[mrk]

Hello,

I am still a newbie and trying to understand some of the basics.

Main question:
How do I determine speed/feed for reamers? (i am looking for the math formulas)

Environment:

• Using HSS tools (value from J&L)
• 6061-T651 (1.500" thick stock)

Background:
My goal is to produce some really precise holes for use with .5" machine dowels. The holes will be through holes and used to locate a part as I flip it over. The stock for the part is 1.500" thick and needs to be machined from all four sides. The dowels will help me as I flip over the part.

The idea that I have is that I will clamp the stock in my KURT vise. The stock is large enough that the part where the through holes for the dowels will hang off the left and right of the vise. I will have two holes spaced 8" apart and the vise is 6" so the stock can be held in the vise with no risk of drilling into the vise.

I figure the first step would be to (G83) drill using a drill that will leave a bit of stock in the hole. I am still not sure what the optimal drill size, speed or the best peck would be. I am going to do some experiments but in the past I had good results drilling a 27/64" hole at 180 SFPM and .002 chip load with .5" pecks. These 27/64" holes were for tapping and they worked well enough but I figure for setting up index dowel I want to be 100% correct with my math.

I have a copy of Machnery's Handbook 26. On pg1029 to 1043 the book discusses drilling and reaming speeds. A chart on pg1039 includes a recommended SFPM of 350-400 for 6061 but this seems way fast based on a conversation I once had with a professional machinist. He recommended 1500 rpm for a 27/64" drill but using a SFPM of 350 would result in 3169 rpm for the drill so his gut feeling number was 50% less then the calculation I make from the book. Also, the book lists feed as f=(0.001 in/rev.) and I have not yet learned how to convert to this to IPM (inch per minute). Also, speed for drilling and reaming seem to based on the same SFPM values in the book. Frankly, the entire book is way over my head. Is it possible I am reading the chart wrong?

Question:
In terms of drilling 6061 T651, is 180 SFPM and .002 chip load good or should these numbers be tweaked? Also, once I decide on SFPM and chip load should I adjust these numbers for different drill sizes and for different hole depths. For peripheral milling, I have been using 260 SFPM on the machine with good results. What would the math formulas look like?

Question:
How would I adjust the math for reaming holes?

[bluechips]

for the ipr to ipm formula
ipm=ipr*rpm
.001 inches per rev * 3169 rpm = 3.169 ipm
(now, to further complicate things, if chip load per TOOTH is important, then a 6 flute can be fed faster than a 4 flute, just like end mills)
The old fashioned method for reaming speeds, as I recall from high school, was 1/2 the drilling rpm, with the same feed (per rev). This rule of thumb should be ignored for high volume production work (make the reamer salesman do the math). But if you are doing a short run, where you can get away with babying your tooling, then I would suggest halving the sfpm (translates into halving the rpm that you would use for a same sized drill) and using the same inches per REV that you would for the same sized drill. This translates into 50% of the ipM you would use on the same sized drill (since the rpm is 50% of the same sized drill, and the ipr is the same).
well, I hope at least the ipm formula helps.

[Geof]

To answer your last question first, using gut informatio (the print in Machinery's Handbook is too small for my olde eyes): Ream at about one quarter the speed you drill at or even less. Feed the reamer maybe ten times as fast as the drill in inch per rev, using plenty of coolant or lubricant, go in and out without any pause between, only take off between 0.005" and 0.015" on the diameter and NEVER, NEVER, NEVER run a reamer in reverse or I will come and haunt your dreams.

Regarding your drilling the numbers you have are okay. 1500rpm is a bit conservative but going above 3000 is starting to push it. For thin material the higher speed is okay but chip build up tends to occur more at higher speeds when drilling deep holes. I know some people might suggest using carbide drills and going like a maniac. That's okay so long as they are not using my drills on my machines. With sophisticated things like through the tool coolant you can go really fast.

Your feed and peck are both okay. To calculate feed it is simply: feed per tooth x number of teeth x rpm. 0.002 per tooth x 2 tooths x 2000 rpm = 8ipm

Adjust things for different drill sizes but maybe back off on the feed for very small and increase it for large and as I mention faster for shallow holes slower for deep may be wise.

Regarding your milling on aluminum with high speed tools you could go faster than 260 fpm such as up to 800 fpm with plenty of coolant. With carbide you could go up to a few thousand but using small tools this works out to astronomical rpm so you never get there.

The approach that is implicit in your comments and questions is the correct one; ask questions, read references and feel your way forward gaining experience.

