Skeinforge Raft
From DEMOZENDIUM
Raft is a plugin to create a raft, elevate the nozzle and set the temperature. A raft is a flat base structure on top of which your object is being build and has a few different purposes. It fills irregularities like scratches and pits in your printbed and gives you a nice base parallel to the printheads movement. It also glues your object to the bed so to prevent warping in bigger object. The rafts base layer performs these tricks while the sparser interface layer(s) help you removing the object from the raft after printing. It is based on the Nophead's reusable raft, which has a base layer running one way, and a couple of perpendicular layers above. Each set of layers can be set to a different temperature. There is the option of having the extruder orbit the raft for a while, so the heater barrel has time to reach a different temperature, without ooze accumulating around the nozzle.
The important values for the raft settings are the temperatures of the raft, the first layer and the next layers. These will be different for each material. The default settings for ABS, HDPE, PCL & PLA are extrapolated from Nophead's experiments.
You don't necessarily need a raft and especially small object will print fine on a flat bed without one, sometimes its even better when you need a water tight base to print directly on the bed. If you want to only set the temperature or only create support material or only elevate the nozzle without creating a raft, set the Base Layers and Interface Layers to zero.
 Raft |
Example of a raft on the left with the interface layers partially removed exposing the base layer. Notice that the first line of the base is rarely printed well because of the startup time of the extruder. On the right you see an object with its raft still attached.
The Raft panel has some extra settings, it probably made sense to have them there but they have not that much to do with the actual Raft. First are the Support material settings. Since close to all RepRap style printers have no second extruder for support material Skeinforge offers the option to print support structures with the same material set at a different speed and temperature. The idea is that the support sticks less to the actual object when it is extruded around the minimum possible working temperature. This results in a temperature change EVERY layer so build time will increase seriously.
More useful info can be found at the Thingiverse blog here and here and on the HydraRaptor blog
More pictures of rafting in action are available from the Metalab blog
Operation
Default: ON
When it is on, the functions described below will work, when it is off, nothing will be done, so no temperatures will be set, nozzle will not be lifted..
Settings
Add Raft, Elevate Nozzle, Orbit and Set Altitude
Default: ON
When selected, the script will also create a raft, elevate the nozzle, orbit and set the altitude of the bottom of the raft. It also turns on support generation.
Base
Base layer is the part of the raft that touches the bed.
Base Feed Rate Multiplier (ratio)
Default: 1.0
This parameter will allow you to change the default speed skeinforge will use to print base layer. The "actual" base layer feed rate (speed the head moves) will be:
"Speed/Feed Rate" * "RAFT/Base Feed Rate Multiplier" / ("RAFT/Base Layer Thickness over Layer Thicknes")^2
Base Flow Rate Multiplier (ratio)
Default: 1.0
This parameter will allow you to change the default extrusion rate skeinforge will use to print base layer. The "actual" base layer flow rate (speed the extruder motor runs) will be:
"Speed/Flow Rate" * "Base Flow Rate Multiplier (ratio)"
Base Infill Density (ratio)
This parameter set the ratio of the base layer fill. Value of 0.1 means that only 10% of the surface will be "covered" and value of 0.9 means that 90% of the surface will be covered. Value depends on how flat your print bed is, how parallel to head path it is etc. Higher value means more time to make raft base, more filament usage but "better base".
Usual values are 0.25 to 0.7
Base Layer Thickness over Layer Thickness
This parameter set how much "fatter" the base layer will be compared to normal layer, so if you set here 1 the base will look "same" as the normal layer but if you put here 1.5 or 2 the base will be "fatter". The "fatness" is achieved by slower movement of the head so more filament per mm is extruded hence fatter the "line".
Usual values are 1.5 to 2
Base Layers
How many layers of "base layer type" to print. The 1 is usually enough but with rough print bed sometimes 2 are needed, more then 2 is just waste of time / filament. The base layer matrix is not rotated by 90degree as one would expected but printed directly on top of the previous one so 2 layers will not make "grid".
Usual value is 1
Base Nozzle Lift over Base Layer Thickness (ratio)
You can modify the nozzle height for base layer by modifying this value. If your print bed is "ok" standard value of 0.375 is good/preferred but if your print bed is damaged you might want to lower the value a bit to allow printer to fill the "scratches" in the print bed. The value is related to layer thickness. In order to get same height as the bfb testra.bfb test raft the value here for 0.45mm layer should be 0.18.
The actual Z coordinate of the head is calculated by:
"RAFT/Bottom Altitude" + 0.5 * "CARVE/Layer Thickness" * "RAFT/Base Layer Thickness over Layer Thickness" + "CARVE/Layer Thickness" * "RAFT/Base Layer Thickness over Layer Thickness" * "RAFT/Base Nozzle Lift over Base Layer Thickness (ratio)"
Usual value is 0.375
Note that this used to be "over HALF layer thickness" before November 2009
Bottom Altitude
What is the Z value for the print bed when tool is homed.
