Program ran fine in Fusion 360 besides the simulation starting at the bottom right, instead of left, which it has done many times in the past without issue. Once I zero out in the bottom left and run with the spindle already in that location I've never had an issue. I went to run this re-surface after testing on a few boards and it seemed like it wanted to start at the right. However, the spindle (starting at left) dug in, instead of lifting all the way to the right if that's what it was going to do? I've confused myself just typing this. I've attached the F360 file, sim video and some pictures. Everything is OB and it's a LEAD 1515. Around 8 seconds of that video sim is when my day was ruined. Maybe related, I have the spindle wired up to the IOT relay. The relay doesn't turn on in time so the bit hits the material, sits there for a second, then it turns on. I had the Z up pretty high as well so something is wrong. Thanks for all the help Rhett E. (Made in : Autodesk CAM Post Processor) (G Code optimized for Grbl 1.1 BlackBox controller) (OpenBuilds CNC : GRBL BlackBox) (Post Processor : OpenbuildsFusion360PostGrbl.cps V1.0.20) (Units = mm) (Drawing name : spoilboard surfacing v3) (Program Name : spoilboard surfacingV2) (1 Operation in 1 files.) (File List ( spoilboard surfacingV2.gcode) (This is file: 1 of 1) (This file contains the following operations: ) (1 : Face2) ( Work Coordinate System : G54) ( Tool 2: Face Mill 3 Flutes, Diam = 25.4mm, Len = 5.59mm) ( Spindle : RPM = 18000.04810713488, set router dial to 1.9) ( Machining time : 1 hours 24 min 49 sec) G90 G94 G17 G21 (Operation 1 of 1 : Face2) G54 G53 G0 Z-10 S18000 M3 G4 P1.8 G0 X1147.97 Y5.415 Z15 Z5 G1 X1147.97 Y5.415 Z-0.255 F1000 X1134 Y5.415 X0 Y5.415 G2 X0 Y23.351 Z-0.255 I0 J8.968 G1 X1134 Y23.351 G3 X1134 Y41.286 I0 J8.968 G1 X0 Y41.286 G2 X0 Y59.221 I0 J8.968 G1 X1134 Y59.221 G3 X1134 Y77.156 I0 J8.968 G1 X0 Y77.156 G2 X0 Y95.092 I0 J8.968 G1 X1134 Y95.092 G3 X1134 Y113.027 I0 J8.968 G1 X0 Y113.027 G2 X0 Y130.962 I0 J8.968 G1 X1134 Y130.962 G3 X1134 Y148.897 I0 J8.968 G1 X0 Y148.897 G2 X0 Y166.833 I0 J8.968 G1 X1134 Y166.833 G3 X1134 Y184.768 I0 J8.968 G1 X0 Y184.768 G2 X0 Y202.703 I0 J8.968 G1 X1134 Y202.703 G3 X1134 Y220.639 I0 J8.968 G1 X0 Y220.639 G2 X0 Y238.574 I0 J8.968 G1 X1134 Y238.574 G3 X1134 Y256.509 I0 J8.968 G1 X0 Y256.509 G2 X0 Y274.444 I0 J8.968 G1 X1134 Y274.444 G3 X1134 Y292.38 I0 J8.968 G1 X0 Y292.38 G2 X0 Y310.315 I0 J8.968 G1 X1134 Y310.315 G3 X1134 Y328.25 I0 J8.968 G1 X0 Y328.25 G2 X0 Y346.185 I0 J8.968 G1 X1134 Y346.185 G3 X1134 