Feed rate on Cold roll

[chakaloso]

What will be a good feed rate for a blind tap 9/16-18 on steel 1018.
depth 1/2".

[Geof]

Originally Posted by chakaloso What will be a good feed rate for a blind tap 9/16-18 on steel 1018. depth 1/2".

One that matches the pitch of the tap for the rpm you use .

I use 1000 rpm and a feed of 55.5556ipm.

[swain]

I tap at 100 rpm so the the time it takes the crunching sound to reach my ears lowers the time it takes me to slap the emergency stop. <ha>
Most tool salesman say i am tapping too slow....they most likely wanna sell more taps. Also...on you blind hole, drill at least .25 deeper than you plan to tap. Then tap using a spiral tap as it will pull the chips out of the hole.

As far as feed rate, that is figured out by dividing 1 by the pitch of tap then times your rpm.

1 divided by 18 = .o5555 x 100rpm = 5.5555 feed rate

Good luck!

Swain

[JDenyer232]

Originally Posted by swain I tap at 100 rpm so the the time it takes the crunching sound to reach my ears lowers the time it takes me to slap the emergency stop. <ha> Most tool salesman say i am tapping too slow....they most likely wanna sell more taps. Also...on you blind hole, drill at least ,25 deeper than you plan to tap. Then tap using a spiral tap as it will pull the chips out of the hole. Good luck! Swain

We routinely tap at a 1000RPM with taps as small as 0-80. Of course we are using form taps in aluminum. I have a 2-56 form tap that has tapped over 5000 holes and looks as good as the day it was bought. Trust your tool salesman here, you can be tapping much, much faster. Hope this helps.

[j-radkemachine]

9/16-18 TAP IN A BLIND HOLE IN 1018 CR

ALWAYS USE A SPIRAL TAP IN A BLIND HOLE.
THE STRAIGHT FLUTE TAPS ARE CHEAPER & WORK JUST FINE FOR THRU HOLES.
RPM- 600 DOES GOOD... YOU CAN GO FASTER AS STATED ABOVE 600's A LITTLE SAFER.

[chakaloso]

I want to understand this.

If I go faster it would be safer.

[j-radkemachine]

600 IS SLOWER THAN 1000 IS WHAT I MEANT BY SLOWER WOULD BE A LITTLE SAFER... TO BE HONEST I MAY EVEN RUN THAT 9/16 TAP @ ABOUT 500 RPM's BUT HAVE DONE IT @ 600

[Geof]

You do not mention what machine you are using but I suggest doing an experiment.

Do not put any tools, parts or tool length offsets in the machine. Write a little program to do your tapping as someone suggests at 100 rpm with a feed of 5.5556ipm. Listen the the machine and see if it is running smoothly while it is 'tapping'. Then try increasing the speed and feed and see how the machine sounds.

My experience is that if you try to go as slow as 100 rpm the machine cannot accurately synchronize the rpm and ipm so the spindle speed fluctuates. As you increase the speed it gets better.

I use 1000 rpm because it seems to run very nice and smooth and I figure why golower if this speed works.

[bremenrules]

I'm a fan of form taps (long lasting, but there are drawbacks), but make sure you keep those flutes(?) clean. I've noticed that 1018 will build up a black crud in the tap that affects the size of the holes.

Technically, Haas says you shouldn't go above 2000 rpm when tapping. I've gone significantly higher than that, but I wouldn't do it blind. Spindle reversal becomes an issue. 9/16" is probably going to run pretty darn slowly, so that shouldn't be an issue. 500-1000 rpm would probably work just fine.

[swain]

Well....the slower tapping comes from the haas hfo not installing rigid tapping
option like they were supposed to back in 99...I had a lot of bad exp breaking taps and killing pieces till I got that sorted out. Once the rigid tap issue was sorted out.....I have broken very few taps. It still makes me pucker up any time a tap enters the metal...hence the slow tap speeds.

The machine I use is a VF-3. It has no trouble tapping at any speed....slow or otherwise. The limitation is me.

On the subject of form taps. I thought they were great in 2000. I made a lot of parts steel and aluminum. They form a small ridge at the top of the thread that is no problem to me or anyone that I explain to reverse bolt a turn before
screwing in. But due to folks that don't know how to not cross-thread a bolt,
I started getting failures coming back that I had to fix. They would start the bolt in the small ridge that is formed at top of thread and use a wrench to ruin
the part. After a year or so of this, I quit using form taps for anything unless
I was going to be the end user. Ever heard the expression..."soandso could tear up an iron anvil in the middle of the desert with nothing but sand". Well...
I am getting cynical in my old age....

Swain

[bremenrules]

Come to think of it, Swain...I haven't had any problem with rigid tapping due to the machine itself. That option was installed by the HFO like the work order called for. For awhile, Mastercam would occasionally post out G84 cycles with a feed rate of 800mm/min regardless of the pitch or spindle speed. Or...if the program was feeling especially helpful, it would revert all my tapping and peck drilling cycles back to regular drill cycles. If anyone here doubts that drilling a tap into a steel workpiece is harmful, I have a small pile of broken tool bits to share with them.

I hear ya' on the form taps. The Greenfield tech suggested chamfering the hole *after* tapping to get that ridge off and all will be well. I've only tried it on 1018, but I think the material is too smeary to cut off cleanly with a bur (my traditional chamfering tool) and it messes up the top of the hole.

I'm probably a whole lot younger than you, and I'm still cynical.

[Geof]

Originally Posted by bremenrules ....If anyone here doubts that drilling a tap into a steel workpiece is harmful, I have a small pile of broken tool bits to share with them....

I believe you and the opposite is also true; tapping with a drill tends to drive the spindle load rather high.

swain you need to grab the bull by the horns or whatever cliche you want to use and just put the rpm up there. If you are dubious whether the tap can handle it or if the material is tough or stringy keep the speed up but do lots of little pecks. That is the joy of rigid tapping you can go at it fast (as in a good rpm) and slow as in several shallow pecks.