Boring Opinions (heh)

[The Metal Butcher]

Hi all. I've got this part I designed for my senior design project. My plan was to weld it all up and then linebore it afterwards to solve any potential warping issues and make it overall easier. It doesn't have to be perfect, there are just splined axles running through into a differential, it can tolerate slight misalignment but I'd prefer it to be close.

So here is the parts. Material is 6061 T6 Aluminum



Here is the bore they need



1.75" by the way for a 7610DLG bearing. I'd also like to face a small area for the snap ring incase it wasn't welded totally straight.

and here is the assembled view basically:



So, when I planned it, I figured I would just chuck it up and bore it with the 4 jaw. Well, that is sort of problematic, as I didn't fully comprehend how long they were until they were done. My longest two big boring bars are both 12". So that isn't really enough in the CXA holder. I could make a longer bar, but then I'd almost assume make it for a CA holder, which I now have a post for, but no holder, so I'd have to make or buy that too...

So, here are the options I can see.

1. Conventionally bore in in the Lagun 1440 in a 4 jaw.
2. Conventionally bore in in the Sidney 18.5x54 in a 4 jaw.
3. Line bore it in the Lagun with a true lineboring setup.
4. Line bore it in my camelback drill press.
5. Line bore it some other way with plate-mount spherical bearings mounted directly to the pieces themselves.
6. Bore it in the Bridgeport with a boring head on one side only, flip it and index in a jig, hope the second side is right.
7. Tilt the Bport head 90 degrees and linebore with it on it's side using the table feed?
8. Drive up to NC and beg Doozer to help out? :P

And the issues with those:

1. The Lagun doesn't handle extreme overhang well. It has a short headstock side of the saddle, and the compound almost already leaves you overhanging. Except for very light cuts, that is asking to lift the tailstock end of the saddle. It's undergibs are tight though. Secondly, I want this held securely, and the 10" 4 jaw won't cut it gripping over 7.5" with the jaws set for OD work. I also want a packing block to spread the load on the 1.75" tube. So that means the 12" chuck. But now, with 7.5", plus probably 1" of packing block, plus 4" of jaws, that is 16.5" of swing required. So I'd have to pull the gap. I'd rather not.
2. The Sidney would handle it fine. Except the cross-slide is whopped out and it doesn't like long bores. The longest I've done was 8". It handed it fine, but I couldn't hit any accurate dimensions. That may be fine if dad's adjustable reamer set goes up to 1.75". I think it may. I could also do a quick fix on the cross-slide with external gib lock screws, something I've been meaning to do for a while. I'd still probably need to ream it or glue the bearings in.
3. Some of the Laguns came with a slotted cross-slide. That would be perfect here. We don't have one. So I could rig something up to go in place of the compound. We have a big 1" thick cast iron angle plate which is about 7x9". That would do it. I'd have to drill some holes in it for the compound bolts, but that isn't the end of the world. I'd also have to make a line boring bar. I don't think we have an MT7 to MT4 adapter, but I could buy one or just make a chucking version. At any rate, a lot of work, but probably the best option. (The Sidney is not a good option due to the ways being bananna shaped. This isn't an issue for turning as it only affects the tool height, but for line-boring it would cut a matching banana.)
4. Another decent option. The two cons are that I don't have a setup built (so MT4 boring bar again, bearing on the table) and it only has 7" or so of quill travel, and no sliding head. So I'd have to raise the table mid bore. It's all doable, but dang that would be a lot of work too.
5. I'm not sure that this option saves me any time over the others.
6. Probably would work given the accuracy requirements. T'would be quick, I'm already tooled up. I'm not sure if I have the vertical height though. Un-rised B-ports have what, 18" between the spindle and table? I could hang it off the front of the table if not but.. eh.
7. Dunno, never tried that. I'd have to build some tooling of course.

So... this is more of a thought experiment than a request for help. I'm not entirely seeking advice, but I do like to hear others opinions. The method I go with will probably still be of my own choosing, whether it's the best or not. So don't fight tooth and nail to try to change my mind. But, what I'd like to know is:

1. Assuming you have the capabilities, how would you do this in your shop?
2. Given the list of possibilities I have mentioned (or something I have overlooked) how would you do it with the machines that I have listed?

