The student version is fully featured. After a few years of paying for F360, my wife finally noticed my $500+ AUD subscription and demanded I cancel it. As a result I’m now back on the free version.
yeah, CAM is available at all levels, but some CAM is not available. free/student does not do 4th axis free does not output rapid moves (maybe student too), which means all moves are limited to 'cutting speed' which can make some types of cuts take a very long time.
Thank you for all the info. I have constructed a model and the CAM in Fusion 360. Just need to get my head around it, as it is the first time, I am doing the whole CAD and then CAM thing. I need to avoid any rapid moves in this small aluminium desktop machine with open-loop Nema17 stepper motors, and not enough power available. I am thinking of using either Openbuilds CAM or Vectric Cut2D Desktop. If I am not mistaken you wrote the post-processor for Openbuilds for Fusion360.
I have created the following program in Openbuilds CAM, as you can see it has not used G2 commands. Is it okay that it only uses G1 commands as the circle is broken out into polylines?
That means you haven't Tuned your Max Rate correctly otherwise it would never be a worry: Grbl v1.1 Configuration Our free and beginner orientated CAM is super simple and doesn't bother with Arcs. If you need proper Arcs, use a more advanced CAM
Hi Peter, yes, you are right I have not tuned the "max rate". I will do that. In regards the not bothering with arcs, I do not mind. I was just wondering if one is better than the other or if defining the arc with G2 is "more accurate" than G1 with polylines. No critisism of software. I am a newbie trying to learn and do not know if one is better than the other with advantages between the G2 or the G1 method. Thanks again.
Apologies, I am unclear in regards to your answer. Are you saying the G1 polyline method for creating a tool path is easier than the G2? Apologies, unsure what you mean. I have read and been told I should not use the G2 with "R" but rather G2 with IJK. But, I have now come across this method (with Openbuilds CAM) using G1 and ploylines for the tool path. I am now not sure which one is best to use. Thanks again for the help.
Easier - for the development of the software yes. Its free software, so the easier option is "better". It works just FINE! But if you need proper Arcs, just use Fusion
you set up the machines GRBL settings maxrate numbers to rates that the machine can safely handle. After that Gcodes G0 moves are at that maxrate, no surprises. if you have Fusion360, you have more CAD and CAM than you will ever use, no need for anything else I built on other peoples work, but have added a lot of functionality to the Openbuilds post, yes.
I need to set up a "home" for my machine. Do I use the G28 or G30 option to set the position? Do I then use G28.1 or G30.1 to find a home? I would appreciate guidance in this regard. Thank you.
neither. machine home is set when the controller turns on (can be useful, see later) and then again when the home cycle is run (best) and it finds the limit switches at the ends of axis travel, usually + ends for X and Y and absolutely must be + end of Z (up as far as it will go without crashing) G28 and G30 are offsets from machine home. They default to 0 offset, and can be set by 1 - jog to a place, Z high (I use G28 as a toolchange position) 2 - issue G28.1 to store 'here' as an offset from machine home. same for G30 Now, issuing a G28 will move to that offset, but if the machine is not homed first you dont really know exactly where that offset will be. So always home the machine after turn on. Homing tells the machine to move Z toward the switch (feedrate in setting $25, when it hits it retracts a little then moves to contact it again, but slower (setting $24). Once it hits the switch the second time it sets machien Z to 0, then retracts by the pulloff distance (settign $27) Then it moves X and Y toward the switches, hits, retracts, hit again slowly, sets X0 and Y0 and retracts by the pulloff distance. Now the machine knows where machine home is, and all stored offsets, which are relative to machine home, are now useful. Now to do some work we need to tell the machine where the raw material is, since the Gcode is relative to the Work Coordinate System that we set in the CAM. This is often the front left corner (XY) at the top of the stock (Z), sometimes in the center of the material at the top of the stock. some people like to use the table as Z zero (don't!). For machines with a vice, the fixed jaw should be used as the Y reference. Now you jog to the spot on the stock that you set in CAM as the 0,0,0 point and use the 'setZero' buttons to tell it 'stock zero is here'. The 'paper method' is most often used for this, where you feel for the tool contacting a piece of paper you hold against the stock as you gently jog up to the paper. This can also be done using a probe cycle , where the machine finds the stock using a probe like the XYZ Probe from OpenBuilds (watch the video) These Work Coordinates (WCS) are also offsets from machine home and they are stored in the controller (and still exist after a power cycle). There are 6 WCS in GRBL, G54 through G59, but most of us use only G54, the default. Later: if your machine does not have home switches, you should get some Xtension Limit Switch Kit However, there is a way to opererate with a stable machine home while you wait for them to arrive. This is the 'fake the home' method, where you use that GRBL feature of setting machine 0,0,0 at power on to your advantage. If the machine is AT the physical home position when the controller turns on or is reset, then you have a sensible home you can use. much has been written, please read it
My apologies! Misterg, I had missed this g-code. I appreciate these examples. This is extremely helpful. Thank you again.
