Machining 316, never done it before

Djstorm100 said:

Most of what I do is in non-ferrous materials. I have a customer down the road that needs me to put 3" holes in 1" thick 316SS.

I haven not machine 316, so I start playing around with CAM to get a idea of how long it will take. I have 234 of these to do.

Cutters I'm looking at are a rougher and then finisher.

Rougher
Helical Tool 5 flute
-or-
Helical Tool 7 flute

then a 5 or 7 flute finisher.


If I was to run 7 flute rougher. Helical's data for the 7 flute are as follows: 265 SFM, up to %20 ADOC, 0.0036 Chip load @ 75-98 HRB


265 SFM (2025rpm) on a 1/2" cutter @ 0.100 WOC, chip load at 0.0038 (W/ chip thinning,actual chip is 0.003).

This equals out to be 52.88 ipm and yield 5 minute cycle time. This is to be done on a new Haas vf2ss 12k spindle.

Is this too aggressive in 316 with a Haas? Possible damage going around this much (repeated movements), plan is to do 3 parts at a time.

Plan would be to helical down and HSM strategy seen below.

Again, I never cut the stuff and looking for advice on the matter. Thanks in advance.

Click to expand...

litlerob1 said:

Helix down isn't a great idea IMO. Drills are the most capable tools in the crib, in context of MRR. Drill-drop Endmill in hole and Helix out (not down).

As Delw said G13-12 is pretty much the best thing Gene ever offered. Super easy canned cycle. But if you need to, you can add a K value to the G13 to helix down AND out, but that's gay. No offense intended.

R

Click to expand...

G12 Circular Pocket Milling CW / G13 Circular Pocket Milling CCW (Group 00)

These G-codes mill circular shapes. They are different only in that G12 uses a clockwise direction and G13 uses a counterclockwise direction. Both G-codes use the default XY circular plane (G17) and imply the use of G42 (cutter compensation) for G12 and G41 for G13. G12 and G13 are non-modal.
* D - Tool radius or diameter selection**
F - Feedrate
I - Radius of first circle (or finish if no K). I value must be greater than Tool Radius, but less than K value.
* K - Radius of finished circle (if specified)
* L - Loop count for repeating deeper cuts
* Q - Radius increment, or stepover (must be used with K)
Z - Depth of cut or increment

*indicates optional

**To get the programmed circle diameter, the control uses the selected D code tool size. To program tool centerline select D0.

NOTE Specify D00 if you do not want to use cutter compensation. If you do not specify a D value in the G12 / G13 block, the control uses the last commanded D value, even if it was previously canceled with a G40 .

Rapid-position the tool to the center of the circle. To remove all the material inside the circle, use I and Q values less than the tool diameter and a K value equal to the circle radius. To cut a circle radius only, use an I value set to the radius and no K or Q value.
%
O60121(SAMPLE G12 AND G13) ;
(G54 X0 Y0 is center of first pocket) ;
(Z0 is on top of the part) ;
(T1 is a .25 in. dia endmill) ;
(BEGIN PREPARATION BLOCKS) ;
T1 M06 (Select tool 1) ;
G00 G90 G40 G49 G54 (Safe startup) ;
G00 G54 X0 Y0 (Rapid to 1st position) ;
S1000 M03 (Spindle on CW) ;
G43 H01 Z0.1 (Tool offset 1 on) ;
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G12 I0.75 F10. Z-1.2 D01 (Finish pocket CW) ;
G00 Z0.1 (Retract) ;
X5.(Move to center of next pocket) ;
G12 I0.3 K1.5 Q1. F10. Z-1.2 D01 ;
(Rough & finish CW) ;
G00 Z0.1 (Retract) ;
X10.(Move to center of next pocket) ;
G13 I1.5 F10. Z-1.2 D01 (Finish CCW) ;
G00 Z0.1 (Retract) ;
X15. (Move to center of the last pocket) ;
G13 I0.3 K1.5 Q0.3 F10. Z-1.2 D01 ;
(Rough & finish CCW) ;
(BEGIN COMPLETION BLOCKS) ;
G00 Z0.1 M09 (Rapid retract, Coolant off) ;
G53 G49 Z0 M05 (Z home, Spindle off) ;
G53 Y0 (Y home) ;
M30 (End program) ;
%
Circular Pocket Milling, G12 Clockwise shown: [1] I only, [2] I, K and Q only.


