Doing my first 3D carve and I have set my feed rate to 110% however I noticed in my detail carve it does not appear to be approaching that value. I left the plunge rate set at 9 in/min (default setting). I was wondering since the z axis has to be at a specified height to move to the next xy coordinate will increasing the plunge rate allow the xy feeds to increase in speed ?
Whenever the Z is also in movement the slower of the 2 (feed or plunge) will come into play for ALL movements. So Lets say you’re carving a dome shape, where the entire time the Z is constantly moving and you have a Feed setting of 150IPM and a Plunge of only 9IPM… well the 9IPM will be in play the ENTIRE carve, making the 150 setting essentially meaningless.
This occurs because the gcode line contains all positions to move to and at the end contains the speed at which to move and it reads both (when the gcode is first calculated) and grabs whichever is slower.
Soo IF your machine can operate at a faster Plunge rate, then setting it faster will make quite a difference. One common issue is that within the Grbl settings saved onto the CNC are MAX settings for Feed and Plunge, so setting any higher than these is once again, a pointless endeavor. Sooo for instance, on a Standard (non-Pro) X-carve the MAX Plunge within the cnc’s settings is 19.68ipm, So setting the Feed to 150 and the Plunge to 150 is kinda pointless because the machine will limit itself to only 19.68ipm UNLESS the user manually edits those grbl settings for the Max plunge rate. (at your own risk)
That was probably a lot of Info and hopefully you’re still tracking.
Optimally you are able to edit your machines Grbl settings to allow a much faster feed rate. maybe even 50ipm. And then the plunge can be set to that new higher plunge rate. And 50ipn plunge vs 9ipm plunge will actually cause the carve to complete in 1/5th the time.
I run my machine (not an X-Carve) at 300ipm Feed and 200ipm Plunge for the finishing toolpath of a 3d carve and it does so with ease.
But before you go changing settings you’d want to do some testing and ensure the Z axis does not lockup at higher speeds and once you find the point it locks up from moving too fast, reduce that by 10-15% to apply a safety factor and then use this new “Fast but safe” plunge setting as the Max Plunge in the Grbl settings.
The page to make these changes and read the current settings in Easel is called the Machine inspector and can be accessed by pressing Ctrl+Shift+D at once OR going to the top menu Machine>General Settings>Machine Inspector
Thanks Seth, I was pretty sure that was the way it worked. I am using a Yorahome 1Mx1M with a Makita 701C router. Just upgraded the router from the standard 24volt spindle so I am trying to learn what speeds and feeds I can work with now. Will experiment some and see what it does. Working in some black walnut now, and pretty sure I can at least double the plunge rate. Will look to see what Easel is using for it’s max. Thanks for the info.