Carve is the most important plugin to define for your printer.
It carves a shape into svg slice layers. It also sets the layer height and edge width for the rest of the tool chain.
The carve manual page is at:
http://fabmetheus.crsndoo.com/wiki/index.php/Skeinforge_Carve
On the Arcol Blog a method of deriving the layer height is posted. That article "Machine Calibrating" is at:
http://blog.arcol.hu/?p=157
Settings
Add Layer Template to SVG
Edge Width over Height
Extra Decimal Places
Import Coarseness
Layer Height
Layers
Layers From
Layers To
Mesh Type
Correct Mesh
Unproven Mesh
SVG Viewer
Examples
Settings
Add Layer Template to SVG
Default is on.
When selected, the layer template will be added to the svg output, which adds javascript control boxes. So 'Add Layer Template to SVG' should be selected when the svg will be viewed in a browser.
When off, no controls will be added, the svg output will only include the fabrication paths. So 'Add Layer Template to SVG' should be deselected when the svg will be used by other software, like Inkscape.
Edge Width over Height
Default is 1.8.
Defines the ratio of the extrusion edge width to the layer height. This parameter tells skeinforge how wide the edge wall is expected to be in relation to the layer height. Default value of 1.8 for the default layer height of 0.4 states that a single filament edge wall should be 0.4 mm * 1.8 = 0.72 mm wide. The higher the value the more the edge will be inset. A ratio of one means the extrusion is a circle, the default ratio of 1.8 means the extrusion is a wide oval.
This is an important value because if you are calibrating your machine you need to ensure that the speed of the head and the extrusion rate in combination produce a wall that is 'Layer Height' * 'Edge Width over Height' wide. To start with 'Edge Width over Height' is probably best left at the default of 1.8 and the extrusion rate adjusted to give the correct calculated wall thickness.
Adjustment is in the 'Speed' section with 'Feed Rate' controlling speed of the head in X & Y and 'Flow Rate' controlling the extrusion rate. Initially it is probably easier to start adjusting the flow rate only a little at a time until you get a single filament of the correct width. If you change too many parameters at once you can get in a right mess.
Extra Decimal Places
Default is two.
Defines the number of extra decimal places export will output compared to the number of decimal places in the layer height. The higher the 'Extra Decimal Places', the more significant figures the output numbers will have.
Import Coarseness
Default is one.
When a triangle mesh has holes in it, the triangle mesh slicer switches over to a slow algorithm that spans gaps in the mesh. The higher the 'Import Coarseness' setting, the wider the gaps in the mesh it will span. An import coarseness of one means it will span gaps of the edge width.
Layer Height
Default is 0.4 mm.
Defines the the height of the layers skeinforge will cut your object into, in the z direction. This is the most important carve setting, many values in the toolchain are derived from the layer height.
For a 0.5 mm nozzle usable values are 0.3 mm to 0.5 mm. Note; if you are using thinner layers make sure to adjust the extrusion speed as well.
Layers
Carve slices from bottom to top. To get a single layer, set the "Layers From" to zero and the "Layers To" to one. The 'Layers From' until 'Layers To' range is a python slice.
Layers From
Default is zero.
Defines the index of the bottom layer that will be carved. If the 'Layers From' is the default zero, the carving will start from the lowest layer. If the 'Layers From' index is negative, then the carving will start from the 'Layers From' index below the top layer.
For example if your object is 5 mm tall and your layer thicknes is 1 mm if you set layers from to 3 you will ignore the first 3 mm and start from 3 mm.
Layers To
Default is a huge number, which will be limited to the highest index layer.
Defines the index of the top layer that will be carved. If the 'Layers To' index is a huge number like the default, the carving will go to the top of the model. If the 'Layers To' index is negative, then the carving will go to the 'Layers To' index below the top layer.
This is the same as layers from, only it defines when to end the generation of gcode.
Mesh Type
Default is 'Correct Mesh'.
Correct Mesh
When selected, the mesh will be accurately carved, and if a hole is found, carve will switch over to the algorithm that spans gaps.
Unproven Mesh
When selected, carve will use the gap spanning algorithm from the start. The problem with the gap spanning algothm is that it will span gaps, even if there is not actually a gap in the model.
SVG Viewer
Default is webbrowser.
If the 'SVG Viewer' is set to the default 'webbrowser', the scalable vector graphics file will be sent to the default browser to be opened. If the 'SVG Viewer' is set to a program name, the scalable vector graphics file will be sent to that program to be opened.
Examples
The following examples carve the file Screw Holder Bottom.stl. The examples are run in a terminal in the folder which contains Screw Holder Bottom.stl and carve.py.
> python carve.py
This brings up the carve dialog.
> python carve.py Screw Holder Bottom.stl
The carve tool is parsing the file:
Screw Holder Bottom.stl
..
The carve tool has created the file:
.. Screw Holder Bottom_carve.svg
| Classes | ||||||||||||||||||
|
| ||||||||||||||||||
| Functions | ||
| ||
| Data | ||
| __author__ = 'Enrique Perez (perez_enrique@yahoo.com)' __date__ = '$Date: 2008/02/05 $' __license__ = 'GNU Affero General Public License http://www.gnu.org/licenses/agpl.html' absolute_import = _Feature((2, 5, 0, 'alpha', 1), (2, 7, 0, 'alpha', 0), 16384) | ||
| Author | ||
| Enrique Perez (perez_enrique@yahoo.com) | ||