[antonio5005]

Need some help with the best option for completing a boring operation on a high quantity order, repeat as well.

Been programming and machining professionally for a few years, I have bored holes with a 4” standard criterion boring head. All bored holes though were single one-off jobs and weren't the best looking. In other words, I’m not very skilled at this. Always low and slow on speeds and feeds in low carbon steel 1018 and aluminum. Always had better luck with aluminum. All that said, I have never tackled a high quantity job requiring bored holes.

Got a part, CR1018, that needs 1x 1.001-1.000 diameter hole 1" deep, it needs to be round and straight, no interpolating. I know reaming is an option, but I haven't had the best of luck with reaming. I either overshoot the tolerance or I don't get that great of a finish. Guess I’m not that skilled at that as well.

This bore has two intersecting .172 hole drilled through to the center of bore. This has given me issues with the boring bar "skipping" around the hole as it passes the cross holes. Makes for a very odd finish. Goes from a “smooth” finish, to a rougher finish with small step at the holes, back to a smooth finish again once it passes those holes. So, there's that as well.

What I’m looking for is a good recommendation for a boring head, or technique for boring it accurately and smoothly. I was recommended a balanced boring head so I can turn the RPM’s up, I'm good with that but seems to have opened the door to a ton of questions... Such as, do I rough it in with a drill, do I interpolate, use a twin boring head, rough it with a standard boring head, what kind of boring bar, type of tool holder (CAT40), how do I deal with the intersecting holes? Lots of questions that I do not have a lot of experience with and unfortunately most of my learning has been on here, trial and error, and youtube.

Also, I’m not opposed to reaming, seems simple and cheap, but I just haven’t had the best of luck with it. Same questions apply to that as well.

I can make something happen but I want it to be right and not fight this thing the entire time.

If any of you experienced machinists could drop some knowledge this way I’d greatly appreciate it!

CR1018
1.001 to 1.000 bored hole
1 in depth, thru hole
2x .172 intersecting cross holes
currently using 4" criterion boring head (not ideal)

[metalmayhem]

you don't mention the machine your doing this on which can play an important role in determining what would be best . If the mill is of quality then interpolation with a 7/8 or 3/4" end mill is the most efficient way to making your hole .
Even the best boring heads will produce poor results if not set up properly . I'm guessing that your bar is sticking out a fair bit more than it needs to , and the first thing I would do if that was the case is to chop the bar down and have it stick out 1.1" from the head . If you want a quality head then d'andrea makes some really nice stuff but it's costly

[antonio5005]

you don't mention the machine your doing this on which can play an important role in determining what would be best . If the mill is of quality then interpolation with a 7/8 or 3/4" end mill is the most efficient way to making your hole .
Even the best boring heads will produce poor results if not set up properly . I'm guessing that your bar is sticking out a fair bit more than it needs to , and the first thing I would do if that was the case is to chop the bar down and have it stick out 1.1" from the head . If you want a quality head then d'andrea makes some really nice stuff but it's costly

Thanks, yea it’s a 1993 Haas VF3, bubble machine, space ship looking time-machine escape-pod. Decent shape for the age but definitely used.

I have to apologize too, I realized it was NOT the 4” boring head I tried on this part but a square shaped S-1-1/2 from criterion. Although… i do have issues with either. I’ll edit my post to show that.

But yes It would stick out about 2” maybe. It is McMaster’s “economy” indexable boring bar for this particular part with a TPMT insert. Sounds like the setup may be part of the problem.

I’d prefer to spend the least amount to achieve this but not opposed to investing in something if it gives me even better results more easily, accurately, and repeatedly. Just would rather not if I can make what I have work.


Sent from my iPhone using Tapatalk Pro

[Jim Dawson]

I would interpolate the hole to around 0.985, then ream. Use a good quality carbide tipped reamer. A floating reamer holder would be the best. It might take a little playing around with feeds & speeds to get it right, generally slow speed with a bit aggressive feed, and flood coolant.

We ream a lot of 5/8'' holes and have had no problem hitting the numbers in production.

[metalmayhem]

Just would rather not if I can make what I have work.

the old vf should be able to interpolate a hole to within .001 . Otherwise try shortening your bar as I mentioned , and interpolate as Jim stated (I'd probably start at .99) , then run your bore . Also what is the diameter of your bar ? Beefier and shorter would get the best results , but even still the interrupted cut due to those side holes may continue to pose a problem .

A 1" reamer should get it done as long as it doesn't grab onto them holes to

[deadlykitten]

Hy, for 1inch hole, 1inch deep, thus 1 l/d, rough it as you like, then go with interpolation with short endmill ( thus rigid ), active length < 1 inch, resize helix to overcome any out of rotund situations ( like make it a bit elipse If needed, or use corection arches, so adjust toolpath to handle any out of rotund issues of your machine, and that will work as long as machine roundness error is consistent ), prepare a set of incremental gauges as long as the hole ( heat treat, -0.03 -0.02 -0.01 0 0.01 0.02 0.03 ) and a um internal hole dial

what about a custom fixture for turning ? kindly