D-bit geometry?

Hi!

I have been asked to turn some tappets. Their problem is the bore:
Hole starts with ø7 mm, 3 mm deep. Then a conical part 9 mm long with the small end being ø 3.4 mm. So 12 mm deep with ø 3.4.

Material is AIS 4137 / 42CrMo4

Now I could buy some P. Horn minis + a holder and break a few along the work.
Or, I could grind my own D-bit (reamer). Grinding one is not the problem. The problem is a geometry that actually works good. Unitl now, my experiments failed more or less.
The primitive and general wisdom is to grind the cone and then split the bit to a tad more than half. These never worked too good, except in brass or soft material.

I think, I need a relief on the (9 mm long) cutting edge. And at least one surface that helps in guiding the bit. Yes, I will pre-drill to 3.4 and 7 mm

So the question is:
Has anybody got a sketch (of the cross-section) or description of it of a conical reamer that actually does makes a nice finish? I won't cut at the front (I'll drill the small diameter)

TIA,
Nick

Nick Mueller said:

Hi!

I have been asked to turn some tappets. Their problem is the bore:
Hole starts with ø7 mm, 3 mm deep. Then a conical part 9 mm long with the small end being ø 3.4 mm. So 12 mm deep with ø 3.4.

Material is AIS 4137 / 42CrMo4

Now I could buy some P. Horn minis + a holder and break a few along the work.
Or, I could grind my own D-bit (reamer). Grinding one is not the problem. The problem is a geometry that actually works good. Unitl now, my experiments failed more or less.
The primitive and general wisdom is to grind the cone and then split the bit to a tad more than half. These never worked too good, except in brass or soft material.

I think, I need a relief on the (9 mm long) cutting edge. And at least one surface that helps in guiding the bit. Yes, I will pre-drill to 3.4 and 7 mm

So the question is:
Has anybody got a sketch (of the cross-section) or description of it of a conical reamer that actually does makes a nice finish? I won't cut at the front (I'll drill the small diameter)

TIA,
Nick

Click to expand...

When you grind your conical section, make the included angle 20* less, to allow 10* per side taper clearance, then split the bit a little more than a tad. You are making a boring bar that gains stiffness from the tapered section. Single point bore and you should get a nice finish

So you suggest to grind a boring bar. Rake is 0° and the relief comes from "splitting over the half". Did I get you right?

Except for the "20*" if that meant "20°" or 20 degree. The cone angle (axis to one side) is just 11.31°. I'd make that just maybe 3° smaller for the back relief.

Edit:
OOOPS! No, that won't work. Cant turn the transit from the 7 mm cylindrical bore to the cone. And if I grind the boring bar's cone more dull, the 3.4 mm at the end won't be right (but maybe acceptable).


Nick

Yes, I think you are getting it! The purpose of grinding the conical section is only to maximize your boring bar strength. You can increase cutter clearance by rolling your cutting edge "down" but only if you need it.

I've literally made 100s of D or single lip cutters for mold details. A lot of them were for use in P-20 (pre hardened 4140) molds. Used one of these
Michael Deckel

You can't be very aggressive, but they do work well. There are a bunch of YouTube videos, just do a search with "Deckal SO".
JR

IME it's best not to over think D bits, so many things seem wrong, but they do work ** - in almost any material - if you can mark it with a file a d-bit will cut it.
E.G. I've done tapered holes in 01 (gauge plate) with no problem - using hardened drill rod (Silver steel) shop made D-Bits- just remember to keep the speed right down, don't be greedy with the cut and use plenty of neat cutting oil

** I believe it's said by scientists the bumble bee can't fly - go figure

I should have stated annealed 01

Aint going to work when they get back from heat treat.

That better Heavey

I've literally made 100s of D or single lip cutters for mold details.

Click to expand...

So you said I should make the D-bit like a single lip cutter?
That I know.

Nick

The part not the reamer.

Nick Mueller said:

So you said I should make the D-bit like a single lip cutter?

Click to expand...

