Hi Folks, I've been having an issue recently with the openbuilds control software and Blackbox. When running a gcode written by Fusion that has more than a few separate steps the controller will at some point ignore the feed speeds programmed in and start moving the bed really fast when it has a straight line. Around corners it slows down but then goes max speed. If I separate out the program, do three or four steps at a time and save those into individual .gcode programs it will run fine at normal feed speeds. I've attached a photo of the program as well as the gcode. Any help appreciated. Gcode located on the Facebook group here: OpenBuilds® CNC Machines and Products
If the forum won't let you upload a g-code file just rename it to a *.txt file, and please upload your Fusion file also. Alex.
Fusion file also please. You can export a Fusion archive file to your computer and upload it from there. Alex.
Heres the fusion F3d. I did edit it since the export to gcode so it's not the same. The speed went nuts at operation 11 on the original file. https://drive.google.com/file/d/1A_YuDVvAlHbg2nTxAzr91By9A7b_CKW7/view?usp=sharing
Your feedrates in the Fusion file are all low, so nothing there that I can see. Your g-code file only contains 9 operations. There are G0 moves after G2/3 moves, but the ones I found were only short movements - most fractions of a mm and a few of a mm or two. If you still have the g-code file that has 11 steps post that here and then hopefully someone like @David the swarfer can have a look at it. Alex.
Yes, I see the problem. I need that Fusion file so I can debug the post. Somehow that operation (and its specific settings) is confusing the state machine and preventing a switch from G0 to G1 moves, hence the rapid motion hmmm, operation 'second top clear' essentially does nothing but it has a clearance height of 7 while other operations have a clearance of 15, in fact there is a confusing array of clearance heights. will dig into it tonight.
@illumiquest I have pushed a new postprocessor version, please upgrade to V1.0.29 and test. (not a release yet, so grab the zip file) Link in the footer of all my postings (-: However, that drilling operation in the middle of the milling bothers me. Milling bits are not drills. Much better is to give the previous op some radial offset (negative in this case) so it clears that boss with a real cut, and the drill op is not needed at all. (and you do know that hole in the boss is drilled offcenter, right?) You also want to add in lead-outs for most operations otherwise the bit will leave a mark when it retracts, and on the final cuts you do not want to start in the middle of a straight section with a plunge, ramp in and out or use a start point on the tip of the hand where it will not leave a mark. Since your bits are so small, make sure that 'linearize small arcs' is ON, which the default in this new version of the post. You will have seen the warning messages about GRBL having a minimum feedrate of 45mm/min. While that is a slightly flexible number (depends on several internal settings) if you have any strange behavior fix those feedrates first!
