Very slow cutting of involute teeth

[allistar]

Hi all,
  I'm cutting a simple 22 tooth spur gear (Module = 5, p angle = 20) using a 4mm flat head milling bit via EMC2. This is in 12mm MDF using 1mm deep passes each time. The hole in the middle and the spokes cut out as fast as can be expected. However, cutting the teeth themselve s is very slow. EMC2 says the gcode should take about 20 minutes to mill. The reality is that it took about 2 hours. It's the cutting of the teeth that is painfully slow - slow enough to burn the wood.

  It's milling this kind of output that is slow:

   G02  X38.4770 Y10.0276 I38.0098 J8.0829
   G01  X38.8059 Y9.9486
   G02  X38.8451 Y9.9387 I38.3387 J8.0039
   G01  X39.1862 Y9.8494
   G02  X39.2252 Y9.8388 I38.6798 J7.9146
   G01  X39.5784 Y9.7387
   G02  X39.6106 Y9.7293 I39.0330 J7.8145
   G01  X39.8526 Y9.6563

Is the a reason this is so slow, and is there anyway to speed this up? Is this a gcode output issue or is it an EMC issue?

Thanks,
Allistar.

[dfmiller]

Look through your code for the last F command. it stays that speed until it gets another one.
What is generatin g the G code. Are you using the 2.5D Gcode option?
If you are you set the feedrate in the right side of the output manager.

It would seem that that is slow.
Dave

[ArtF]

Hi:

  If its not feedrate, try increasei ng your point distance in the settings. The reason Point Distance exists is that some controlle rs go very slow when a
group of small moves is in the queue. Making your point distance larger can make all the motions larger increasin g speed on controlle rs that do that.
  For example if .001 is making it slow, set point distrance to .01 , it shoudl run much faster if the problem is the controlle rs ability to queue motions together.

Art

[allistar]

It's not the feed rate. I've discovere d that setting "G64 P.2" first makes all the differenc e. This sets the path control mode in EMC. It may result in a less accurate output, but .2mm is accurate enough for me! The speed of cutting the teeth is now nearly 3 times as fast. I alse set the point distance to .4 (mm) which greatly reduced the number of lines of GCode to run. I'll see how this all impacts the meshing of the teeth in the final gears.

Is there a way to include hand coded Gcode into the final output from the output manager? In my case I would always get it to output "G64 P.2" first. If not, it's a good idea for a potential enhanceme nt.

Thanks for the help,
Allistar.