Circle Mill Finish Feedrate

[Mr. Wizzard]

Tool feedrate = 60. I have finish feedrate @ 30. No posty post, it stays 60.

Has anyone figured a workaround for this?

[Mr. Wizzard]

I used this. I have 3 circle mill ops. It posted for the 1st op, not the other 2. I regened all ops, thinking it would fix it. Now it won't post the finish feedrate for any of the ops.

[Guest CNC Apps Guy 1]

It's been posting fine for me and I have numerous circle mill ops in the last part I worked on.I use MPMaster. WHat post you using?

 

To boot, I have a plunge feed, a feed, a semi feed and finish feed. All make it to the code last I checked.

[Guest]

Well, I just tested this on a 1" circle.

 

If I do NOT use a lead in/lead out move, the finish values update, however, that is no code I would ever run at a machine, the G40 isn't cancelling the G41 properly

 

O0000(T)
(DATE=DD-MM-YY - 15-10-11 TIME=HH:MM - 10:03)
(MCX FILE - T)
(NC FILE - C:\USERS\JOHN\DOCUMENTS\MY MCAMX5\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T239 |  1/2 FLAT ENDMILL | H239 | D239 | WEAR COMP | TOOL DIA. - .5 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T239 M6
N106 G0 G90 G54 X0. Y.19 S5000 M3
N108 G43 H239 Z2.
N110 Z.05
N112 G1 Z-.3 F15.
N114 G3 Y-.19 I0. J-.19 F60.
N116 G41 D239 Y.19 I0. J.19
N118 G1 Y.24
N120 G3 Y-.24 I0. J-.24
N122 Y.24 I0. J.24
N124 S4500 M3
N126 G1 Y.25 F30.
N128 G3 Y-.25 I0. J-.25
N130 Y.25 I0. J.25
N132 G0 Z.25
N134 Z2.
N136 G40 M5
N138 G91 G28 Z0.
N140 G28 X0. Y0.
N142 M30
%

 

 

 

However, when I click Transition and click lead in/lead out, I get no value changes at all. I get better code but no speed and feed update from the finish values

 

O0000(T)
(DATE=DD-MM-YY - 15-10-11 TIME=HH:MM - 10:12)
(MCX FILE - C:\USERS\JOHN\DOCUMENTS\MY MCAMX5\MCX\NO CHANGES.MCX-5)
(NC FILE - C:\USERS\JOHN\DOCUMENTS\MY MCAMX5\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T239 |  1/2 FLAT ENDMILL | H239 | D239 | WEAR COMP | TOOL DIA. - .5 )
N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T239 M6
N106 G0 G90 G54 X0. Y.095 S5000 M3
N108 G43 H239 Z2.
N110 Z.05
N112 G1 Z-.3 F15.
N114 G41 D239 X.0246 Y.1868 F60.
N116 G3 X0. Y.19 I-.0246 J-.0918
N118 Y-.19 I0. J-.19
N120 Y.19 I0. J.19
N122 X-.0246 Y.1868 I0. J-.095
N124 G1 G40 X0. Y.095
N126 Y.12
N128 G41 D239 X.0311 Y.2359
N130 G3 X0. Y.24 I-.0311 J-.1159
N132 Y-.24 I0. J-.24
N134 Y.24 I0. J.24
N136 X-.0311 Y.2359 I0. J-.12
N138 G1 G40 X0. Y.12
N140 Y.125
N142 G41 D239 X.0324 Y.2457
N144 G3 X0. Y.25 I-.0324 J-.1207
N146 Y-.25 I0. J-.25
N148 Y.25 I0. J.25
N150 X-.0324 Y.2457 I0. J-.125
N152 G1 G40 X0. Y.125
N154 G0 Z.25
N156 Z2.
N158 M5
N160 G91 G28 Z0.
N162 G28 X0. Y0.
N164 M30
%

 

I tried using start at center and all the combinations including perpendicular entry

 

This is an X5 Generic 3 axis mill post

 

I will also note, I just tested this in X6 and it DOES work properly

[gcode]

This is X5 MU1

 

It looks OK to me

 

 

 

%

O0000(T)

(DATE=DD-MM-YY - 15-10-11 TIME=HH:MM - 09:22)

(MCX FILE - C:\JUNK\CIRCLE MILL.MCX-5)

(MATERIAL - ALUMINUM INCH - 2024)

( T239 | 1/2 FLAT ENDMILL | H239 | D239 | WEAR COMP | TOOL DIA. - .5 )

G20

G0 G17 G40 G49 G80 G90

T239 M6

G0 G90 G54 X0. Y0. A0. S1069 M3

G43 H239 Z.5

Z.1

G1 Z-.25 F15.

G3 X-.0264 Y-.051 I.0361 J-.051 F25.

X.0361 Y-.1135 I.0625 J0.

X.0722 Y-.102 I0. J.0625

X.1514 Y.051 I-.1083 J.153

X0. Y.235 I-.1875 J0.

X-.235 Y0. I0. J-.235

X0. Y-.235 I.235 J0.

X.235 Y0. I0. J.235

X0. Y.235 I-.235 J0.

X-.1175 Y.1175 I0. J-.1175

S3800 M3 <-----------------------SPINDLE

G1 X0. Y0. F40. <--------------- FEEDRATE

G41 D239 X.125 Y.125 <-----------COMP ON

G3 X0. Y.25 I-.125 J0.

X-.25 Y0. I0. J-.25

X0. Y-.25 I.25 J0.

