Hello all I have designed some parts in fusion360 and manufacture it with their software. I am using the openbuilds cnc blackbox post processor to get gcode file. The simulation on fusion shows the part being cut out correctly(cutting around the part and then turning the laser off to move to its next part to cut. However when I run it on the actual machine, some parts are getting burned through bc the laser is not cutting off when it makes a linking move. The laser turns on and off correctly with the m3/m5 commands. And some times during the job, the laser will turn off on a linking move but other times not. This seems to show that the laser is receiving commands to turn on and off. Any idea what would be causing this? thanks!
Checkout Grbl v1.1 Laser Mode · gnea/grbl Wiki - the Grbl Wiki is a must-read to understand the firmware Please enable Laser Mode when using the Laser: See Grbl v1.1 Configuration · gnea/grbl Wiki
I have always used the laser, and it has always worked fine. Although, most of the time I use lightburn to produce my cgode file, instead of fusion and then openbuilds. I just checked and I have $32 set to laser mode on. It seems to me it is something to do with the post processor file that I am sending to the Control software. Thanks!
The odd thing about it to me is the 3d file in open builds doesn't look the same as the 3d simulated file in fusion 360. It appears to be missing parts in the 3d view of Control. However, it did cut the parts although they are not showing, but it also burned across them when making a linking move... I attached the gcode file and an image of what the simulation looks like on the fusion file Edit: Also, a note, in the fusion image it shows a warning about linking. I tried removing lead in/lead out (this removes the warning on the fusion page) and tried to burn the file, but I get the same result. Thanks!
GCODE header says you are still on v1.25 v1.30 is latest Releases · OpenBuilds/OpenBuilds-Fusion360-Postprocessor at the time of this reply Might not be it - but just a note you are out of date a bit
there have been alot of changes and some bug fixes since .25 so please update ASAP and regenerate the Gcode. OBControl (and others) does not show moves correctly unless there are Z moves.
initial look at the gcode says , yes, there is a problem there since there are no G0 codes except the first move. This is probably because you have the personal license and it (Fusion) does not output G0 moves. I think I did fix this in the post, upgrading and regenerating will prove it one way or the other. You should see G0 moves around the pierce comments.
Here is the gcode with the updated post processor. The 3d image still looks the same, but this is normal? I have not tried to actually burn it. Edit: if I am looking at it correctly, it still doesn't appear to be right. I don't see the pierce comments on the updated version, but at this line G4 P1.8 there are no G0 other than the first one. Thanks!!
Remember that a later edit doesn't pop up a notification - i coincidentally noticed you made an edit. Just a tip that a reply would be better - so there is a notification. If a party already read your reply, then you edit, they wouldn't know to go look at it again
I am modifying the edit above to a reply. if I am looking at it correctly, it still doesn't appear to be right. I don't see the pierce comments on the updated version, but at this line G4 P1.8 there are no G0 other than the first one. Thanks!
Probably not useful to you, but I was able to transfer the fusion file to lightburn by saving the sketch in fusion as dxf and importing dxf file to lightburn. It cut as expected on the laser. So, I believe the hardware/grbl settings to be correct. It could be in the manufacturing settings of my fusion file, but I don’t think so as the simulation looks correct in fusion. I have never created gcode for laser by creating dxf file and importing to lightburn, but FWIW, it was pretty easy to do. Thanks!
well, I cannot get my test drawing to output code like yours, mine 'just works' (though the pierce delay is useless in laser mode because of the way GRBL handles M4 motion). so, please send me your fusion file (save as f3d and give me that)
Ok, I am attaching it. I did a lot of random things trying to get it to work, and it is def. not best practice on how it was created! I'd love feedback on a better way..... However, I think it should give you the gcode file I posted yesterday. Thanks!
I believe the problem is the way you have placed the various parts of the drawing at different heights. Things that are below the top of the stock box do not get 'retracts' and therefore do not get a rapid move between them. So selecting all the letters in 'National' gets no rapids (top faces below stock box), but selecting the shapes on the left gives rapid retracts since the faces are at the level of the stock top. so, make all the bodies share the same top level and then all the outlines of the tops should cut properly. nope, wrong..... turn off 'keep nozzle down' in the linking tab
So, I would need to do both of these for it to work properly? I am almost positive tried unchecking keep nozzle down and got the same issue. But I see what you are saying with the other faces at different heights. Also, in fusion, what would be the easiest way to align all of the faces with the same plane? I know you can do it with the align tool, but you have to do it one part at a time. Is there an easier way? thanks!
I was only able to align the letters one at a time, but in the end got bored with that and tried the nozzle thing instead after having a brainwave (boring repetitive tasks tend to do that so, you only need to ensure that 'keep nozzle down' is OFF and it should work ok. (though the drawing makes more sense if everything is on the same plane)
Ok. Thanks! I thought I tried that but I guess not. What exactly does the “keep nozzle down” do? I have checked it before and it was beneficial for something but I can’t remember what?
It is really for plasma cutters which have Z motion. With it off, the nozzle will lift after every cut before moving to the next cut, then has to descend before starting the cut. This takes time and is not always needed, but some plasma cutters need it for the automatic height control to work its magic. Turning on 'keep nozzle down' will thus prevent these retracts so long as they are shorter than the maximum keep down distance, so longer rapids will still retract, depending on the settings. In our case GRBL is automatically controlling the laser on/off for us (Grbl v1.1 Laser Mode · gnea/grbl Wiki). Since we are using M4, we need the retracts to trigger G0 moves in the post, otherwise Fusion is not giving us G0 moves between cuts, instead I believe it is giving onPower events to turn the laser off and on which this post does not make use of (yet, maybe it should - but only if 'keep nozzle down' is on). Given that we are using M4 we do not want M4 and M5 sprinkled around in the Gcode since that interferes with the speed advantages of using M4 in the first place. However, if we want pierce delays then we have to use M3 mode when cutting, but not when etching, which will introduce a whole new level of if..then...else...but...except logic in the post (-: Starting to make sense to do a laser specific post, then there is less to go horribly wrong.
Great Explanation! Thank You! So, for now, any cutting done with laser should have "keep nozzle down" unchecked to prevent the possibility of missing some 'laser off' commands? This may take a little longer, but will give better results. Thanks!