These G codes assume cutter compensation, so you do not need to program G41 or G42 in the program block. However, you must include a D offset number, for cutter radius or diameter, to adjust the circle diameter.

These program examples show the G12 and G13 format, and the different ways that you can write these programs.

Single Pass: Use I only.

Applications: One-pass counter boring; rough and finish pocketing of smaller holes, ID cutting of O-ring grooves.

Multiple Pass: Use I, K, and Q.

Applications: Multiple-pass counter boring; rough and finish pocketing of large holes with cutter overlap.

Multiple Z-Depth Pass: Using I only, or I, K, and Q (G91 and L may also be used).

Applications: Deep rough and finish pocketing.

The previous figures show the tool path during the pocket milling G-codes.

Example G13 multiple-pass using I, K, Q, L, and G91:

This program uses G91 and an L count of 4, so this cycle will execute a total of four times. The Z depth increment is 0.500. This is multiplied by the L count, making the total depth of this hole 2.000.

The G91 and L count can also be used in a G13I only line.
%
O60131 (G13 G91 CCW EXAMPLE) ;
(G54 X0 Y0 is center of 1st pocket) ;
(Z0 is on top of the part) ;
(T1 is a 0.5 in. dia endmill) ;
(BEGIN PREPARATION BLOCKS) ;
T1 M06 (Select tool 1) ;
G00 G90 G40 G49 G54 (Safe startup) ;
G00 G54 X0 Y0 (Rapid to 1st position) ;
S1000 M03 (Spindle on CW) ;
G43 H01 Z0.1 (Activate tool offset 1) ;
M08 (Coolant on) ;
(BEGIN CUTTING BLOCKS) ;
G13 G91 Z-.5 I.400 K2.0 Q.400 L4 D01 F20. ;
(Rough & finish CCW) ;
(BEGIN COMPLETION BLOCKS) ;
G00 G90 Z0.1 M09 (Rapid retract, coolant off) ;
G53 G49 Z0 M05 (Z home, spindle off) ;
G53 Y0 (Y home) ;
M30 (End program) ;
%

Click to expand...

ChipSplitter said:

Do you have the High Speed Machining option?

If ya don't it's not gonna work to use an HSM strategy.

A Haas will top out at about 100 ipm without it.

Click to expand...

Rick Finsta said:

Thing is the SFM will be low enough with stainless that you'd need to get down to like 5% radial before you're hitting 100ipm+ in feed rate.

Click to expand...

litlerob1 said:

Good lord children. HSM techniques aren't really the answer here anyway. I know HSM is the new black, but it's a hole.

R

Click to expand...

litlerob1 said:

Good lord children. HSM techniques aren't really the answer here anyway. I know HSM is the new black, but it's a hole.

R

Click to expand...

ChipSplitter said:

Sure, it's not for soft material like 10xx steels, but it CAN be a lifesaver....... ask me how I know.

Click to expand...

litlerob1 said:

Uhhhhm--No.

Click to expand...

dodgin said:

I agree with the others...put a hole in it first.

Those 7 flute Helical EMs you linked to are awesome. We're machining 17-4 and 13-8 PH with them right now and they are making quick work of it. Your numbers are pretty close, but I'm thinking you could squeeze 300 SFM out of it and maybe a bit more out of the feed then, also.

Click to expand...

Djstorm100 said:

Looking at drills now with thru spindle coolant and peck it. If I'm using a 1/2" end mill, use a 13mm drill to give added diameter clearance?

Click to expand...

ChipSplitter said:

Ever try running a 1/2" EM 1.625" doc at full slot in 4140 PH ?

Didn't think so.

Click to expand...