Finally got my Nomad up and running, and after doing the tutorials, I used Meshcam on a project and instead of using the toolpath wizard I selected my own settings because I thought it might be better to use 3 different bits and wanted to select them. However, my results were not smooth; and I assume it’s because my settings were not ‘High Quality’. How do I guarantee smooth results when creating my own toolpaths like the wizard?
Lots of things come into play. I am presuming that you were going for a smooth, flat surface rather than a scalloped surface. A better idea of what you are trying to accomplish would make it easier to address, but I’ll take a stab.
If that is so, then I would use a flat end (square end) bit for most of the job. A ball end will never give you a flat surface.
Where you must use a ball end for a flat surface (such as on an angled face), the distance between passes determines how smooth/flat the result is. The height of the scallops is a function of the diameter of the tool and the stepover. For a stepover of 1/2D (where D is the diameter of the tool), the scalloping will be roughly 7% of the diameter. A stepover of 1/4D gives about 1.5%. If your tool is 0.125" diameter, and the stepover is 0.031", the height of the scalloping will be 0.002". Your stepover appears to be a lot more than that. On an angled face, the net step along the surface is often a combination of machine stepover (parallel to the X-Y plane) and depth of cut (advance of the tool along Z), and you need to adjust these in combination to get the finish you want.
For example, machining across a 45 degree slope with a 0.125" ball end, to get the 0.031" effective step, I might step over 0.021" and down 0.021". (By the magic of Pythagoras, I find that I get sqrt(0.021^2+0.021^2) = 0.030, for a scallop height of just under 0.002") This is done automatically by some CAD/CAM packages. I do not know if MeshCAM can do it. Note that the parameters vary with the direction you are cutting relative to the slope.
When using a ball end, use the largest you can to get flatter/smoother surface. Only use a smaller one where you must, and reduce the stepover correspondingly.
When you do most of the work with a larger tool that won’t fit into all of the corners, you need to take consideration of what the remainder (called the ‘rest’ in many packages, to be followed by ‘rest machining’ t clear it) will be, and how to get to it without making a mess. There is no easy answer here. Waterlining is a very good technique, but can lead to chow if the prior work didn’t get uniformly into the corner. You have places where that occurred (the scallop tops versus the bottoms where the waterline pass went). If you plan to waterline with small tool to get a crisper edge, run the larger tool first to reduce this.
Another issue I see (I presume this was not the intent) is the tool moving through already cut ares (such as the diagonal move across the ‘I’). This can be avoided by selecting the surfaces to machine or avoid during a particular operation, and being sure that your clearance height is sufficient. Sometimes this means breaking up a single operation into several to force the software to lift the tool. Again, it varies with the particular software, strategies used, and work being machined.
If this is not addressing your issue,then more information is needed, such as: what tools are you using? What is the desired result?