.251 Reaming Problems

CapnBlake · Jun 3, 2020

Hey, so this is my first post on here, this might not be the best section for this question.
Also somewhat new to machining.
So I'm working on a part that has four .251 +/-.0005 with .001 true pos. Im cutting them with the part attached firmly to a spud in a ddr rotary in a mori seiki dv. I have a .234 drilling the thru hole, as there are two holes on one face and the other 2 mirror them on the opposite face. The .2505 reamer is cutting to size at the top and the bottom at S550 feeding 4. Though it is tapering a few tenths from top to bottom which is throwing off on the cmm.

Basically would leaving .0085 per side from a letter A drill for a .2505 reamer cause it to taper smaller from top to bottom? or should I bring in a letter C Drill to lighten the load?

Thanks

kenton · Jun 3, 2020

Might try using an end mill to circle out a smaller drilled hole to .240ish and then ream. The endmill will make sure the starting hole is straight for the reamer to follow. You could probably bump the feed up a bit too.

DanASM · Jun 3, 2020

You have a few too many variables to solve this problem right away but I will try to help you narrow it down.

Reamers like to taper when they aren't lined up correctly. You have 2 good holes on top and 2 tapered ones on the bottom so that tells us the reamer is probably lined up correctly.

Next thing is to check the holes. Maybe the drill "walks" a little and the hole could be tapered before reaming. Check holes before reaming for taper.

I did this same hole recently and I think I left .014-.016 before reaming (I believe .007-.010 is what the book says to leave per side). It looks like you are on point with that.

how long is the reamer stickout?

I am leaning more towards the hole being tapered before reaming or somehow the reamer is off just a bit. Try half speed of the drill with twice the feed rate.

Although in my world if its tapered a tenth or 2 it most likely wouldnt even be noticed.

We need more info. What material? How deep is the hole?

litlerob1 · Jun 3, 2020

You have chips making your hole bigger. 5% of the Reamer's diameter is what you want. On any rotary, holding .001" TP is not for the feeble minded. I'm guessing you need a better Reamer. There are as many styles of Reamers as boring Japanese Sedans.

R

Whysosharp · Jun 3, 2020

Use a letter C drill. Or interpolate with and endmill. Knowing depth and material would help

DanASM · Jun 4, 2020

I am leaning toward the chips getting in the way. If you have buildup in the flutes from the first 2 holes what you can do is reverse spindle direction in between holes to "fling" the chips off of the reamer. Just a quick little reverse and right back to forward should do the trick.

Larry Dickman · Jun 4, 2020

there are a gazillion variables, and you haven't given us muck to work with. Be that as it may, drill your hole undersize, bore it with one of these or equiv

METRIC PRE-REAM ENDMILL

then ream with the correct size reamer. Make sure your reamer is indicated in, any runout will give you a shit hole.

Mike1974 · Jun 4, 2020

I can't say a reamer won't work. But I would probably just interpolate it with a 3/16" or 6mm endmill and be done, especially trying to hold +/-.0005"

Did not see total depth however, so maybe a solid carbide boring bar (but that gets expensive when you need to dial tenths)...

Badbascom · Jun 4, 2020

Kind of going thru the same thing, I would use a boring head.

litlerob1 · Jun 4, 2020

I'm not sure you guys that are recommending Boring are looking at the size of the hole. (It's in the Title). Not saying that Boring isn't possible or an option, but who the fuck Bores a 1/4" hole? Waste of time. If we're going to recommend a different process altogether--just Drill them with a good Drill and be done with the job.

R

Badbascom · Jun 4, 2020

litlerob1 said:
I'm not sure you guys that are recommending Boring are looking at the size of the hole. (It's in the Title). Not saying that Boring isn't possible or an option, but who the fuck Bores a 1/4" hole? Waste of time. If we're going to recommend a different process altogether--just Drill them with a good Drill and be done with the job.

R

I am currently boring .2360+/-.00035 holes. It is the true position he has to worry about, he is only allowed .0005 radial error. Add in machine positioning error, machine squareness error, & CMM error and 0.0005 is not easy. Then throw a reamer which I envision will bend more than a boring head and you have a lot of problems.

litlerob1 · Jun 4, 2020

Badbascom said:
I am currently boring .2360+/-.00035 holes. It is the true position he has to worry about, he is only allowed .0005 radial error. Add in machine positioning error, machine squareness error, & CMM error and 0.0005 is not easy. Then throw a reamer which I envision will bend more than a boring head and you have a lot of problems.

I'm interested to know how you came up with .0005" radial error. We don't know what material condition is on his print. Either way, Boring is slooooow. I'd confidently do it with a Drill. TP and Diameter.

