That would explain the errors (which are very small) I am getting - working in "wood" I have been using conventional milling. Alex.
We actually have a video coming out tomorrow on calibrating the WorkBee with the Duet controller. However i will go over it here. I find it best to cut a square which you can then measure with calipers. Also it is best to cut a material which will not change its form post cut, so avoid wood, and is also flat. I like to use aluminium. In addition i always cut calibration pieces with a rough pass having a 0.2mm allowance, then a finish path to take off this final 0.2mm to reduce the forces on the machine. After cutting measure your calibration piece. For example if the calibration piece is meant to be 100mm on the X-Axis, but it cut a 100.5mm, you would do (100/100.5) * (Current Steps Per mm for that axis). The steps per mm setting is found in config.g, the M92 command. So for example by default the X-Axis on a screw drive is 400, so for this example we would change it to (100/100.5) * (400) = 398. Then save the config file and restart your board.
Cheers @Ryan Lock Now I need to get some aluminum, some bits to cut it, make my clamps, this is going to take a while.... Cheers Colin
Do you have a 3d printer @Colin Hart? If so there are a variety of clamping systems on Thingiverse.com. I got some from there which I found very good. If you are interested I will let you have an exact link. Alex. PS be careful what aluminium you get - some alloys do not machine well.
awww so... Yes for 3D Printer. Yes please for link What aluminium do you recommend? I'm just browsing ebay for some.. Cheers Colin.
Link to the ones I use is; www.thingiverse.com/thing:2782653, but if you go to thingiverse.com and search for cnc router clamp or hold downs you will find a wide variety. I believe the alloy most people on here have recommended is 6061 aluminium I haven't (successfully) machined any aluminium, but the stuff I have is an unknown alloy and I suspect it is too soft. Alex.
These are great hold down clamps as well. Reversable Hold-Down for T-Slot Tables by WorksBySolo I like them because they are longer so your knob/bolt are further from your work surface. I have had a couple instances when using other clamps where my dust shoe hit the knob. But, that is because I was not paying attention to that, or under estimated how close the knob was.
Hey, Regarding the promised video, that is now coming out next week, we had to fix some last minute issues with the video.
@Ryan Lock do we get to see the blooper reel then??? The latest made for some light lunchtime viewing...
This is a few days late but I had exactly the same thing happen to me just now so you have my empathy! I thought it was my poor use of cable ties but I feel better reading that it happened to someone else. Probably a little bit late as you are using Fusion (I need to start learning it) but I went Alex's route and made a rectangle in Open Builds CAM and got it to cut a pocket to surface my spoil board - worked a treat. Cheers Adam
Hi @Award - You are not alone... every alteration to the manual I have made someone has had experience of. Fusion is great, I am very fortunate that I use Solidword at work, so Fusion is fairly straight forward for me. For most stuff it is overkill, but I'm familiar with it and I can draw simple things out without having to think too much. If you use Fusion look at one of my other "Mistakes" and make sure you install the Post Processor from Ooznest (if you are using a WorkBee) or you GCODE will cause your machine to mill things in unforeseen places ;-)
Afternoon All... So I thought I would continue this thread.. more GCODE funnies... So I was all set for an afternoon of milling, making a guitar Last night I successfully faced of the wood, today I wanted to cut the pocket This is the model of the operation in Fusion, a simple 2D pocket. I checked the machine home, hit the go button and I get the following: Not a very helpful error message for the rookie CNC machinist. So I wanted to try and work out the error, so I line by line pasted each line of GCODE into the console until the error appeared, thus highlighting the offending line. So My G-CODE is as follows, note this all works ok, so this is good code. (1001) G21 G90 (2D Pocket1) G0 X1.420 Y-3.904 Z36.000 G0 X1.420 Y-3.904 Z36.000 G0 X1.420 Y-3.904 Z31.000 G1 X1.420 Y-3.904 Z25.600 F1440 G1 X1.420 Y-3.896 Z25.506 F1440 G1 X1.421 Y-3.874 Z25.415 F1440 G1 X1.421 Y-3.838 Z25.328 F1440 G1 X1.422 Y-3.789 Z25.247 F1440 G1 X1.422 Y-3.728 Z25.176 F1440 G1 X1.423 Y-3.657 Z25.115 F1440 G1 X1.424 Y-3.576 Z25.065 F1440 G1 X1.425 Y-3.489 Z25.029 F1440 G1 X1.426 Y-3.398 Z25.007 F1440 G1 X1.427 Y-3.304 Z25.000 F1440 G1 X1.443 Y-1.892 Z25.000 F1440 Then came the offending line G1 X2.688 Y110.158 Z25.000 F1440 The mill started to travel along the Y Axis and then G2/G3 error appeared and the machine stopped. This picture shows where the machine stopped, the Blue X marks the approx home position (its more at the edge of the stock), the red arrow shows the direction of the Y. So a little about the fusion post process: My Work Home Position in machine coordinates is: Clearly, I am having a moment and missing something obvious, any suggestions greatly welcomed... Cheers All.. Regards Colin.
