Home : Workshop : CNC :


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

Carving AutoselectUsing Automatic Functions : Create objects automatically (autoselect) and selecting the "Carve inside only" option works pretty well for text - minimal path additions/deletions needed. Unfortunately the carving options do not include weighted inside/outside options, e.g. the weighted "Create holes and parts" example. The easiest way to get the same results when carving between the lines is to use the "Carve inside and outside" option. Unless its a real simple drawing, autoselecting and deleting unwanted paths is significantly faster than manually creating the paths. To get the same paths in Easel use perimeter pockets constrained with 0 height island pockets.
[ comment | link | top ]admin

Carving Raised Text

Carving Raised TextA few tips based on my first attempt. In a nutshell, getting this to work well depends on the 'Carve pocketing tool' diameter and the 'Depth limit' setting. When using a pocketing tool it's the 'Maximum [pocket] width' to the right and left of the letters - 99 would be fine (the default is tool diameter).

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 ]admin

Tool Length Sensor

Tool Length SensorAs with any Estlcam probe function, the probe plate can be a simple piece of aluminum (tape) attached to the probe wire. Using the one click automatic tool length measurement function speeds up and simplifies tool changes, no probe menu navigation or manual touch off required. While a 3-axis probe plate makes a handy sensor, a spoilboard mounted sensor is needed if the surface of the material will be machined away.

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 ]admin

Center Origin

Center OriginA center origin is used when you want to center a project/drawing on the material being cut. It's easy if your drawing has a center point mark (Zero/origin first 2 options), but there are a lot of shapes (3 shown) that have a circumcenter (three point/triangle circumcircle center) which makes for a pretty flexible third option... which could also be used to find a close to center point on irregular shapes.

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 ]admin

Autoselect and Layers

Autoselect and LayersEven on simple projects, having CAM programs auto-select cutting paths can be hit and miss. If the project involves more than one type of cut, e.g. inside and outside of the line, auto-select will be weighted to one or the other and paths will probably need to be edited. Easel auto-selects by default and provides three unweighted options (in/out/on) when importing a drawing. Estlcam auto-select is optional, includes more cut types (e.g. drilling) and the multiple (de)selectable options are weighted (e.g. image) / constrained (e.g. holes under/over a specified size get drilled/routed). Unlike Easel, Estlcam can read DXF layers which makes (auto-)selection so much easier.

Autoselect and LayersThis example image is a layered DXF generated by the BeeHome project and imported into Estlcam. The layer names provide all the information needed to auto-select (e.g. weighted inside/hole) and set the parameters for cutting the paths (bit size, cut depth and pocket). I spent a whole lot of time on just one part of that DXF trying to edit all the paths in Easel before deciding it was just too tedious for a one off project.

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 ]admin

Estlcam VS Easel

...Most of what I post in the Estlcam category will have some Estlcam VS Easel aspect. Both are CAM, G-code senders, and motion control packages and I spent a lot of time with Easel before switching to Estlcam. While Estlcam has a lot more advanced features than Easel (...I see Pro finally has ramping), the interface is not as clean/intuitive as Easel and v-carving text is easier with Easel (...but it's now subscription based and Inkscape to Estlcam is actually pretty easy).

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.

Estlcam VS EaselWhile Estlcam will cut into the adjacent line if the space between two lines (e.g. text) is smaller than the bit, it can cut to the right/bottom or left/top of open paths, e.g. lines. While this is a very useful feature, e.g. being able to cut a shape on the end/edge of a board, it has some bass-ackward constraints.

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).

Estlcam VS EaselAnother area where Estlcam and Easel differ is when cutting pockets. The example is a complex maze and both programs were set to cut parallel/offset (Estlcam changed/Easel default). Both generated paths that jump around a lot and it isn't obvious which moves around more. Both appear to use an ~40% stepover, but Estlcam leaves an ~20% path around the perimeter. While this does result in an additional path in some places, that 20% path is cut last - no finish pass required... Side note: Estlcam set to parallel provides the best results on narrow pockets, but the algorithm is too conservative/safe, i.e. too many unnecessary and time consuming passes... because parallel stepover is limited to 45% (regardless of bit settings).

Estlcam VS EaselThe Easel generated path includes some full width cuts along the perimeter (more likely to leave wall marks and top tearout). While both can leave islands (which can break and tear grain) and it would be nice to see everything cut from center out, Estlcam saving the perimeter for a 20% wide final pass is a big plus.

[ comment | link | top ]admin

Estlcam Screen Rounding

Most on screen number entries in Estlcam are rounded to two (mm) or three (inch) decimal places and the common assumption is that Estlcam is storing/using the rounded numbers. The rounded on screen numbers do not appear to be stored or used by Estlcam. Many of the numbers Estlcam stores/uses appear to have sixteen decimal places. To see some of those numbers view the 'Settings CNC... .txt' file in 'Program Data Estlcam...' (set show hidden files in Explorer if Program Data is not visible).

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 ]admin

Back to: CNC