How do I keep Fusion 360 from adding the G53 commands below? Those cause issues with my gcode. Without them, the program runs fine. With them, it goes down and touches the sheet on the plasma table, then comes up to zero and scrapes across the part to the start spot. Then raised to the pierce height, etc... G53 G0 Z-0.3937 G0 X-0.3395 Y-0.1366 F63 G0 X-0.3395 Y-0.1366 Z0.4
no need to remove anything, just raise Z to the top and reset the blockbox there. That is the simplest 'fake the home' move of all since 'home' is where the blackbox turns on or resets and we want Z home to be a high as possible. After that the G53 move will raise the Z to a safe height before moving to the start position, as intended.
Or even better, just install Homing switches. It really is worth the couple bucks to have repeatable machine coordinates. HOME, ZERO, RUN SIMPLE
If you're already going to G54 Z0.4 based on a touchoff, makes the most sense. I'd do 24V switches, active low, at the very least. If for some reason you want to avoid switches (and on a plasma, there are certainly reasons why), is a pretty easy method and if you add a "G53 G0 Z0" block to the end of every file right before the M2/M30, the machine will do all the work for you and it'll be reset in place every time you start a new piece.
I don't think @Chris611 got the answer he deserved. I have the same question, how can I make the post processor not add the G53 every time. We all have different use cases and in my case I don't want to home the machine before every run. because I have a setup that will crash the machine into my work holdings if it should always use the G53 command. I don't need that in my case since I "home" the machine on the workpiece I want to mill by probing it. So please, give us a proper answer on how it can be removed from the post processor. And no, the answer is not that I just can remove it in a editor afterwards, because that takes time if you have to do this every time you generate a Gcode.
The correct answer is "install proper home switches". The foundation of any meaningful automation is starting at a repeatable, known location with defined travel limits. I hit Ctrl+Home in the morning when I turn the machine on and walk away, it's pretty trivial. If I'm not doing something like calibrating the axis screws, I only need to home when I turn the machine on. If you leave it switched on permanently and never crash, you might only ever have to home once. There's certainly no reason to home before *every* run. This... Isn't a good thing, though. Homing the machine on the workpiece and leaving your G54 WCS offset at zero is simply not how machines are designed to be run, hence your difficulties.
I mostly mill part that are waaay smaller than the work area of the lead 1010 so I honestly don’t see the problem of using workcoordinate G54 and probe. If machines are designed to use the G53 in the start, why does not the official grbl post prosessor add it then? I don’t buy your argument. And by the way, I have endstops on all axis. It’s not about that.
it does (kinda), but by using G28 instead (because the folks at autodesk did not actually read the GRBL wiki) . G28 is a 'user settable position' and the default in GRBL is G28=0,0,0 offset from home. When GRBL has no home switches and is not homed, then 'home' (machine 0,0,0) is where it turned on or reset. This is pretty much ALWAYS not a safe place to return to unless the machine is homed or the user is properly aware of what they are doing.
My machine has no switches I use the 'fake the home' method. How to 'Fake the home' I use a macro to park the head at 'home' before I turn it off. This means it is already at 'home' when I turn it on and I have nothing further to do. If you did this then homing would take a few seconds after turn on since it would not have to go far to find home. After that a single button click will return it to the previous jobs G54 0,0,0 position, ready for you to probe for a new part. home sweet home Home, Fusion360 and G53 Z moves
are you a programmer? if you are then editing the postprocessor is an option. I am a programmer, with some 30 years of experience. Safe startup and ending movements are part of what the post is doing, and considerable time has gone into making it do what it does to keep your fingers/clamps/tools/junk (ok, your machien does not have tools and junk on the table, but mine does, any flat spot is victim to 'stuff' around me) out of the path of a sharp spinning thing with more power than your kitchen blender being moved by a screw system that you cannot hold back, ie it will not stop because your hand/electricscrewdriver is in the way. Keep in mind that OB systems are used everywhere from your/my craft room to industrial settings doing commercial work. As such, safety is vital, and adherance to industry standards is what we must do, both for our users safety, and probably for insurance purposes too in those OSHA aware environments. So, there is no easy way to disable the use of G53 and there will never be a way to make it more dangerous just because a few (2) people don't like how long it takes to home. (hint, use a macro to park near home before you turn off, then homing takes seconds) here is that parking macro Code: G17 G90 G21 G53 G0 Z-5 G53 G0 X-5 Y-5 That will park 5mm from the switches so it only has to seek that far to find home. Won't take long, and has all the benefits of homing for free.
it has nothing to do with the time. It's the practical stuff around it. But anyway, I have used it without G53 for a long time and no crashes because of that, as long as I don't mix in G53 command in the gcode. Im not sure if it's properly explained how I use it. The question was a modification question , well aware of that a machine should have known machine home for most cases. I have a lot of experience with codes so I know perfectly how to park the machine. Im not a programmer. nice for you that you are. That's why I asked for help to edit the postprocessor in the first place... Never asked open builds to change the post processor for the official version.
I too would like to remove the g53 from the code ..It simply doesn't make any sense to have it using a different wcs to go to a safe z position when you are already probing for your material in the g54 wcs.. Especially on a machine that doesn't have a tool changer Or on a controller that doesn't support a tool change ..Even in that case you would have your tool change and safe z location saved in the m6 macro ..I think most people are using the top center of the part for the zero location so going to a home position would be very wasteful ..I have home switches on my machine and home so i can run my soft limits to avoid crashes but i do not want homing in the middle of a file .My files have many different operations so editing a file of several hundred thousand lines of code is not feasable
Without getting into the debate about the inclusion of G53, there's some stuff that's wrong: G53 isn't a WCS (Work Coordinate System), it references Machine Coordinates, so is outside anything that's done with probing or zeroing to the work. Commands using Machine Coordinates can be relied on to send the machine to a specific place (e.g. Z top), without generating errors, regardless of which WCS is active and how it has been set up. There's no reason you would need to 'home in the middle of a file' - home the machine at power up, and you're good to go for as long as you like. G53 doesn't send the machine home, it just references the machine coordinates that are relative to the home position. There is always the option of using the Autodesk POST and selecting 'Clearance Height' as the safe position if you really don't like having to home the machine.
