Drill+Reamer, feeds/speeds, and any tips

[Hursty]

Here are some of my ideas for drill & ream.

[Geof]

Originally Posted by mrk ......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]

Originally Posted by Geof 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]

Originally Posted by 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.

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

[Paul_S]

Originally Posted by 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)?

What I mean by indexing is a rate like .015 per dia of a tool. This method works with drills and end mills equally as well.

A 5/16 drill using 250 SFPM works out to 3061 RPM and using an .020 index value your feed would be, yes, 19 IPM. Using parabolic hi helix drill you may be able to use an index value of .04 and used a 38 IPM feed. As SFPM of 300 would then be 45.6 IPM! And assuming all the drill RPMs are within the range of your spindle and you only used those parabolic style drills. This feed rate of 45.6 IPM would be used regardless of drill size in aluminum.

The SFPM effects tool life. And SFPM should be picked based on material. If you are given a range for SFPM use the lower end for longer tool life and the upper end for better material removal rates.

Now if you find a certain feed rate works better for a given drill and material. Take that feed rate divided by the RPM and divided by drill dia to get your index value. Use that new better value for calculating your drill feeds from then on using that style drill and material.

So let's say your 5/16 drill 118 degree standard drill works best for you at 32 IPM. And you are using 3670 RPM. Your index value becomes 32/3670/.312 that is, .028 per dia.

So a 1/16 drill using a 10000 RPM spindle would be drilling at 17.5 IPM.

Typically the SFPM for drilling in aluminum alloy is between 250-300 SFPM. I personally use 275 for Alluminum alloys generally regardless of grade. Referencing 6061, 7075 and 2024. T6 or what that alloy typically comes as.

In milling aluminum I use 400 SFPM for HSS cutters and as fast a feed the machine, setup and tool will take. The recommended range for HSS end mills is really between 600-800 SFPM. If you use preseting and have the extra tool in holder preset on hand as part of the set up, use the highest SFPM that you can get a way with.

Carbide cutters in aluminum, run as fast as the spindle, tool and horse power, setup will allow. I use 1000 SFPM for my carbide end mills.