Concentric Bores.......

[justmakingchips]

I could use some help with these new parts. I am making some parts out of round S7 that are around 10" long. The parts have a linear hole thru the entire length that is .204" in diameter that we are doing in a gundrill application. Then the part has a bore in the one end that is .427" in diameter that is roughly 2.5 deep. The two bores have a callout of less than .001" concentricity. We have failed in this area several times in the past and could use some help on machining these bores. I have tried gundrilling the .204" bore thru and then using a 3 flute c'bore bit with the pilot ground to .2035" with no luck. Any advice would be appreciated!

 

[gregormarwick]

How are they being checked?

 

[SIP6A]

You could try gundrilling from both ends.

 

[michiganbuck]

QT(The two bores have a callout of less than .001") to the Od or to each other?


I have bored all from one end and then skimmed the OD a few thousandths by turning or grinding with the part held between centers.
Using a Norton point-mounted "center lap" stone/wheel by hand makes a nice bevel to the Id to be used on the machine centers.
Also,
I have made centered plugs to go into the part ends to be used as part centers.
*Be sure you have a way to pull such plugs.

Also, a 7/16 reamer might be ground into a special step reamer to match the larger bore to the smaller bore in the same holding...allowing -.00025 -.0003 on both reamer and step.

Center Lap Mounted Points

Center lap mounted points are used on Excell-O center lap and similar machines. Achieve precise dimensional tolerances and ensure accurate and smooth center

www.nortonabrasives.com

 

[justmakingchips]

QT(The two bores have a callout of less than .001") to the Od or to each other?


I have bored all from one end and then skimmed the OD a few thousandths by turning or grinding with the part held between centers.
Using a Norton point-mounted "center lap" stone/wheel by hand makes a nice bevel to the Id to be used on the machine centers.
Also,
I have made centered plugs to go into the part ends to be used as part centers.
*Be sure you have a way to pull such plugs.

Also, a 7/16 reamer might be ground into a special step reamer to match the larger bore to the smaller bore in the same holding...allowing -.00025 -.0003 on both reamer and step.

Center Lap Mounted Points

Center lap mounted points are used on Excell-O center lap and similar machines. Achieve precise dimensional tolerances and ensure accurate and smooth center

www.nortonabrasives.com

The callout is to the OD and each other. We do grind the OD using centers

 

[michiganbuck]

Step tool nose -.0002 to .00025 with plenty of coolant.
A warm part and -.0005 nose may be the problem...double .0005 takes up your tolerance.

 

[MCritchley]

.001 is tight! I speak from a very low volume perspective, so my way of thinking would be to perhaps add a step or two so i have zero rejects and am confident everything is within a few tenths.

After gun drilling, grind the OD off of plugs that slide into the drilled bore. Make a couple of plugs in .0001 increments so you always have the perfect plug. Now your bores run within a few tenths of the OD. After grinding, indicate each side and bore. That would be a tough bore to cut, perhaps heavy metal bar territory for sure.

 

[guythatbrews]

So .001 each bore and the OD. Wow. How many pieces? Is the .204 hole straight within .001 and how can you check that? Lots of questions but little help here.

I'd drill the .204, indicate each end true and bore centers, grind the OD, rough drill the .427 with a flat bottom, then bore the .427 hole with some kind of a bar that might not chatter with a very small TNR, working off the OD of course.

Last step for me will probably be throw the parts away because I doubt I can make them. Wait, I'll just throw the material away before I cut anything and save a ton of work.

Good luck and be sure to tell us how you manage.

 

[memphisjed]

Do the counter bore first.

 

[michiganbuck]

Might you gun drill the .204, grind/turn OD between centers, put the but end on a lathe headstock center with the out end in a steady, and bore the .427?
Yes, grind your step tool/cutter to be a rougher at 13/32 or so.
.o10 a side would be a fast take and .0005 to .0007 concentricity should be not difficult.

Might leave the OD +.010 if steady marking would be a problem. and then finish grind/turn the OD .

I usually put a part between centers, and then bring my steady to a shim feel to the part.

The fancy setup would be to make the part OD a very close slip fit to a bearing and a bearing on the part with the bearing held in the steady.

I would turn a mild center in the lathe headstock so that center would be dead true.

I would have two gun drills so one could go/be out for sharpening.
Doing a lot of gun drill work I would have a Tc grinder because gun drills are easy/quick to end sharpen...most would take 5 to 10 minutes with the GD tail on a center and the nose in a bushing...no fancy sharpener is needed.. the wheel at an angle and the wheel head raised and lowered to make clearance angle, a wheel on both ends of the spindle so to stay finely dressed.