pressure on the tap flutes?

I'll say part of the idea is that the machine has more torque at a higher rpm... But most of the idea is that you are cutting aluminum at tough steel speeds.

Also might be worth mentioning, although not important, even if you program it to go 6000rpm, the machine will figure it out, and may not ever get that fast before it slows down for retract.

It'd be fine for aluminum if you were on a bridgeport and had to reverse the spindle motor yourself while following along with the quill but there's no real reason to go so slow nowadays.

30 years ago machines might have a hard time following the pitch at higher rpm, but the machine you are running probably cries internally when you tell it to go slow...
 
Mine currently looks like this:

G77 X5.875 Y-0.255 Z-0.85 R0.2 j20 P0 Q0.2 F10

The speed is set at the top at the tool change line and is s200.

Your code is not good for your brother machine. make your code look like mine. add Q if you want to peck. maybe Q 0.6 .. you don't need to peck every 200 thousandths in 6061. you could tap at 6000 if you want or go 2000 or 3000 if you're chicken. no need to start the spindle with the tool change. the spindle is controlled by the S code in the G77 line. Also there are no M codes for 'rigid' tapping on the brother. brother uses synchronized tapping
 
Last edited:
The 10X RPM based on pitch with a feedrate of 10 IPM is standard here and we're one of the biggest mold shops in the world and routinely do taps up to 3" DIA, mind you most of our stuff is P20-HH or 1018/1020 and not that gummy Aluminum stuff.

1"-8 Tap we would run at 80 RPM's and 10 IPM.
 
The 10X RPM with a feedrate of 10 IPM is standard here and we're one of the biggest mold shops in the world and routinely do taps up to 3" DIA, mind you most of our stuff is P20-HH or 1018/1020 and not that gummy Aluminum stuff.

That makes sense. use G84 instead of G77. In aluminum do 100 x tpi for rpm and F100 IPM. On the brother I would use the G77 with J for TPI and S for RPM, Q for pecking.
 








 
Back
Top