Is it possible to choose whether Openbuilds control is in G90 (absolute) or G91 (relative) motion? Am I correct by default, it is in G90 mode unless you state G91 in your g-code. Thank you.
I may be wrong, but I thought OB defaults to G91 as the moves are relative to the defined work XYZ zero location. Actually, thinking it through, it’s likely less to do with OB and more to do with your CAM software configuration. OB will just do what the code tells it to do. The standard would still be relative to the user defined work XYZ zero location
Let me rather ask my question differently. What is happening when jogging, is that absolute or relative?
I’d have to go out to the workshop to check as I can’t recall ATM. Also, My CNC is in bits ATM so I’ll leave it to someone else to answer.
It is the machine controller that is responsible for movement - Openbuilds Control is just the messenger (same for UGS, etc.). G90 / G91 are modal commands, so the machine controller will be in the state it was last set to. (This is persistent through power cycles, etc.) It is dangerous to assume that it will be in any particular state, so this sort of thing should be set explicitly at the start of your Gcode file that Control sends to the machine controller. At the start of the examples I posted, the following Gcodes appear: G90 G94 G17 G21 It's worth including similar at the start of all gcode files. There's a good reference here if you don't understand them. Jogging is relative to the current position *regardless* of the current modal settings.
it is in whatever mode tha tlst Gcode set it to. G90/G91 are part of a modal group, things that once set, stay set until changed. Gcode generated by openbuildsCAM/Fusion360 etc run in G90 mode, which is absolute mode (which is, confusingly, relative to the WCS ) G91 mode is set when needed by things like probing macros, and every Gcode program MUST set G90 is that is what it expects, do not ever 'assume' a mode, set what you need every time.
As @David the swarfer said, plus if you ever write your own g-code macros always put the appropriate (the "norm" is G90 for absolute moves) code on the end if you use relative moves in the macro. Then if you use a g-code command to move (eg G0 X0 Y0 to move to the workplace XY zero) you know what it is going to do. Alex.
Thank you, Misterg. I have attached an image. I would instead send a command (serial console) then use the jogging buttons, as I end up crashing these axes for my laboratory desktop CNC machine. I have attached a picture of the machine. I am getting very confused when I jog. But when I use a G92 G0 X2 command, for example, I can understand. I will also do further tests using my digital dial gauge to re-check how much the axes move.
I'm not sure why you are using G92, and I don't believe you are using it correctly - it is for setting the workplace zero for the current wcs. Did you mean G91 (relative move)? If so don't forget what @David the swarfer said about G90/91 being modal and the need to set it back to G90 for absolute movement mode. Alex.
Thank you, Alex, for this comment and your previous comment. So am I correct that for my machine, wherever the X, Y and Z-axes are sitting in space, if I run the command/g-code "G92 X0 Y0 Z0" sets my machine at "X=0", "Y=0" and "Z=0". Am I understanding you correctly? I like to test and send commands before just running g-code. Thanks again.
I don't use it myself, but that is my understanding. If you want to move relative to where you are now then use G91, but most control software will do that for you if you are just using it for jogging (and put the movement mode back to absolute (G90) for you. You seem to be making an awful lot of extra work for yourself, although understanding g-code is a good thing in my opinion. Alex.
do NOT use G92 yes it creates offsets (sets your displays to 0), that may be useful in some cases, but it creates GLOBAL offsets that mess up every other offset, including tool length offsets. Because it is global is will BITE you at some point because something unexpected (and possible expensive) will happen. The correct way, without sideffects, is to use the 'setZero' buttons built into the OpenBuildsCONTROL program (and all other GUI programs for GRBL controllers). These set the offsets for the current WCS and do not sideeffect tool offsets or anything else. These are what your CAM program will be expecting to be in effect. (the setZero buttons use the G10 L20 Pn ... command , which is the correct one to use G Codes )
