Openbuilds Lead1515 I am carving a piece of stock that is 1 1/2" thick. I have my z-rail all the way up and my router up as far as I can in the holder. I did this in an attempt to get the most upward travel possible. My start point is the top of the lower left corner I used my probe to set zero. When I hit "RUN", the system raises the Z all the way up and triggers the Z limit switch and sets off the alarm - thus stopping the program from running. Is there a way to control how far the z travels when it starts it's initial move? If so, how do I do this? My retract height is set to 1/4"
By Homing and setting Start and End of Job to a negative number. See Search Results for Query: Fusion g53 | OpenBuilds
Thank you for the response. I did finally find a post where you addressed this with another member (I think it was called "Z drop" or something like that). As you probably know, My G53 was set with Z-0.3XXX. I changed this to Z-0.05 and it worked PERFECTLY for the start...but when the program ended, it drug the bit through 3/4 of my piece and ruined a 4 hour carve. I am still very new to G-Code and to CNC, so I apologize for the elementary question(s) coming up: Can you explain "homing" and is there a video showing the process?
docs:blackbox:hello-world [OpenBuilds Documentation] Probably not homing related per-se. Post the files so we can check what the ending said to do
Tagging in @David the swarfer as I don't see anything off (may be wrong) - it is our post (was making sure) etc
While we wait, do you mind posting pics of the accident too - may also have clues Is your setup sufficient that Z didn't "top out" mechanically during any moves (go up too far, stalls out, Z position changes)
Sorry for the delay. I have been away from the computer for a little while. I am attaching the photos with this response. The Z was topping out when it started. Hence the reason, initially, for this thread. But, I changed the G53 G0 Z-0.3937 to Z-0.05 or possibly Z-0.00. Sorry, i changed this in the G-Code editor in CONTROL but not in the stored G-Code that I sent earlier. This fixed the initial topping out when the program started, but it ended with what you see in the pics. Ignore the lower corner where the other f-up is. That was when I was playing around with the Z settings - but I could have repaired this.
Yes, but start and end is the same exact gcode. And thus this is most likely related. Hand editing is not trivial
Yep. I guarantee that's what happened. The attached gcode file is fine. But if Z-0.3937 would have hit your stock at the beginning of the job and you didnt surface any stock from the top during the job, then its certainly is going to hit your stock at the end. You only changed the start of the program, not the end.
It wasn't hitting my stock. It was hitting the limit switch on the Z-axis and setting off an alarm - thus stopping the program. This all came about when the initial move was to raise the z-axis before traveling to the start point from 0. This is when the initial issue occurred. By changing the initial z movement to -.05 or -0, it no longer raised far enough to hit the limit switch. By NO means am I arguing the resultant consensus, I just need to know how to fix it so that it will not raise far enough to hit the limit switch, but will stay clear when it returns after the program has ran - which is where I am assuming I need to set the HOME location.
So you changed it in the gcode file at the start (line 22) but not in fusion360 post options, so the ending G53 G0 Z-0.3937 is what dragged through the work. The reason for this is that your workpiece is thick enough that 10mm (0.3937") below Z home (top of Z travel) is in contact with the work. Thus you have to change the Z offset in the post options to -1 (always in mm, 0.05" is about 1mm) Note the popup help is visible here too The default is -10mm, which is always more than enough to clear the home switch. GRBL sets Z0 home to the spot where the switch is actually triggered so if you go to machine home with G53 G0 Z0 it will cause an alarm. Therefore the starting (and ending) safety move always stops below Z0 using G53 G0 Z-10 (in mm or equiv in inches) In the case of your thick workpeice you will have to set this to a smaller value so that the bit still safely clears the work. Fusion should remember this setting for the post once you have set it but for every job you need to think about clearance for a moment before running the job. Is it a particularly thick job? What are the safe height and clearance height settings? Will they fit given the length of the bit? Are they small enough to fit between the workpeice and the top of Z travel? Is G53 Z-0.3937 high enough to clear the work? OR this if you are using the NCprogram interface to the post: I suggest running some simple 1 minute jobs on insulation foam, trying different thicknesses and settings until you get this figured out (fail fast, fail cheap). Running a 4 hour job on expensive wood is perhaps not the best way to learn (-:
Nothing wrong with the Gcode, Z moves are the default -10mm but this job clearly does not have the clearance. I wonder if we can put a link to a resource about this in the Gcode?
I recently updated the post to utilize the new property naming and grouping features (submitting updated pull request shortly). I thought it would be cool to have a clickable link to the openbuilds doc section. Unfortunately that's not possible, However, we can do something like this if you want (see first section):
Happy to add a page to the Docs - just haven't had time to write a nice explanation of what Machine coordinates are, why always homing is important etc And a seperate page for the Fusion Post docs may be good too - even if just to allow us to say "go see here"
Yes, I am busy processing your pull request. Problem is the difference between the old post options display and the newer NCprograms style display. The group names work great in the new display but not in the old display (which is selectable as a default). Yes, I know Fusion now defaults to creating NC programs and most people will see that, but the old post options must still make sense, even to a new user. I like that, though I was thinking of a comment in the Gcode just above the G53 move that says something like (if the start of your job is acting weird then read the docs at http:/linkheretohowandwhytohomeandWCS/MCSoverview/doc ) so probably go with both (-: IFF having a link in a comment does not break the Gcode with illegal characters. So, just need a link to the relevant doc page (-:
I do, for one, so I can see what the post is displaying, and I prefer it to the NCprograms anyway since I tend to be testing single operations and also I normally cut one operation at a time. and if I use it, so do about 1 in 10 other people and I will not ignore their needs (-:
Thank you for this information. And, I will reiterate that I am new to the CNC world and trying to learn as much as I can. I am also new to Fusion 360 (12 year Solidworks user) What I have learned from this post, so far, is that I should home the machine before every carve before I set zero. Next - I have to take all of the information listed in your post in consideration before carving as well. If I change the start Z, I must also change the end Z. Now, I have to ask, as I am not overly familiar with the look of your images, What program were these taken in and where can I find them? Apologies for all of the newbie and hand holding requirements. I promise I will run one day. OH..and i also broke my Sharkbit 1/8" end mill when it did that move as well...so it wasn't just the wood. i did not figure this out until I went to try my next carve a few minutes ago.
Incorrect, you should NEVER change Gcode by hand... Fix the value in the Post Options! If -10mm (10mm below the limit switch) didn't work for you, and you wanted to use -5mm for example, enter -5. Must always be negative (switch = 0. Negative = from switch to spoilboard. Positive = other side of switch - cannot reach. See Frequently Asked Questions · gnea/grbl Wiki to understand why)
@David the swarfer @Peter Van Der Walt @sharmstr Thank you for your contributions to this post and sorry I haven't replied sooner. Honestly, I just had to step away for a few days before I tried tackling this again. On another note, any idea why Fusion 360 gives me an Invalid Work Coordinate System and tells me to "Select WCS1..6 in SETUPost{rocess tab"? When I go look at the postprocessing Tab, I don't see any where to set this.
Because you have your WCS Offset set to 0 in the setup. Its just a warning that you havent set it up and that it will default to G54, If you want to avoid this you have two options. 1 - Change your WCS to 1 in your setup. 2 - After changing your WCS to 1 in your setup, right click and select save as default. Then every new setup you create will auto set WCS to 1.
