Indie game storeFree gamesFun gamesHorror games
Game developmentAssetsComics
SalesBundles

PixelCNC: Handy 3-Axis Mill/Router Toolpath Generation For Images!

A radical new CAM program for CNC artists to generate original and interesting toolpaths from 2D images! · By Deftware Industries

Roughing and Finishing Pass

A topic by billb0169 created Mar 03, 2018 Views: 81 Replies: 2
Viewing posts 1 to 3

Was wondering how to rough out large areas with a larger end mill then do a finishing pass with a smaller one?

Developer

Hi Bill,

For roughing you could setup a horizontal operation with a step size of half the tool diameter, a cut depth from 1x tool diameter to about 2x diameter, depending on the actual flute length and the tool size/project size. The horizontal operation in the current public release is a bit temperamental, and has issues with smaller cut depths. I'll be releasing v1.15a sometime this next week which has a lot of the problems with the horizontal operation resolved. So far it's still not quite 100%, but it's pretty close, maybe 98-99% reliable, while previous versions are more like 75-80%. In the 1% case where it does break, it at least won't crash the whole program anymore, so that's good. If you do encounter a problem with the horizontal operation usually tweaking your step size and cut depth values, by a small amount like .05", can make all the difference.

Otherwise, you could setup a parallel operation and set the step size to ~75% of the tool diameter, and the cut depth to the same you'd use on the horizontal operation. Be sure to use the 'mixed' cutting direction, so that you're not spending time moving the tool back to one side of the project. That way it will just zig-zag back and forth across the whole thing in one long cut. The conventional/climb options are there for finishing passes, really, as they can really make a difference in the cut quality in most cases.

For a finishing pass most of the other operations will work, just set your cut depth to the same as the tool flute length. If your tool doesn't actually have a flute length as deep as your project's Z size just pretend and that will let you setup one of the 3D contouring operations (i.e. parallel/spiral/chevron/labyrinth) with a deep cut depth so the tool will be able to reach the bottom of the project without having to make successive passes of flute length depth.

If you don't know already, be sure to use good speeds and feeds that won't cook the material or wear out or break your cutters, there are online calculators that can help with that. I'm thinking about integrating an 'auto speed/feed' button to operations which will look at tool flute count and everything else.

Once PixelCNC no longer has new features being added and it leaves alpha to enter beta I will get a step-by-step how-to guide going, as the existing guide is more of a reference that just documents the interface. If I took the time to write one now, with PixelCNC still evolving somewhat, I'd have the extra work of updating and revising it. There's already plenty of work to do just on the software side, especially now that PixelCNC is available to paying customers. I'm going to spare myself the added work just for the duration that PixelCNC is in alpha. Once we're in beta all that's really left are bugfixes and minor changes, so I'll be able to focus more on marketing, promotion, and all the peripheral stuff like tutorials and demonstration videos.

Developer

By the way, setup both of your tools and operations in one project and if you want to export separate G-code files for each operation (i.e. if you need to do a manual tool change) you can set which operations to include/exclude in the outputted CNC program by clicking the little pencil icon in the operations list next to each operation (when in 'operations' mode). This toggles whether or not the operation will be included when G-code is exported. This is useful for smaller CNC machines that don't have automatic tool changing capabilities.