Steel Boring / Minimal Removal

MikeLight77 · Sep 20, 2018

Aerospace part - material is 4340 Alloy Steel
Heat Treated to 260-280 KSI

We have a hole that we are shooting for a diameter of 3.7826, and on our last pass, we are currently at 3.7811-3.7814, so we're about .0012 below our target.

The problem is, our boring bar is now just rubbing on the surface, when only trying to take about .0006 bite. The boring bar did fine as long as it was taking a decent size chip. Now it's vibrating and not cutting anything. We're afraid if we open the bar up much more, it'll take a big bite and blow us oversize.

Are there any different inserts that would function better when only taking such a small bite? Or can we adjust our angle on our insert, more positive or more negative?

Thanks!

Guest · Sep 20, 2018

The bigger the nose radius the bigger the minimum depth needed. If you want to only take .0006 consistently you will need a dead sharp corner.

Finegrain · Sep 20, 2018

Might try a positive rake, sharp, uncoated insert meant for aluminum. Yes, of course the edges of these are far too fragile for general use in 4340, but for a 1/2 thou skim cut it might be fine.

Regards.

Mike

DDoug · Sep 20, 2018

Might prove better to leave a few thou and hone afterwards.

Or

Is the job large enough qty to justify a roller burnisher tool (cogsdill) ?

Guest · Sep 20, 2018

Finegrain said:
Might try a positive rake, sharp, uncoated insert meant for aluminum. Yes, of course the edges of these are far too fragile for general use in 4340, but for a 1/2 thou skim cut it might be fine.

Regards.

Mike

Do they make dead sharp inserts in that style? The lowest I have ever seen or bought is a .002r.

DMF_TomB · Sep 20, 2018

MikeLight77 said:
Aerospace part - material is 4340 Alloy Steel
Heat Treated to 260-280 KSI

We have a hole that we are shooting for a diameter of 3.7826, and on our last pass, we are currently at 3.7811-3.7814, so we're about .0012 below our target.

The problem is, our boring bar is now just rubbing on the surface, when only trying to take about .0006 bite. The boring bar did fine as long as it was taking a decent size chip. Now it's vibrating and not cutting anything. We're afraid if we open the bar up much more, it'll take a big bite and blow us oversize.

Are there any different inserts that would function better when only taking such a small bite? Or can we adjust our angle on our insert, more positive or more negative?

View attachment 238328 View attachment 238329

Thanks!

.
boring bar length to boring bar dia ratio is the most important factor. a longer boring bar is more unstable and less predictable. yes most boring bars have minimal reliable repeatable cut amounts. usually at least .0010" dia change needed where less it wont bore 1 for 1 ratio.
..... obviously many boring bars have backlash and when lock is loose i push insert to smaller size while i tighten. even the amount of push pressure when tightening can have a effect. and of course when reversing you usually go a lot extra and then come back to take up backlash
.......better boring bars use a type of fine adjust spring where you got .010" range where you do not have to loosen lock but can just turn it and change size within a limited range. basically some boring bar designs are 10x easier to fine adjust and 10x more repeatable and easier to use
.
sometimes if i need .0002" bigger dia i just rerun at a higher rpm and boring bar wobble increases at higher rpm and hole sometimes cuts .0001 or .0002 bigger

Mtndew · Sep 20, 2018

Your insert doesn't look bad, those usually have relatively light tool pressure. See if you can find a more positive rake insert with as small of a radius you can get.

Is it a thru hole? Can you hone it?
There isn't much stock left for jig grind either.
Try again with no coolant maybe?
Can you interpolate it on a mill?

Ox · Sep 20, 2018

Looks like a blind hole, so a hone wouldn't werk, but maybe you can emery the rest out if you have enough patience?

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

Think Snow Eh!
Ox

DDoug · Sep 20, 2018

Ox said:
Looks like a blind hole, so a hone wouldn't werk

How do they Hone VW cylinders ?

and Air-o-plane engine cylinders for that matter ?

Mtndew · Sep 20, 2018

Ox said:
Looks like a blind hole, so a hone wouldn't werk, but maybe you can emery the rest out if you have enough patience?

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

Think Snow Eh!
Ox

You may be right, that hole in the bottom looks like it could also be on the side wall.
I guess it's all how you look at it. I couldn't really see an edge where the floor meets the wall.

Larry Dickman · Sep 20, 2018

digger doug said:
How do they Hone VW cylinders ?

and Air-o-plane engine cylinders for that matter ?