X.25 Y0. I0. J.25

X0. Y.25 I-.25 J0.

X-.125 Y.125 I0. J-.125

G1 G40 X0. Y0. <----------------COMP OFF

G0 Z.5

M5

G91 G28 Z0.

G28 X0. Y0. A0.

M30

%

CIRCLE MILL.MCX-5

[NOTW Programmer]

Here's my X5 output.

%
O0000(T)
(DATE=DD-MM-YY - 15-10-11 TIME=HH:MM - 11:17)
(MCX FILE - T)
(NC FILE - C:\USERS\WILLIAMJ\DOCUMENTS\MY MCAMX5\MILL\NC\T.NC)
(MATERIAL - ALUMINUM INCH - 2024)
( T239 |  1/2 FLAT ENDMILL | H239 | D239 | WEAR COMP | TOOL DIA. - .5 )
G20
G0 G17 G40 G49 G80 G90
T239 M6
G0 G90 G54 X0. Y0. A0. S1069 M3
G43 H239 Z.25
Z.1
G1 Z0. F6.42
G3 X-.0625 Y-.0625 I0. J-.0625 F60.
X0. Y-.125 I.0625 J0.
X.1875 Y.0625 I0. J.1875
X0. Y.25 I-.1875 J0.
X-.3125 Y-.0625 I0. J-.3125
X0. Y-.375 I.3125 J0.
X.4375 Y.0625 I0. J.4375
X0. Y.5 I-.4375 J0.
X-.5 Y0. I0. J-.5
X0. Y-.5 I.5 J0.
X.5 Y0. I0. J.5
X0. Y.5 I-.5 J0.
G1 Y0. F30.
G41 D239 Y.5
G3 X-.5 Y0. I0. J-.5
X0. Y-.5 I.5 J0.
X.5 Y0. I0. J.5
X0. Y.5 I-.5 J0.
G1 G40 Y0.
G0 Z.25
M5
G91 G28 Z0.
G28 X0. Y0. A0.
M30
%

[Mr. Wizzard]

I'm using MPMaster mill post for 3-axis output (Haas TM-1). Lead in/out 90 degree sweep, start at center, computer cutter comp, not control.

 

Don't get it. Something is F'd up. I just created a new circle mill op, same settings as the others. First time, I backplotted and the finish feedrate drops to 30 like it should. Post it and it comes out fine.

 

Then, regen the toolpath. Now it's broken. Won't change to 30 in backplot or posted code. What the crap is going on?

[gcode]

Do you have the feedrate lock on in System Config?

If so, try turning it off. You may have found a bug.

[Mr. Wizzard]

Good try, but no dice. It's unchecked. I downloaded your sample and it worked fine for me. I changed to computer comp (how mine is set) and it still worked. Regen a few times and it still worked. Mine won't for some reason. I even swapped my Machine Def for yours, regen, still works fine on your file.

[Mr. Wizzard]

Wait, it gets better. It appears i only have one shot per session. I've done this 3 times in a row with the exact same results.

 

If i open Mastercam, same file, and try a Circle Mill toolpath, it will work ONCE. The finish feed rate will backplot and post. If i regen it or create a 2nd Circle Mill toolpath, it fails. If i close Mastercam and then fire it back up, i will get the same result. One shot toolpath, then it breaks. It just happened three times in a row. This would explain why it worked on my first toolpath.

 

I don't get it. Why does it work just once?

[gcode]

Are you selecting points and defining the diameter?

I always use Enitity an pick the arc, letting the size of the arc define the toolpath.

Maybe that is the difference?

[Mr. Wizzard]

I was using points, just tried by selecting an arc and still no worky work....

[Mr. Wizzard]

Ok, some more weirdness. If i have semi-finish and finish only, no worky work. If I add roughing, it works. Thing is, I don't want roughing since i already have a pilot hole and don't need to cut from the center out. I know how much stock needs removed and just figured how many semi-finishing passes I need and how many finishing passes I want.

 

For you guys that had it work, did you have roughing selected as well, or just semi-finish and finish like i did? Could you do me a favor and try without roughing selected and see if you get the same result? Backplot and post, then regen, add another op with same settings and see if it works? Maybe it's just me, but it won't work properly without roughing selected.

[Mr. Wizzard]

G, maybe i'm thinking wrong here, but let me know. I tried yours again and deselected the roughing passes. I left the finish pass, which was .015. On a 1.00 circle, wouldn't you get a cut @ .970, then a finish pass of .015 to finish size? It only makes one pass @ 1.00 with the original tool feedrate, not the feedrate set in the finish pass.

 

Am i having a bad Monday, or just a moron?

[gcode]

If you have Finish pass set to 1 that's what it does.. 1 pass at the feedrate defined on the tools parametr page,

If you have roughing or multiple semifinish passes defined they run at tool feedrate and the last pass at defined finish feedrate.

[Mr. Wizzard]

Ok, so simply adding a finish pass of .xxx @ Fxxx will produce nothing, UNLESS you have roughing or semi-finish selected as well. Seems to me i had the same brain fart on a simple contour path a while ago. I think it's because, whether you have roughing or not, I think you should just be able to get a finish pass, by selecting a finish pass. Sometimes i forget that's not the way it works.

 

BUT, it still won't work correctly with semi-finish passes and finish passes. It will work with roughing. If it's not designed to work that way, why will it work the first time, but not after regen?

 

I guess i'll just have to use roughing passes to get it to work.