Here’s a tip for just about any cutting or etching CNC process driven by sheetcam toolpaths, but in my case its usually for plasma…
As more of a frugal hobbyist than a business metal shop, I find myself saving and later using many remnants rather than full, 1/2, or 1/3 sheets. Often times I have a remnant sheet that presents a close fit for a toolpath (Part). If the Part will tolerate it (as in artsy/crafty), I scale it to fit, either in CAD (Lightburn) or Sheetcam (right click Parts window, select Scale). But the bigger challenge can be, depending on size, getting at least 1 straight edge of the remnant sheet exactly square with XY on the table. Sheetcam has a feature to make this task easy peasy. menu Mode-Align. This feature relocates and rotates a Part on the XY drawing grid using 2 points. Make sure you have menu View-‘Show segment ends’ ON, the segments ends are the ‘points’ we’ll reference using Mode-Align.
Here’s how the process works…
For an easier visualization (or demo) of this, clamp your material to the table such that one straight edge is obviously askew of parallel to X axis (usually the gantry). By obvious, I mean make it at least 10mm askew to parallel. I like to use front (bottom of drawing) left corner as my X0Y0 origin in sheetcam, and thus on the table. Now-
- zero XY to the front left corner of the material straight edge to match your drawing origin.
- jog X to the far right end of the material. Don’t jog Y, leave Y on 0, just jog X. It should be off the edge of the material +/-10mm (as noted above) on the Y axis, that’s intentional for this demo. Note the controller digital readout (DRO) as to the distance X has traveled from X0 (the front left corner of material). Now jog Y so that it is aligned over the edge of the material. Note the DRO of Y.
- use sheetcam menu Mode-Shape to draw a rectangle (or line) if needed where X dimension is the value of X coordinate from step 2. The Y value of the rectangle is not relevant. If your Part has a bottom straight edge, great, use that dimension when jogging X and there is no need to draw a rectangle (or a line). Position the drawn rectangle or line such that the bottom left corner is on X0Y0, drag it with the mouse while in Mode-Shape before or after adding it to the current Part (must be in Mode-Shape).
- Now were going to align the Part to the material on the table. menu Mode-Align. Right click on the drawing, select ‘Alignment tolerance’. Use a value 2x the distance of the Y DRO reading, that is, 2x the askew amount to be safe. Now click the first alignment segment end, the node on X0Y0, a popup window will present with the coordinates of that node, just press enter to confirm it in this case, or you can enter a new coordinate in which that node and the Part will move to. Now click the second alignment segment end. On this coordinate window, enter the Y value from the DRO. This will rotate the Part on the first node landing the second node on the Y coordinate, provided the rotation is within the radius of the afore ‘alignment tolerance’ distance.
Done. The Part is now aligned to the askew material clamped on the table. There are easier variants of this process if you plan ahead and draw the X axis alignment line or rectangle in CAD and anchor it to the bottom left corner of your Part, or if your Part has a bottom straight edge, just use it.
Another variant is using a CAD with overhead table camera feature, such as Lightburn (LB). With LB, I just throw some remnants on the table, project the image on the CAD grid, and visually check if my Part(s) fit, and use it’s rotate feature to align the Part to the material, then it’s baked into the DXF. In this case, LB has code that factors out the distorting lens optics of the camera such that the image is within 1mm of true material dimensions.
update: Another use case for Mode-Align, perhaps a more important one, is repositioning material on the table for continuing a job in cases where the material sheet is larger than the work area. I run into that use case from time to time. After shifting the uncut material into the work area of the table, use 2 points from the previous [sub]job to re-align the ‘Part’ to a partially cut toolpath if needed. You’ll want at least 0.5mm of overall accuracy (not afore mentioned ‘alignment tolerance’) for such a re-alignment. Replace the torch nozzle with a used nozzle with a toothpick glued into it, to use a pointer. Know your alignment target, it will usually be contour edge since you are using a node on the contour in sheetcam, however, if the contour is an open shape, then the toolpath is likely ‘No Offset’ from the contour and you’ll have to bump XY so the torch pointer positioned 1/2 the kerf to adjust.
I hope this helps with your plasma job setups.