High Feed Option

[Thoob]

Does anyone use this mode? Reason I ask is I have come across something that I think might either be a bug or perhaps its supposed to be this way but if you try to use this mode with wear compensation, it seems to ignore it. Basically I am trying to finish around a block and I am using high speed machining but on the corner I need it to slow down slightly, hence why I want to use Mastercam's high feed option. However when I select it with wear compensation, it tells me the program time will be reduced to 0min 0 secs. What its doing is using the parameters feed entered but doesn't adjust on the corners. Does anyone else know about this?

[Machineguy]

What machne are you running?

 

Machineguy

[Colin Gilchrist]

If you only want to adjust the feed at the corners, you should look into "adjust feed on arc move" instead of the High Feed option.

[Thoob]

Would the adjust feed on arc, just change feed suddenly? The high feed option adjusts before for acceleration and deceleration. If I don't use that, the machine shakes too much. Why should I not use the high feed option? Machine I'm running is a Mazak VTC 250D Milling Center.

[Colin Gilchrist]

Yes, Adjust feed on arc move would cause a sudden change in feedrate, so that wouldn't work for what you are after.

 

I'm guessing some other parameter you've got set is not correct. I just tried a Contour toolpath, using Wear compensation, and Highfeed seemed to work just fine. Here is the code it output below. For reference, I set this path at 200 ipm for feed, 100 ipm for plunge, and 300 ipm for retract.

 

%
O0000(T)
(DATE=DD-MM-YY - 08-08-13 TIME=HH:MM - 16:53)
(MCX FILE - T)
(NC FILE - C:\USERS\CMG\DOCUMENTS\MY MCAMX7\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 X-3.25 Y-.5 A0. S1069 M3
N108 G43 H239 Z5.25
N110 Z5.2
N112 G1 Z5. F100.
N114 G41 D239 X-3.0833 F5.
N116 X-2.9167 F25.
N118 X-2.75 F45.
N120 G3 X-2.5587 Y-.4619 I0. J.5 F65.
N122 X-2.3964 Y-.3536 I-.1913 J.4619 F83.36
N124 X-2.25 Y0. I-.3536 J.3536
N126 G1 Y.2222 F103.36
N128 Y.4444 F123.36
N130 Y.6667 F143.36
N132 Y.8889 F163.36
N134 Y1.1111 F158.94
N136 Y1.3333 F138.94
N138 Y1.5556 F118.94
N140 Y1.7778 F98.94
N142 Y2. F78.94
N144 G2 X-2. Y2.25 I.25 J0. F58.94
N146 G1 X-1.7647 F78.94
N148 X-1.5294 F98.94
N150 X-1.2941 F118.94
N152 X-1.0588 F138.94
N154 X-.8235 F158.94
N156 X-.5882 F178.94
N158 X-.3529 F198.94
N160 X.5882
N162 X.8235 F178.94
N164 X1.0588 F158.94
N166 X1.2941 F138.94
N168 X1.5294 F118.94
N170 X1.7647 F98.94
N172 X2. F78.94
N174 G2 X2.25 Y2. I0. J-.25 F58.94
N176 G1 Y1.7647 F78.94
N178 Y1.5294 F98.94
N180 Y1.2941 F118.94
N182 Y1.0588 F138.94
N184 Y.8235 F158.94
N186 Y.5882 F178.94
N188 Y.3529 F198.94
N190 Y-.5882
N192 Y-.8235 F178.94
N194 Y-1.0588 F158.94
N196 Y-1.2941 F138.94
N198 Y-1.5294 F118.94
N200 Y-1.7647 F98.94
N202 Y-2. F78.94
N204 G2 X2. Y-2.25 I-.25 J0. F58.94
N206 G1 X1.7647 F78.94
N208 X1.5294 F98.94
N210 X1.2941 F118.94
N212 X1.0588 F138.94
N214 X.8235 F158.94
N216 X.5882 F178.94
N218 X.3529 F198.94
N220 X-.5882
N222 X-.8235 F178.94
N224 X-1.0588 F158.94
N226 X-1.2941 F138.94
N228 X-1.5294 F118.94
N230 X-1.7647 F98.94
N232 X-2. F78.94
N234 G2 X-2.25 Y-2. I0. J.25 F58.94
N236 G1 Y-1.7778 F78.94
N238 Y-1.5556 F98.94
N240 Y-1.3333 F118.94
N242 Y-1.1111 F138.94
N244 Y-.8889 F158.94
N246 Y-.4444 F143.36
N248 Y-.2222 F123.36
N250 Y0. F103.36
N252 G3 X-2.75 Y.5 I-.5 J0. F83.36
N254 G1 X-2.9167 F103.36
N256 X-3.0833 F123.36
N258 G40 X-3.25 F143.36
N260 Z5.2 F5.
N262 G0 Z5.25
N264 M5
N266 G91 G28 Z0.
N268 G28 X0. Y0. A0.
N270 M30
%

[happycat64]

Does anyone use this mode? Reason I ask is I have come across something that I think might either be a bug or perhaps its supposed to be this way but if you try to use this mode with wear compensation, it seems to ignore it. Basically I am trying to finish around a block and I am using high speed machining but on the corner I need it to slow down slightly, hence why I want to use Mastercam's high feed option. However when I select it with wear compensation, it tells me the program time will be reduced to 0min 0 secs. What its doing is using the parameters feed entered but doesn't adjust on the corners. Does anyone else know about this?

im having the same problem but i get a message at the bottom left coner stating -----"cutter compensation in control: left, feed rate not adjusted"

[Thoob]

That's weird. I have no issues using it with wear comp off (usually the case) but for some reason it doesn't with it on. I mean there is no error, its just that the confirmation dialogue box says new time will be 0 min 0 secs. Then of course there are no feeds outputted in the post, only the main feed I entered in originally. I may have to call support for this. Thanks for the verification Colin.