Almost forgot. When you plan on doing a precise located reamed hole always spot drill before drilling. Drills often wander and this is much more likely if you just plunge straight in; a spot drill self centers and leaves an accurately placed dimple to center the drill. Reamers always follow the drilled hole so if the drill has wandered the reamer will wander. To be most precise you should spot, drill, bore then ream.

[jackson]

her is a copy of a pockett chatr for speeds and feeds conv.....

[mrk]

Okay, I think I am starting to understand but still I am not sure about my math.

I am sure that there are some great calculators for this stuff on the web (although I am actually still looking so recommendations are always welcome). For now I am using an excel spread sheet that I am building as I learn stuff. It could be that someday "gut" feelings will take over but for now since my gut is stupid I like doing the calculations.


My current thoughts for drilling and reaming the .500" dowel holes are as follows:

1) Spot drill
(can I use a .75" 3 flute counter sink for this and make a .1" deep hole?)
G00 Z0.25
S1737 M03
G81 G99 X0.9272 Y0.9944 Z0.25 I-.1000 F4.34

2) Peck drill with a 31/64" drill
G00 Z0.25
S1794 M03
G83 G99 X0.9272 Y0.9944 Z0.25 I-1.0000 B.5 F4.49

3) Ream with the .499" reamer
G00 Z0.25
S1794 M03
G85 G99 X0.9272 Y0.9944 Z0.25 I-1.0000 B.5 F4.49

I hope to try this out this weekend with plenty of coolant.

[Willbird]

OK, your speeds and feeds will be differant for aluminum that what I ran most of my career in cnc tool and die. But here goes. First a little willbird-theory, IMHO most simple jobs take longer to setup and program than they do to run, so the surface feet per minute does not NEED to be topped out to get a lot of work done, getting it too HIGH spoils a part and sometimes the tool. SO to me it makes sense to be conservative :-).

To reach our goal of getting the machine tool machining...lets use this formula SFM * 4 / dia of cutter = RPM. Now that is not EXACT, the answer ends up a bit...conservative..:-)...BUT you can do it in your head. I used 150 sfm for carbide tooling and 50 for high speed tooling...if I ended up watching the machine for long WHILE it was running I dug out machineries handbook and jacked the sfm up to what the book says...what the book says has never failed to work for me.

so for a 1" carbide endmill we go 150 * 4 /1 = 600 rpm...for a finish cutter I ran .01" per rev to start...so that is 6" per minute, if you want more double it to 12 or run 9 :-)...easy and quick.

now for making holes on location...I would use a SPOT drill (not a center drill) and use a dwell...I would use positive approach if the machine has it.....I would then drill 1/32 under ream size, then "bore" the hole with a regrind .500 carbide endmill...if you are going super deep like 1" or more relieve the od so it does not rub.....then to ream I always started at .01" per rev feed, and ran 25sfm for the rpm. if the hole is a touch small drop the feed by 25%...if it is a bit big increase it by 25% to 50%....about half the reamers that do not cut to the size they measure will respond to the feedrate change..if they do NOT, run the reamer in REVERSE at the rpm your reaming with, and LIGHTLY stone the OD and very very lightly sort of run the stone around the cutting chamfer, sort of a radius movement but with the lightest touch you can muster...it idea here is sometimes the reamer has a bit of a chip welded on it or some such that is making it cut big.

Also if your putting your remaer in a tool holder take just a minute and indicate it to run true...

One other theory....short reamers suck IMHO...they will typically cut bigger...you can USE this to some extent sometimes and choke up on one to make it cut bigger....BUT a good reamer repeats, one that cuts larger than it's measured size is really a loose cannon :-)....if you do everything perfect and have a nice reamer it will actually cut a few .0001 SMALLER than it measures.

You can adjust the SFM to suit your machine, material and situation......the speeds/feeds I mnetioned will work with most any steel, ad, d2, 4140 pre heat treat, m4, 8620 etc.

[jackson]

I added the speed and feed chart to my previuse post not sure why it got taken of im sure i did someting, but anyway my mentor when i first started gave me these SFM as just kind of a stander i dont use it much but its something to start

FOR STEEL

LIGHT = 80 - 175

MEDIUM = 80 - 120

HARD = 50 - 80

TOOL = 30 - 50

BRASS = 100 - 300

ALUM. = 100 - 600

[mrk]

Making a hole sure is complex but I feel like I am learning a lot in this thread. Big thanks to everyone. For me the CNC is hobby stuff so production speed is not very important. I want to reach high levels of quality to make fairly precise parts and have repeatable processes even though everything I do will be short runs. I must admit that I still think I only understand just a small part of these threads because prior to this past few months I had no experiance with CNC or machining so a lot of this stuff is greek to me. You guys have been a big help so super thanks.