I'd sure try it. Unless the parts are over 40Rc, it shouldn't be a problem.
JR

Hi Nick:
The thing with D bits that many don't realize is that you can only make an un-relieved one if the D bit is cylindrical.
Any other geometry will require you to put relief on it if you want it to cut.
For a project like you're describing, I prefer to make a multi flute properly relieved cutter, and for tapered reaming a 2 or 3 flute cutter has been most successful of the ones I've tried.
Here's a link to an example on my website:

Implant Mechanix ? Design & Innovation » Precision Grinding

Go down toward the bottom of the page and you'll see a series of photos about a mini plasma nozzle that was made using such a cutter.

For a little one like the example, I give it about 0.07mm of relief; enough to cut cleanly but not enough to chatter.
It's fussier than most people are aware of; if you get it just right the reamer will cut very cleanly; too much and it will snatch at the hole sidewalls and break; too little and it will grind chips into the sidewalls of the hole and make a big mess.
You can grind the tip to be center cutting if you're so minded, but I usually make them non center cutting and pre drill a start hole unless I'm making them for a tunnel gate on an injection mold, in which case I make them ball nosed and center cutting.
The blank is first gashed on the surface grinder, then all the other operations can be very nicely done on a Deckel SO cutter grinder if you have one.

To run it, you need relatively slow speed (200 RPM or thereabouts for a 3 mm diameter cutter), very small and incremental downfeed and some kind of tapping fluid to get the cleanest cut; I prefer Relton Rapidtap.
I have no idea what a German equivalent might be.
I'll typically do peck increments of 0.025mm to 0.050 mm.
Cheers

Marcus
Implant Mechanix – Design & Innovation - home
Vancouver Wire EDM -- Wire EDM Machining

Hi Nick,

The Paul Horn mini's look good to me. Paul Horn super mini en mini draaien - YouTube

I like the way they filmed that with the cut away side... interrupted cut? seems like they are very robust

I think that AIS 4137 is 34CrMo4, 42CrMo4 is AIS 4140, which machines nicely, so you should get a good finish.

Are you going to harden them yourself?

Ray

Here's a link to an example on my website:

Click to expand...

I love the broach!
So you suggest a reamer like a reamer has to look like.

For a little one like the example, I give it about 0.07mm of relief;

Click to expand...

The 0.07 mm relief puzzles me. With a close look at the pictures, I see the following:
After the cutting lip, there is a small land, then the relief (a flat like for single lip cutters) and then you get conical again.
With the 0.07 mm, did you mean the width of the land? I think so.

I think I will take that route.

BTW: great work samples!

The blank is first gashed on the surface grinder, then all the other operations can be very nicely done on a Deckel SO cutter grinder if you have one.

Click to expand...

I do have a Walter 3CY T&C grinder. With a different head, he will do as well. No Deckel needed.



Nick

RayG said:

Hi Nick,

The Paul Horn mini's look good to me. Paul Horn super mini en mini draaien - YouTube

I like the way they filmed that with the cut away side... interrupted cut? seems like they are very robust

<>

Ray

Click to expand...

BTW, I think those cut away shots were made with a strobe light synced to the rotation of the cut away part. VERY cool idea. I first thought they might be "an artists's rendition." But the chip flow and small burrs forming at the edges of the cut suggest a real cutting tool in action. Looks like a technique one could use to learn more about what is going on real-time with a cutter with respect to chip clearance etc. I do not want to hijack this very interesting thread. But thought I would just make that comment as photography has been an interest of mine in a former life and I have not seen this particular application of strobe video photography.

Denis

BTW, I think those cut away shots were made with a strobe light synced to the rotation of the cut away part.

Click to expand...

Yes, that's how they did it. You can see it when RPM changes, the strobe doesn't sync quickly enough. And yes, that video is very cool! But I didn't look at it.

While looking for an HSS-blank, I discovered two Horns that would work. Somehow, I did get them somewhere. But I'll stay with the reamer.