So thanks all, try to keep it fun.

[mattthemuppet]

I'd knock out most of the hole on your camelback with a big azz drill. Then I'd cobble together a fixture plate for the logan that I can bolt to the carriage somehow ( make a dovetail like clamp and attach it to the cross slide dovetail with the cross slide removed, through bolt it to a plate under the carriage, something like that) and then bolt the whatsit to that. Make a long single cutter boring bar to hold between centers, stick a cutter in it that can be adjusted with a screw at the end and then line bore it.

Seems simple from this chair

[nickel-city-fab]

If you have access to a decent scrap pile and some HSS, I would make a line-boring bar that holds 4 pcs of HSS, one for each plate. On the Sidney, that way the total travel of the part only has to be the thickness of one plate. Minimizing the error due to wear over such a short travel. Have the part jigged up somehow and clamped on the cross slide, boring bar between centers and driven with a dog or whatever.

Just a long-enough bar centered on the ends and 4 holes drilled crosswise... believe it or not Harbor Freight has a decent deal on a box of assorted HSS, about $7. I use the little 1/4 inchers for things like that. Or cut up a bunch of old drill bit shanks. Yea, I'm that cheap.

FWIW this is the technique they use at my job, for line-boring the pin and bushing hoes on Caterpillars -- Boring bar maybe 6 feet long but the total travel is only a few inches because its doing all the bores at once. Using a DI stuck to a vee-block to set the tool height off the OD of the bar.

[LKeithR]

If you have access to a decent scrap pile and some HSS, I would make a line-boring bar that holds 4 pcs of HSS...

This will certainly work IF you're short of travel but it's a lot extra work to set up 4 cutters and get them
exactly the same. Make your bar with one cutter and take advantage of the travel of the lathe. And don't
skimp on the size of the bar--make it as large as possible.

[nickel-city-fab]

This will certainly work IF you're short of travel but it's a lot extra work to set up 4 cutters and get them
exactly the same. Make your bar with one cutter and take advantage of the travel of the lathe. And don't
skimp on the size of the bar--make it as large as possible.

True, but he can't do that on the Sidney -- too much bed wear over that length. He would end up having to reset the cutter for each cut.

[The Metal Butcher]

If you have access to a decent scrap pile and some HSS, I would make a line-boring bar that holds 4 pcs of HSS, one for each plate. On the Sidney, that way the total travel of the part only has to be the thickness of one plate. Minimizing the error due to wear over such a short travel. Have the part jigged up somehow and clamped on the cross slide, boring bar between centers and driven with a dog or whatever.

Just a long-enough bar centered on the ends and 4 holes drilled crosswise... believe it or not Harbor Freight has a decent deal on a box of assorted HSS, about $7. I use the little 1/4 inchers for things like that. Or cut up a bunch of old drill bit shanks. Yea, I'm that cheap.

FWIW this is the technique they use at my job, for line-boring the pin and bushing hoes on Caterpillars -- Boring bar maybe 6 feet long but the total travel is only a few inches because its doing all the bores at once. Using a DI stuck to a vee-block to set the tool height off the OD of the bar.

Ooh, interesting idea. I hadn't thought of that.

True, but he can't do that on the Sidney -- too much bed wear over that length. He would end up having to reset the cutter for each cut.

I don't think I would use the Sidney anyway. The Lagun would be the happier machine for lineboring, it has a dead-flat cross-slide that is tight. The only way the Sidney would be better is if I could direct mount it to the saddle. And since the discontenued adding Tee-slots in the '30s and '40s, that would require drilling holes and then building some cross bars. I'm not eager to do either of those.

All in all, I think LKeithR is probably right for lathe-line boring. One bar, plenty long. If I can bore 8" deep with a 1" overhung bar, then a 20" 1.25" or 1.5" bar supported on both ends would actually be equally stiff if not stiffer. And then I don't have to file 4 square holes or setup a cutter 4 times.

[SVS]

Just to be different...you could vertical line bore it on the Bport. Mount work with hole just clearing back of table and to side of knee. Rotate & retract turret & ram to suit and support bottom end of line boring bar (on a dead center?) attached to column. Alternatively, bar could run through a bushing integrated with the work holding fixture.

