@Peter Van Der Walt @Alex Chambers Thanks for your help.... I generated a few tools paths and was able to run it on my machine in the control software and it operated no differently than when I run gcode generated out of Vcarve Pro. The one issue I had which I think is a user issue in Fusion but when I go to post process and save I get this pop up: Warning: Invalid Work Coordinate System. Select WCS 1..6in SETUP.PostProcess tab. selecting default WCS1/G54 I know I am diverging into the Fusion 360 black hole.....
That's just telling you that you didn't set which work co-ordinate system you wanted to use in the cam (manufacturing) section of Fusion, and it's going to use the default. If you want to stop that there is a setting in the first part of the setup in manufacture - post process - which gives you the option to set the wcs. I recommend setting it to 1 (the default anyway) Alex.
Peter that doc needs to be updated to the latest release link https://github.com/OpenBuilds/OpenB...nload/V1.0.18/OpenbuildsFusion360PostGrbl.cps
Thanks Alex - is there a better place here to discuss this? I would like to know if when I go to post process do I always have to select the post processor for the OB Box the .cps file as well as this WCS?
not whenever you do a post, whenever you do a 'setup' within fusion. yes you can just ignore this warning on the assumption that you will always use the G54 work coordinate system. However, I must advise you to get into the habit of setting the WCS in every setup because if you don't that one vital multi setup job that requires something other than G54 will waste a lot of time and material when G54 is assumed <-: it is 2 extra clicks.... create the setup then in edit select the 'post' tab and set the box to '1'. that is the only addition to the normal stuff you edit on a setup.
In SETUP is this what your speaking about (first image or second or both )? I am a new born fusion 360 user.
Not sure if this is intended behavior or not, but when I turn on my Blackbox controller and start up Control, the position is displayed as arbitrary large positive numbers. Even as I jog the machine, it maintains this new reference point. If i were to go to G28 (which i have set at my home position), it will go off into the abyss. I need to home my machine before the coordinates shown reference my G54 coordinate system and G28/G30 work appropriately. Is this how it is supposed to work or do i have something wrong in my settings? Thanks in advance.
All offsets (G28, G30, G54-59.1) are all based off Machine position + stored offset. Homing sets the Machine coordinates, thereafter all stored references become valid to physical space again
So is the MCS cleared out after every power cycle requiring a re-homing and re-setting of MCS each time? I understand that at power up the controller has no idea where anything is, just wondering if previous position should be stored and remembered at power on.
Not quite, "depends" technically, if you ran without switches you could "fake" home by parking in correct spot before powering off. With homing turned on Grbl boots up and goes into a locked state requiring either Homing or Unlocking, with unlock being a "i know what I am doing is wrong I actually should Home" as explained in gnea/grbl and gnea/grbl
I had asked this in the Vectric forum & didn't get a response. Maybe you know... what's different about the Vectric Openbuilds post from the generic Grbl one? Anything I'd notice?
- Extra code for enabling a spindle via IoT relay - Remove unsupported grbl commands that the Vectric post sometimes adds and improved compatibility with Grbl overall Refer to OpenBuilds/OpenBuilds-Vectric-Postprocessor and OpenBuilds/OpenBuilds-Vectric-Postprocessor
Okay, cool. I've stuck with the generic Grbl post because it just worked & I was buried with work, but things have eased up so it's a good time to switch posts & see how things go.
Hi all - it's not clear to me whether this is the proper place to ask this question or not - so feel free to point me in the right direction if not... I'm using Control v1.0.238 and trying to setup a javascript macro. When I use the sendGcode() function it appears this simply queues the Gcode command for later sending. Is there a way to perform this function in a way that appears to operate synchronously, so that the macro waits for the Gcode to be sent and completed before continuing on? Also, is there a way to detect errors that may be thrown from the executed Gcode (even just an ok/bad indication would be good-enough)? So - probably a better way to ask that is: Is there a way to sendGcode() then wait for an event that this gcode has completed? If so, is there a way to determine in/from the event whether the gcode was successful or not. Thanks.