Having the precise dowel positions in the fixture should really help for making the parts I want. My first part needs to be machined from four sides so I need fixtures with index pins to flip.

I guess it is time to buy a spot drill (I never owned one before so it will be a new tool for my growing shop). A quick search of J&L resulted and I find they have spot drills (I figure that for now I might stick with HSS to keep cost under control especially since I am in the learning and tool breaking stage). For the .500" dowel hole what size spot drill should I use? I wonder, since the spot drill only makes a dimple could I simply use a big one all the time and not go down very far so I only leave a dimple that will be as big as I need but no bigger.
http://tinyurl.com/3yu9do

Working with 6061 would the following work?

Would 3/8" spot drill, S1986 and F4.9 work? (or is it better to go faster and use less feed to make sure the drill starts well?)

After the spot drill, would the normal drill run well as 31/64" with S1537 and F3.8?

I don't have any reground end mills and to be honest I still am such a newbie that I don't understand the boring step. Would it be possible to skip this step and simple run the reamer after the normal drill.

For the reamer would a .499" be good at S373 and F11?

-Mark

[mrk]

ALUM. = 100 - 600

For aluminum the range is so large 100 SFM to 600 SFM is a fairly large range. What do you think about for picking a value in the range?

[jackson]

for the 3/8 drill rpm S4,000 F9. that is figur you sfm 330-390

[jackson]

sorry i looked at the wrong alloy i fogot you said 6061 sfm 210-260
you should use at least a 5/8 spot so S1600 F.013(mill F7.)
31/64 drill S2,100 F.012 ( mill F8.5)

[jackson]

on your drill how deep are you drilling

[Hursty]

Here are some of my ideas for drill & ream.

[Geof]

......I wonder, since the spot drill only makes a dimple could I simply use a big one all the time and not go down very far so I only leave a dimple that will be as big as I need but no bigger........

Going over 3/8" for the spot drill is not needed. Your dimple does not need to be the same size as the drill and if you have a large spot drill the center web leaves a flat spot at the bottom of the dimple which will allow a small drill to start to wander again.

[jackson]

Going over 3/8" for the spot drill is not needed. Your dimple does not need to be the same size as the drill and if you have a large spot drill the center web leaves a flat spot at the bottom of the dimple which will allow a small drill to start to wander again.

unless you want to use the spot drill to chamfer the hole as well,

[jackson]

what does that little green box mean "on a distinguished road"

[mrk]

Thanks everyone!!!!!!

I REAMED my very first hole and it was great. No slop, perfect fit, and a big smile on my face. It's like I am 19 all over again []

Thanks so much for all the advise along the way.

[Paul_S]

Generally I use indexing for drill feeds. Generally for steel .015 x the drill dia. for IPR. For aluminum .020 x dia. Using this method I have successfuly drilled using various size drills from about an 1 inch dia down to .028 dia.. For tool steel like H13 I needed to use a smaller index of .013-.011 do to the fact that at break thru the drills would break using .015 index. If the holes were blind, the .015 index works ok.

[mrk]

Forgive my stupidity but what does the term "indexing" mean?

Generally I use indexing for drill feeds.

If I understand your formula for drilling a 5/16" in Aluminum at 250 SFPM the calculation would work out as 3056 RPM and 19 IPM. Do I understand the formula correctly? I have not tried such quick drilling. Do you think this would work with HSS drill bits on 6061?

How does someone go about picking a SFPM value for 6061-T651? Is SFPM constant for the relationship of tool and aluminum materials? (i.e. once I pick a SFPM value for 6061 and HSS is it always used or do I adjust SFPM based on operation)?

[jackson]

Generally I use indexing for drill feeds. Generally for steel .015 x the drill dia. for IPR. For aluminum .020 x dia. Using this method I have successfuly drilled using various size drills from about an 1 inch dia down to .028 dia.. For tool steel like H13 I needed to use a smaller index of .013-.011 do to the fact that at break thru the drills would break using .015 index. If the holes were blind, the .015 index works ok.

This may work for you but im in this buisness to make money and using your calculations that is to slow atleast for me, guess it would also depend on the drill you were using