View Full Version : Issues with Fusion360

04-23-2018, 06:59 PM
trying to run some gcode thru a DeskTop pro.
Using Fusion360, and shopbot open post processor.
The tool is acting very oddly.
Using an adaptive 2D function for a deep pocket that should take about
8 minutes to run according to Fusion, but took 15 minutes not even get thru half of the pocket depth.
Alot of times after making a cutting path, the tool just sits and hovers above the last cut, moves back and forth without cutting any material. Some of the moves are not uniform feed speed either.
Any help would be appreciated.

Marc F. Lupien
04-23-2018, 08:30 PM
I recently observed some hole making toolpaths where the bit also spent too long to execute causing some plastic to melt around my bit. I did not diagnozed it properly. Afterward, I found some ramp values a bit odd but I had to reset all the shopbot value to default ones for some other reason and since that, I did not had any other problems though I did not make that many projects with Fusion.

Is it possible that there are some overlapping lines that define your pocket contour ? I am curious what your 8 minutes pocket looks like ;-)

04-23-2018, 08:54 PM
Might be helpful to see both the Fusion and the SBP file that it posted.

04-24-2018, 07:16 PM
here's a zip file of the sbp for the relief cut on the back of the strat.
thanks for looking at it...

04-24-2018, 11:52 PM
There's a spiral down 'ramp' into the cut at the start of each level and that may be what you see as hovering. Along with that, there are two different feed rates being applied. The feed rate that is set for those spiral ramps is very slow at 0.2187 in/sec (about 13 in/min), and then the rest is at 2.5 in/sec (150 in/min). So, each time it goes down one more level, it moves very slow during the spiral down ramp. I don't use Fusion360 and have only played with it a bit, but you should be able to choose a different ramp in strategy (like zigzag or smooth) and you should also be able to set the feed rate for that the same as your main toolpath feed rate or at least some faster. It would appear that Fusion360 has two feed rate settings, one for ramping into the material and then the main feed rate. Find where that is being set and change it.

You could also just edit the code for each of those slow MS, 0.2187, 0.2187 speeds to be something else or remove them all together and set the first one at your intended feed rate (you have MS, 2.5, 2.5). Due to the small size of those spiral ramps, the machine will likely just run them at ramp speed.

04-25-2018, 07:44 AM
Thank you Scott!!
I did notice that the ramping looked funny but wasn't sure if there wasn't something else not quite right as well.
Gotta get better at looking at the code.
I'll go thru the ramping parameters(there's a whole tab in Fusion per operation), and try to get more familiar with it.
thanks again