Nick

Nick,

Tough little job in my opinion. Let us know what you find to work.
You don’t say how close the size of the 7mm, concentricity require and if you need a super finish or just one with not having chatter, or if it is a high number job or just a few. Certainly the D drill is the easiest cutter to make and try.
Another cutter possibility could be to use a M8x.5 or a M8x.75 solid carbide 3 flute tap (a used one to save costs) and grind from it a 3 flute special cutter that would cut the taper and finish the 7MM with back spinning the circle grind for taper then grinding to a small circle land (Perhaps .1 MM or .2) with an axial relief of perhaps 10*/12*. Flute face rake attitude? You would have to play with that as too much positive would dig and negative might drag chips or roll material.
(A HSS cutter would (might) be OK made the same way.)
(That Paul Horn Super mill makes it look easy)

That bottle is too big for the job. I will bring my glass and be right over.

Good luck, Buck

A simple,very old style reamer can be made by just grinding an angled surface of about 30º on the end of a round rod. HSS would be good. I have used this type reamer.

Hi Nick:
The picture of the reamer is a bit misleading; there is no land and the primary relief goes all the way to the cutting edge, so it's ground just like a tapered milling cutter (in fact that's exactly what it is).
There is also secondary relief on the cutter
With regard to the amount of primary relief, I realize it's normally expressed as an angle, which is probably why it makes no sense to you.
Since I often grind these kinds of cutters on a Deckel SO (single lip cutter grinder for those who don't know this machine) I have problems setting up a multi flute cutter to get the proper relief.
On the Deckel, there is a swiveling blade on a stem that is used to position the split cutter blank properly and a graduated swivel on the base of the collet holder that allows you to set the relief angle, but it works easily only with a single lip cutter (a D bit).
So for multi flute cutters I adopted a different way to get to the same goal.
I loosen the collar that sets the rotational stop on the collet spindle, and then snug it back up until it just drags with enough force that I can still rotate it.
I spin grind my OD.
Then I add another 0.075mm, set the stop deliberately high, and take a pass.
I am left with a large land.
I then twist the collet holder against the stop in the OPPOSITE direction to that which you'd normally take when grinding relief, and take another pass, and I keep doing this until I've reduced the land to nothing.
This shifts the stop to the proper position to grind my cutter flute with zero land.
Then I snug up the collar to lock the stop, and grind the rest of the relief in the normal way.
I do that for each flute.
It gives me the correct primary relief without using the setting blade which does not work for multi flute cutters.
It also lets you make variable pitch flutes which can work to your advantage sometimes.
If you have lots of Deckel SO time under your belt, you'll understand perfectly what I'm babbling about; otherwise it sounds like gibberish...my apologies!
But the goal is to get about 5 to 7 degrees of primary relief; the same as a milling cutter or maybe a twitch less.
If you do lots of these, you get to know instinctively how much to reduce the diameter to get the primary relief that will cut properly.
Cheers

Marcus
Implant Mechanix – Design & Innovation - home
Vancouver Wire EDM -- Wire EDM Machining

Nick Mueller said:

Hi!

I have been asked to turn some tappets. Their problem is the bore:
Hole starts with ø7 mm, 3 mm deep. Then a conical part 9 mm long with the small end being ø 3.4 mm. So 12 mm deep with ø 3.4.

Material is AIS 4137 / 42CrMo4

Now I could buy some P. Horn minis + a holder and break a few along the work.
Or, I could grind my own D-bit (reamer). Grinding one is not the problem. The problem is a geometry that actually works good. Unitl now, my experiments failed more or less.
The primitive and general wisdom is to grind the cone and then split the bit to a tad more than half. These never worked too good, except in brass or soft material.

I think, I need a relief on the (9 mm long) cutting edge. And at least one surface that helps in guiding the bit. Yes, I will pre-drill to 3.4 and 7 mm

So the question is:
Has anybody got a sketch (of the cross-section) or description of it of a conical reamer that actually does makes a nice finish? I won't cut at the front (I'll drill the small diameter)

TIA,
Nick

Click to expand...

I know what a debit is.. never heard of a d-bit....
Some taper pin reamers may just fill the requirements with a little altering... check the sizes you need and the reamers are left hand spiral right hand rotation... they cut and leave a very good finish.