User Tools

Site Tools


Translations of this page:

Sidebar

I think it, i tinker it, i make it!



—-

Recent updates:


en:tinkering:cnc:woodnameplateformontessoribedgiulio

Wood nameplate for montessori bed: Giulio

Intro

Some time ago, my friend Cristian started a job: a montessori bed for the son of our friend Teresa, Giulio.

I have decided to complete the nice work of Cristian with a name plate CNC crafted, quite a challenge because a big size of the object would have been 200 x 80 mm and i have only a small desktop CNC, the FABtotum personal fabricator.

After some “dry run” tests in order to check the real travel limit of X axis, i done the job with success.

Workflow

Designing the plate in Inkscape

  1. Designed the plate in Inkscape and placed near the origins (lower left corner), the units and the rulers are in millimeteres
  2. Selected the text of the inscription and from menu: Path → Object to Path, this convert the text into lines used by CAM software (Makercam, in this case) to recognize the areas
  3. Saved the design using: Save as… and select Plain SVG

Generating the path (GCODE) with Makercam

  • In menu select Edit → Edit preferences

  • Set the DPI to 90, as suggested for import a drawing for Inkscape (default is 75, for Illustrator)

  • Open the plain SVG saved with Inkscape

  • Select and delete unwanted object (e.g. squares used as spacers)

  • Select the inscription to be engraved, the inscription must be red

  • From menu select CAM → pocket operation

  • I have used this parameters:
    • name: scritta (translation: inscription)
    • tool (mm): 1 (this is the mill diameter)
    • target depth (mm): -2 (2 mm engraving)
    • safety height (mm): 10 (before move the tools, lift it 10 mm)
    • step down (mm): 0.25 (in each pass remove 0.25 mm of material)
    • feedrate (mm/minute): 400
    • plunge rate (mm/minute): 100

  • Select the screw holes templates
  • From menu select CAM → pocket operation

  • I have used this parameters:
    • name: segni per viti (translation: signs for screws)
    • tool (mm): 1 (this is the mill diameter)
    • target depth (mm): -1 (1 mm engraving)
    • safety height (mm): 10 (before move the tools, lift it 10 mm)
    • step down (mm): 0.25 (in each pass remove 0.25 mm of material)
    • feedrate (mm/minute): 400
    • plunge rate (mm/minute): 100

  • Select the external shape of the drawing, the border
  • From menu select CAM → profile operation

  • I have used this parameters:
    • name: taglio pezzo (translation: cut piece)
    • tool (mm): 1 (this is the mill diameter)
    • target depth (mm): -7.5 (7.5 mm cutting, for 8 mm stock is safe, the worked piece must be separated from stock using a cutter blade but it's safe for milling bit)
    • safety height (mm): 10 (before move the tools, lift it 10 mm)
    • step down (mm): 0.25 (in each pass remove 0.25 mm of material)
    • feedrate (mm/minute): 400
    • plunge rate (mm/minute): 100

  • From menu select CAM → calculate all

  • From menu select CAM → export gcode

  • Select all calculated toolpaths, export and save the GCODE file on PC. This is the complete workout GCODE and must used only after verified that the cut is small enough for the CNC

  • repeat, from menu select CAM → export gcode

  • From calculated toolpaths, select the cutout toolpath only, this can be useful to check if the tool can do the work for the entire width of the machine without triggering the limit switches

  • The GCODE export is ended, maybe useful save the makercam svg + metadata of the paths, from menu File → Save SVG file

Post process the GCODE

Now, the GCODE is available, Makercam has produced the GCODE for GRBL parser but i have a Marlin derived CNC (3DPrinter firmware derived), the FABtotum Personal Fabricator. I've written a GCODE post processor that eliminate the weird behaviour (caused from not understanded GCODEs) and optimize the working speed, accelerating the travels.

It's called MakerCAM2FABtotum and it's available on GitHub.

It's a Linux bash script but you can run it also in Windows, in FABtotum wiki there is an example.

For processing the produced gcode, for example you can do:

# ./post_process.sh input.gcode 12000

And the script produce an optimized GCODE with a configured spindle speed @ 12000 RPM.

Now you can then load the _postprocessed.gcode files into the FABtotum object manager and use it for milling.

I have run the cutout only GCODE for first in order to check if the tool can do the work for the entire width of the machine without triggering the limit switches; the cutout job is the largest job, the other job may go well.

Photos

Resources

en/tinkering/cnc/woodnameplateformontessoribedgiulio.txt · Last modified: 2015/11/07 02:39 by alessio.cavalieri