Bad Chatter Finish and need help....

[twocik]

Now I know this part looks like a chewed up POS and I normally clamp my material down to the table, but thought I'd try a vise. It was definitely a chatter problem and not sure if it's my tooling length, feed rate, RPM's, etc.. I'm using the machining calculators for the correct RPMs, IPM, etc..





Aluminum 6061 at 0.770" thick. The last cut ends at 0.76", leaving .06" material to push the part out after MOPs are down. All CW conventional milling, no climb.




MOP 7 (roughing)

- 1/4" 2FL End Mill ( cutting length of 0.75" )
- Cut Feed Rate 10.3 IPM
- Spindle Speed 2567 rpm
- DOC 0.090"
- Roughing Clearance 0.01"
- Target depth -0.720"
- Max Crossover distance 0.7
- Coolant on



MOP 8 (finishing)

- 1/4" 3FL End Mill (with a cutting length of 1.75")
- Cut Feed Rate 8 IPM
- Spindle Speed 2567 rpm
- DOC 0.76"
- Roughing Clearance 0
- Target depth -0.760"
- Max Crossover distance 0.7
- Coolant on



The DOC was -0.760 all the way down (cleaning up the roughing clearance of 0.01"). Started with a spindle speed of 2567 RPM's, then tried 2000 RPM's, 1500 RPM's (No go Lots of noise and was using flood coolant). Not sure if I should fix my DOC, crank up the feed rate, or go all the way thru with mop 7 (roughing mop) re-editing my Cam file to make mop 7 straight thru with no roughing clearance....




Has anyone here had any success with using a vise making a part similar to mine and ending with a nice finish ?




