Hi,

I have read all about slow feedrate issues when cutting arcs. I have experienced this and can live with it until we have constant velocity contouring (ver 4?). I am also experiencing the oposite. Recently, when cutting some heavy aluminum plate, my machine was cutting happily at 3" a minute along a nice straight line. I came along to an arc, where the machine whipped around it at what seemed like the max start speed? which is much higher than the feed rate I specified. As you can imagine, this can be interesting to watch. No damage was done, but my poor home made machine was flexing nicely. The second time I tried it, I broke an endmill. After I was done, I tried a dry run and was ready with my feedrate overide when I came to the arc. No effect. Anyone else experience this?

Eric

Hi Balsaman,

I can't help you specifically, but machines will do some weird things if the controller gets confused with a command that is incorrect in syntax.

Take my Shadow controller for example: if I have anything on a line with a tool offset command, the machine immediately rapids all the way down to the Z- limit :eek: This is obviously a case of where the software people did not properly trap for incorrect syntax.

So I'd suggest that you take a look at your arc commands, make sure they are laid out exactly as "the book" says they should be, and that you are using correct arc center coordinate format. Do not include any other commands on the same line as the arc command, to try to isolate the issue.

Here is part of the gcode of the time I broke the bit. Top of stock is at .5" 3 passes to cut through. Plunges at 2" and cutting at 3". Circle is broken (by the POST Processor) into 4 quadrants. The feedrate of the G03 was ignored. The plunge feedrate of F2 is fine.

Eric

G00 Z1.5
G00 X6.9979 Y9.861
G00 Z.6
G01 Z.3 F2
G03 X5.5604 Y11.2985 R1.4375 F3.
G03 X4.1229 Y9.861 R1.4375
G03 X5.5604 Y8.4235 R1.4375
G03 X6.9979 Y9.861 R1.4375
G01 Z.1 F2.
G03 X5.5604 Y11.2985 R1.4375 F3.
G03 X4.1229 Y9.861 R1.4375
G03 X5.5604 Y8.4235 R1.4375
G03 X6.9979 Y9.861 R1.4375
G01 Z-.1 F2.
G03 X5.5604 Y11.2985 R1.4375 F3.
G03 X4.1229 Y9.861 R1.4375
G03 X5.5604 Y8.4235 R1.4375
G03 X6.9979 Y9.861 R1.4375
G00 Z1.5
G00 Z2
G00 X0. Y12.
M05 (Spindle off)
M18 (Drive off)
M02 (The End)

It probably won't help, but have you tried using the G03 command with I and J letters instead of the R? I'm only mentioning it coz in the instructions he doesn't mention the feedrate with the R example, only with the I and J. It may be possible that is not programmed in. Just a thought.

That is possible. I should try a gcode with the i and j. The post processor was downloaded from the Turbocnc conference for use with Mastercam tho. I don't know how to edit it to use i and j for arcs. I will manually make a short gcode with a slow feedrate using i and j and see what happens.

Eric

Eric,
My machine feed rates are set at inches per minute not Feet per minute if the feed rate specified has a period (like F3.0) . But , if a feed rate does not have a period (as F2 does not in your code) it will assume units are .001", so the feed rate is in mils/minute.
Now my machine would of run the your 4th line (F2) at 2mils/min which is basically stopped (unless your an anthropoligist) but this is not the case as your eye could see it move. But my machine would of moved the arc feed rate( F3.0) at
around 1000 times faster.
What I'm really getting at is your 4th line does not have a period in the F2 and this could be the source of your head ache.
Hope this helps
Tony

Balsaman,
One the main things tat I tell my trainees is NOT to ignore the decimal point. I don't know how much of the will ause your problem but I know that in some certain machines it could be a issue. Using I an J or R shouldn't make any difference at all. Usually, the machine slows down while going around the corners. I sometimes have to go and manually insert a feed rate for going around corners to maintain a even feed along the cut. Just for curiosity, what type of controller you have ? I have a feeling that there is a velocity setting that is not properly set.
Regards,
Sorin