[Chalkboard247]

I just got a job to make some head plates for a Cummins in-line 6 diesel engine. There are 3 holes that I have to machine that match up with dow pins that stick out of the top of the engine block. He INSISTS that these holes are bored out using a boring bar.

On the same note, I have a 2011 HAAS VF-3 that will interpolate an endmill with a finish tool/pass to meet tolerances easily of plus or minus .0005". The tolerance he is expecting is .6325 plus or minus half a thou. Material is H13. Thickness is under an inch. I am good at making sure tool deflection is minimal.

So am I crazy for thinking this guy is crazy about using a boring bar when a rougher/finishing interpolating endmill will work just fine? Lead in and lead out will be used of course. Also, will he be able to tell a difference in surface finish from a boring bar? Never used a boring bar except for in school using an old Bridgeport. Thanks!

[txcncman]

As long as you can produce the part to the size and finish specifications, what does it matter how you accomplish the task? Why not drill and ream it?

[Khalid]

So am I crazy for thinking this guy is crazy about using a boring bar when a rougher/finishing interpolating endmill will work just fine? Thanks!

I think the guy dont know about the magic of CNC.. I will also suggest you to make some Mockup test on similar material and check the dimensional toleances of drill

[mcarvey]

Whether or not you actually need to bore the hole out is not really the point. If the customer insists, and expects you to use a boring bar, and you don't, he is probably going to be a bit ticked off (I know that I would be) which is obviously not desirable. I generally agree with txcncman's comment, but would add that if he is insisting on boring those holes there is an important piece of information that is missing that can be fixed with some communication. He is either 1. Not up to speed with the tolerances that new, modern, cnc equipment can hold. 2. Not spec'ing out the holes correctly. A quick phone call should go a long way to resolve either issue.
A properly set up boring bar should be able to produce a better surface finish than a milled part because it removes the material as a continuous chip. I would expect that both options should be able to easily meet the surface finish requirements. The key word is properly set up- a chattering boring bar will obviously produce a crappy surface finish.
Regardless of the needs of this project, it's absolutely worth the time to re-familiarize yourself with a boring head one evening- there are many projects that necessitate the use them. Why not take a block of aluminum and make a few holes using various strategies so you can see the differences between them. You'd get up to speed with a boring head, if you wanted you could show/teach the customer, and everyone wins.

-Matt

[dertsap]

if this is for dowel pins then hole roundness will be best produced with the use of a boring head , also positional tolerance will be important , so it is generally best to approach each hole from the same direction each time , which means approaching the hole diagonally in x and y , this way any backlash issue will be minimized , the best of mills can vary ever so slight , even if they are fitted with temp control or what have you , a machine that sits can easily loose a few tenth positionally . Theres no such thing as the perfect cnc

[Khalid]

Theres no such thing as the perfect cnc

There is no perfect boring bar..nothing is perfect in this world.. You always need REAMER for getting required tolerances/finish for dowel pins.. But it also depends are those dowels used on Rocket or in a low cost machine..

[dertsap]

reamers have issues of their own , the possibility of wander being one .
I agree that nothing is perfect, but on the many parts that I've had to machine over the years that had to have near perfect pin holes and locations , then it was accomplished consistently with quality boring heads , along with the method I mentioned previously

[txcncman]

reamers have issues of their own , the possibility of wander being one .
I agree that nothing is perfect, but on the many parts that I've had to machine over the years that had to have near perfect pin holes and locations , then it was accomplished consistently with quality boring heads , along with the method I mentioned previously

How do your reams wander? Mine follow the drilled hole.

Personally, I would refuse the job if the customer demanded I use a certain machining technique. Or, I would increase the price proportionally with the additional time/labor/tooling/frustration required.

[Khalid]

I always allow 0.2mm material left to be machined through Reamer to avoid wander/wildness of Reamer..

[dertsap]

How do your reams wander? Mine follow the drilled hole.

.

drills wander , reamers follow
some machining practices are hand downs which have been used for years and are still practiced because they are proven to work .
boring technology isn't a thing of the past and some of the boring heads that are being manufactured are the best that have ever been , and in a few years they will be even better .
I'm not by any means saying that reamers are not a good tool to use but there is a time and place for them and in my opinion this isn't one of those times .
I do not agree with " the magic of cnc " statement in this case , and I disagree with interpolating the holes out and hoping that they would be good enough as well
take it for what it's worth or not , I'm just trying to be helpful and pass along some worth while knowledge



.




.

[Khalid]

drills wander , reamers follow
some machining practices are hand downs which have been used for years and are still practiced because they are proven to work .
boring technology isn't a thing of the past and some of the boring heads that are being manufactured are the best that have ever been , and in a few years they will be even better .
I'm not by any means saying that reamers are not a good tool to use but there is a time and place for them and in my opinion this isn't one of those times .
I do not agree with " the magic of cnc " statement in this case , and I disagree with interpolating the holes out and hoping that they would be good enough as well
take it for what it's worth or not , I'm just trying to be helpful and pass along some worth while knowledge

.

