When I transferred my tool path from Vcarve to do a photo using the openbuilds software I was expecting a carved photo might appear on the blank that I had setup on my machine. The first thing that happened was that the bit almost drilled through the 5/8" blank and then stalled. I rechecked all the settings in Vcarve, re-did the tool path and the same thing happened, just at a different start point. One more check and the simulation seemed to be transposed to the upper right corner (instead of being in the centre) and once again the bit dug in to almost the bottom and I aborted the job. So, at this point I am lost as to what to check next. The maximum depth of cut was set at .025 inches, the bit was a 1/4" 60 degree carving bit, and the tool was referenced to the bottom left corner, surface of the job. Can any one shed some light on what might have gone wrong - especially the plunge depth?
Did you remember to SetZero so the machine knows where the stock is. Remember to set it in the same spot that you have Origin set in CAM
It is probably what Peter mentioned above and I know you checked your settings, but Vcarve gives you the option of setting zero on the spoil board or on the top of the work piece. Things can go horribly wrong if you do not realize a setting got changed prior to generating your gcode. In my case I normally zero on what would be the spoilboard but since it was a rotary project that is "center of cylinder". Somehow the setting got switched to "surface of Cylinder". When I started the job, the endmill plunged all the way down through the stock piece to the center of the material thinking it was the top. That wasn't so bad... until the rotary engaged and snapped the endmill. I need one of those E-stop buttons we often talk about on the forum.
I just did the same thing this week on a flat part, except in my case it was because when I was setting up the tool table, it was only taking Y offsets and not Z heights, because the stupid little radio button was in the wrong place because I'd probed in a different order than usual. So I had three tools in holders with apparently zero height. Luckily the Z motor driver cut power before it carved a hole through the vise (closed-loop! ). Still lost the 1/4" end mill though. There's always something! In this case, stock probing seems more the issue, though it might be worth posting the first few lines of code just in case there's something weird.
Regarding the set zero response. I set the origin of the work at the bottom left corner of the blank (x=0, y=0, z=0) all three times - that was the origin also set in Vcarve. Before starting the job, i moved the bit to a random point and tested it to see that it would return to origin, and it did. However, when the bit got stuck in the wood from plunging too deep, perhaps the origin of the table top was screwed-up in all three dimensions. Would that have caused the bit to repeatedly plunge too deep? I have attached a snippet of my gcode starting from the first line. T1 G17 G20 G90 G0Z0.2000 G0X0.0000Y0.0000 S16000M3 G0X2.1456Y3.2048Z0.2000 G1Z-0.0191F15.0 G1X2.1418Y3.2086Z-0.0167F45.0 G1Z0.1000 G1X2.1417Y3.2658 G1Z-0.0118F15.0 G1X2.1493Y3.2582Z-0.0094F45.0 G1X2.1608Y3.2467Z-0.0189 G1X2.1723Y3.2353Z-0.0174 G1X2.1799Y3.2276Z-0.0144 G1X2.1952Y3.2123Z-0.0178 G1X2.2029Y3.2047Z-0.0148 G1Z0.1000 G1X2.2593Y3.2054 G1Z-0.0159F15.0 G1X2.2554Y3.2093Z-0.0170F45.0 G1X2.2476Y3.2171Z-0.0079 G1X2.2437Y3.2210Z-0.0084 G1X2.2359Y3.2288Z-0.0149 G1X2.2281Y3.2366Z-0.0144 G1X2.2203Y3.2444Z-0.0126 G1X2.1931Y3.2716Z-0.0145 G1X2.1814Y3.2833Z-0.0186 G1X2.1775Y3.2872Z-0.0182 G1X2.1736Y3.2911Z-0.0153 G1X2.1658Y3.2989Z-0.0158 G1X2.1619Y3.3028Z-0.0183 G1X2.1503Y3.3144Z-0.0136 G1X2.1464Y3.3183Z-0.0134 G1X2.1425Y3.3222Z-0.0112 G1Z0.1000 G1X2.1423Y3.3796 G1Z-0.0093F15.0 G1X2.1539Y3.3680Z-0.0107F45.0 G1X2.1616Y3.3602Z-0.0139 G1X2.1771Y3.3447Z-0.0132 G1X2.1926Y3.3292Z-0.0159 G1X2.2043Y3.3176Z-0.0090 G1X2.2236Y3.2982Z-0.0154 G1X2.2314Y3.2905Z-0.0122 G1X2.2469Y3.2750Z-0.0127 G1X2.2546Y3.2672Z-0.0185 G1X2.2624Y3.2595Z-0.0110 G1X2.2740Y3.2479Z-0.0122 G1X2.2817Y3.2401Z-0.0162 G1X2.2895Y3.2324Z-0.0127 G1X2.2934Y3.2285Z-0.0132 G1X2.3011Y3.2207Z-0.0194 G1X2.3089Y3.2130Z-0.0117 G1X2.3166Y3.2052Z-0.0133 G1Z0.1000
I’d argue that first G0Z0.2000 should be a G53G0Z-0.2000, but other than that, you say that you set Z0 to be the bottom of the 5/8” part in your first post, and that you wanted 0.25” DOC. So the Z-0.1000 and other small ramp numbers suggest that your CAM is operating from the top surface of the part. I often suggest to set feed override super low- 10-20% and watch for the plunge with some scrap stock to test. Observe what the code says and where grbl says you are in G54/work coordinates as it occurs. If it says ~0.620 on Z as you enter the workpiece, there’s your answer.
I set Z=0 at the top of the work piece so that G0Z0.2000 puts the bit at .2"above the work surface - is that not correct? I am referencing the top surface, bottom, and left corner of my work piece to start the cuts. From there it starts a ramp cut into the work piece that is about 1/2" deep and starts carving from there.
Confusion over words - most of us would call that origin point front, left, top. The g-code you posted doesn't have anything as deep as you say the machine is going - could you please post your V-carve file? Alex.
That's a gcode - Alex wants to check your actual Vectric project so see how you set up the origins etc - ie the .CRV file
V-carve file seems OK - simulation in V-carve works fine. I have attached the g-code produced by the Openbuilds GRBL (Inches) (*.g-code) post processor. Simulation in Openbuilds Control appears to work fine - I can't try it on a machine as I don't have a grbl machine. If you are still getting a plunge deep into the workpiece then it does not appear to be a software problem. Alex.
Ok, We have ruled out the obvious problems. I wil give it another try this morning to see if it works any differently. My plan is to calibrate the machine on the start point of the blank, then remove the blank and see just what happens without any blank in place. I should be able to see if it takes a deep dive as it has in the past. Rick
Just one other metric, how does the (known good) Hello World go down docs:blackbox:hello-world [OpenBuilds Documentation] May just help to have a known good basic start
Yes, this could mess up your XYZ zero point because of missing steps. Whenever you have a "crash" of some sort, assume you lost steps because the motors were not able to move to where the controller thinks they moved the tool to. Re zero after a crash.
Re-home and re-probe. The machine has no idea where it is. And remember, this... ...isn't specific to this situation, but a general troubleshooting methodology for unknown offsets.
Thanks to everyone. It worked the fourth time and I got the results I was expecting. I need to do some fine tuning of the project and other things before I produce the final product.