At this time, sendGcode does not return status directly, in part because Grbl sends the OK when it goes into the planner. Not when it is executed. So instead we monitor the other statusses and events. Here is an example that does Help getting started with Javascript Macros in Control... Of course Pull Requests are accepted at github.com/OpenBuilds/OpenBuilds-CONTROL if you want to add a sendGcodeAndWait() function for example
today I got my Lead 1010 router built to the point of wanting to be able to power up and move the machine, Following along with the youtube video. I do not get the same info on the software page I am not able to see the "alarms"to turn them off or on, I do not get any way to select a machine, did I miss something?
No further suggestions unless you have more details to work from? It will only alarm if something is wrong (like you forgot to home - and have Homing cycle enabled - it will enter Alarm until you either Home or Unlock) You'll have to take the time to read the Grbl Wiki: gnea/grbl to understand How Grbl works. So if you don't get the alarm like Matt did in the Video, it means you probably don't have Homing enabled yet (great, better for beginners) Also see docs:software:openbuilds-control [OpenBuilds Documentation] for an introduction to OpenBuilds CONTROL. Beyond that, you'd need to tell as where you get stuck, show us whats on screen (screenshots are golden) or tell us a little more than the initial post did Also watch
Is there a way using OpenBuilds Control Software to specify the Z axis zero point without moving to that point. For example, if I want to run my GCode that has a coordinate system based off the bottom of the material. The material is in the way so I can only zero off the Z on the top of the material. I am not sure if there is a command that will allow me to specific a "Set Z zero at -35.52mm" without actually moving. It sounds like the G92 command might be what I am looking for but not sure if this will move the machine or if it will actually accomplish what I am after. Thanks in advance.
yes there is such a command, and though G92 will work it is not the best way since it has sideeffects. G Codes so the process would be measure the material set zero on the top of the material, leave Z at this zero issue command G10 L20 P1 Z35.52 P1 means use G54 Work Coordinate System, adjust as needed if you are not using G54 Z35.52 means make Z be 35.52 at the height it is at now, ergo Z = 0 would be 35.52mm lower than this place.
Oh cool! I got a response from THE David the swarfer! It's awesome when you get to interact with some of the celebs of the maker industry. Hi David! That is really helpful. Thank you for breaking it down. If I have my wasteboard like super perfect surfaced, is there anything stopping me from just homing my machine, working out the best possible height to my wasteboard and typing in the command to offset my Z each time? So home, hit zero for all, run G10 L20 P1 Z35.52 (if that was my height to drop down to touch my wasteboard) and in programs like Fusion360 set all my starting coordinates at the bottom of the stock? This is the code I am using before each of my toolpath command sets (please don't ask me why there is 2 x mm-mode commands.. I am using some hacky post processor that I still need to learn how to fix): G21 ; mm-mode G54; Work Coordinates G21; mm-mode G90; Absolute Positioning M3 S1000; Spindle On G0 Z0 I know limit switches probably aren't perfect either but they are probably more accurate than the other person I am sharing the CNC with. He just goes "stuff it.. if I cut 5mm extra into the wasteboard we can just throw it out in a month and buy another one for AU$70". Which doesn't sit well with my OCD nor my wallet.
thanks <-: I would use 'the paper method' to find the surface of the waste board with the tool before mounting the stock. Note that you need to do this everytime you change the tool unless you have TTS or similar quick change repeating tool holders. yes, that will work fine so long as you always touch off the tool on the surface correctly. if you are using OpenBuildsCONTROL then you should be using Openbuilds GRBL post ... it is the thing to have (-: aaargh! but the limit switch homing will be within 0.05mm usually so that will work for most things with the occasional wasteboard 'scratch'. if you are mounting with the masking tape and superglue method then you will want to create a 2 layer tape sandwich and zero the tool on that, then you cut the material but not the tape and the tool stays clean. . to sum up: always touch off the tool, every tool, everytime. I park my machine at home and trust the XY after a power cycle, but always check Z.
I was forgetting about the tool change! So helpful. I had trouble with the OpenBuilds post processor (my fault) so I went back to as basic as I could. It was doing things I didn’t expect. Will get back to working that out and ask in a different thread. Will follow the instructions you have given me here and I should be right now. Thanks again.