Usual value is 0
Infill Overhang over Extrusion Width (ratio)
Usual value is 0.1
Interface
Interface is the second "upper" part of the raft that is in contact with the printing object. It is usually denser then base layer and usually thinner. Interface layers are printed rotated 90degrees to base layer but they are all on top of each other (they form grid with base layer but not with themselves).
Interface Feed Rate Multiplier (ratio)
Default: 1.0
This parameter will allow you to change the default speed skeinforge will use to print interface layer. The "actual" interface layer feed rate (speed the head moves) will be:
"Speed/Feed Rate" * "RAFT/Interface Feed Rate Multiplier" / ("RAFT/Interface Layer Thickness over Layer Thicknes")^2
Interface Flow Rate Multiplier (ratio)
Default: 1.0
This parameter will allow you to change the default extrusion rate skeinforge will use to print interface layer. The "actual" interface layer flow rate (speed the extruder motor runs) will be:
"Speed/Flow Rate" * "Interface Flow Rate Multiplier (ratio)"
Interface Infill Density (ratio)
This parameter set the ratio of the interface layer fill. Value of 0.1 means that only 10% of the surface will be "covered" and value of 0.9 means that 90% of the surface will be covered.
Usual value is 0.5
Interface Layer Thickness over Layer Thickness
This parameter set how much "fatter" the interface layer will be compared to normal layer, so if you set here 1 the base will look "same" as the normal layer but if you put here 1.5 or 2 the base will be "fatter". The "fatness" is achieved by slower movement of the head so more filament per mm is extruded hence fatter the "line".
Usual value is 1
Interface Layers
Default: 1
Defines the number of interface layers to print.
Interface Nozzle Lift over Interface Layer Thickess (ratio)
With this value you can modify the thickness of the interface layer. Value of 1 will not "press the layer in" but let it settle on it's own. Less then 1 will press the filament "a bit" and more then 1 will let it "drop" so some curling might occur depending on the filament type.
Usual value is 0.45
Note that this used to be "over HALF layer thickness" before November 2009
Name of Alteration Files
If support material is generated, raft looks for alteration files in the alterations folder in the .skeinforge folder in the home directory. Raft does not care if the text file names are capitalized, but some file systems do not handle file name cases properly, so to be on the safe side you should give them lower case names. If it doesn't find the file it then looks in the alterations folder in the skeinforge_plugins folder.
Name of Support End File
Default is support_end.gcode.
If support material is generated and if there is a file with the name of the "Name of Support End File" setting, it will be added to the end of the support gcode.
Name of Support Start File
If support material is generated and if there is a file with the name of the "Name of Support Start File" setting, it will be added to the start of the support gcode.
Operating Nozzle Lift over Layer Thickness (ratio)
Way to modify thickness of the "normal layers" (layers of the object). Range that makes sense is 0.4 to 0.6.
Usual value is 0.5
Note that this used to be "over HALF layer thickness" before November 2009
Raft Size
Raft Additional Margin over Length (%)
Usual value: 2.0
Raft Margin (mm)
I use 5-15mm. This value define how much raft will be larger then the object
Support
Good articles on support material are at: http://davedurant.wordpress.com/2010/07/31/skeinforge-support-part-1/ http://davedurant.wordpress.com/2010/07/31/skeinforge-support-part-2/
Note:For support to be active you must have Raft and Add raft activated. If you don't actually want a raft just set Base and Interface layers to 0
Support Cross Hatch
Turns the orientation of the support layer by 90 degrees on every other layer to create a stronger support structure. Note that stronger support structure is harder to be removed so if you are printing support with same material as the main object it is best to keep this off for easier removal of the support.
Support Flow Rate over Operating Flow Rate
Default: 0.9.
Defines the ratio of the flow rate when the support is extruded over the operating flow rate. With a number less than one, the support flow rate will be smaller so the support will be thinner and easier to remove.
Support Gap over Perimeter Extrusion Width
Default: 0.5.
Defines the gap between the support material and the object over the perimeter extrusion width.
Support Material Choice
Default: 'None' because the raft takes time to generate.
Choices:
- None - No support material.
- Empty Layers Only - Support material will be only on the empty layers. This is useful when making identical objects in a stack.
- Support material everywhere - Support will be created where needed, somethimes inside the object. This might be problematic because support might be in place where you cannot reach to remove it after print is finished
- Support material on Exterior only - Support will be created only on the outside of the object
Support Minimum Angle (degrees)
Default: 60 degrees
Defines the minimum angle that a surface overhangs before support material is added. If angle is lower then this value the support will be generated. This angle is defined from the vertical, so zero is a vertical wall, ten is a wall with a bit of overhang, thirty is the typical safe angle for filament extrusion, sixty is a really high angle for extrusion and ninety is an unsupported horizontal ceiling.
Check here for the overhang examples and some testing.