R

R

Badbascom · Jun 4, 2020

litlerob1 said:
I'm interested to know how you came up with .0005" radial error. We don't know what material condition is on his print. Either way, Boring is slooooow. I'd confidently do it with a Drill. TP and Diameter.

R

R

He said his true position tolerance is .001.

litlerob1 · Jun 4, 2020

Badbascom said:
He said his true position tolerance is .001.

But if he's got MMC or LMC that changes a lot.

DMF_TomB · Jun 5, 2020

CapnBlake said:
Hey, so this is my first post on here, this might not be the best section for this question.
Also somewhat new to machining.
So I'm working on a part that has four .251 +/-.0005 with .001 true pos. Im cutting them with the part attached firmly to a spud in a ddr rotary in a mori seiki dv. I have a .234 drilling the thru hole, as there are two holes on one face and the other 2 mirror them on the opposite face. The .2505 reamer is cutting to size at the top and the bottom at S550 feeding 4. Though it is tapering a few tenths from top to bottom which is throwing off on the cmm.

Basically would leaving .0085 per side from a letter A drill for a .2505 reamer cause it to taper smaller from top to bottom? or should I bring in a letter C Drill to lighten the load?

Thanks

.
some leave material above top of finished hole and ream before, then machine material off, so tapered hole part is machined off. tapered hole part usually top 0.1" of depth, depends on material hardness
.
also if ream .2490 then ream .2505 that might help with taper, was common in old days ream -.001 to -.005 then finish ream. if you ever hand ream doesnt take long to realize much harder to hand ream more than .005"

ChipSplitter · Jun 5, 2020

litlerob1 said:
I'm not sure you guys that are recommending Boring are looking at the size of the hole. (It's in the Title). Not saying that Boring isn't possible or an option, but who the fuck Bores a 1/4" hole? Waste of time. If we're going to recommend a different process altogether--just Drill them with a good Drill and be done with the job.

R

It's true that boring MIGHT improve positional accuracy by eliminating the chance of the drill wandering.
But unless he has a junk drill or is drilling on a sloped surface he shouldn't have to worry about that.
And yes, boring would be painfully slow....... :eek:

>>>OP, look at combined drill and reamers, called dreamers. Fullerton Tool makes them as well as other grinding shops.
Nice, quick hole-in-one. They get used around here on automotive components so they should be good enough for you.

theperfessor · Jun 5, 2020

I didn't see whether these are blind holes, but the way the OP worded it makes me think that's the case. Dreamers are usually used on thru holes. The few times we've had to drill holes to that level of precision on both size and position we drilled and then bored before reaming. Anything you do beyond drilling and reaming one time will take more time. Orbit a mill, double ream, bore, take off some of the surface, it will all add time. If you get good results with more than one method then just run the speed/feed/time #s and pick the quickest. I pesonally go with the drill/bore/ream method, a retired T & D guy told me that was the way he did it (successfully). A good carbide boring bar can bore a 1/4" hole pretty quick, and since your following that with a reamer the sizing of the bored hole isn't too fiddly.

ChipSplitter · Jun 5, 2020

theperfessor said:
I didn't see whether these are blind holes, but the way the OP worded it makes me think that's the case. Dreamers are usually used on thru holes. The few times we've had to drill holes to that level of precision on both size and position we drilled and then bored before reaming. Anything you do beyond drilling and reaming one time will take more time. Orbit a mill, double ream, bore, take off some of the surface, it will all add time. If you get good results with more than one method then just run the speed/feed/time #s and pick the quickest. I pesonally go with the drill/bore/ream method, a retired T & D guy told me that was the way he did it (successfully). A good carbide boring bar can bore a 1/4" hole pretty quick, and since your following that with a reamer the sizing of the bored hole isn't too fiddly.

The OP never specified hole end condition. He never even came back after the first post, so we are all shooting from the hip. :crazy:

As far as the boring goes, with a 1/4" hole and 0.002 ipr gives you only 10 ipm at 5000 rpm. You can't increase the SFM too much for obvious balance reasons.
Waste of time, IMO.

theperfessor · Jun 5, 2020

Whatever works! That's what I love about this trade, there are lots of ways to get the same end result. Many good ideas here.

litlerob1 · Jun 5, 2020

theperfessor said:
Anything you do beyond drilling and reaming one time will take more time. Orbit a mill, double ream, bore, take off some of the surface, it will all add time.

What this describes is not "adding time", it's sinking the boat.

.251 Reaming Problems

Plastic

Stainless

Hot Rolled

Diamond

Cast Iron

Hot Rolled

Titanium

Diamond

Plastic

Diamond

Plastic

Diamond

Plastic

Diamond

Diamond

Titanium

Cast Iron

Titanium

Cast Iron

Diamond

Similar threads