Common machining myths

OK. There are many things that I read over and over here and things I used to hear in the shop that are just plain old myths.

So, let's clear a few things up.

I'll start:

1) You can't/shouldn't cut through a flame cut edge. Maybe this was true in the old days of HSS and poorly controlled NC torches. In the carbide era, this is a non issue. The scale from the flame cut is a bit abrasive, just like hot rolled mill scale, but it is not hard. Mild steels can't be hardened this way, there is not enough carbon.

2) Tapping takes a lot of torque. I'm guessing this is a common myth because it feels like a lot of torque with a tap handle. Even the wimpiest Bridgeport should be able to tap 3/4-10 with the back gears in low. Even small VMCs usually have plenty of torque for this kind of operation. Form taps take more torque, but are rarely used in large sizes.

2B) Taps need to be held in special collets. Related to the last one. I wish I had thought of those ER tap collets. What a racket. I've tapped bazillions of holes with taps in regular ER collets without issue. This includes form taps up to 5/8".

3) Moly Dee/whatever oil is required for tapping. Maybe in some god awful material. For 95% of material, a regular flood coolant with an EP additive (they all have that) will work just fine. Keep the concentration around 8-10%. I've tapped bazillions of holes with nothing but flood coolant. That includes form taps. The sticky oil is really a detriment in really stringy materials like aluminum. It can trap the chips in the flutes.

4) Form taps don't work for XYZ material. I haven't machined everything, but I've used form taps in tons of different materials. The only things you can't tap with a form tap is cast iron (brittle materials), steel over 32RC, and most plastics. It works great in 304 stainless, mild steel, aluminum (including 7075), and tool steels up to 32RC. I do use oil with the tool steels, but everything else is run with just flood coolant.

5) Carbide drills chip/break in steel. I'm guessing this is happening to the manual guys. Carbide drills need a lot of feed. Even small 5/16" drills should be fed at .0125/rev. I've drilled bazillions of holes in all kinds of steel with carbide drills.

6) You can't peck with an insert drill. Why the hell not? I've done it plenty of times with plenty of drills. Never an issue.

7) You need to spot for HSS drills. BS. Holes are not precision locators. If you need precise locations, a drill should be the first step in a multi-step process. A good quality, sharp, HSS drill should hold .02" true position all on its own as long as you are drilling into a flat machined surface. If you need a chamfer on the hole, a spot with a 90 degree spot drill to the chamfer diameter before drilling is a handy time saver. For general clearance holes, it's not needed.

8) Coated drills won't work in aluminum. Sure they do. Black oxide is not the greatest for this application, but it's not going to self destruct. You need lubrication for aluminum. Once again, I've drilled bazillions of holes in aluminum castings with TiAlN coated carbide drills.

I'm sure I will come up with more. I'm interested to hear what folks have to say.

I agree with most all that. But would only add one caveat to number 2): large NPT taps can really bog down a spindle.

And I tapped with plain ole' collets for years myself. Until I found "Bilz" style holders. Now I'm just spoiled. I have a full set of #1's. They were like my Talon-Grip jaws, I just couldn't live without them LOL (okay, I just really wanted them).

wheelieking71 said:

I agree with most all that. But would only add one caveat to number 2): large NPT taps can really bog down a spindle.

Click to expand...

Start buying interrupted tooth taps. They cut a lot more freely. I don't use anything else. However, I don't think you are supposed to use them on cast iron.

Once again, I hold them in regular collets.

ewlsey said:

For 95% of material, a regular flood coolant with an EP additive (they all have that) will work just fine. Keep the concentration around 8-10%. I've tapped bazillions of holes with nothing but flood coolant. That includes form taps. The sticky oil is really a detriment in really stringy materials like aluminum. It can trap the chips in the flutes.

Click to expand...

I do the same but at 4-5%. Usually with the tap in a collet with thru spindle on runing thru the gaps in the collet.

ewlsey said:

6) You can't peck with an insert drill. Why the hell not? I've done it plenty of times with plenty of drills. Never an issue.

