What's new
What's new

Opinions for tolerance required on a "REAM" Callout?

Johnny SolidWorks

Hot Rolled
Joined
Apr 2, 2013
Location
Rochester
Hey Gang - Kind of a weird question:

I have an old, old print with a thru hole callout for "REAM .501"

The obvious thing to do is run a .501 reamer through it, but I don't like reamers, and my mill has very limited Z travel, so reamers don't really like me either. I would much prefer to interpolate the hole...but to what size? I know it's not all that hard to get under or over sized holes with a reamer (which is one of the reasons I don't like them) but also what would a fair tolerance range be? Even if I did want to use a reamer, who's to say it would match the original reamer they had when the print was made some 60 years ago?

I know there are a lot of unknowns, but I'm just looking for a rule of thumb or best practice expectation for results with a reamer that I can duplicate on a print with an actual tolerance.

And no, asking the customer isn't an option (long, weird story) and I don't have the mating details, and can't get them.

Thanks All!

Edit after a couple of replys: Maybe a better question is: If I buy a .501 reamer and follow the manufactures recommendations for SFM and amount of material left to remove, what's a fair tolerance to expect? Is the .501 +/-.0002" reasonable?
 
I would guess you are overthinking this. I'd make it so a .500 pin goes through but a .502 doesn't. If you are worried aim for .5005 to .5015.

Of course I may just be a hack.
 
I have a saying for times like this. "Unless otherwise specified you get what I give you."

I see prints like that often and they can call them out multiple ways. Just helix a slip fit for a 1/2 dowel pin.

No need to over think it. Whoever drafted the print didn't.
 
Call up the customer and find out....why guess? From job shop experience, it is interpereted diffrently from one market to another, (IE-areospace-commercial).
 
From a design standpoint, if I specifically called out a reamed hole, and it came back interpolated, it could be problem. Depending on the quality of the equipment, interpolated holes can have geometry issues that are hard to live with. Not to say reamers don't have their own set of issues. When in doubt, bore.
 
From a design standpoint, if I specifically called out a reamed hole, and it came back interpolated, it could be problem. Depending on the quality of the equipment, interpolated holes can have geometry issues that are hard to live with. Not to say reamers don't have their own set of issues. When in doubt, bore.

That's a fair point, and if you had shouted it loudly enough I probably would have heard you! (I live in Good Ol' Wayne County - I was actually in Canandaigua for dinner just last week!)

For my curiosity: I know straight-flute reamed holes have a tendency to be tri-lobed due to flute flex, but besides taper, what kind of weirdness is typically seen with interpolated holes?
 
Call up the customer and find out....why guess? From job shop experience, it is interpereted diffrently from one market to another, (IE-areospace-commercial).

"And no, asking the customer isn't an option (long, weird story) and I don't have the mating details, and can't get them"

To the op: Doesn't matter whether you like reamers or not, that's the callout. Buy or modify a short 501 reamer to fit your machine. You will at least have a leg to stand on if they bitch about it. Otherwise not so much
 
That's a fair point, and if you had shouted it loudly enough I probably would have heard you! (I live in Good Ol' Wayne County - I was actually in Canandaigua for dinner just last week!)

For my curiosity: I know straight-flute reamed holes have a tendency to be tri-lobed due to flute flex, but besides taper, what kind of weirdness is typically seen with interpolated holes?

If you have a little backlash, you can get steps and sizing issues through the quadrants. Can also get them if you don't lead in/out properly as well. Endmill may taper a bit, wear on the bottom as opposed to the top, etc., (normal stuff really). The theory is all there for a perfect hole, but the actual may differ. A boring head is a decent option, but if a chip gets caught in the spindle, your size goes out, (not too often though).
 
What's block tolerance for three places on the print? That's technically what they're asking for. Anything better than that's a freebie.
It's a dumb way to call out a hole, but I imagine they would say the "ream" spec is tighter than the typical +/- .010 for 3 digits.

It's a minor pet peeve of mine when the draftsman tells me how to make a hole. Just tell me how big you want it, I already know how to make a hole. And don't tell me "drill .201 dia tap 1/4=20 thru". 1/4-20 UNC 2B thru and the location is all I need. I'll take it from there. I might want to form tap it or thread mill it. I'll get the minor right, don't worry.

If I see "Ream .501" and that's all, I am going to assume it's a slip fit for a 1/2" dowel pin. I'm going to give him a hole that is .501 +.0005/-0.

I'm not going t tell him how I made it, but I would probably use a reamer anyway.
 
My understanding of such a measure is that a half-inch solid something should fit a half-inch opening. The 0.501" goes with 0.500", where the larger value is the tolerance minimum and the smaller the opposite. That way you have a thou of tolerance. Depending on the length of the fit other deviations such as roundness and straightness are caught up. Never forget that straightness is the most difficult property of bores.

This is the reason for reaming, with a reamer and some experience you can achieve rather round and straight bores. The next better process would be honing.
 
