Skip to content
Snippets Groups Projects

4. Practical Applications

Last edited by francisco

Content

Several programs have been set up in mods for use as part of the most common digital fabrication techniques, including:

  1. Cut (vinyl)
  2. Cut (laser)
  3. Mill 2D
  4. Mill 2.5D

This tutorial focuses on 2D milling and demonstrates how mods can be used end-to-end.

@TODO: Prepare tutorials for the other techniques.

PCB milling

One of the first HTMAA and Fab Academy assignments for which mods proves very useful is making an in-circuit programmer during the Electronics Production week.

There is a set of mods programs that aid you in the process:

  1. Generate toolpaths and G-code file 
    machines / G-code / mill 2D png
  2. Generate toolpaths and G-code file and send commands to a machine 
    machines / Roland / mill / MDX-20 / PCB png
machines / Roland / mill / SRM-20 / PCB png
machines / ShopBot / mill 2D png PCB

Notes:

  • You could generate toolpaths only using processes / mill / raster, though it is not all that useful on its own. The programs mentioned above build on it and go further.
  • There are svg flavors of most png programs.
  • The industry-standard, and recommended, format for PCB designs is gbr — Gerber files, instead of using image files like png. Make sure to learn how to generate and handle Gerber files in the Electronics Design week, keeping in mind that mods does not currently support importing Gerber files.

Part 1: Generate toolpaths and G-code file

In mods, open the program (not module) machines / G-code / mill 2D png then follow these steps, where each refers to a module requiring your input:

  1. read png

    This is straightforward. You can use any PNG's or use the ones for this particular exercise (download here). Just pay attention that the resolution (dpi: dots per inch) value is preserved when you upload it so as to maintain the correct dimensions for the design.

    A chain of modules will then turn the image into black/white, among other steps, before vectorizing it. The output will be fed into a toolpath generator.

  2. mill raster 2D

    The toolpath generation algorithm will treat white as high (material is kept) and dark as low (material is milled away), and will offset paths from light to dark.

    Here is an overview of the available settings:

    @TODO: Add visualizations where necessary.

    • tool diameter

      Values recommended for flat-end mills:

      • 1/64 (0.0156) inches or 0.4 mm — for isolation (traces).
      • 1/32 (0.0312) inches or 0.8 mm — for cutting edges.

    • cut depth

      How much the tool mills away in the Z axis in one pass.

    • max depth

      How much the tool mills away in the Z axis in total.

      Should be equal to or larger than the cut depth. If they are equal, there will be only one Z axis pass in total with the depth value specified. If max depth is larger, the total number of Z axis passes will be passes = ceiling(max/cut).

    • offset number

      How many times the tool should mill around the original traces. The higher the number, the more time the mill job will take, but the better the margin between traces will be (assuming the design allows for it).

      Minimum value is 1. Recommended value is 2 to 4. A value of 0 means everything apart from the traces will be milled away.

    • offset stepover

      How much the toolpath goes further away from the original traces after each round it makes around the traces, assuming the offset number is larger than 1. The stepover is expressed as a fraction of the tool diameter.

      A value of 0 means the tool will go around along the same exact path each time. A value of 1 means it will go out a full tool diameter, i.e. there will in theory be no overlap between any given offset round and the one before/after it. The recommended value is something in between to balance between a nice finish (the lower the stepover, the smoother the surface finish) and time (the lower the stepover, the more time it will take to mill away the same amount of material if compared to a higher stepover). Expressed mathematically:

       m = d * (1 + (n - 1) * s)

 given n > 0 and where:
 	m: total distance milled away measured from edge of traces
 	d: tool diameter
 	n: offset number, integer greater than 0
 	s: offset stepover, fraction between 0 and 1

    • direction

      climb vs. conventional

    • path merge

      @TODO: investigate

    • path order

      @TODO: investigate

    • sort distance

      @TODO: investigate

    Once done, do NOT click calculate just yet.

  3. path to G-code

    Settings (pay attention to the unit being mm/s):

    • cut speed

      X-Y feedrate when cutting.

