# Need to bore a 3/4" hole 3.75" deep



## devils4ever (Apr 16, 2021)

Hi all,

I'm looking to drill/bore a hole that is 3/4" in diameter and is 3.75" deep in mild steel.

Originally, I was planning on doing this on my lathe with the square stock in a 4-jaw chuck. But, now I'm realize I don't have a lathe boring bar that long plus I'm worried about the vibrations caused by the offset nature of my stock. So, I'm thinking of doing this on my PM25 mill.

I could get a 3/4" drill bit with a 1/2" shank, but I've read that is a no-no because the mill can't handle it.

I do have a Criterion boring head, but my boring bars are too short. I'm having a hard time finding long boring bars for the boring head. All my searches lead me to boring bars for the lathe. 

So, can anyone suggest a boring bar that is long enough for the boring head?

Can I use lathe boring bars in my boring head? I guess I would have to run it backwards?

Or, can I use a 3/4" drill bit with reduced shank?

Thanks!


----------



## sdelivery (Apr 16, 2021)

You have not mentioned what tolerances are desired.....
Drill on the lathe in steps i.e. 3/16, 1/2, 3/4 or 23/32 and ream to 3/4


----------



## devils4ever (Apr 16, 2021)

I would like to keep it tight enough for a 3/4" rod can slide smoothly with minimal wobble. So, +/- 0.002"??

It is for a tool rest for a belt grinder I'm building.


----------



## SLK001 (Apr 16, 2021)

I would do it all on the lathe.  If you don't have a boring bar long enough for the task, get one.


----------



## devils4ever (Apr 16, 2021)

Yeah, I was planning on that. But, I realize the hole is offset from the center and the piece is 2.5" X 2.5" X 3.75" and my mini-lathe might start to shake apart!


----------



## epanzella (Apr 16, 2021)

Counterweight and then determine how slow you have to go. If this part is going to be slit with a pinch bolt drilling is good enough.


----------



## BladesIIB (Apr 16, 2021)

devils4ever said:


> I would like to keep it tight enough for a 3/4" rod can slide smoothly with minimal wobble. So, +/- 0.002"??
> 
> It is for a tool rest for a belt grinder I'm building.


In addition to your balance issue. A bar that small sticking out that far will have a tendency to chatter and flex away so could be challenging. If concentricity of the bore with the OD is not critical I would consider the reamer option.  If done in steps as mentioned your Mill should be able to handle it.


----------



## machPete99 (Apr 16, 2021)

That might be a bit deep for a boring bar, unless you had some exotic carbide bar. The flex could otherwise be a problem.
Another option would be to drill it slightly undersize on the lathe (maybe by 1/64) and then ream it to size.
Or, just drill it out at 3/4 on the lathe and hope that it is not too oversized.


----------



## devils4ever (Apr 16, 2021)

epanzella said:


> Counterweight and then determine how slow you have to go. If this part is going to be slit with a pinch bolt drilling is good enough.



Yes, I'm cutting a slit lengthwise with a bolt to pinch it for adjustments.

I thought the maximum diameter for a small mill and small lathe is 1/2" since that's the size of the chucks. I know you can buy reduced diameter shanks, but I thought that was a no-no.


----------



## SLK001 (Apr 16, 2021)

devils4ever said:


> I know you can buy reduced diameter shanks, but I thought that was a no-no.


Sometimes, you gotta do what you gotta do.  Just remember to take small steps up to the final diameter, or get close, then bore to final diam.


----------



## Winegrower (Apr 16, 2021)

A bigger lathe, longer boring bar, Silver&Deming drill set, maybe a mill...I don’t see the problem here.


----------



## mmcmdl (Apr 16, 2021)

Use a dreamer .


----------



## macardoso (Apr 16, 2021)

100% for the reamer.

Rough drill, maybe kiss it with a boring bar so you know it is straight (chatter won't matter), and ream to finish. I like to have the starting hole for the reamer be 97% of the finish hole diameter.

