I think I must be doing something wrong in MeshCAM. I loaded up this simple heart model, and cut it out of wood.
As you can see from the YouTube time-lapse (http://youtu.be/n0zgGclnXsM) , instead of doing smooth cuts around the shape, during the roughing phase the cutting looks more like a sewing machine stitching around the edge. This doubles or triples the estimated cut time because the cutter spends a lot of time moving around without cutting.
Other than setting the stock size, I think I’m using the default MeshCAM “Carbide Auto Toolpath” to generate the toolpath. Here are the resulting settings:
My original thought was that I was generating the STL file from my model at too low a resolution, and MeshCAM was keeping true to the polygon facets. I tried generating a very high poly count STL, and the results were almost indistinguishable.
Is there something obvious I’m missing?
Try it again without “3D roughing”
and or try using a bigger bit (.125). the smaller the bit the longer it takes.
i made some hearts last weekend.
Great looking hearts. What type of wood are they made from and what setup/parameters did you use to cut them?
sjg, uncheck “Use parallel path” under roughing. “Use parallel path” does tell MC to make orthogonal toolpaths rather than contour-following roughing paths.
screaminmonkey, the “3D roughing” concerns the Z plane, and MC will attempt to make smooth transitions between the levels rather than terrace-like stairsteps. For a 3D shape like this, it’s a good thing.
Randy (not a Nomad user but a MeshCAM user)
Thanks to everyone for the feedback. I tried another cut this evening, and it was definitely faster without the parallel paths. But it does still seem like it spends a lot of time doing “sewing machine” action (see http://youtu.be/UBcHWZc-Ifs), and I’m still not clear why. I’m happy with the final product output, but I’m perplexed by the way it gets there.
Here are the settings I used (except for unchecking parallel paths, it’s straight results of the Carbide Auto Toolpath wizard):
Could it be that I’m cutting too small a margin, and that MeshCAM is trying to do what I’m telling it without widening the margin?
You are fine on the machining margin. It is applied at the centerline of the cutter, so it is not “crowding” the part. I’d suggest tightening the calculation tolerance. I always use .0001" for final toolpaths, and it does make a material difference in the toolpath smoothness, especially on pencil moves. There has been a lot of discussion of tolerance over on the MeshCAM forum. It doesn’t seem to be an actual physical parameter on the part, but in some way an internal “fineness” setting. You might try .001" and .0005" first as an experiment. MC will show you the toolpaths before you write them to disk–you can visibly tell if there are less retracts as you tighten the tolerance.