    • plunge speed

      Z feedrate. No distinction between cutting and not cutting.

    • jog speed

      X-Y feedrate when moving around without cutting (aka rapid feedrate).

      @CONFIRM: This number is actually not reflected in the G-code (or does not take effect even if it was). The machine will go at a predefined rapid feedrate that is part of the machine settings and has to be changed there.

    • jog height

      Z height when moving around without cutting.

      Too low and it may scratch the material if it is uneven. Too high and it will travel distances further than it needs, which leads to more time. Usually 3-5 mm should be fine.

    • spindle speed

      Self-explanatory.

    • tool

      @TODO: investigate

    • coolant

      Makes a difference only if your machine supports coolants. Otherwise, it will be ignored.

    • format

      Units. Make sure you choose the correct option used in your designs and mill settings.

      Feedrates in this module are not affected, as they are only in mm/s.

      @TODO: Check the above and also consider moving this option somewhere more suitable.

      @TODO: Check if jog height is affected by the unit picked here.

    Now you are ready to click calculate to generate the paths!

    After a few seconds, a .nc file will be downloaded, which you can then load into the software that comes with the machine or a tool such as UGS (Universal Gcode Sender) to send G-code to a connected machine.

    Or you can use mods to do that.

Part 2: Send commands to a machine

Background

It is common practice for most digital fabrication machine manufacturers to provide their own, mostly proprietary, software to operate their machines. Desktop software assumes that the machine being operated is connected to the same computer via a serial port (e.g. USB) or to the same network via Ethernet or WiFi.

For mods to bypass/replace such software and talk to the machine directly, it has to:

  1. Have a connection with the machine

    Given that mods runs in the browser (client side), it does not by default have access to low-level hardware such as serial ports, for security reasons. One way to overcome this is to have a tiny webserver which does have access to serial ports and send messages from the client side to the server side via websockets.

  2. Send commands in a format the machine understands

    G-code is one of the standards, but it is far from sufficient to run a machine. Here, again, most manufacturers choose to keep documentation proprietary.

    Through special agreements with a set of manufacturers (@CONFIRM), mods has implemented interfaces for the following machines, each of which having its own module/program:

Connecting to a machine

Assuming you have set up a local instance on the computer connected to the machine:

  1. Open a terminal window at the root directory of the mods repo then navigate to the js directory and run the relevant webserver.

    cd js
node printserver.js
# OR 
node serialserver.js ::ffff:127.0.0.1 1234

    @TODO: Add more details about which script is for which machine.

  2. Back to mods in the browser, open a program that allows you to connect to the desired machine. The names of such programs typically end with connect.

    machines / Roland / mill / MDX-20 / PCB png
machines / Roland / mill / SRM-20 / PCB png
machines / ShopBot / mill 2D png PCB

    @TODO: Add more details about which script is for which machine.

  3. Open a websocket to the server

    In the program you just opened, look for a module that allows you to enter an address and a port. Each program may use a different module for this, but the module will typically have the word WebSocket in it, e.g. WebSocket print, WebSocket device, WebSocket serial.

    Here is a list of all available settings (each module has a subset of this list):

    • address

      Enter 127.0.0.1 if you are running the main mods server (http-server) and the websocket server(s) on the same computer. If not, enter the IP address of the machine running the websocket server(s).

    • port

      Enter 1234 or whatever value you specified in the first step, i.e. node serialserver.js ::ffff:127.0.0.1 1234

    • serial device

      • Unix-based OS: something similar to /dev/ttyUSB0 or /dev/ttyACM0. One way to figure out which port is by running dmesg | grep tty. Note that sometimes you have to enter the entire name (including /dev/) and sometimes it is taken care of for you.
      • Windows: e.g. COM3. Use the Device Manager to figure out what port your machine is using.

    • baud rate

      @TODO: investigate

    • flow control

      @TODO: investigate

    Once done, click Open. The status field will show opened, if successful, or an error message.

    Depending on the program, a button that says waiting for file will turn into send file when the workflow has executed and there is data to send over to the machine.