Reamers can have their shanks reduced by turning very easily


----------



## MrWhoopee (Apr 16, 2021)

Ream with a drill. Bore to within .010-.015 of size, then finish with the drill. The small amount of metal removal prevents the grind of the point from affecting size.


----------



## Mtnmac (Apr 16, 2021)

MrWhoopee said:


> Ream with a drill. Bore to within .010-.015 of size, then finish with the drill. The small amount of metal removal prevents the grind of the point from affecting size.


This is what I would do.  But be sure the drill is on center, use a indicator to check it.  If it‘s off center at all, it will act like a boring bare and cut oversize.


----------



## Flyinfool (Apr 16, 2021)

±.002 is pretty tight for any drill to hold. You need to either ream or bore for that tolerance.

Since this is a through hole, you can also drill and bore from both ends, now you only need a 2 inch boring bar.

You can either buy or make a heavy boring bar that is long enough. You want the biggest diameter bar that will fit in the starting hole.

You can use the reduced shank drill as long as you don't get greedy. Buy a set of drill bits and step your way up to final size. This will prevent overloading the mill.


----------



## markba633csi (Apr 16, 2021)

I'm going to ask the question no one else did:  can you change the design and/or material so you aren't looking at such a daunting operation?
If I was looking at making a hole that large and that deep I would be asking myself "do I really need to do it this way?"
-Mark


----------



## devils4ever (Apr 16, 2021)

A chucking reamer might be impossible since they're 9.5" long and I don't have that Z capacity in my mill. I guess I could use a hand reamer? They don't seem to have as many options as the chucking reamers (i.e. over/under by 1 or 2 thou from .0750").

For drilling, I guess I could start at 1/2" and go up in 1/16" steps (9/16", 5/8", 11/16") with a Silver & Deming drill bits? I'm assuming I want the 3-flat version so the bit doesn't slip in the chuck?

I could change the design if I had to, but would prefer not to.

As to drilling and boring from each end, I'm not sure I could align things perfectly after turning the part around.


----------



## macardoso (Apr 16, 2021)

This is about as good as they get.









						.751" HSS Chucking Reamer   | eBay
					

Find many great new & used options and get the best deals for .751" HSS Chucking Reamer  at the best online prices at eBay! Free shipping for many products!



					www.ebay.com


----------



## devils4ever (Apr 16, 2021)

Yes, but it's 9.5" long.


----------



## macardoso (Apr 16, 2021)

devils4ever said:


> Yes, but it's 9.5" long.


Ah Right. Shoot


----------



## BladesIIB (Apr 16, 2021)

devils4ever said:


> Yes, but it's 9.5" long.


The reamer is easily shortened. Grind around the circumference and then snap it off. I shorten reamers all the time.


----------



## epanzella (Apr 16, 2021)

devils4ever said:


> Yes, I'm cutting a slit lengthwise with a bolt to pinch it for adjustments.
> 
> I thought the maximum diameter for a small mill and small lathe is 1/2" since that's the size of the chucks. I know you can buy reduced diameter shanks, but I thought that was a no-no.


The biggest horsepower eater on the drill bit is the center web which has nearly zero cutting speed. If each size drill you use has been preceded  by a pilot hole drilled with a diameter at least as big as the center web you should be able to step up to a 3/4" hole even on a small machine. This job could have been done in the time it took to read all these posts.


----------



## mikey (Apr 16, 2021)

I would just buy a 1/2" diameter carbide boring bar and bore it on the lathe. That is a simple boring job. Off set it in a 4 jaw, counterbalance if needed or go slow enough to get it done. If you can find a bar that takes AK aluminum cutting inserts then going slower will work fine. Get the smallest nose radius you can find.