Admittedly, lot of tramming and indicating involved.

[The Metal Butcher]

No, that's not a bad idea at all, SVS. It woukd have to be off the front, dro rod on the back. 22" bar, crank up the knee to position to each bore, then just quill fees the 1/2"... I'd probably mount a plate mount bearing to the bottom. I'm not sure it saves me anything over doing it on the Lagun though and requires more spending.

[BCRider]

What's the C to C length on the Sydney lathe? Can you run an extra long bar between centers and do the work down at the tail end of the lathe where the bed would have very little wear?

This seems like it's tailor made for line boring in the lathe using a long bar between centers. It would suffer far less overhang issues than any of the other options you're looking at And it could easily reduce the alignment issues you may encounter.

The other option would be to weld a few buttons to the assemblies which then get machined to act as reference surfaces Or possibly if there's low enough distortion in the assemblies from welding you could spot touch some reference spots on the existing parts. Then you could flip things around willy nilly and just clock the stuff in for each side to get it right.

The first obvious option is to skim off the ends of all the corner tubes so the plane the ends mark out is square as possible to the two ends. And then with one set of four faced off flip and skim the other ends so both are exactly the same "thickness". After that pick something you can spot off to use for the other two axes.

I've gotten inspired by Joe Pie's more recent videos on the steam engine and now his lathe over using reference spots machined into the actual part or into the excess waste material and how handy they become. And if your assembly doesn't have any waste material? Make some with build up spots of weld or weld on some little blocks? I'm thinking that if needed adding build up spots on the OD of the corner tubes could then be milled so the four on each side are machined so they describe a place which is square to the skimmed and length sized tube ends pretty easily. And that would give you the references you need to set up and bore the two near sides and then to flip it and bore the other two. In fact I can see it now using a dialed in angle plate with a corner stop and you use the ends of the tubes against the face and two of the register bumps against the corner angle reference clamped to the angle plate as your stops. This assumes that the holes are right in the middle for both. If there's some other alignment then you'd need two corner stops on the angle plate.

This way you can bore the holes in your mill and you only need to clear the 2.125" reach on each end. But with some care and checking with dial and DTI gauges you should be able to keep things centered to within a couple of thou at most. And I'm thinking it could easily come out tighter than that.

This all rests on getting the ends of the tubes sitting parallel from top to bottom and matching and then the machined resting surfaces on the one long side dead on square to those two planes and square as practical to the two ends.

I also assume here that the plates that take the bearings will be spot faced"

That's a lot of typing. I hope what I've said is fairly clear?

[tom_d]

I would follow the procedure as described in post #3. Don't worry about extra work filing four square holes. HSS is available in round. Any old broken end mills are ripe for donation to the cause here. Hack up some geometry that's close with the grinder and you're good to go with the cutters. Hold the boring bar in a three jaw, support with a tail stock live center. Hardest part is whatever you cobble up to mount the weldment to the cross slide. If you have the bed length for the additional travel it might only require two cutters.

[The Metal Butcher]

What's the C to C length on the Sydney lathe? Can you run an extra long bar between centers and do the work down at the tail end of the lathe where the bed would have very little wear?

54". It's possible down at the TS end would be better, but since I haven't mapped out the wear it's just very unpredictable. For conventional boring it would probably be my preference just due to the mass. But for line boring I don't see if offering any real advantages over the Lagun with the tight cross-slide and perfect ways.

This seems like it's tailor made for line boring in the lathe using a long bar between centers. It would suffer far less overhang issues than any of the other options you're looking at And it could easily reduce the alignment issues you may encounter.

Agreed, it is sort of the right piece for that machine. The only better machine would probably be a HBM. I do wish lathes still had Tee-slots though on the saddle.

The other option would be to weld a few buttons to the assemblies which then get machined to act as reference surfaces Or possibly if there's low enough distortion in the assemblies from welding you could spot touch some reference spots on the existing parts. Then you could flip things around willy nilly and just clock the stuff in for each side to get it right.

I'm not sure I understand.