Gcode File

( T2 : 0.125 )
( T3 : 0.375 )
( T4 : 0.125 )
( T5 : 0.366 )
( T6 : 0.125 )
( T7 : 0.25 )
( T8 : 0.25 )
G20 G90 G91.1 G64 G40
G49
( T2 : 0.125 )
M09
G28
T2 M6
G43 H2
( Drill1 )
G17
M3 S5140
M08
G0 Z0.2
G0 X-0.99 Y0.3173
G83 Z-0.26 Q-0.125 R0.2 F12.0
G83 X0.0 Z-0.26
G83 X0.99 Z-0.26
G80
( Drill2 )
( T3 : 0.375 )
M09
G28
T3 M6
G43 H3
M3 S3820
M08
G0 Z0.2
G0 X-0.99 Y0.3173
G81 Z-0.087 R0.2
G81 X0.0 Z-0.087
G81 X0.99 Z-0.087
G80
( Pocket 1 )
( T4 : 0.125 )
M09
G28
T4 M6
G43 H4
M3 S5140
M08
G0 Z0.25
G0 X-0.7275 Y0.5796
G1 F3.0 Z-0.041
G1 F20.5 Y0.6142
G1 X0.7275
G1 Y0.5796
G1 X-0.7275
G1 F3.0 Y0.5296
G1 F20.5 X-0.7775
G1 Y0.6642
G1 X0.7775
G1 Y0.5296
G1 X-0.7275
G1 F3.0 Y0.5796
G1 Z-0.082
G1 F20.5 Y0.6142
G1 X0.7275
G1 Y0.5796
G1 X-0.7275
G1 F3.0 Y0.5296
G1 F20.5 X-0.7775
G1 Y0.6642
G1 X0.7775
G1 Y0.5296
G1 X-0.7275
G1 F3.0 Y0.5796
G1 Z-0.123
G1 F20.5 Y0.6142
G1 X0.7275
G1 Y0.5796
G1 X-0.7275
G1 F3.0 Y0.5296
G1 F20.5 X-0.7775
G1 Y0.6642
G1 X0.7775
G1 Y0.5296
G1 X-0.7275
G1 F3.0 Y0.5796
G1 Z-0.164
G1 F20.5 Y0.6142
G1 X0.7275
G1 Y0.5796
G1 X-0.7275
G1 F3.0 Y0.5296
G1 F20.5 X-0.7775
G1 Y0.6642
G1 X0.7775
G1 Y0.5296
G1 X-0.7275
G1 F3.0 Y0.5796
G1 Z-0.167
G1 F20.5 Y0.6142
G1 X0.7275
G1 Y0.5796
G1 X-0.7275
G1 F3.0 Y0.5296
G1 F20.5 X-0.7775
G1 Y0.6642
G1 X0.7775
G1 Y0.5296
G1 X-0.7275
( Profile 1 )
S5140
M08
G0 Z0.2
G1 F2.0 X-0.7975 Y0.5096
G1 Z-0.169
G1 F6.0 Y0.6842
G1 X0.7975
G1 Y0.5096
G1 X-0.7975
( Profile 2 )
S5140
M08
G0 Z0.2
G0 X-0.6055 Y0.5904
G1 F3.0 Z-0.229
G1 F20.5 Y0.6034
G1 X0.6055
G1 Y0.5904
G1 X-0.6055
G1 F3.0 Z-0.289
G1 F20.5 Y0.6034
G1 X0.6055
G1 Y0.5904
G1 X-0.6055
G1 F3.0 Z-0.349
G1 F20.5 Y0.6034
G1 X0.6055
G1 Y0.5904
G1 X-0.6055
G1 F3.0 Z-0.409
G1 F20.5 Y0.6034
G1 X0.6055
G1 Y0.5904
G1 X-0.6055
G1 F3.0 Z-0.43
G1 F20.5 Y0.6034
G1 X0.6055
G1 Y0.5904
G1 X-0.6055
( Profile 3 )
S5140
M08
G0 Z0.2
G1 F3.0 X-0.6155 Y0.5804
G1 Z-0.44
G1 F8.0 Y0.6134
G1 X0.6155
G1 Y0.5804
G1 X-0.6155
( Pocket 2 )
( T5 : 0.366 )
M09
G28
T5 M6
G43 H5
M3 S1711
M08
G0 Z0.3
G0 X0.0742 Y-0.2984
G1 F3.0 Z-0.05
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
G0 Z0.3
G0 X0.0742
G1 F3.0 Z-0.1
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
G0 Z0.3
G0 X0.0742
G1 F3.0 Z-0.15
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
G0 Z0.3
G0 X0.0742
G1 F3.0 Z-0.2
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
G0 Z0.3
G0 X0.0742
G1 F3.0 Z-0.25
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
G0 Z0.3
G0 X0.0742
G1 F3.0 Z-0.29
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
G0 Z0.3
G0 X0.0742
G1 F3.0 Z-0.3
G1 F19.0 Y-0.3842
G1 X-0.0742
G1 Y-0.2984
G1 X0.0742
G1 F3.0 X0.2206
G1 F19.0 Y-0.5306
G1 X-0.2206
G1 Y-0.152
G1 X0.2206
G1 Y-0.2984
G1 F3.0 X0.367
G1 F19.0 Y-0.677
G1 X-0.367
G1 Y-0.0056
G1 X0.367
G1 Y-0.2984
( Pocket 3 )
( T6 : 0.125 )
M09
G28
T6 M6
G43 H6
M3 S5140
M08
G0 Z0.2
G0 X-0.0375 Y-0.5151
G1 F3.0 Z-0.335
G1 F20.0 Y-0.0401
G1 X0.0375
G1 Y-0.5151
G1 X-0.0375
G1 F3.0 X-0.0875
G1 F20.0 Y0.0099
G1 X0.0875
G1 Y-0.5651
G1 X-0.0875
G1 Y-0.5151
G1 F3.0 X-0.0375
G1 Z-0.37
G1 F20.0 Y-0.0401
G1 X0.0375
G1 Y-0.5151
G1 X-0.0375
G1 F3.0 X-0.0875
G1 F20.0 Y0.0099
G1 X0.0875
G1 Y-0.5651
G1 X-0.0875
G1 Y-0.5151
( Profile 4 )
S5140
M08
G0 Z0.2
G1 F3.0 X-0.0062 Y-0.5201
G1 Z-0.43
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
G1 F3.0 Z-0.49
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
G1 F3.0 Z-0.55
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
G1 F3.0 Z-0.61
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
G1 F3.0 Z-0.67
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
G1 F3.0 Z-0.73
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
G1 F3.0 Z-0.75
G1 F20.5 Y-0.0351
G1 X0.0062
G1 Y-0.5201
G1 X-0.0062
( Profile 5 )
S5140
M08
G0 Z0.2
G1 F2.0 X-0.0162 Y-0.5301
G1 Z-0.76
G1 F8.0 Y-0.0251
G1 X0.0162
G1 Y-0.5301
G1 X-0.0162
( Profile 6 )
( T7 : 0.25 )
M09
G28
T7 M6
G43 H7
M3 S2567
M08
G0 Z0.3
G0 X-0.5287 Y0.0424
G1 F4.0 Z-0.09
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.18
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.27
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.36
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.45
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.54
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.63
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
G1 F4.0 Z-0.72
G1 F10.3 Y-0.8276
G3 X-0.3937 Y-0.9626 I0.135 J0.0
G1 X0.3937
G3 X0.5287 Y-0.8276 I0.0 J0.135
G1 Y0.0424
G1 X1.15
G3 X1.285 Y0.1774 I0.0 J0.135
G1 Y0.8276
G3 X1.15 Y0.9626 I-0.135 J0.0
G1 X-1.15
G3 X-1.285 Y0.8276 I0.0 J-0.135
G1 Y0.1774
G3 X-1.15 Y0.0424 I0.135 J0.0
G1 X-0.5287
( Profile 7 )
( T8 : 0.25 )
M09
G28
T8 M6
G43 H8
M3 S2567
M08
G0 Z0.1
G1 F2.0 X-0.5187 Y0.0524
G1 Z-0.76
G1 F8.0 Y-0.8276
G3 X-0.3937 Y-0.9526 I0.125 J0.0
G1 X0.3937
G3 X0.5187 Y-0.8276 I0.0 J0.125
G1 Y0.0524
G1 X1.15
G3 X1.275 Y0.1774 I0.0 J0.125
G1 Y0.8276
G3 X1.15 Y0.9526 I-0.125 J0.0
G1 X-1.15
G3 X-1.275 Y0.8276 I0.0 J-0.125
G1 Y0.1774
G3 X-1.15 Y0.0524 I0.125 J0.0
G1 X-0.5187
G0 Z0.1
M09
M5
G28
M30

