Guys, I have been reaching out to Spark Concepts the makers of this board, Ooznest the supplier and Vectric software to try and resolve an issue I am having. I am new to CNC and have built my own C-Beam kit that was supplied from Ooznest. I initially tried to use Inkscape along with Makercam but found this far to complex, probably okay for some but for me it didn't work. I then purchased Vectric Cut2D and then realised I should have purchased VCarve instead. Needless to say Vestric wasn't very sympathetic to my error and found myself with two pieces of Vectric software. I have followed a tutorial from the Vectric website that involved creating a simple double sided box. The resultant toolpaths from following along with this tutorial is where it all goes wrong. X and Y axis appear okay but the Z axis appear to have a mind of its own and plunges deep into the workpiece and into the spoilboard. Carving simple names and profiles appear to work okay, but in honesty I haven't carried out extensive test on either but first test runs appear okay. Pocket toolpaths appear to be the issue and only on the Z axis. My first question is, is anyone using Vcarve or Cut2D with the Xpro V3 software on a Windows 10 machine? Second question. Anyone have any ideas what could be wrong?
I've used Vectric software alongside xPro controllers. I also took a quick glance at that tutorial. The basic problem you are having likely has to do with how you are aligning your Z-axis. Vectric has two options for z-axis zero. You can tell it that at Z=0 the bit is at the very top of the material. In this case, all machining happens when Z is negative. So if your piece is 10mm thick, the cut will happen between 0 (top of workpiece) and -10 (spoilboard). The other option is to tell it that Z=0 is on the top of the spoilboard. Here all machining happens when Z is positive and Z should never ever go negative on a normal job. On a 10mm thick piece, machining will happen between 10 (top of workpiece) and 0 (spoilboard). Either way works. And the tutorial mentions the idea of using one option for one side and the other option for the other side. But if you do this, it is crucial that you reset your Z-axis zero accordingly when machining. If you set the software one way and the actual machine the other, you will either be cutting entirely in air or cutting deep into the spoilboard. For me, I find it best to set '0' to be the spoilboard and keep it consistently that way no matter what. In this way, homing switches can be used to ensure that you only have to set it again when you change bits rather than with every new job or when you reset the machine. Best of luck. -D
Thanks for that, I understand what you are saying. being a bit thick here. If you have your bit on the spoil board can you get it aligned with the end of the workpiece? Are you saying that your bit is never directly over the work piece and that you butt up your work piece to the cutting bit? Sorry can't visualise how it works
There are a lot of options on aligning your workpiece and finding a 'zero'. But if you don't have homing switches, your best bet is to have Z=0 on top of the workpiece and jog the workpiece to a known corner with every cut. The downside of this is that it takes a lot of time and it isn't very precise. You can do two-sided machining like this, for example, but not where precision alignment really matters. If you have homing switches, a lot more options open up. With homing switches, you can have the same coordinate system and re-use it indefinitely. For my case, my vectric layout files always look basically the same. The 'material' is a square as wide and tall as my actual working envelope is. And if I draw or import a file and move it to a location, it will correspond to that real location on my machine. I have a series of stops along the top and right edges and just push the material up against them and fix it in place. So I just need to make sure that whatever I am cutting out is located relative to the upper-right corner of that material box and is smaller than the piece of stock. I used the machine itself to cut holes for the stops. So I know that the stops are aligned according to the machine's own coordinate system. However, there are a ton of other ways to go. For example, you can have the CNC machine drill holes at known places and put pegs or locating pins in them. Some people cut a regular series of holes in their bed or use aluminum plate with threaded holes in order to be able to precisely set up operations on any part of their machine. You can even set up jigs with precise cutouts and clamping to do a particular kind of job. For example, my stops are too widely spaced to be useful engraving a small 50mm x 50mm piece. But I could get a larger piece of material and cut out a 50mm x 50mm hole at a known spot. Then I could align the larger piece against the stops and place my 50mm x 50mm piece at the precisely located point inside it, clamp it down, and start engraving. Anyhow, there is a trade-off in all of this. If you are mostly cutting out of the same kinds of materials, or cutting the same kinds of jobs, you can create jigs and stops to make each one quicker to do. But if every job is completely different or is irregularly shaped, then the jigs and stops are probably not worth the initial effort since they would only ever be used once. -D