Y364.121 I0 J8.968 G1 X0 Y364.121 G2 X0 Y382.056 I0 J8.968 G1 X1134 Y382.056 G3 X1134 Y399.991 I0 J8.968 G1 X0 Y399.991 G2 X0 Y417.927 I0 J8.968 G1 X1134 Y417.927 G3 X1134 Y435.862 I0 J8.968 G1 X0 Y435.862 G2 X0 Y453.797 I0 J8.968 G1 X1134 Y453.797 G3 X1134 Y471.732 I0 J8.968 G1 X0 Y471.732 G2 X0 Y489.668 I0 J8.968 G1 X1134 Y489.668 G3 X1134 Y507.603 I0 J8.968 G1 X0 Y507.603 G2 X0 Y525.538 I0 J8.968 G1 X1134 Y525.538 G3 X1134 Y543.474 I0 J8.968 G1 X0 Y543.474 G2 X0 Y561.409 I0 J8.968 G1 X1134 Y561.409 G3 X1134 Y579.344 I0 J8.968 G1 X0 Y579.344 G2 X0 Y597.279 I0 J8.968 G1 X1134 Y597.279 G3 X1134 Y615.215 I0 J8.968 G1 X0 Y615.215 G2 X0 Y633.15 I0 J8.968 G1 X1134 Y633.15 G3 X1134 Y651.085 I0 J8.968 G1 X0 Y651.085 G2 X0 Y669.02 I0 J8.968 G1 X1134 Y669.02 G3 X1134 Y686.956 I0 J8.968 G1 X0 Y686.956 G2 X0 Y704.891 I0 J8.968 G1 X1134 Y704.891 G3 X1134 Y722.826 I0 J8.968 G1 X0 Y722.826 G2 X0 Y740.762 I0 J8.968 G1 X1134 Y740.762 G3 X1134 Y758.697 I0 J8.968 G1 X0 Y758.697 G2 X0 Y776.632 I0 J8.968 G1 X1134 Y776.632 G3 X1134 Y794.567 I0 J8.968 G1 X0 Y794.567 G2 X0 Y812.503 I0 J8.968 G1 X1134 Y812.503 G3 X1134 Y830.438 I0 J8.968 G1 X0 Y830.438 G2 X0 Y848.373 I0 J8.968 G1 X1134 Y848.373 G3 X1134 Y866.308 I0 J8.968 G1 X0 Y866.308 G2 X0 Y884.244 I0 J8.968 G1 X1134 Y884.244 G3 X1134 Y902.179 I0 J8.968 G1 X0 Y902.179 G2 X0 Y920.114 I0 J8.968 G1 X1134 Y920.114 G3 X1134 Y938.049 I0 J8.968 G1 X0 Y938.049 G2 X0 Y955.985 I0 J8.968 G1 X1134 Y955.985 G3 X1134 Y973.92 I0 J8.968 G1 X0 Y973.92 G2 X0 Y991.855 I0 J8.968 G1 X1134 Y991.855 G3 X1134 Y1009.791 I0 J8.968 G1 X0 Y1009.791 G2 X0 Y1027.726 I0 J8.968 G1 X1134 Y1027.726 G3 X1134 Y1045.661 I0 J8.968 G1 X0 Y1045.661 G2 X0 Y1063.596 I0 J8.968 G1 X1134 Y1063.596 G3 X1134 Y1081.532 I0 J8.968 G1 X0 Y1081.532 G2 X0 Y1099.467 I0 J8.968 G1 X1134 Y1099.467 G3 X1134 Y1117.402 I0 J8.968 G1 X0 Y1117.402 G2 X0 Y1135.338 I0 J8.968 G1 X1134 Y1135.338 G3 X1134 Y1153.273 I0 J8.968 G1 X0 Y1153.273 G2 X0 Y1171.208 I0 J8.968 G1 X1134 Y1171.208 G3 X1134 Y1189.143 I0 J8.968 G1 X0 Y1189.143 G2 X0 Y1207.079 I0 J8.968 G1 X1134 Y1207.079 G3 X1134 Y1225.014 I0 J8.968 G1 X0 Y1225.014 G2 X0 Y1242.949 I0 J8.968 G1 X1134 Y1242.949 G3 X1134 Y1260.884 I0 J8.968 G1 X0 Y1260.884 G2 X0 Y1278.82 I0 J8.968 G1 X1134 Y1278.82 G3 X1134 Y1296.755 I0 J8.968 G1 X0 Y1296.755 G0 Z15 G53 G0 Z-10 M5 G0 X-10 Y-10 M30 %
I spun the bit till it stopped when and clicked set XYZ. Can you elaborate on it being 10mm below the machine during that move, please? Is it possible I set the tool up wrong in Fusion? I didn't see that Sharkbits in the F360 library.