Using right End Mill (Minum acceptable runout etc) with right machine (rigid, accurate, zero-backlash etc) with right cutting parameters (feed, speed, DOC, Coolant etc) and with right CNC Programmer/Operator , I challenge the interpolated hole with End Mill shall be straight down within tolerances and comparable to boring bar...Once the interpolated Hole machined keeping some stock (~0.2mm left), use reamer... You will get acceptable results..
Drills are not accurate, so hole with drill too..no use of reamer for taper holes ...
I am still at the stance that CNC is MAGIC...

[forrey45]

A few company's back was producing parts for a customer that had tight tolerances of position, size and roundness and we could never get the holes that were interpolated (Matsura VMC) past the customers inspection for roundness and had to go over to using boring bars, no problems after that.
Forrey.

[txcncman]

drills wander , reamers follow
some machining practices are hand downs which have been used for years and are still practiced because they are proven to work .
boring technology isn't a thing of the past and some of the boring heads that are being manufactured are the best that have ever been , and in a few years they will be even better .
I'm not by any means saying that reamers are not a good tool to use but there is a time and place for them and in my opinion this isn't one of those times .
I do not agree with " the magic of cnc " statement in this case , and I disagree with interpolating the holes out and hoping that they would be good enough as well
take it for what it's worth or not , I'm just trying to be helpful and pass along some worth while knowledge

.

.

Do you know what a head plate for a diesel is even for or how important the tolerances really are? If it is what I remember a head plate to be, it is a plate that is bolted into place on the cylinder block to hold the cylinder sleeves in place and to mimic the stresses of having a head bolted into place while boring the cylinders. I am willing to bet if the plate is 1/16" off location or size, it would still work. The call out for the 0.6325" dimension is so the holes will have a slip fit/running fit over 0.625" dowel pins.

[RICHARD ZASTROW]

Could be a closer fit to a 16mm pin. A jig borer reamer doesn't follow a reasonably drilled hole.

Dick Z

[Boots]

I can't beleave these holes are for a .625 or 5/8 dowell pin. That's just plain dumb. Interpolated holes are only as good as the machine they are cut on. In all the 4 quadrants there will be a line where the axes change direction and backlash occurs and shows up on the finish and the hole will be out of round. A bore Bar may be a better tool here to get position and finish. Rapid to whith-in 1/8 in. on the x and y and feed into position for hole location before boring. Use the proper G-Code for a Bore Bar canned cycle so it stops and moves off center before retracting so as not to hit the finish with the insert. CNC's are Magic but you have to know how to perform the trick.

[txcncman]

I can't beleave these holes are for a .625 or 5/8 dowell pin. That's just plain dumb. Interpolated holes are only as good as the machine they are cut on. In all the 4 quadrants there will be a line where the axes change direction and backlash occurs and shows up on the finish and the hole will be out of round. A bore Bar may be a better tool here to get position and finish. Rapid to whith-in 1/8 in. on the x and y and feed into position for hole location before boring. Use the proper G-Code for a Bore Bar canned cycle so it stops and moves off center before retracting so as not to hit the finish with the insert. CNC's are Magic but you have to know how to perform the trick.

What size hole would you call out for a slip fit/running fit on a 5/8" diameter dowel pin?

How much out of round will it be?

[bvfd09]

I guess I'm reviving an old thread, but hey, this is a fun argument anyway.

Does anyone know of and have a link to a proper (preferably recent) study comparing the finished holes in terms of roundness, taper, and anything else I'm missing for holes produced by the methods mentioned above, boring, interpolating, and reaming?

[dertsap]

too many variables to create a study based on those items mentioned . Experience and common sense usually prevails . The method I posted previously is proven to be the best method time and time again for tight hole and positional tolerances , the denial of that kind of method is only masks the desire take shortcuts which is an overly common thing in this day and age . All mentioned methods work and all methods have their time and place , a guy has to decide at the time which is the best option for the job

[CarbideBob]

Interpolation will always make a lobed or not round hole as compared to a rotating tool like a boring bar.
T'is the nature of the beast. As stated many variables so each machine tool is different.
But this application does not need micron or sub micron roundness.

Thinking perhaps the user has had a bad experience somewhere so wants it done this way and you want to make him/her happy.
Cylinders, which dowel pin holes are have other features to worry about. Get that you are making cylinders, not holes.
Surface finish is way down the list.

Standard reamers do in fact flex and follow the wavy path a drill has left and made to do such.
They only cut on the tip as the side area is circle ground with a back taper (IE: it can only rub not cut, they are not endmills)
This back taper keeps them from binding as they follow the wave.
Ball sizing does the same.
Bob