Accurate hole diameter and position on a Bridgeport.

moonlight machine · Apr 20, 2020

I need to bore some holes on a Bridgeport, 4.9152-4.9148 diameter. I have a Sunnen dial bore gauge, reads .0001 and the micrometer setting fixture so hitting the diameter should not be a big deal. The problem is I have to move the table to measure the diameter because of the length of the bore gauge. My DRO only reads .0005 so I worry about getting the table back in exactly the correct spot. I was thinking about making a good solid hard stop with a .0001 indicator on it. I'll leave Y locked and only move X. The next bit of fun is I need to flip the part and do the same diameter on the other side as well. Thinking about making a piece to bolt on the table, OD same as my bore diameter. Indicate it true to the spindle, set the part on it after boring the first side, it should be lined up with the spindle. Am I missing anything?

Thunderjet · Apr 20, 2020

Not enough info.

How many holes?

Are they spaced?

If there is only one hole, leave room to grind in to your dims.

If there are multiple holes, you won't hit those callouts with a fifty year old Bridgey, tenth indicator or not........sorry.

dgfoster · Apr 20, 2020

As above plus general dimensions of the part, general location of the hole on said part, part material and importance of location relative to features vs just concentricity of the two holes being crucial but their location on the part not that critical. With that and the info requested in the above post, it might be possible to make useful suggestions.

Denis

Finegrain · Apr 20, 2020

moonlight machine said:
Am I missing anything?

Temp control
Play in the knee ways or quill
Tram error

Regards.

Mike

lucky7 · Apr 20, 2020

How deep is the hole? Makes head tram, and need to stay at same table location, even more important/difficult if deeper.

Ooooh, for a Moore jig bore...

L7

moonlight machine · Apr 21, 2020

Thunderjet said:
Not enough info.

How many holes?

Are they spaced?

If there is only one hole, leave room to grind in to your dims.

If there are multiple holes, you won't hit those callouts with a fifty year old Bridgey, tenth indicator or not........sorry.

2 parts, 7075T6, 14" long 6" wide 4" thick, one bore each side, 1.98 between bores, must be concentric, location on part +- .005 My main concern is getting the table back to 0 when I have to move it to measure the diameter.

moonlight machine · Apr 21, 2020

lucky7 said:
How deep is the hole? Makes head tram, and need to stay at same table location, even more important/difficult if deeper.

Ooooh, for a Moore jig bore...

L7

I could really use a jig bore on this one. I tram the head on a 9" diameter roller bearing race with the quill extended. It ends up dead nuts true.

DMF_TomB · Apr 21, 2020

moonlight machine said:
I could really use a jig bore on this one. I tram the head on a 9" diameter roller bearing race with the quill extended. It ends up dead nuts true.

.
bridgeport table famous for not being flat especially if heavy part on it and or clamping to table distorts as you tighten clamps
.
just saying its not the best for high precision, just the act of tightening gibs or X,Y,Z locks it can vary each time you loosen and retighten. obviously you'd need a .0001" indicator to see
.
be more like a dog chasing its tail going round and round checking measuring

Terry Keeley · Apr 21, 2020

moonlight machine said:
My main concern is getting the table back to 0 when I have to move it to measure the diameter.

A PITA for sure but could you indicate over the bore each time you move the table back?

Mount an indicator on the boring head somehow?

dgfoster · Apr 21, 2020

moonlight machine said:
2 parts, 7075T6, 14" long 6" wide 4" thick, one bore each side, 1.98 between bores, must be concentric, location on part +- .005 My main concern is getting the table back to 0 when I have to move it to measure the diameter.

Thanks for the additional info. Part of the reason for the added info request was to see if instead of using your BP, perhaps doing the job on a mid-sized lathe faceplate might be an option. Depending on how central along the long axis the bore might be, it sounds like this could be a good option. As a way to make precisely dimensioned, round, concentric holes in a part that lends itself to fixturing on a faceplate, it would be excellent. You probably already considered that option, but discarded it due to equipment availability concerns.

Denis

Thunderjet · Apr 21, 2020

moonlight machine said:
2 parts, 7075T6, 14" long 6" wide 4" thick, one bore each side, 1.98 between bores, must be concentric, location on part +- .005 My main concern is getting the table back to 0 when I have to move it to measure the diameter.

You should be able to hit those numbers. ( =/ - .005 is easy peasy.)

I would make certain the block is SQUARE and PARALLEL before I started the boring op.

Is there room for a construction/datum hole someplace? This would be very helpful to be sure you're back on location after the flip.

Does this mill have a DRO? if so, your good to go.

If not, be mindful of the backlash, and don't unlock the knee. until you're done.

jim rozen · Apr 21, 2020

moonlight machine said:
2 parts, 7075T6, 14" long 6" wide 4" thick, one bore each side, 1.98 between bores, must be concentric, location on part +- .005 My main concern is getting the table back to 0 when I have to move it to measure the diameter.

You don't need to. The diameter spec is what, +/- 0.0004, right?

As far as I can tell you don't have an absolute postion called out to any particular precision, only a diameter spec.