----------



## sdelivery (Apr 16, 2021)

Considering it's use and the fact it will have a pinch bolt drill it and be done


----------



## mksj (Apr 16, 2021)

Maybe I am missing something here, the PM-25 is capable (at least per their website) of drilling up to 1" in steel. Drill a 1/2 or 5/8" hole first then follow with a 3/4" drill held in a R-8 holder. Do not use reduced shanks in a drill chuck, the alignment will be bad any you will probably fracture the chuck, in particular a self tightening type. I already learned the hard way and busted a 1/2 precision keyless chuck using a reduced shank drill. If you need a bit more clearance you can run it under slow speed with a 0.751" reamer, doesn't matter about the reamer shank length. Alternative, which I frequently use on both my mill and lathe is an annular cutter, takes much less cutting force and you get very clean, accurate straight bores. In a smaller mill hold it with a R-8 3/4"collet, I would run it at around 250 RPM with lube. Key to using annular cutters is not to hunt and peck, keep a nice even pressure, I back off occasionally to allow the swarf ribbons break and then gradually reengage the cutter. A boring head is not going to cut it in that size mill.









						Drill Bits for sale | eBay
					

Get the best deals on Drill Bits when you shop the largest online selection at eBay.com. Free shipping on many items | Browse your favorite brands | affordable prices.



					www.ebay.com
				




Alternate option if you can hold it in a 4J independent chuck would be to run it with MT drills in the tailstock, if you have a mini-mill then I doubt any of the options will work very well. I routinely drill or bore with my lathe as deep as 8". I also use annular cutters in the tailstock for work up to 4" deep and then run it with a boring bar to final dimension.

Last option, assuming the plate is not too big or heavy to mail, ship it to me with the specs that you want and I will drill the hole and return to you for the cost of shipping.
Mark


----------



## devils4ever (Apr 17, 2021)

Yes, that makes sense! Excellent idea. I can accept end mills and drills up to 3/4" in my mill using either R8 collets or ER32 collets which would run truer and hold better than a drill chuck. Or, can I use reduced shank drill bits (S&D) in a collet? This might prove more useful in future projects plus all the shanks are 1/2" which is nice since using a collet to hold a 47/64" shank might prove troublesome.

For reaming, I'm thinking I'll need to drill to about under size at 47/64". Would a 47/64" shank tighten properly in a 3/4" collet (1/64" undersize)?

I'm just a bit leery of doing this on my lathe. I can just see it vibrating and moaning and objecting to this operation. I think my mill is more capable.

Thanks for the offer. I'd like to do this myself, if possible as a learning experience.


----------



## devils4ever (Apr 17, 2021)

BladesIIB said:


> The reamer is easily shortened. Grind around the circumference and then snap it off. I shorten reamers all the time.



So, I can use my 4-1/2" angle grinder to score all the way around the shank and it will snap off? Is the shank hardened?


----------



## BladesIIB (Apr 17, 2021)

devils4ever said:


> So, I can use my 4-1/2" angle grinder to score all the way around the shank and it will snap off? Is the shank hardened?


Maybe more than just a score depending on the size of the shank.  Go maybe half way through total and yes, typically the whole reamer is made from HSS or Cobalt so the shank is hard. Also gives you a piece you may be able to use later in your lathe for a tool bit.


----------



## SLK001 (Apr 17, 2021)

devils4ever said:


> So, I can use my 4-1/2" angle grinder to score all the way around the shank and it will snap off? Is the shank hardened?


Why do that?  Just use the grinder to cut it off where you want the length to be (use a cutoff wheel, not a grinding wheel).


----------



## mksj (Apr 17, 2021)

If you are drilling in steel with decent twist drills, I find that the hole diameter is quite close to spec. I will run the hole with a reamer 0.0750" or +.001" over just to take out the ridges or waves. My reamers are around 12", I do not see any reason to cut them shorter as I primarily use them to clean up the hole or slightly oversize the whole. Given the length of the hole and depending on the shaft dimensions  you may need a +0.001" oversize.  I find that drilling the pilot hole with say a 5/8" drill first followed by a 3/4" works better than just trying to drill the hole with a larger drill. Softer metals is a differnt story. I would try not to use reduced shank drills if possible, the holding power will be reduced and often they have flats for use in smaller drill chucks.


----------



## devils4ever (Apr 24, 2021)

I was successful in getting this hole done this morning. It took a good 2-3 hours all told between trying to figure out the best way to hold the part, aligning it, tramming the mill, and drilling in succession. I used 2 parallels stacked flat to raise the part enough to not have me drill into my mill table.