The first obvious option is to skim off the ends of all the corner tubes so the plane the ends mark out is square as possible to the two ends. And then with one set of four faced off flip and skim the other ends so both are exactly the same "thickness". After that pick something you can spot off to use for the other two axes.

Tubes are to dimension. That maybe wasn't the smartest as they aren't in a perfect plane after welding.

I've gotten inspired by Joe Pie's more recent videos on the steam engine and now his lathe over using reference spots machined into the actual part or into the excess waste material and how handy they become. And if your assembly doesn't have any waste material? Make some with build up spots of weld or weld on some little blocks? I'm thinking that if needed adding build up spots on the OD of the corner tubes could then be milled so the four on each side are machined so they describe a place which is square to the skimmed and length sized tube ends pretty easily. And that would give you the references you need to set up and bore the two near sides and then to flip it and bore the other two. In fact I can see it now using a dialed in angle plate with a corner stop and you use the ends of the tubes against the face and two of the register bumps against the corner angle reference clamped to the angle plate as your stops. This assumes that the holes are right in the middle for both. If there's some other alignment then you'd need two corner stops on the angle plate.

I think I get what you are saying. If I were to make a jig, here is how I think I would do it. I'd drill and bore one end roughly in the center to finish size. Being within a 32nd or so is plenty. Then I would turn a plug that was a snug fit. After that I could turn the other end in the lathe or using the plug in the mill. But that's not to say your method wouldn't work. I'd rather avoid more welding if possible, and especially machining of welds. They do not machine nicely.

This way you can bore the holes in your mill and you only need to clear the 2.125" reach on each end. But with some care and checking with dial and DTI gauges you should be able to keep things centered to within a couple of thou at most. And I'm thinking it could easily come out tighter than that.

This all rests on getting the ends of the tubes sitting parallel from top to bottom and matching and then the machined resting surfaces on the one long side dead on square to those two planes and square as practical to the two ends.

I also assume here that the plates that take the bearings will be spot faced"

Ideally. These aren't overly precise bearings. They have set screws after all, meant to be a slip fit on shafting. Even if the snap rings only touch in one spot, the thrust forces will be very low, so they aren't going to twist the bearings in their bores.

That's a lot of typing. I hope what I've said is fairly clear?

Eh... not entirely lol. Maybe it's my reading comprehension though.

And for a third question: How would you measure the bore while line-boring it? I have tele-scoping gauges, but they won't fit with anything but a tiny bar.

[tom_d]

And for a third question: How would you measure the bore while line-boring it? I have tele-scoping gauges, but they won't fit with anything but a tiny bar.

Knowing the diameter of the bar all you need is a small hole gauge to determine the gap between the bar and hole. Make several measurements and take an average if the bar is not running concentric. Gap x 2 + bar dia. = hole dia. Note: gap should equal the cutting tool projection from the bar.

[The Metal Butcher]

I would follow the procedure as described in post #3. Don't worry about extra work filing four square holes. HSS is available in round. Any old broken end mills are ripe for donation to the cause here. Hack up some geometry that's close with the grinder and you're good to go with the cutters. Hold the boring bar in a three jaw, support with a tail stock live center. Hardest part is whatever you cobble up to mount the weldment to the cross slide. If you have the bed length for the additional travel it might only require two cutters.

I'm not sure I need more than one cutter. Since setup is so much longer than the cutting, cutting one bore and then moving the cutter from one hole, to another, to another, is really no slower than setting 2 or 4 cutters and cutting 4 bores at once. That and there is less cutting pressure, though I could cut on opposite sides to mitigate that. However, I think that twice the length of bar and only setting the cutter once for each cut would be easiest.

Knowing the diameter of the bar all you need is a small hole gauge to determine the gap between the bar and hole. Make several measurements and take an average if the bar is not running concentric. Gap x 2 + bar dia. = hole dia. Note: gap should equal the cutting tool projection from the bar.

Bamm!! That's why I love this site. Okay, question 3 solved. I have small hole gauges. That will work. Thanks!

[Doozer]

Bring it on over !

-D

[nickel-city-fab]

I actually don't use square holes on my boring bars. Too much work. I use round holes that are 1.414x the size of a square bit
Could easily make a between-centers bar like that before lunch