I thought VW cylinders went thru. Haven't played with one in years. Parts we have honed with blind holes will always have a full radius relief at the bottom.

Ox · Sep 20, 2018

digger doug said:
How do they Hone VW cylinders ?

and Air-o-plane engine cylinders for that matter ?

Aint those all bolt on jugs?

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

Think Snow Eh!
Ox

MikeLight77 · Sep 20, 2018

It is a through hole and there is some interrupted cut in the middle.

HuFlungDung · Sep 20, 2018

You know, you can always increase the rake angle of the insert by grinding the top rake face. I do it constantly, shit .0012" is a mile to go yet, enough for 2 trial cuts and then a finish

Check that your insert actually has front clearance, it shouldn't take any force to penetrate. If the holder is positioning the insert below centerline of the hole, this can be an issue.

Finegrain · Sep 20, 2018

Dualkit said:
Do they make dead sharp inserts in that style? The lowest I have ever seen or bought is a .002r.

By "sharp" I mean the top edge, not the nose. Most steel inserts have essentially a rounded-over edge. Al-specific inserts should be sharp enough to easily cut you (DAMHIKT), not so much with inserts for steel. Coatings make it worse, hence the difficulties some folks (like me) have with ZrN-coated endmills in Al -- the coating, from what I've read, is relatively thick and "desharpens" the edge.

I'm talking tenths here, not the .016" or .032" nose radius you typically see.

Regards.

Mike

Ox · Sep 20, 2018

MikeLight77 said:
It is a through hole and there is some interrupted cut in the middle.

Sounds like a hone job to me then.

If you don't have a Sunnen on site, doo you maybe have an engine rebuild machine shop nearby?

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

Think Snow Eh!
Ox

Matt_Maguire · Sep 20, 2018

MikeLight77 said:
Aerospace part - material is 4340 Alloy Steel
Heat Treated to 260-280 KSI

The problem is, our boring bar is now just rubbing on the surface, when only trying to take about .0006 bite. The boring bar did fine as long as it was taking a decent size chip. Now it's vibrating and not cutting anything. We're afraid if we open the bar up much more, it'll take a big bite and blow us oversize.

Thanks!

280ksi strength is max useable hardness for 4340, with a good quench & 400°F temper it ends up in the mid 50’s Rc…

It’s hard to judge the mass from a pic but a 12x12x12” lump will still be high 40’s to 50Rc in the center. Even with very good tooling & stiff machinery it’s going to make some real high pitch noises when you cut it.

For finishing with sub .004” DOC you’re really in the world of grinding to have a good day IMO. Diamond tool possible?

Sunnen makes hones that will straddle holes & work with an interrupted cut but that looks to be a pretty cashy part to learn with.

Good luck,
Matt

hanermo · Sep 20, 2018

I *think* you could roller-ball (burnish) it to size with a simple shop made tool of the appropriate size.
These are supposed to be good for about 0.01 mm of diameter changes, incremental (normal workshop sizes).

Simple O1 round blank sized a bit oversize, hardened dead hard at the tip / skin with no tempering,
ground/polished lapped to size.
And a tiny 0.02 mm relief after the toolbit hard tip perhaps == 1/2 of D of tool.
(or less, the contact length might be really short).

High surface speed, feed in and out like a reamer, done.

At least that´s how i understood it works.

---

From what I learned, the good part about roller burnishing is that it has one size, follows the hole, and wont make major changes in anything, and only minor ones in size.
So it avoids errors in bellmouthing, wandering bores, banana-shaped bores, etc.

Commercial US providers sell roller burnishing tools.
I suspect they could easily set you up with something that would work for your app, with commercial level confidence.
Later, you might try your hand at shop-made-tools if you want.

---
In auto production cylinder bores are diamond-honed with a single use rigid hone coated with the diamond stuff.
It is a 15 secs op, for a car cylinder.
Tools cost about 3 grand and last about 300k units or one year.

I´ve been at plants and handled some of the diamond tools, and talked to the guys in charge.
And sold MT stuff to them.
That´s all.

--

gappmast · Sep 22, 2018

Call Sunnen and talk to your local rep. If you have a hone he can help if you don't he can tell you if there are any hone shops in the area that can.

Don't take it to an automotive rebuild shop this more than their equipment can handle

Steel Boring / Minimal Removal

Plastic

Guest

Guest

Diamond

Diamond

Guest

Guest

Diamond

Diamond

Diamond

Diamond

Diamond

Titanium

Diamond

Plastic

Diamond

Diamond

Diamond

Stainless

Titanium

Cast Iron

Similar threads