Click to expand...

Inserted drills are (usually) designed with the idea of a continuous chip. Are they ridged enough to peck? Of coarse they are, but you trade off insert life.

#7 needs repeating,especially this part "Holes are not precision locators. If you need precise locations, a drill should be the first step in a multi-step process."

Geez,people post stuff like,"I can't hold my hole tolerance to .002 diameter and my location is off .002,I"ve checked everything,WTF ?"Funny.

That you need 8 bazillion rpm to make a carbide insert work. This is false, you just need properly finished inserts to work with your setup.

I think exkenna has lost his hair trying to express this point.

ewlsey said:

OK. There are many things that I read over and over here and things I used to hear in the shop that are just plain old myths.



5) Carbide drills chip/break in steel. I'm guessing this is happening to the manual guys. Carbide drills need a lot of feed. Even small 5/16" drills should be fed at .0125/rev. I've drilled bazillions of holes in all kinds of steel with carbide drills.

6) You can't peck with an insert drill. Why the hell not? I've done it plenty of times with plenty of drills. Never an issue.

Click to expand...

Usually The reason carbide drills chip is because people chuck them in cnc lathes (Non Driven) and there not on center line in a mill this is not an issue or with driven tooling on the turret, providing the turret has not been smashed badly off center.

As for pecking with insert drills (not the full interchangeable point type only one's with indexable inserts) the only problem that can arise is that a stray chip can stay in the hole and when the drill comes back in it hits the bottom jamming the chip and rubs on the bottom of the hole and can break the insert.

"Carbide does not like an interrupted cut." <--- the kind of crap you read on a home shop machinist forum.

I haven't put my foot in my mouth yet today and I'm running out of time so here goes..........In answer to number 4 comes my comment about form taps and cast iron. I have valve guide knurling tools that are basically a form tap. I use them on cast iron cylinder heads. They create threads, the hole gets smaller and then another form tool is twisted through to form the desired size.

7) You need to spot for HSS drills. BS. Holes are not precision locators. If you need precise locations, a drill should be the first step in a multi-step process. A good quality, sharp, HSS drill should hold .02" true position all on its own as long as you are drilling into a flat machined surface. If you need a chamfer on the hole, a spot with a 90 degree spot drill to the chamfer diameter before drilling is a handy time saver. For general clearance holes, it's not needed.

8) Coated drills won't work in aluminum. Sure they do. Black oxide is not the greatest for this application, but it's not going to self destruct. You need lubrication for aluminum. Once again, I've drilled bazillions of holes in aluminum castings with TiAlN coated carbide drills.

I'm sure I will come up with more. I'm interested to hear what folks have to say.

Click to expand...

7)You do need to spot or center drill if you are gonna tap it later though. Also general clearance holes quite often require tighter tolerance than 20 thou out.

8)TiAlN coating is NOT for aluminum.
Its just not how this coating works. Aluminum just sticks to it and galls up the flutes really fast. You get BUE and bad surface finish.
You must have meant TiCN or something

end mills don't plunge well - hehe these ones have extra clearance on the face across the lugs

reedeprintice said:

end mills don't plunge well

Click to expand...

They don't plunge well at all. I spent a lot on endmills before I figured out how to make halfway decent toolpaths that ramp or helix into the part.

You can say that EM's will plunge, but you can ramp or helix in far faster with less tool damage.

Your video appeared to show a 1/2" EM stepping down .1" or less with a .3 or so stepover in mild steel. Looks like a 1/4 HP cut with an endmill that can handle 20 HP if it had less stickout. If you did a shallow lead in at the full DOC of the endmill with a .075 or so stepover you could remove material a lot faster and without burning the bottom .1" off your endmill while the rest is still new.

I mill a lot of 1045 with a coated 1/2" 4 flute and it's amazing how fast you rip out a pocket with a steep ramp in toolpath.

As far as myths go-

I was taught to break the chip every turn when hand tapping with a straight flute tap. I find the tap usually makes it through a hole as deep as the flutes before the flutes pack when you don't bother.

