Roughing stock left for finish

I'm curious since I have a lot of time in this profession, but not a lot of variety.

If you are roughing, then finish milling after. How much stock do you leave to clean up on both radial and floor?

For Aluminum?
Radial = A
Floor = B

For carbon Steel
Radial = C
Floor = D

And why that amount?

My answers for carbide end mills are

A= .02
B= .01

C= .01
D= .03

I like a little more floor on the steel so that it hopefully gets a little more heat in the cut and doesn't tear the floor.

A .003/.005
B .003
C .003/.005
D .003

Because of habit.

Maybe I should have a number, as I can't tell you the number of parts I've wrecked by not leaving quite enough to clean up. That also includes "saving" money by sawing raw stock a bit too close.

A .005/.01
B .005
C .01/.02
D .005/.01

If I use the same finishing tool for roughing and finishing for aluminum I sometimes leave 0 but apply a spring pass. Some other factors are the total depth of cut apply which may end up with multiple spring passes.

Houndogforever said:

I'm curious since I have a lot of time in this profession, but not a lot of variety.

If you are roughing, then finish milling after. How much stock do you leave to clean up on both radial and floor?

For Aluminum?
Radial = A
Floor = B

For carbon Steel
Radial = C
Floor = D

And why that amount?

My answers for carbide end mills are

A= .02
B= .01

C= .01
D= .03

I like a little more floor on the steel so that it hopefully gets a little more heat in the cut and doesn't tear the floor.

Click to expand...

.
.
depends on of course
.
1) cutter deflection
2) part deflection
3) machine tracking tool path accurately
4) accuracy of setting tool dia and length comp
.
i have seen plenty of deflection over the years from long tools and raw horsepower. i have seen old cnc with wear and backlash problems at higher feed rates over .010" error following tool path is common. many many times i have seen roughing marks not clean up cause not enough stock left.
.
a source of common tool error is carbide insert mills where inserts on end the pockets are damaged and inserts rotated a bit. i have often seen inserts on end at .005 or smaller diameter than next set of inserts down. so a combination factors can easily combine and cause problems. carbide end mills i have seen many long length end mills bend quite a bit from cutting forces. depends if you are pushing the limits under a cloud of coolant smoke

For me depends on the rough tool.
But typ. Is .01 wall .005 floor but
I run the wall first then floor with
The spring pass of wall.

A: .01
B: .005

I will usually leave .005 on the floor, .010 on walls for just about anything. If need be, I'll do a semi-finish pass on the wall, leaving .005 for a finish pass, if it's a deep wall (3x D or more).

Usually .01" and .01". Small tools I will go down to .005 and .005. I will do the floor first staying off the .005 or .01 and come back and finish the walls. If I'm surfacing something I'll typically leave .020 on the surface.

obviously depends on length to diameter ratio of tools and what cutting forces or horsepower is involved.
.
2 hp or 20 hp, obviously can push part with tons of force. obviously 2" diameter end mill sticking out a foot not going to run same as 2" dia shell mill only 2" long
.
i have seen many parts vibrate easily over .010", raw horsepower can make parts weighing tons vibrate severely quite easily and sound can easily be heard 100 feet away
.
obviously a 6" dia facemill taking 5.5" width passes at 0.2" depth at 50" per minute can vibrate a part very severely. facemill can easily handle 60" per minute as long as part not vibrating. i have often seen chatter marks not clean even taking .015" for finish pass. aluminum parts same facemill at over 100 ipm many a part vibrating too much and have to reduce cutting rate. part cannot take it