Hi @Colin Hart, did you home all your axes before starting this morning? (and have you disabled "allow moves without homing"?) If you haven't done both of those the machine can get confused about where it's limits are. Alex.
Hi @Colin Hart Would an online gCode anyalizer program have helped prior to running it on the machine?
Hi Alex, so yes to homing before hand, the 2nd bit I've not heard of, what is this black magic allowing move without homing you speak of? Sorry just putting the brisket in the oven..
g2/g3 are arc errors. Again, I dont have a duet, but I believe that error message is misleading. What's the next line of gcode after this one: G1 X2.688 Y110.158 Z25.000 F1440?
If you go to settings in Duet Web Control there's a box (on the first screen I think) that says "allow moves without homing" - it needs to be unticked or the machine does not know where the machine limits are. I did put it in my build report. Alex.
Evening all.. been tied up this week so finally got power back in the garage. I do not see this option "allow moves without homing.. Screen shot of my settings incase my glasses are faulty
Very true @Colin Hart, your second screen shot - in the machine control section - is where it is in mine. If you are concerned you could try switching on your machine and then jogging it before you home any axes. If it doesn't move you are safe. You could also (VERY cautiously) try jogging past zero (front left) again, if it won't do it you are safe. Alex.
hmm ok i can jog my machine around before homing. very strange.. the same error still appears.. do you think Alex @ Ooznet may be able to assist in the morning? I have some time at home tomorrow so can call them....
Maybe you guys should confirm that you are on the same firmware and web interface versions. Again, I dont have a duet, but according to the doc, the setting is fairly new.
Thanks @sharmstr, I was about to suggest that, but went off to experiment with my machine. @Colin Hart - @hobdayd has found a solution in the duet wiki that might work for you. Config.g line M564 - if set to H0 will allow moves without homing. If set to H1 S1 will prevent moves without homing AND prevent moves outside the machines defined limits. Out of curiosity I will check later what firmware version I am on. Alex
PS did you solve your guitar problems? I am certainly not the person to pontificate about G code, knowing very little about it, but I thought your G90 code meant use absolute co-ordinates and on my machine all co-ordinates are positive (your Y is negative until the offending line when it moves a long way positive) Alex.
AGGGGGGGHH lkdklswjkl; fkl kl snfkla lsnglksdf I fixed it.. There appears to be an issue with the post processor by Oooznest, I installed the V1 Fusion post processor and Presto it Worked!!!! This is good news.. also M564 was not set, I have done this and now no moving without homing!!! Thank you all for your comments... right time to get back to a nice pint of Hop House.
Being from Ireland I hate Guinness's version of this Lager (13)...Preferring instead the new Rockshore...... But being weened on Real Ale its not often I sup the stuff lol Cant beat a nice pint of Black Sheep
a bit of old peculiar... after 4 pints one find themselves propping the bar up... back in the day....
Hi @Colin Hart, I've been using the Oozenest Fusion 360 post processor for a few weeks now with no problems albeit with only one toolpath at a time. Where did you find the V1 post? Alex
Hey Alex, G90 Absolute doesnt mean what I think you think it means. Its sounds like you think that G90 means that all moves are positive. G90 means all coordinates are relative to work 0,0,0. If you set your origin in the middle of the stock then, theoretically, 1/4 of the moves will be negative in both x and y. G91 Incremental means that all coordinates are relative to the last position. @Colin Hart : Glad you got it sorted, but you never answered my question above. The way Fusion handles arcs can some times cause issues, especially when adaptive strategies are used. You'll usually get a G2/G3 error. When this happens, your machine will not process that G2/G3 line and throw an error. That's why I believe that the line after the one you posted is probably the one that caused the problem. If you look at the notes on the latest Ooznest post, you'll see that they are attempting to add a fix for this. It didnt work in your case. Anyhow, if you would have answered, I would have suggested changing the minimumCircularRadius property to a higher value. That probably would have fixed your problem. Without seeing your code this is only a guess. Hope this info helps someone.