I was taught to center drill with a center drill and quickly figured out that spot drills are king and are not needed for most drilling operations. Spot drilling wastes time for most programs.

I was taught you had to turn the compound to some magic number to thread on a lathe. Threads turn out just fine if you don't bother.

Told to never use the side of a grinding wheel. I tried it once and nothing bad happened. Been using the sides of my bench grinder wheels for many years now. Works fine.


Overall, I've been taught lots of generalizations that just aren't true across the board. There are times when you need to use a HSS form tool in a CNC lathe, times when you need to turn an 1/8" pin with a negative rake CNMG432 at 500 RPM and it works, times when you plunge with a side of a lathe insert that isn't supposed to cut, but it does, times when you chuck a square part in a 3 jaw to part it off or put a lathe parting blade in a 3 jaw drill chuck for an instant slotter to cut that little keyway.

zero_divide said:

7)You do need to spot or center drill if you are gonna tap it later though. Also general clearance holes quite often require tighter tolerance than 20 thou out.

8)TiAlN coating is NOT for aluminum.
Its just not how this coating works. Aluminum just sticks to it and galls up the flutes really fast. You get BUE and bad surface finish.
You must have meant TiCN or something

Click to expand...

Stop perpetuating this BS.

There is no need to spot for a tapped hole other than to get the chamfer. A hole .02 out of position is not going to break a tap. If you need locations tighter than .02 TP, go ahead and spot. How often is that needed? If it needs to be .001 or less, you need a few follow up tools.

TiAlN works fine on drills for aluminum. Buy yourself a Guhring 5515 or YG-1 Dream drill in your favorite size. Those are both TiAlN coated. Now turn on the flood coolant and drill a few thousand holes in the shittiest, gummiest aluminum you can find. I guarantee positive results. We used to get 4000 holes with them in abrasive cast aluminum. TSC helps, but is not necessary. I never pecked anything under 5XD.

Fear Factory said:

As for pecking with insert drills (not the full interchangeable point type only one's with indexable inserts) the only problem that can arise is that a stray chip can stay in the hole and when the drill comes back in it hits the bottom jamming the chip and rubs on the bottom of the hole and can break the insert.

Click to expand...

This is the part that is a myth in my mind. An insert drill is a center cutting tool, even though each flute only cuts half the total diameter. So, anything "trapped" in front of the drill is just going to get drilled. That's the whole point of a drill.

If the geometry of the tool was such that a chip could somehow get under the cutting edge do some kind of damage, it seems like it would not be able to cut in the first place.

ewlsey said:

This is the part that is a myth in my mind. An insert drill is a center cutting tool, even though each flute only cuts half the total diameter. So, anything "trapped" in front of the drill is just going to get drilled. That's the whole point of a drill.

If the geometry of the tool was such that a chip could somehow get under the cutting edge do some kind of damage, it seems like it would not be able to cut in the first place.

Click to expand...

I think what can happen is that the edge of the insert hits the chip at the bottom of the hole, and instead of sitting still and being cut, the chip catches the insert edge and spins around with the drill. So now the drill is not spinning in relation to the chip, and it's as if you're trying to push the insert edge through the chip at zero rpm. Sometimes there will be enough friction between the chip and the bottom of the hole, so it'll stay still and be cut, but sometimes the insert edge will break first.

1) The sharpest tool in the box is the best on for the job. Wrong, often a duller tool does much better. Ever change a lathe insert, and started getting chatter all the sudden? Ever change an Endmill and have the same problem. Dead sharp is rarely desirable, it causes cutting edge chipping, and for some reason I've yet to understand, can encourage chatter. This also extends to drilling, in some materials, notably beryllium copper, a new drill is last thing you want to use.