I started with a spot drill, then went to 7/16". This was followed by 1/2", 9/16", 5/8", 11/16", 47/64" drill bits. I'm glad I stepped up in 1/16" increments because the motor seemed to struggle a bit.

Finally, the 0.7500" reamer was used to finish the hole. The reamer was shortened by about 1.7" to fit between the quill and part. I used my angle grinder with a cutoff disc. It cut through surprisingly fast for HSS. I have to use it more often. I never think of using it. I finished with a grinding disc to smooth the cut edges.

I used lots of cutting fluid throughout. 

The hole is perfect for the rod. No noticeable play at all. Slides really nice. Now, I'm hoping the hole doesn't change dimensions when I cut the slot! Pray for me!

Hopefully, I'm not boring (pun intended) anyone by posting these pics of the process.

Setup pic.



First hole drilled.



Next size up.



9/16" drill.



Ready to ream.



Done.



Finished with matching rod inserted.


----------



## BladesIIB (Apr 24, 2021)

Thanks for the follow up. Glad your part worked out as planned. Worst case if it springs tight when you slit it you can always put one set screw to push it open and the other set screws to clamp it shut.


----------



## devils4ever (Apr 24, 2021)

Yes, that's a good idea. 

Or, I could try to ream it again assuming I can get it in the same exact position.


----------



## mikey (Apr 24, 2021)

BladesIIB said:


> Thanks for the follow up. Glad your part worked out as planned. Worst case if it springs tight when you slit it you can always put one set screw to push it open and the other set screws to clamp it shut.



How likely a scenario is it for a work piece to spring tight after being slit? I've never seen or heard of this before so this is a real question. I've slit a lot of work pieces with holes and have never seen it get tighter.


----------



## devils4ever (Apr 24, 2021)

That's good to hear. This is the first time I'm creating a slit for a rod to be clamped in a closely matched hole. So, I am a little worried based on the next paragraph.

I needed to mill out a "fork" shape for my belt grinder build. The fork was cut at the end of 1-1/2" square stock. It was about 1"+ deep and 1" wide. This fork was the pivot point for the tracking wheel arm. I decided to use my bandsaw to remove the bulk of the material before milling it. As I finished the bandsaw cut, I heard a "ping". I'm assuming the steel moved from internal stresses. I don't know how it moved since I left enough material to cleanly mill out the fork.


----------



## MrWhoopee (Apr 25, 2021)

Not unheard of to have a piece of steel move unexpectedly in the least desirable direction. Expect it, anticipate it, plan for it. 
In this case, if possible, stress-relieve with a torch before splitting. If not, spread and insert shim then stress-relieve or re-ream while clamped in the "relaxed" condition.


----------



## extropic (Apr 25, 2021)

@devils4ever​
Is there some reason you didn't remove the ER chuck and mount the reamer in (a collet, in) the spindle?
You may be in love with the ER chuck, however in this case, I don't think it was your friend.
In your circumstance, I wouldn't have shortened the reamer. Hopefully, the reamer won't be "too short" for the next deep 3/4" hole.


----------



## devils4ever (Apr 25, 2021)

Yeah. I messed up on that. Good catch. I was planning on using R8 collets and removing the ER chuck. I forgot in the heat of battle and realized it afterwards.

I did some quick calculations and measurements and I think it would have just made it if I didn't shorten it.


----------



## SLK001 (Apr 25, 2021)

MrWhoopee said:


> Not unheard of to have a piece of steel move unexpectedly in the least desirable direction. Expect it, anticipate it, plan for it.
> In this case, if possible, stress-relieve with a torch before splitting. If not, spread and insert shim then stress-relieve or re-ream while clamped in the "relaxed" condition.



Yeah, do this BEFORE you final ream the hole!


----------



## devils4ever (Apr 25, 2021)

Well, I guess I got lucky. I cut the slit and nothing seemed to move. The rod still is movable in the hole with no play. Win!


----------

