Hello Guest it is May 20, 2019, 05:09:17 PM

Author Topic: feedrate & units per min are different  (Read 6082 times)

0 Members and 1 Guest are viewing this topic.

feedrate & units per min are different
« on: October 22, 2008, 11:10:58 PM »
After a tool change, the speeds specified by the Gcode seem to be ignored and the speed in "motor tuning" is used. Before the tool change everything works as planned. I am using the latest legacy mach 3 and Gcode from RhinoCam. I have mach3 set to stop and wait upon tool change.

It happened specifically here:

X-0.4673 Y-0.1964
X-0.5287 Y-0.3053
Z0.1250  F15.0
(Deep Drill )
G00 Z0.0000
G00 X0.0000 Y0.0000
M6 T8
M03 S10000
X0.0000 Y0.0000 Z0.1141
G83 X0.0000 Y0.0000 Z-0.3 R0.1 Q0.05
G80
G01 Z0.1141  F4.0
(2 1/2 Axis Pocketing)
G00 Z0.0000
G00 X0.0000 Y0.0000
M6 T2
M03 S10000
X-0.1066 Y-0.1975 Z0.0312  F15.0
Z-0.0196  F1.0
X0.1066  F3.0
X0.1177 Y-0.1911
X0.2244 Y-0.0064
Y0.0064
X0.1177 Y0.1911
X0.1066 Y0.1975
X-0.1066
X-0.1178 Y0.1911
X-0.2244 Y0.0064
Y-0.0064
X-0.1177 Y-0.1911
X-0.1066 Y-0.1975
Z-0.0392
X0.1066
X0.1177 Y-0.1911
X0.2244 Y-0.0064
Y0.0064
X0.1177 Y0.1911
X0.1066 Y0.1975
X-0.1066

Instead of deep drilling at 4 ipm, it did it at my Z motor tune speed of 12.... Then instead of profiling at 3 IPM it went at 20. The FRO says the correct speed... but units/min says the motor tune speed...
Is there some setting in general config I may be missing?
« Last Edit: October 23, 2008, 12:23:54 AM by hoop »

Offline Hood

*
  •  25,811 25,811
  • Carnoustie, Scotland
    • View Profile
Re: feedrate & units per min are different
« Reply #1 on: October 23, 2008, 02:56:39 AM »
I am certainly no expert with G Code but from what I see above you are going straight from G0 moves into your feed moves but you have no G1's there so the G0 are still in effect.
Hood
Re: feedrate & units per min are different
« Reply #2 on: October 23, 2008, 11:19:02 AM »
You are also adding an F word to a G00 line which is invalid.


G00 X0.0000 Y0.0000  <<------- G00 mode starts here
M6 T2
M03 S10000
X-0.1066 Y-0.1975 Z0.0312  F15.0  <<<------ still in G00 mode, F word has no effect
Z-0.0196  F1.0
X0.1066  F3.0
X0.1177 Y-0.1911
X0.2244 Y-0.0064

So Mach is doing exactly what it is programmed to do.

Damn machines always run the actual code, not what you want it to be. :-)

Offline jimpinder

*
  •  1,233 1,233
  • Wakefield, West Yorks, UK
    • View Profile
Re: feedrate & units per min are different
« Reply #3 on: October 24, 2008, 07:23:47 AM »
This is the problem with what I call "short" programming.

When writing my code, I always put in the complete line e.g. G0 X0 Y0, not just the co-ordinates I want to move to. Similar when I want a cutting move, G1 F4 X3 Y3. It makes it a lot easier to check the code when something like this happens, because you don't have to trace back to see what the machine is actually doing..

Unfortunately if you use a CAM program, you are stuck with what it gives you.
Not me driving the engine - I'm better looking.