Estlcam
Estcam contains CAM and CNC motion control programs. Vector graphics (dxf and svg) and 3D (stl) files can be imported and machined using Estlcam. While doing everything in Estlcam is the simplest and most reliable route, the programs can be used individually to generate G-code for another controller (GRBL, Mach3, etc.) or to machine G-code generated by another CAM program (Vectric, Fusion 360, etc).
The Estcam motion control program is easy to install on a lot of ATmega microprocessor/GRBL compatible hardware (e.g. Uno/Nano) and Estlcam will backup anything currently installed on the hardware. If the hardware isn't recognized, USB drivers may need to be installed (drivers for FTDI or WCH serial chips are the most common). See also: Hardware
The Estlcam control program is free, the CAM program is free to try (becomes nagware w/ increasing wait times to generate/machine G-code) and ~$60 to buy.
The following topics are pretty random and most are incomplete snippets, questions and comments are welcome.
Carving Autoselect

[ comment | link | top ]

Carving Raised Text

The main window is only vaguely helpful with the pocketing showing up as gray. The Preview window is much more useful, it shows the paths and how much of the pocketing needs to be done by the V-bit (smaller stepover, e.g. 5%, and lighter blue)... Tweaking/previewing larger signs requires some processing power and can be slow.
[ comment | link | top ]

Tool Length Sensor

To setup the sensor go to Setup : CNC controller : Length sensor. I use a speed of 60mm/min for all automatic probing functions. The fixed location option requires homing be enabled. Locating (mounted or not) the sensor relative to the project origin/0,0 point is also possible.
Warning: Unlike other probe options, the Z-axis will start moving when you click the icon. When you move the tool over the sensor and click the icon, the tool will automatically travel down, touch and retract. After the first touching off of the tool length sensor, the material top also needs to be touched off/zeroed. After that the sensor will automatically adjust the Z-axis zero point after tool change sensor probes. Note: 1) After a sensor touch off, Esc does nothing and the message will only go away when you do something else. 2) The default 6mm/min speed is typo - super slow, pretty much undetectable (v11.244).
A 3-axis probe plate works great for one-off projects where the corner won't get machined away. With the tool a bit in from the corner (wherever you normally start a 3-point probe) start by clicking the length sensor icon. Do the 3-point auto probe after and you're good to go. After tool changes go to that 'in from the corner' position, slide the probe plate in position and click the length sensor icon. To have the machine automatically go to that 'in from the corner' position for tool changes, add G00 coordinates (e.g. G00 X15.0000 Y15.0000) to Setup: program : text : tool length.
[ comment | link | top ]

Center Origin

You can either mark the center of the material and manually center the bit/zero X/Y, or use the Estlcam center probe options to precisely center the bit and automatically zero X/Y. Note: The probing options work on parts/outside and holes/inside, e.g. zero probing inside and outside corners. Probing at 45 degrees also works and can be handy when probing circles.
[ comment | link | top ]

Autoselect and Layers


10-23-21: While Estlcam can lock/unlock DXF layers to allow (auto-)selecting paths by layer, running auto-select multiple times (e.g. on multiple layers for multiple bits/DOC's) requires locking the already selected/configured paths and the layer so that they don't get modified or re-selected on subsequent runs.
Since it took me a while to get it:
The View : Layer list : layer lock only prevents the creation of (new) paths on that layer.
The Edit : Lock only prevents the modification of already created and selected paths.
Note: There is no need to 'unlock all' and there seems to be a bug (v11.244) where hole/part paths can revert to on line when unlocking all.
Using layers makes (auto-)selecting easy and reliable, great for any project with any combination of cut types and bits/DOC's.
Depending on the project, I use Autosketch or Inkscape for creating my layered DXF files... Because I find Inkscape easier for text and Autosketch easier for geometry, I've found a use for the Estlcam File : Insert option which adds the inserted file as a new layer. The bottom-left of inserted DXF pages (not the drawing) will register with the Estlcam default (bottom-left) origin point. The top-left of inserted Inkscape SVG pages (not the drawing) will register with the Estlcam origin (seemingly regardless of the SVG page origin). I was registering inserted SVG's by fiddling with X/Y coordinates (Move DXF) until I discovered that inserting saved as v14 DXF removes that hassle. Note: The "Insert"ed origin is the page corner, the "Open"ed origin is the drawing corner.
[ comment | link | top ]

Estlcam VS Easel
One of the key functional differences between Estlcam and Easel is that Easel can only cut inside/outside of a closed line/path (e.g. a circle). Any shape with ends that don't meet (e.g. a line) can only be "Cut on shape path". I'm guessing that the closed line restriction/awareness is why Easel will never cut into an adjacent line (on the same closed path). Any irregular pocket cutting (e.g. text) with a straight bit is affected. If the space between two lines is smaller than the bit, Easel won't cut it.

The default is bidirectional cutting. While bidirectional cutting is fast and efficient (great for roughing) any machine/bit flex will create noticeable ridges on the cut face because each pass will flex the machine in the opposite direction, i.e. not ideal for hobby level machines.
The solution (when one side of the cut is waste) is to add a finish pass to right or left of the line cuts. It's not a very efficient solution because both the roughing and finish pass cuts are unidirectional. While less than ideal, the loss of bidirectional roughing would be acceptable if the configured cut direction settings were honored, they are not.
Right of the line cuts are always climb cut and left of the line cuts are always conventional cut (both cut bottom to top, top and bottom of the line paths are cut right to left). The cut direction workaround is to manually set the point to point path (1st point = cut start). There may be some logic that I am missing because I've only used the engraving function for edge cutting (edge > cut > waste).


TBC
[ comment | link | top ]

Estlcam Screen Rounding
While entering something like 8.016mm for X-axis distance per revolution will be rounded to 8.02 on screen, the stored/used number will be 8.0159997940063477. I have no idea where that number comes from, but it is only off by .0000002mm. For a frame of reference, the rounded .004 difference divided by 20,000 equals the .0000002 stored/used difference.
[ comment | link | top ]