So you mount the part, bore it to within ten or 20 thou of final size, using a dial caliper. Take the part out and
measure the close tolerance diameter with the bore gage. Zero the table using your DRO. Then take the
final cut, calculating based on the bore gage reading. Yes you will move the hole location. But it willl be on size.

Tougher part is flipping it over and mounting it to your boss.

I suggest an aternative: a tooling plate with three dowel pins. This permits removing the part to measure and
getting it right back. Sounds like you are boring from both sides because you don't have enough Z travel, or are
both holes blind?

moonlight machine · Apr 21, 2020

DMF_TomB said:
.
bridgeport table famous for not being flat especially if heavy part on it and or clamping to table distorts as you tighten clamps
.
just saying its not the best for high precision, just the act of tightening gibs or X,Y,Z locks it can vary each time you loosen and retighten. obviously you'd need a .0001" indicator to see
.
be more like a dog chasing its tail going round and round checking measuring

It's what I have, I'll have to make it work... Thought about doing it in the lathe on a faceplate. The bores are for ceramic bearings and need to have a flat bottom. This means you need to change tools to do the bore closest to the face plate. I could qualify the second tool in the area between the bearing bores. No way to measure the second bore till I remove it from the lathe, it's a bit late to do any adjustment then!

moonlight machine · Apr 21, 2020

jim rozen said:
You don't need to. The diameter spec is what, +/- 0.0004, right?

As far as I can tell you don't have an absolute postion called out to any particular precision, only a diameter spec.

So you mount the part, bore it to within ten or 20 thou of final size, using a dial caliper. Take the part out and
measure the close tolerance diameter with the bore gage. Zero the table using your DRO. Then take the
final cut, calculating based on the bore gage reading. Yes you will move the hole location. But it willl be on size.

Tougher part is flipping it over and mounting it to your boss.

I suggest an aternative: a tooling plate with three dowel pins. This permits removing the part to measure and
getting it right back. Sounds like you are boring from both sides because you don't have enough Z travel, or are
both holes blind?

May as well be blind, they have a shoulder for the bearing to sit on.

moonlight machine · Apr 21, 2020

Thunderjet said:
You should be able to hit those numbers. ( =/ - .005 is easy peasy.)

I would make certain the block is SQUARE and PARALLEL before I started the boring op.

Is there room for a construction/datum hole someplace? This would be very helpful to be sure you're back on location after the flip.

Does this mill have a DRO? if so, your good to go.

If not, be mindful of the backlash, and don't unlock the knee. until you're done.

8 odd shaped triangular holes are through the part already. All the outside machine work has been done. All crazy angles except where the brake caliper bolts on and at the top 90* to where the camber block bolts on. The top area is only 2" wide and the caliper mount pads are 1" wide. Yes I have a DRO.

dgfoster · Apr 21, 2020

moonlight machine said:
It's what I have, I'll have to make it work... Thought about doing it in the lathe on a faceplate. The bores are for ceramic bearings and need to have a flat bottom. This means you need to change tools to do the bore closest to the face plate. I could qualify the second tool in the area between the bearing bores. No way to measure the second bore till I remove it from the lathe, it's a bit late to do any adjustment then!

So, you couldn’t bore the first hole to size and depth.

Remove part from the faceplate and turn a stub on the faceplate the same diameter as the bearing race or a couple tenths under .

Replace part on the faceplate using the stub for concentric location of the first bore.

Bore the second hole to depth and diameter?

Denis

Finegrain · Apr 21, 2020

Regardless of how you do it, you ought to nail down with the customer under what conditions they are going to measure. Given the tolerance, I would expect a temp-controlled metrology room. As such, you sort of need to have a temp-controlled shop. 3* F swing either way will blow your +/-.0002" tolerance, if I have the math right.

Regards.

Mike

moonlight machine · Apr 21, 2020

Terry Keeley said:
A PITA for sure but could you indicate over the bore each time you move the table back?

Mount an indicator on the boring head somehow?

Good Idea. I can make a bit to hold my 0-.005-0 .0001 B&S indicator in one of the other boring bar holes in the boring head.

moonlight machine · Apr 21, 2020

Finegrain said:
Regardless of how you do it, you ought to nail down with the customer under what conditions they are going to measure. Given the tolerance, I would expect a temp-controlled metrology room. As such, you sort of need to have a temp-controlled shop. 3* F swing either way will blow your +/-.0002" tolerance, if I have the math right.

Regards.

Mike

All good points. I hold my shop at 65* No metrology room though. Lucky though the customer is reasonable and not going to go crazy about a tenth or two.

Terry Keeley · Apr 21, 2020

moonlight machine said:
Good Idea. I can make a bit to hold my 0-.005-0 .0001 B&S indicator in one of the other boring bar holes in the boring head.

Yup, what I was thinking but wasn't sure what boring head you have.

My cheap Criterion has 3 holes in the bottom...

Accurate hole diameter and position on a Bridgeport.

Diamond

Stainless

Diamond

Diamond

Titanium

Diamond

Diamond

Diamond

Titanium

Diamond

Stainless

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Titanium

Similar threads