I’m clearly doing something stupid, which resulted in a gash in my workpiece. I’m new so this is all scrap. Also note my temporary work surface while I get some MDF.
I’ve attached a screenshot of the viewer window from the onefinity interface, and nothing else, as I hit my upload and link limit for new users.
You can see that the enter/exit paths (red) go horizontally in my attempt, and are much higher in the OneFinity example.
I’m using the F360 machine setup and post-processor from @blaghislain
Your not “missing” anything you just need to adjust your safety heights and starting heights in Fusion. You need to set the clearance height so the machine knows it has to lift the bit up above the wood (by whatever you specify) on each cut, Not only will what you have do this for this initial cut but with out that it will do that at the bottom of every plunge. There are a lot of video’s on YouTube showing how to set this in detail.
You can see the ramp line in the preview goes up to the right at an angle vs lifting the bit up up the clearance height then moving horizontally over to your first cut.
I’m familiar with clearance height, and the tool path retracts properly between pockets in my design. The only time it doesn’t do that is the move at the beginning and at the end. Screenshot provided.
I’ve inspected the generated GCode a little, and found some oddity. Comments at the end of the Gcode lines are mine.
(1001)
(MACHINE)
( VENDOR KIRBRE ENTERPRISES INC)
( MODEL JOURNEYMAN)
( DESCRIPTION ONEFINITY COMMUNITY EDITION V2022.02.21.1)
(T1 D=0.25 CR=0 - ZMIN=-0.125 - FLAT END MILL)
N10 G90 G94 G17 G91.1
N15 G20
(WHEN USING FUSION 360 FOR PERSONAL USE, THE FEEDRATE OF)
(RAPID MOVES IS REDUCED TO MATCH THE FEEDRATE OF CUTTING)
(MOVES, WHICH CAN INCREASE MACHINING TIME. UNRESTRICTED RAPID)
(MOVES ARE AVAILABLE WITH A FUSION 360 SUBSCRIPTION.)
(2D POCKET1)
(T1)
N20 S5 M3
N25 G54
N30 G0 X6.694 Y1.7885 // This moves to the XY point of the first pocket location.
N35 G43 Z0.5906 H1 // This moves vertically upward to the clearance height
N40 G1 Z0.1969 F39.37 // This moves downward again.
N45 Z0.0984 F13.12 // Move downward movement
N50 Z-0.125 // Move downward into stock
N55 X6.7008 Y1.7937 F39.37// First horizontal move as part of pocket operation
N60 X6.7079 Y1.7983
So, why does it move horizontally first, then up to the clearance operation before plunging down again? As this is not represented in F360, I’m wondering if it’s either an error in the post processor, or some setting the post processor is looking for that I’m not providing.
It would appear your clearance height is set incorrectly, the first move is a G0 rapid move which should be controlled by the clearance height value (I believe it’s is by default to retract height + .25" or there about)
In addition to the video Alex suggested here is one specific to the heights tab in Fusion 360
EDIT: I looked back at your first post and line 10 N20 G0 Z0 would tell the Z axis to move to the top before it moves anywhere in X and Y. This line is removed from the second script you posted.
More inspection of the Post Processor indicates that my machine setup may not be correct. I’ve been confused by the videos that exist on that topic, as they show features in the machine setup that I don’t have. (I am using the free version of F360, if that makes a difference here.)
Mine outputs the “G53 G0 Z0” line as the first “move” operation in the code which retracts the Z all the way up and out of the way for the first X/Y move. Your first post had it as line 10, the second one does not, that is what is causing the crash you’re experiencing. Why it’s missing I can’t explain.
Figured it out, chasing the G53 suggestions. I made sure to set G53 as the Safe Retracts option in the Post window, and it worked. The visualizer tools didn’t show anything different, but it behaved exactly the way I thought it should on the machine with this option selected. I think the default was G28, and the Clearance Height option didn’t work either (tried them all).
Very nice find! It’s a known issue that the G53 absolute moves aren’t shown correctly in the visualization or in the calculation of the tool path fitment. I had my post add in a “G53 X800 Y800” to the end of my programs to move the spindle to the middle back and it would always show “over”/“no fit” (I forget now, Masso controller has removed this issue)
for new users.