2) The best way to solve chatter is by reducing cutting parameters. I always try a little more feed first, then perhaps a little more or less speed (I let my musicians guttural instincts decide). Then I try a duller cutter, (see above). About once a month, while assigned to the lathe department for the night, I will walk over and find the Job I'm going to be running is something like .5" in diameter, 6-9 inches long. The operator will have slowed the finish pass down to 100 rpm, and .002 inched per rev. Now I normally don't take our lathe spindles over 2000 rpm, because of the pucker value, an the parts are normally big enough it's not really needed. But in this situation, seems to work really well, then I bump the feed factor up by 4 or 5. I get a better finish, and much faster cycle times.

3) Files should not be kept in a drawer, because if they bang against each other they chip. I've had the same files in one drawer for the last 15 years, the only damage I can see is on my lathe file, from when I was spinning to fast, and used it to break an edge. Also see number 1, for some reason I've always preferred a well worn file, over a brand new one, they catch less, and seem to leave a better finish.


To the the comments about tapping collets not being necessary, I've run into situation where they were. This issue HAS always been on a lathe with live VDI holders. If you've not used one of these poorly designed nearly worthless hunks of crap, barely suited for cutting wax; It would be easier to change a car tire a with a pipe wrench, than too get the right amount of torque on the ER40 collet they hold. This machine has a turret that needs replaced or retro fitted, due the the years and abuse it has seen. The problem is, the tap pushes up into the collet over a run. I've never had an issue with the ER32's we use most often in the mills. In a Bridgeport, I often tap using a drill chuck, wanting it to slip if I bottom out.

Oh, I forget... Coolant!

Thicker is better.....


NO, NO, NO, NO NO. You could not be farther from the truth. More oil means less cooling capacity. If you are using a modern coolant. ( I like Castrol Hysol MB 20 Semi Synthetic Coolant, 5 Gallons ) It should read what they tell you it should on the refractometer. I like 6-7 from milling and turning, 5-6 for grinding. (the thin side)

We also use conditioned water at my shop to prepare our coolant. (mainly to help with the mineral deposit problems we were having with fully synthetics) but you should never fill a tank with coolant made from conditioned water, only replenish it with such. This helps with foaming.

And then theres, "High pressure, wherever available" that ones bad to. Unless you really need the extra cooling capacity because of a heavy cut, need to get chips away from the cut (or say, knock them off a tap) you are just wasting coolant, and making a mess. Your average cut does not need 2000 PSI of coolant, directed towards the cut. (yet flying in all direction) Yes it's needed for many a modern application, but not when you're chamfering.

Some would argue this is not a myth (customers). Your labor is free, or too expensive, their job is the most important, the only one in the shop, and should have been done and shipped 2 days ago.

ewlsey said:

Stop perpetuating this BS.

There is no need to spot for a tapped hole other than to get the chamfer. A hole .02 out of position is not going to break a tap. If you need locations tighter than .02 TP, go ahead and spot. How often is that needed? If it needs to be .001 or less, you need a few follow up tools.

TiAlN works fine on drills for aluminum. Buy yourself a Guhring 5515 or YG-1 Dream drill in your favorite size. Those are both TiAlN coated. Now turn on the flood coolant and drill a few thousand holes in the shittiest, gummiest aluminum you can find. I guarantee positive results. We used to get 4000 holes with them in abrasive cast aluminum. TSC helps, but is not necessary. I never pecked anything under 5XD.

Click to expand...

You said your self that at least for roll form tapping hole needs to be exactly in line with the tap.
And I did agree with it 100%. Also there is much more chance to break even cutting tap if hole is out.
Besides I can't recall when was the last time I saw such a generous tolerance on a drawing. You get 10 thou out on tap hole, add 10 thou on corresponding clearance hole and bam your assembly doesn't assemble at all.

I never ran "shittiest, most abrasive" aluminum before. But 80% of what I do is 6061
TiAlN coating there simpy does not work. Have to use right coating or nothing at all.TiAlN may have worked in that particular application but it doesn't justify saying lets use it for all aluminums.

No.6 - totally agree. The amount of morons I've had to disprove on this point doesn't bear thinking about.

I was told recently that you can't use an inserted drill ('U-drill' where I come from) like a boring bar to enlarge the drilled hole, "because it bends the drill". Hmm - I must have been going wrong for 20 years...dick.