Boring Article - Or Rather an Article About Boring

Too All:

Here are some excerpts from an American Machinist online article.


formatting link
Rounding Up the Usual Suspects

12/28/2009 By Matt Tegelman

When boring performance falls off, the cause may be any one or a combination of factors. These include workpiece stability, adequate stock allowance, tooling rigidity, insert grade and geometry and the matching of speeds and feeds to cutter capability.

Part stability Although the machining center and fixtures usually are not the first factors shops may consider, these can seriously impact tool performance if the part is not stable when being machined.

Stock allowance

Often, operators are unsure of how much stock to leave for boring applications. This is especially true in rough boring applications where a twin cutter is used. It is not uncommon to see drills that are so close to the final size of a part that only 0.020- to 0.030-in. of stock is left on diameter, which isn?t enough material to engage both insert tips on a twin cutter. This leads to chatter and poor tool performance.

Tool assembly rigidity

Modular tooling systems offer an infinite number of combinations for maximum rigidity and usage. In cases where tool length is needed, it is important to start with a larger base size and then reduce the tool diameter as necessary, rather than using the same bar diameter for the entire length of the tool.

Insert grade and geometry

The most rigid boring assembly, complete with a balanced boring head, can perform miserably if the insert is not suited to the application.

Speeds & feeds

Ideally, the boring bar is run at high speeds and more moderate feedrates; but again, this can be limited depending on the conditions previously cited. A common mistake during rough boring is simply to multiply singlepoint feedrates by two when using a twin cutter. This usually is not an effective calculation; twin cutters can operate at feeds four times faster than those of finishing tools for the same diameter because a much larger nose radius can be used. Feeding a twin cutter too slowly will lead to chatter without the right stock allowance. Rough cutters are designed for heavier cuts, requiring more material and harder feedrates.

Matt Tegelman is an application manager at BIG Kaiser Precision Tooling Inc. =============================================================

Reply to
Loading thread data ...

So whats your favorite boring bar? Mine, the name eludes me right now, I believe at one time Devlig micro bore? They are carbide tipped threaded $cartrages$ with a dial on the threads for adjustment in tenths! limited in size range with different dia. bars. Sweet system. No out of balence issuses ect.

My place just bought me an ajustable TPG? screw on insert type bar for doing 35mm +.000"-.0005" ball bushing bores a few weeks back. It worked ok for the $450 (OUCH!) The age long problem I've had, is on gear drive head CNC's, there are harmonics at higher RPMs. creating chater. So its SLOWWWWWWW Very boring operation. The Heide control has a a dead spindle x moveover retract - no drag. Took me a few trys to figure out what position the spindle orients to by program selection. Nice drag lines on the first atempts. Ah well it was 6061 AL.

-- ~g~

Reply to

Being a lathe guy like Dobe Dave, I always want to bore rather than interpolate on the mill. Set feed to IPR and G76. Q = amount of shift.

Reply to


I think this might be an example of a difference in basic machining-philosophy outlook - influenced by alternate types of work.

Take for instance the creation of a machined seat for a bearing. You can drill/mill a blind counterbored hole, then bore it, measure it, then adjust your boring head to finish it. But it's going to probably take a couple of holes to get it Right-On because taking differing amounts of material will deflect the boring bar in unpredictable ways.

Or you can do the counterbore with one tool, an End Mill. Helix in, rough interpolate most of the material away, do a semi-finish pass leaving .005 on the wall to finish. Measure with a dial-bore gauge and then take the appropriate amount of material on your finish pass. You only need one tool, less chance of needing to use a couple of parts to dial in the process, the wear is spread out over the length of multiple End Mill flutes instead of at the single point of a boring insert, and the bottom corner will be sharp for the bearing to seat in, whereas if the boring bar was required to make the corner SHARP the wall finish may suffer or take an inordinate amount of time with a super-fine feed.

If you're making 1,000 parts - boring to the final size may very well be more productive. But I would tend to believe that on onezies-twozies prototype work that doing it all with one End Mill might be the better way to go.

Have I overlooked anything here? Always, willing to learn something new. We won't be roller burnishing the bearing seat walls, will we? LOL

Reply to

For one-off I learned to take roughly equal amounts several times say .005 or .010 per pass while your still a ways away from finish....making minor adjustments in order to get myself dialed in--then so long as I take basically the same amount for the finish pass the deflection will be predictable ( and it will already compensated for in my dial position as well)--and if there's more than one part, now simply leave the boring head alone--and for the remainder of the run I will pre-bore using an plung endmill or circular interp or somesuch.

Reply to
Uhh Clem

Uhh Clem, That's pretty much my procedure also. I do a fair amount of close tolerance holes (.0005 and less total tol.) and I find that boring is much more predictable than either reaming or interpolating.

Reply to

No arguement in particular with your methods. I'm a lathe guy and boring a hole just seems the "right" way to do it. I generally interpolate because it doesn't require as much hands-on attention, but when the tolerances get down to less than .002 then I bore.

Reply to

UC & GD:

Everyone knows the standard rule of thumb for like dowel pin holes that have to be within a couple of tenths (.0002), is to drill, bore for location, then ream for size. I don't think very many people are boring dowel pin holes to finish size - too time consuming. Although you may have to try the reamer in a piece of scrap of the same material you're machining to make sure it's cutting the proper size. I've heard that wire EDM'ing dowel pin holes to finish size in hardened A2 & D2 die blocks is standard procedure now-a-days.

But back to the above rule of thumb, I often substitute plunge end milling with a slightly ground down standard end mill, for boring. Grinding the outer edge of the flutes doesn't effect it's plunging ability - since it's only cutting on the end. Of course it can never be used to cut on it's side again without being resharpened. If the hole is DEEP, then I relieve the end mill even more while leaving 3/16-1/4 on the end at the regular undersize amount. Did that sentence make sense?

I'll add that if it's something other than a standard thru dowel pin hole - a blind-hole, not a standard reamer size, etc. Then UC's & GD's creeping up boring method is the way to go.

Oh, and one other point. If your machine isn't able to interpolate a hole WITHOUT quadrant steps, then obviously you're back to boring, reaming, roller burnishing, or wimping out and sending it out to be honed.

Reply to

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.