[holbieone]

I'd use a carbide end mill with a shorter flute length 1", put as much of the tool shank in the holder as you can

on your machine i'd run the tool at 3800 rpm at 40 ipm


looks like your slotting , i see chip marks in your cuts

try using two passes per depth one off the wall and the next on the wall so your not slotting

if your machine has no backlash i would climb mill on the wall surface

you need to adjust your coolant nozzle so it removes the chips and your not re cutting them

[twocik]

"I'd use a carbide end mill with a shorter flute length 1", put as much of the tool shank in the holder as you can
"

Not a 100% sure, but I think that finishing tool in the picture is carbide... I could be wrong, it's been awhile...



Yes this is the shortest I have at the moment, and have order more. Thought I might be able to finish out this project before Wed. Problem with the .75" 1/4 EM is after .75" it has some weird bevel tapered shank, leaves my top edge really bad looking.



B]
"on your machine i'd run the tool at 3800 rpm at 40 ipm"
[/B]

For my finishing cut ?






"try using two passes per depth one off the wall and the next on the wall so your not slotting"


Like a step over ?




"if your machine has no backlash i would climb mill on the wall surface"

You know I haven't really taken this thing apart yet to see, only because I haven't had any big problems yet.



"you need to adjust your coolant nozzle so it removes the chips and your not re cutting them"


Yes looking to definitely order more hoses. 5/8 is the correct size right ?


.

[flick]

Since you've got a piece of scrap to play with now, you might as well convert the rest of it into chips. Play with all 4 variables. Start out slow, then turn things up. There are so many different reasonable combinations that the only way to get a good feel for it is to do it.

[BobWarfield]

Lots going on here that could improve your results.

- Use a shorter tool as mentioned. It should both be shorter overall and have a shorter fluted length. The portion of the tool with flutes is not as rigid as the shaft.

- Definitely use carbide for a more rigid tool.

- Also, for this periphery cut, use the largest diameter tool that will fit your radii. Assuming you were, and 1/4" is the radius, if you are doing both a roughing and a finish pass, consider a 1/2" rougher and a 1/4" finisher. I often use a 5/8" indexable endmill for roughing, or a "corncob" rougher if the job is 4 flute friendly.

- The way the part is clamped in the vise it's easy on a job like this for the vise to pinch the cut. The one piece of stock that is thin will bend easily and either pinch or hold less securely. To use a vise for this job, you're better off setting the part really high, with just a little bit held in the jaws, say 0.1". Use stock that is at least that much too thick. Machine your part only down to the 0.1" step. Flip it, and use soft jaws shaped like the finished part to hold it while you face mill the 0.1" step off.

- Alternatively, if you insist on holding it in the jaws like that, machine it with tabs to hold the part. Keep the cut such that plenty of meat remains to hold the jaws open so the part won't pinch. When done, use an abrasive cut off to cut the tabs. Belt sand the nibs off to clean it up.

