Struggling with Boring Head

steamandsteel · Jul 26, 2019

Hello,

Trying to simply bore out some holes and get a good finish that's within my specs.

Basically, looking to get around a 1" hole, or just a few tenths under.

Current order of operations:

Centerdrill with 3/16" bit
Drill out with 63/64" bit
Bore to final dimension with brazed carbide bar

The boring bar in my boring head doesn't seem to be giving a decent finish at all, and also has one hell of a spring pass on the upstroke.
Powerfeeding down at 1/2" per minute, probably running 800-1000rpm

Here are some pictures, any thoughts or advice are greatly appreciate.

I did have some decent luck previously with a HSS bit at a 90 degree angle, and a 31/32 bit. However, burned the 31/32 bit and HSS didn't hold up too well.

g-coder05 · Jul 26, 2019

That tool doesn't look very sharp and the boring head doesn't look very heavy. What kind of mill are you using? Quill size?

After looking at the pics again it almost looks like in pic 1 the bar is turned way above center. Then looking at pic 2 zoomed in you can see were the carbide is rubbing below the edge. change your relief angle and check that the tool is on center....

CarbideBob · Jul 26, 2019

Your carbide bit has not been ground yet. Strange that people sell them that way (not to mention the shitty job of pocketing at the braze op)
Put picture #1 into MS paint.
Draw a circle centered where the head spins touching the front cutting tip (your bore)
You will see that the side of carbide is not clear of the hole you are trying to poke.

You'll need a diamond or at least a green grinding wheel and some hand work.
Grind the side and end for relief and dust the top. Put some backtaper on it so that only the tip touches the bore and a nice small corner rad or 45.

You can turn the bar to get the heel clear maybe, which will make it sort of work but it still won't cut very nice.

I bet it has one hell of a spring pass on the way out. Look at those burrs....

Bob

kctallguy · Jul 26, 2019

The carbide tip is ahead of center line of the tool. It needs to be ground back so the tip of the carbide intersects the center line of rotation of the tool when it's spinning. A little positive take as well would help tremendously.

Sent from my Moto G (5) Plus using Tapatalk

gbent · Jul 26, 2019

If its within your ability you need to make a HSS boring bar. A piece of stock to fit your boring head, and a HSS lathe bit tack welded or silver brazed on the end. The HSS can be sharpened to a keen edge, which carbide can't (yea, I know, but not in this instance).

What you are now using isn't really a cutting tool.

steamandsteel · Jul 26, 2019

Okay, I think I've got half an idea of what you're saying.. basically the cutting edge of the carbide needs to be higher up than the back edge of the carbide. So grind a slight angle there, and a slight angle down on the end of the bit, so I have just a small part of the tip touching the actual bore with the other surfaces tapered away from there.

These are some China Specials from eBay.. yikes

I'm not fundamentally against HSS, I'm just not sure what to do there.

Also - if the drill bit (63/64) is drilling the hole anywhere from .985 to .996, is that still enough meat to bore it out to .9995? Or should I purchase a new 31/32" bit?

CarbideBob · Jul 26, 2019

kctallguy said:
The carbide tip is ahead of center line of the tool. It needs to be ground back so the tip of the carbide intersects the center line of rotation of the tool when it's spinning. A little positive take as well would help tremendously.

There is no ahead or behind on a rotating tool. The centerline is spindle rotation center to the tool tip. There is no zero orient.
People hold a tool and get some silly zero in their head. The machine and cutting tool don't.
The only reason for an "axis" on a boring head is calibration of the adjust screw.
I'm not sure even twisting this tool 20 degrees clockwise or grinding the top to nothing makes it cut as the slide offset is not very big.
A smaller bar and more offset and you get more room to play but you go way negative which tiny bars don't like.
Bob

thermite · Jul 27, 2019

CarbideBob said:
I bet it has one hell of a spring pass on the way out. Look at those burrs....
Bob

No shit!

I can get better looking holes in one go with ta da.. a one-inch HSS-Cobalt parabolic-grind twist-drill! Drop diameter down and use a reamer, better-still.

With juice, BTW. Not dry.

The material, section, and shortage of surrounding beef doesn't look to have the stability to justify even taking the smallest of the Chandler-Duplex heads out of the drawer to shoot for anything better.

Trying for .9995" off .960" ?? How ROUND is the hole, how accurately has the position survived - before you even advance the bar, and how are you measuring success?

Might be kidding yerself?

Any "precise" hole simply won't long remain that way, that material & section, especially if you bugger them in the beginning.

Might be ahead to just plunge mill then "D" ream them? PDQ-Marlin VS, I could swap tool, do that without moving the table, each hole, have near-zero burr, either side.

2CW

ripperj · Jul 27, 2019

Also looks like your boring bar is 3 times longer than it needs to be, short and stubby is more rigid

Sent from my iPhone using Tapatalk Pro

thermite · Jul 27, 2019

ripperj said:
Also looks like your boring bar is ^^^ 30 ^^^ times longer than it needs to be, short and stubby is more rigid

Fixed that for yah.

