ddm

RhinoCam Tutorial


Content

Jump to the topic you are looking for


RhinoCam Workflow

RhinoCam_Workflow


Setup

RhinoCam_Setup_1

Setup Document:
  1. Verify Units: go to Options > Units: make sure the document-units are set to millimeters When you create a new document: select Small Objects - Millimeters

RhinoCam_Setup_2

Locate Geometry:
  1. draw a box representing your material to check that everything fits inside

  2. make sure, that all your geometry is positioned in positive X, positive Y and negative Z Origin(0,0,0) at the top-upper-left corner of the box

  3. Setup Post-Options: select ShopBot-LVML as Current PostProcessor and .nc as Posted File Extension. You find the right PostProcessor under the following path on the server: \01_DesignStudio\01_INPUT_02 Workshops\04 CNC

  4. left-click on Stock > Box Stock

  5. define the top-lower-left corner = (0,0,0)

RhinoCam_Setup_3

RhinoCam_Setup_4


Tools

RhinoCam_Tools_1

  1. go to the Cutting Tools Browser > if it‘s not yet visible, select the menu RhinoCAM > Cutting Tools Browser

  2. you can define your own tools or

  3. Load Tool library

  4. select shopbot-toollib.csv > OK > this should load 6 tools (3,6,12mm, ball- and flatnose) to your library

  5. select the tool you want to use (we will start with the 12 mm Flatnose)

RhinoCam_Tools_2

Different results with different tools and same stepsize:
left: 6mm ballnose tool
right: 12mm ballnose tool
The result is smoother with the bigger tool!

for flat surfaces, select flat-nose tools
for slopes, select ball-nose tools
for smooth surfaces, select larger tools
for narrow valleys, select thinner tools
for fast milling, select big diameters
for fine details, select small diameters

RhinoCam_Tools_3

A) houses stand too close to each other
B) large tool (12mm) doesn‘t fit inbetween > a lot of rest material
C) ballnose tool leaves rounded edges
D) result with a flatnose tool


Machining operations

Machining Operations are different strategies to generate toolpaths - three dimensional lines in space as paths for the milling bit.

RhinoCam_Machining_1

  1. switch to the Create tab

  2. click 3 Axis Adv > Horizontal Roughing > the roughcut quickly gets rid of a lot of material, step by step.

  3. in the dialog-box that pops up, go to the Cut Parameters tab
    a) set the Stock (e.g. 3 mm for foam)
    b) under Cut Pattern, select Linear
    c) under Cut Direction, select Mixed
    d) under Stepover Control set % Tool Diameter to 90 for foam, less for harder materials…
    e) in the Cut Levels tab under Stepdown Control put % Tool Diameter to 100%-200% for foam, 50% for wood

  4. click Generate to calculate the toolpath > you should now have a subfolder of Setupv 1 called Horizontal Roughing, which contains all the different components / parameters that defines the operation > double-click on one of them to change the settings > a red star on one of them means Regeneration necessary (right-click > Regenerate)

  5. switch to the Simulate tab and hit play

  6. configure visibility using these buttons:

RhinoCam_Machining_2

RhinoCam_Machining_3

A) Part visibility
B) Stock visibility
C) Material Texture visibility
D) Toolpath visibility
E) Toggle Machine GSYS
F) Tool visibility
G) Holder visibility
H) Machine Tool Visibility

RhinoCam_Machining_4

  1. switch back to the Create tab

  2. if necessary, select a different tool from the list

  3. click 3 Axis Adv> Parallel Finishing >in this operation, the tool will follow the surface

  4. in the dialog-box, that pops up, go to the Cut Parameters tab
    a) set the Stock to 0 (normally) and Cut Direction to Mixed
    b) define the Angle of Cuts and the % Tool Diameter > depending on the desired pattern (min 25, max 90).
    c) in the Feeds and Speeds tab, set the Speed to 16‘000 RPM and the Cut (cf) to 200 mm/min.
    d) don‘t forget to set your tools in the tool tab

  5. click Generate again and Simulate the operation > you can create as many machining operations as you like until you are satisfied with the result.

RhinoCam_Machining_5

The most helpful Milling Operation Are „Horizontal Roughing“, Parallel Finishing“, „Curve Machining“ and „Engraving“. But you can also experiment with „Pocketing“ or „Between 2 Curves Machining“ and other operations.


Regions and Curves

RhinoCam_Regions_1

Closed curves can be selected as so called Regions - either before the Machining Method is chosen or under the Features/Regions tab by clicking Select Curves as Regions.
These curves then act as boundary to limit the toolpath to the specific area. Curves can also be nested (islands).

RhinoCam_Regions_2

Engrave a road

  1. select a (open or closed) 2D curve

  2. for sharp edges, select a flatnose mill from the list

  3. click 3 Axis Adv > Curve Machining

  4. in the Cut Parameters tab, define a negative stock

  5. click Generate

  6. RhinoCAM automatically projects the curve onto all visible geometry and runs the tool along the rail

RhinoCam_Regions_3

boarder of a river…

  1. select two 2D curves (both open or both closed)
  2. click 3 Axis Adv > Between 2 Curves Machining
  3. click Generate
  4. RhinoCAM creates not parallel toolpath-lines but lines that „blend“ curves into one another. Stepsize is smaller where the curves are closer and bigger where they are more distant > the resulting pattern integrates well in the landscape if for example the two borders of a river are selected…

RhinoCam_Regions_4

RhinoCam_Regions_5

To mill the inner area (red), select the white bounding curve

RhinoCam_Regions_6

To mill the outer area (red), select the white AND yellow bounding curve

RhinoCam_Regions_7


Post Processing

RhinoCam_Post_Processing_1

  1. post the individual jobs to separate files. right-click on the machining operation you want to post and click [Post]

  2. specify the folder location and the filename (e.g.: NAME_12Ball_6Flat.nc)

  3. click [Post] to write G-Code file

  4. put your G-Code on a USB stick and bring it down to the RapLab

RhinoCam_Post_Processing_2