Tool Feed rates/RPM way too aggressive?

[Rich05]

Here is an example of the feeds and speeds X2 is generating.

With
1/4 carbide drill, stock material, flood

3200 rpm, and 12 inch per minute plunge.

this seems way out of whack.

It should be more like 400 rpm and 1 ich per minute correct?

There is no place to put horsepower in the machine definition also.

What is going on here thanks.

R.

[Geof]

What material are you drilling?

That speed and feed would be okay for a HSS drill in 6061.

[Rich05]

mild steel forgot to put that in sorry.

1018 i think

[Geof]

A carbide drill should be okay at that speed and feed in 1018; certainly 400rpm and 1ipm is much too slow.

[JIMMY]

I would run my carbide thru spindle drill at 1800 rpm. I run my feed rate at about 8 ipm. If you are only using flood and not thru spindle you should probably back of on what I said. I hope I helped you.

[cnc-king]

Originally Posted by Rich05 Here is an example of the feeds and speeds X2 is generating. With 1/4 carbide drill, stock material, flood 3200 rpm, and 12 inch per minute plunge. this seems way out of whack. It should be more like 400 rpm and 1 ich per minute correct? There is no place to put horsepower in the machine definition also. What is going on here thanks. R.

you are babying that carbide drill in 1018 steel, you will end up with premature wear. that is the speed i use for regular high speed drills. you should be able to double your chip load due to the chips not breaking very easily in that particular type of material

[Rich05]

thanks for advise why would MC recomend 3200? my max spindle speed.

[Mike Stevenson]

I say run those feeds and speeds. They look good to me at a .083 peck increment.

[tobyaxis]

Carbide drills generally do not cut but tear material. 3200RPM at 15 IPM because you have to figure at least a .003 radius on the lips.

Carbide over HSS a 30% increase in spindle speed and feed is acceptable.

1018 is Gummy so with a 1/4 in diameter drill I usually use the rule of one peck equals 1 times the diameter. If your depth is equal to or less than .75 deep (.25*3) drive straight through without pecking. For deeper holes reduce your peck by about 25% per 1 inch in depth.

Drill your first 10 holes and check the Margin for plastic deformation. If you have any plastic deformation reduce your RPM in 10% increments or as needed.

Chips should be a little long in 1018 steel so make sure you protect yourself and surrounding equipment with a guard.

Cheers and Happy cutting

[Geof]

Originally Posted by tobyaxis .....Drill your first 10 holes and check the Margin for plastic deformation. If you have any plastic deformation reduce your RPM in 10% increments or as needed.....

This puzzles me.

By plastic deformation do you mean a rim around the hole?

If the answer is 'Yes' my comment is why reduce the speed; I would have expected increase.

[Mike Stevenson]

I don't understand the term "plastic deformation" applied to steel cutting with a drill either. Not sure if I buy that carbide tears the material idea too.

[tobyaxis]

Originally Posted by Geof This puzzles me. By plastic deformation do you mean a rim around the hole? If the answer is 'Yes' my comment is why reduce the speed; I would have expected increase.

Plastic Deformation is a tirm used for Carbide Tool Wear. It kind of looks like the Margin on the ends of the Lands were melted. This is caused from too high of an RPM and not enough Feed Rate. Also the reason why most destroy carbide drills in steels.

There is a large section in the Machinery's Handbook about Plastic Deformation which at the moment I am unable to locate go figure.

A good friend Tim Jones (aka tjones here on the zone) is a Carbide Tool Maker. He specializes in 5 Axis grinding of Common and High Performance Tools. Very talented guy informed me of the proper use of carbide drills feeds/speeds ect.

The drill below is his creation Modeled in Alibre Design.

http://www.indtools.net