- If the holes I see are through holes, you may do the job with a fixture held in the vise and the through holes to keep the part held down while you machine the periphery.

- This is a periphery cut, but it was executed like a pocket. It'll take longer, but if your roughing clears away all the workpiece, there will be a lot of chip clearance available for the finishing pass. You could even use a 4 flute, which is the equivalent of twice the rpm, to get a finer finish. Can't use a 4 flute while you're down in a slot. However, you could use a 3 flute which might give you a better finish.

- Gotta make sure the chips are really blasted clear and not being recut.

- Climb milling will yield a nicer finish.

- Keep an endmill that is only used for finishing and do a tool change to it for the finish pass.

The noise you heard was probably the chatter. Try these various steps to increase rigidity. If that all fails, then try some radically different speed regimes.

Cheers,

BW

[dertsap]

if all else fails then take a stone and run it lightly over the cutting edge , many times the tool being sharp will become a disadvantage , especially on a long series end mill

[twocik]

Yes 1/4" would be the biggest size at the moment, but if this doesn't work I'm rethinking it..


As for the tips I've written all of them down and will figure this out tomorrow. It's driving me nuts. I've cut 4 parts out and only 1 had an ok finish. I've come to conclusion that my last tool (mop 8) was to long and the left side of the raw material after MOP 7 was gone and caused it to pinch. I also see little gashes on my part & stock and think this was from the tool bouncing being to long. I don't think it was the chips being recut, I move the hose for every corner to prevent this. Not saying maybe a few here and there might have, but I would have heard the smashing/grinding noise.

Speaking of which, how do they measure the loc line (from the OD or ID of a knuckle or the bubble ) ?



Few questions...


Now that I own a mill that can actually climb cut I hope, I'm not sure about feed rates, rpms, FPT... Is it the same as conventional milling or should I use a slower feed rate, rpms, etc.. ?


Last, for climb milling finishing cuts, recommend feed rate and rpms ?


Should I for Mop 8 (last mop) use one pass to clean up a roughing clearance of .01" or 2, 3, 4 passes or lessen my roughing clearance to 0.009" ?

[BobWarfield]

Climb milling uses the same speeds and feeds as conventional milling.

For finishing, you may want to slow the feed down while keeping spindle rpms constant and as high as recommended for your tool and cutting situation. You should also reduce width of cut, though you may not want to reduce depth of cut so you cut the whole thickness in one pass for appearance sake. I like to use 5% of cutter diameter for finishing width of cut.

When slowing the feed it is important to keep in mind that you don't want to slow so much that the tool starts rubbing. This is a function of the chip thickness winding up less than the radius of the cutting edge (that would be the "knife" edge of the flute). If the chip's radius is less you can visualize that you suddenly have a very negative (rather than positive) cutting geometry that wants to push the chip back down into the workpiece.

This leads to burnishing, which heats the tool and can drastically reduce tool life, although sometimes it can also lead to a nice finish! I have even seen a recommendation from time to time to make a pass with just a few thou cutting depth and the cutter running in reverse, which guarantees burnishing and a very dull endmill.

How in practice do you know how much feed is too little? That starts to be hard, particularly when you consider that the very light depths of cut also involve chip thinning. What I will typically do is use my G-Wizard calculator to determine what the actual chip thickness is (chipload or IPT) even under chip thinning conditions. I then manual adjust feed in the calculator for a chip that is between 0.0005 and 0.001" thick.

Cheers,

BW

[dertsap]

Climb milling uses the same speeds and feeds as conventional milling.

For finishing, you may want to slow the feed down while keeping spindle rpms constant and as high as recommended for your tool and cutting situation. Y

BW

I generally do the opposite when it comes to a long series end mills , I take the finish cut with a heavier feed with a slowed down speed which keeps the harmonics down

[BobWarfield]

I generally do the opposite when it comes to a long series end mills , I take the finish cut with a heavier feed with a slowed down speed which keeps the harmonics down

A heavier cut can help chatter harmonics, however, it is clear for this job a long series endmill is not the tool of choice.

BW

[thackman]

Just my .02 cents but from the shape of the part you might as well be cutting a tuning fork. The right size of the stock is a rigid setup but everything from the center to the left is unsupported. Your only option may be to leave more stock on the left and back edges and bandsaw it off later.

[keithorr]

nevermind