[Machineguy]

I just did a countor ramp path, turned on the High Feed button, adjuster the parameters. It locked the toolpath and posted fine. Looks like Colins' posted file above with feedrates on every line, and slowing down in the corners.

The program ran fine. I did not use wear comp.

Normally I dont need to use this feature in the Hass VM-3. I just turn on the G187 P3 in MIsc OPs. It will slow down in the corners with it set as P3. This is the Fine cutting mode in a Hass. P2 is for normal cutting. P1 is wide open, used for roughing at high speeds. I have no issues with the way Hass does thios.

The program above ran at 125 IPM and dropped down to 59 IPM. Part was small so I didnt need to go faster.

 

Machineguy

[Thoob]

I just did a countor ramp path, turned on the High Feed button, adjuster the parameters. It locked the toolpath and posted fine. Looks like Colins' posted file above with feedrates on every line, and slowing down in the corners.

The program ran fine. I did not use wear comp.

Normally I dont need to use this feature in the Hass VM-3. I just turn on the G187 P3 in MIsc OPs. It will slow down in the corners with it set as P3. This is the Fine cutting mode in a Hass. P2 is for normal cutting. P1 is wide open, used for roughing at high speeds. I have no issues with the way Hass does thios.

The program above ran at 125 IPM and dropped down to 59 IPM. Part was small so I didnt need to go faster.

 

Machineguy

 

Ya I don't have a problem with it when comp is off. Actually it seems to be when I am using the ramp option with it. Ramp on its own with no comp is fine, as soon as I try to ramp with comp on, it doesn't work. See pictures. First one is the dialogue box showing the time difference. The other ones are the program outputs. Its the 3rd one with ramp and comp that is wrong.

 

 

 

[Jayson Kramer]

So I am figuring you want something like this:

 

O0000(TEST)

(DATE=DD-MM-YY - 09-08-13 TIME=HH:MM - 08:58)

(MCX FILE - T)

(NC FILE - C:\USERS\JKRAMER\DOCUMENTS\MY MCAMX7\MILL\NC\TEST.NC)

(MATERIAL - ALUMINUM INCH - 2024)

( T1 | 1/2 FLAT ENDMILL | H1 | D1 | WEAR COMP | TOOL DIA. - .5 )

N100 G20

N110 G0 G17 G40 G49 G80 G90

N120 T1 M6

N130 G0 G90 G54 X.1 Y-2.55 A0. S5000 M3

N140 G43 H1 Z2.

N150 Z.2

N160 G1 Z-.5 F15.

N170 G41 D1 Y-2.35 F20.

N180 G3 X0. Y-2.25 I-.1 J0. F5.

N190 G1 X-3. F20.

N200 G2 X-3.25 Y-2. I0. J.25 F5.

N210 G1 Y2. F20.

N220 G2 X-3. Y2.25 I.25 J0. F5.

N230 G1 X3. F20.

N240 G2 X3.25 Y2. I0. J-.25 F5.

N250 G1 Y-2. F20.

N260 G2 X3. Y-2.25 I-.25 J0. F5.

N270 G1 X0. F20.

N280 G3 X-.1 Y-2.35 I0. J-.1 F5.

N290 G1 G40 Y-2.55 F20.

N300 G0 Z2.

N310 M5

N320 G91 G28 Z0.

N330 G28 X0. Y0. A0.

N340 M30

%

 

This just a standard Contour with no high feed and using the following.

[Thoob]

So I am figuring you want something like this:

 

O0000(TEST)

(DATE=DD-MM-YY - 09-08-13 TIME=HH:MM - 08:58)

(MCX FILE - T)

(NC FILE - C:\USERS\JKRAMER\DOCUMENTS\MY MCAMX7\MILL\NC\TEST.NC)

(MATERIAL - ALUMINUM INCH - 2024)

( T1 | 1/2 FLAT ENDMILL | H1 | D1 | WEAR COMP | TOOL DIA. - .5 )

N100 G20

N110 G0 G17 G40 G49 G80 G90

N120 T1 M6

N130 G0 G90 G54 X.1 Y-2.55 A0. S5000 M3

N140 G43 H1 Z2.

N150 Z.2

N160 G1 Z-.5 F15.

N170 G41 D1 Y-2.35 F20.

N180 G3 X0. Y-2.25 I-.1 J0. F5.

N190 G1 X-3. F20.

N200 G2 X-3.25 Y-2. I0. J.25 F5.

N210 G1 Y2. F20.

N220 G2 X-3. Y2.25 I.25 J0. F5.

N230 G1 X3. F20.

N240 G2 X3.25 Y2. I0. J-.25 F5.

N250 G1 Y-2. F20.

N260 G2 X3. Y-2.25 I-.25 J0. F5.

N270 G1 X0. F20.

N280 G3 X-.1 Y-2.35 I0. J-.1 F5.

N290 G1 G40 Y-2.55 F20.

N300 G0 Z2.

N310 M5

N320 G91 G28 Z0.

N330 G28 X0. Y0. A0.

N340 M30

%

 

This just a standard Contour with no high feed and using the following.

 

No, read post 3,4, and 5

[Jayson Kramer]

Got it sorry.

[Matthew Hajicek - Singularity]

im having the same problem but i get a message at the bottom left coner stating -----"cutter compensation in control: left, feed rate not adjusted"

 

IIRC it's never worked with comp in the control. As I understand it, it's pretty much a safety, since with comp in the control the operator could substitute a different diameter cutter.