I deleted my post after reading yours again. Anyhow, what it should do is move the spindle to machine z-10. Thats machine coordinates, not your work coordinates. Its considered a safe height (but that's not always true) That's this line G53 G0 Z-10 Then spindle comes on S18000 M3 Then it pauses to let the spindle come up to speed. You can increase this if you need. G4 P1.8 Then it heads over to where its going to make its first cuts. G0 X1147.97 Y5.415 The simulator starts the cutter in the work 0 position, which in your case is lower left. What you cant see in the sim because you are looking at it from the top, is the cutter moving up to machine Z-10 (above your stock) before going to the lower right.
So it sounds like you're saying when I clicked 'SetZero XYZ' I somehow set the machine coordinates instead of work or maybe that's what's blowing it up in F360? Initially, my spindle definitely didn't move up to 10 then wait for the spindle to turn on. I'd say it was almost the opposite. Is Z not moving up to 10 at the 9-10 second mark of the video I attached? Thank you for your patience, Shawn.
No, not saying that at all. That's why I deleted my first response. My second response was merely a "here's what's supposed to happen" based on your code and fusion file.
machine Z home needs to be as high as Z will go in order for Fusion to work correctly and safely. It that the case on your machine? Then the Z clearance needs to be set, -10mm is the default but if -1 will clear your limit switch correctly then you can use that. This is in the post options, if you hover over each option in turn you will get some popup help.
what you are seeing in the simulation is CONTROL's inability to display a G53 move correctly. not many Gcode previewers do this correctly. the Gcode is fine, it is saying: G53 G0 Z-10 ; raise Z to a safe height that does not trigger the limit by staying 10mm below the limit S18000 M3 ; start spindle G4 P1.8 ; delay - this is adjustable in the post options G0 X1147.97 Y5.415 ; go to the XY start position (Z is still high up and safe) Z15 ; come down to to 'safe height' i think fusion calls it Z5 ; come further down to retract height (swap as needed with the above, I cannot open Fusion now to check) G1 X1147.97 Y5.415 Z-0.255 F1000 ; enter the cut at 1000mm/min, straight down X1134 Y5.415 ; do the first cut sweep from right to left and so on.
Thank you for all the detailed and prompt responses. I'm embarrassed to admit, but the problem was I didn't home the machine before running the program. I repeated the same steps and program but homed the machine, removed the bit, and it functioned as you all have described. Luckily, this learning lesson didn't cost me a sharkbit like my last one, just some man points on the forum. There is still the slight issue of the spindle starting the cut at the front right instead of the origin (left). I'm fairly certain this is a Fusion issue because it does the same thing in the Fusion simulation. I've messed with all the setup and toolpath settings but can't seem to move it. I'll keep playing with it. Not deal breaker though but would be nice to know exactly where the tool is going.
Happens to the best of us. Why does it matter where it starts? And since you are using Control, why not use the flattening wizard? It will clean up the edges at the end which wont happen the way you programmed Fusion.
You're right, It doesn't really matter where it starts, I just wasn't expecting it. More like throwing a ball with my opposite hand when it starts from the right. I played with the flattening wizard but it seems to create it's own offset and I couldn't customize it. My file in fusion has overlaps to compensate for the edges. The wizard is also in metric only and I kept going back and forth with my conversions, even though I ended up using metric with fusion.
It runs the exact outline size you specify, it offsets inward by half-endmill diameter to ensure the cut size is accurate as entered (ie the outside diameter of the endmill, cleans up the edge of the dimensions you entered). Just enter the correct endmill size, and final dimensions
I was confused by this as well. But as Peter explained, think of it as a pocketing operation instead of a facing operation.