Material that thin could be "bored" with a bleedin' flycutter!

jz79 · Jul 27, 2019

to illustrate what CarbideBob said about "ahead or behind" in regards to a boring head, see the picture below, red line is what people associate with a center line when looking at boring heads, and it is not the center line of the cut, it is the diameter feed direction, center line is the green line, and if this blank carbide bit is used in this fashion, when adjusted so that it doesn't rub, it essentially creates a negative rake geometry, which explains why it worked so poorly and why others say the setup may lack rigidity, which it doesn't, it is all about the cutter grind
right side of the pic shows how I grind my cutters, that radius I put in with a handheld diamond wheel, with like a dremel sort of tool

the next picture shows side and front view with additional relief angles, but these cheap carbide cutters are quite brittle when you put all of the reliefs on them, and I agree with others that said HSS can be a better option, just mind RPM depending on the side of the bore to not burn the HSS

all this is basic info, used to be in the older boring head manuals, newer ones show mostly bars with inserts, where the appropriate bar design for the cut and insert takes care of all the relief angles

ripperj · Jul 27, 2019

Just FYI
Curtis (Exkenna ) here on PM sells cutting tools.
He has boring bars that take inserts that are not too expensive and are magnitudes better than what you have.
Here’s the 1/2” one

Sent from my iPhone using Tapatalk Pro

kctallguy · Jul 27, 2019

jz79 said:
to illustrate what CarbideBob said about "ahead or behind" in regards to a boring head, see the picture below, red line is what people associate with a center line when looking at boring heads, and it is not the center line of the cut, it is the diameter feed direction, center line is the green line, and if this blank carbide bit is used in this fashion, when adjusted so that it doesn't rub, it essentially creates a negative rake geometry, which explains why it worked so poorly and why others say the setup may lack rigidity, which it doesn't, it is all about the cutter grind
right side of the pic shows how I grind my cutters, that radius I put in with a handheld diamond wheel, with like a dremel sort of tool
View attachment 261980

the next picture shows side and front view with additional relief angles, but these cheap carbide cutters are quite brittle when you put all of the reliefs on them, and I agree with others that said HSS can be a better option, just mind RPM depending on the side of the bore to not burn the HSS
View attachment 261982

all this is basic info, used to be in the older boring head manuals, newer ones show mostly bars with inserts, where the appropriate bar design for the cut and insert takes care of all the relief angles

This is I was trying to explain. I apologize if what I said was more confusing than helpful.

Sent from my Moto G (5) Plus using Tapatalk

gmach10 · Jul 27, 2019

Worked for a guy back in the day who made a one and done cutting bit out of oil hardening drill rod. Heat, quench, grind use.

DMF_TomB · Jul 27, 2019

length to dia ratio when you exceed 5x you get problems. if .4" dia boring bar bit thats 2.0" length stickout
.
just saying even when sharpened correctly, if sticking out too long a length it will vibrate too much

thermite · Jul 27, 2019

gmach10 said:
Worked for a guy back in the day who made a one and done cutting bit out of oil hardening drill rod. Heat, quench, grind use.

I reached thirty years of age before I had more store-bought drills of my own than "D" drills (SLOW! it's about clearing chip... or not) and - much faster to use, chips not a big deal - "D" reamers, item-count-wise.

We ALL did that when we wanted any arbitrary size that had to be right ON size. Read: "often enough that a collection grew off the back of it" .

Time-cost now, custom grind off a few endmills or off stock-size reamers (think spares..) could be cheaper.

steamandsteel · Jul 27, 2019

Hmmm

jz79, thank you for the very helpful diagrams. I will give this a try.

Ripperj, those bars look real nice. I may look into one if I can't make headway here.

I've attached a few pictures. The first two are of the HSS bit setup I had in the boring head previously that gave me a fair surface finish.

The last one is what I'm trying to make. It's for the rotation of a platen on a belt sander I've been building. However, I suspect due to the surface finish of the bore and the size of it, it isn't gripping that pivot pin the greatest. Pin is 1" CR, and mics at that size.

So maybe it's not so much "how do I bore this hole" as it's "how can I make this work better and am I doing this in the best way possible"

Terry Keeley · Jul 27, 2019

I struggled too using those brazed carbide boring bars with my baby Clausing mill (rigidity). Found dead sharp HSS worked better, slow speed and feed and lots of cutting oil. Cold rolled (1018) steel was the worst, it looks like that's what you're working with.

I finally got a nice Dorian boring bar and Iscar inserts, that set up cuts like budda!

thermite · Jul 27, 2019

steamandsteel said:
The last one is what I'm trying to make. It's for the rotation of a platen on a belt sander I've been building. However, I suspect due to the surface finish of the bore and the size of it, it isn't gripping that pivot pin the greatest. Pin is 1" CR, and mics at that size.

So maybe it's not so much "how do I bore this hole" as it's "how can I make this work better and am I doing this in the best way possible"

View attachment 262001

Seems not enough contact area, even with a perfect hole?

Just me, but either the pierced rail needs to be thicker, everywhere, or there should be a boss at each pin socket /pivot position so it can pretend better.

It will surely not be brand-new and hold brand-new specs for very long. CRS isn't famous for wear resistance. Hardened shoulder-bolts & dowel pins are stocked for the die-set trade. Bushings exist, too. If you can adapt to those, you'd then have stock items for the wearing parts.

steamandsteel · Jul 27, 2019

Thank you everyone for the help.. Seems like indexable carbide or HSS is the way to go. I have some 1/2" TCMT inserts, Terry is that what your bar takes?

I'm going to try resharpening the little HSS bit I have, and look through my stuff for a smaller flycutter.

Thermite, thank you for the design input.

Struggling with Boring Head

Aluminum

Titanium

Diamond

Aluminum

Diamond

Aluminum

Diamond

Diamond

Stainless

Diamond

Stainless

Stainless

Aluminum

Hot Rolled

Diamond

Diamond

Aluminum

Titanium

Diamond

Aluminum

Similar threads