An interpolated hole is never "round" or circular. How far out is expensive to measure.
One can never comp out or "zero-backlash build out" reversal errors at all the differing speeds a cnc has to operate inside.
(stick-slip, screw windup, multi-axis servo following error mismatch... lions and tigers and bears oh-my.)
Then again a reamed or bored hole will have errors also but usually to a smaller degree.

At the very best a nicely performing reamer will do +/-.0002 as that is the standard tolerance for making one.
60 years ago and today although arguably today's reamers are held to this spec better due to better measuring equipment and machines.
(and then there is a true to form cylinder vs a hole... :willy_nilly:)

Nowadays you can punch piston holes in a engine block all day long to .0002 tolerance, 60 years ago this was a dream and 10 times this was just about impossible in production.

People like using pins to measure holes. This makes me shutter in the now world of cnc interpolation.
One can make squares on your cnc that fit oh-so nicely to a gauge pin but....... perhaps that would work for your application.

Given the print age and lack of other information you may have to make a best guess as to why a ream was called out remembering that cncs were not a option back then and jig boring was expensive to do.
Often a ream was called out to prevent just drilling a hole.
"Drill and ream" was a staple of "nice finish and closer held". The tolerance block should not be looked at here, it is otherwise noted.
Put on your engineer and draftman's hat and think about why and what the application needs, ...... then go with your gut.
Bob
 
Best idea would be to ask the customer to avoid sending out parts that arent fit for purpose, why cant you ask the customer or find some other responsible person?

If that really isnt an option, and there is no tolerance on the hole, simply apply the general drawing tolerances to the hole and then spec a reamer to ream to mid limit, 0.501". That way you have reamed the hole as per drawing and applied the correct tolerance to it.

If its wrong, its not your fault for having a shit drawing.
 
.......

If its wrong, its not your fault for having a shit drawing.

Yea, that is the point where I tell "machinists" not to let the door hit your ass on the way out.
One expects some amount of brain power, not excuses that the print was not exact.
Min wage button pushers get the slack for not understanding what they make, real and well paid machinists do not.
Bob
 
I drew up whole machine worth of prints that had reamed hole call outs on them. These were for internal use only and never meant to be seen by the outside world. fast forward to a couple of years after our shop closed. The customer called me at home (I had retired by that that time) and said they needed to get two more machines built and who I would recommend to build them. ( I also retained the only full set of prints).

Out of all those prints with hole call outs, two had call outs for wired holes both for diameter and location. That caused all kinds of confusion for the new shop making them. I told them look at the assembly drawing and that would explain it all. well, they did and it didn't.(To them anyway.) I ended up going over the whole machine and process with them.

The whole key to the machine working properly were the wired holes. All of the reamed holes were to locate to adjoining parts that not critical to the proper operation of the machine.
 
If a hole is spec:ed to be reamed do not bore mill/file it adhere to the print as there is in general a reason for such a spec(form/fit/function) if in doubt about any tolerance ask for a revised print or have someone mail you a mail where the tolerance is explicitly stated unless you can derive yourself from the prints(ie through a global tolerance or by looking at mating parts).
What you do not want to do is guess and hope that it’s correct since it will be your reputation on the line, and if all of the above fails do not make the part(delivering bad parts is worse then not making parts at all).
 
I used to be a drafter. We did remove 'processes' from older prints, unless there was a reason for that particular process. The main reason is cost. If a supplier could produce a part to specs, ie size, surface finish etc. then why limit them. Also, if they had certain types of machines that gave a different finish, say Blanchard ground.
Now on the reverse of that, I was in an interview and mentioned this. One of the interviewers had an example of parts cracking, due to it being ground vs milling.
I also worried about how a part was dimensioned. I tired to dimension (GD&T), to the design intent of the part. I do remember on supplier wanting the part dimensions in a particular way. It was obvious to me that it suited their equipment and would be costlier to other to produce.
I think in the OP situation, it would be basically a 0.500 slip fit hole. IE 0.501 +/-0.0005
 
Yea, that is the point where I tell "machinists" not to let the door hit your ass on the way out.
One expects some amount of brain power, not excuses that the print was not exact.
Min wage button pushers get the slack for not understanding what they make, real and well paid machinists do not.
Bob

I agree to some extent with your opinion, but I was also taught that the print was God and it is not the machinist's place to try to interpret the design intent. Not to say that given the opportunity to ask talk to the designer about what they actually want should be passed up. But when push comes to shove if I made to spec what was on the print, no matter how stupid, I did nothing wrong.

Of course this does not apply to my current position and probably does not apply to the OP since it sounds like he is acting as a designer to some extent.

Edit: Just realized I contradicted my earlier post. :crazy:
 
You asked for opinions....
If I was making the part I would throw a .5007 carbide reamer in (we have those on hand where I work) and let it buck. Probably around 45 SFM and .006/.008 per rev (steel numbers) and let it go. I would expect the hole to end up a snug .501 fit but I would assume the customer wants a semi precision .500 shaft or pin to slide through the hole.
I am not intending to be a dick.......but your problem is more about your fear of reaming and less about what is a crappy callout on a print.
Solution....get to reaming. This is not the last time you will ever need to do it.:reading:
 








 
Back
Top