Drawing Workbench

The Drawing module allows you to put your 3D work on paper. That is, to put views of your models in a 2D window and to insert that window in a drawing, for example a sheet with a border, a title and your logo and finally print that sheet. The Drawing module is currently under construction and more or less a technology preview!

GUI Tools


In the picture you see the main concepts of the Drawing module. The document contains a shape object (Schenkel) which we want to extract to a drawing. Therefore a "Page" is created. A page gets instantiated through a template, in this case the "A3_Landscape" template. The template is an SVG document which can hold your usual page frame, your logo or comply to your presentation standards.

In this page we can insert one or more views. Each view has a position on the page (Properties X,Y), a scale factor (Property scale) and additional properties. Every time the page or the view or the referenced object changes the page gets regenerated and the page display updated.

Scripting
At the moment the end user(GUI) workflow are very limited, so the scripting API is more interesting. Here follows examples on how to use the scripting API of the drawing module.

Simple example
First of all you need the Part and the Drawing module: import FreeCAD, Part, Drawing Create a small sample part Part.show(Part.makeBox(100,100,100).cut(Part.makeCylinder(80,100)).cut(Part.makeBox(90,40,100)).cut(Part.makeBox(20,85,100))) Direct projection. The G0 means hard edge, the G1 is tangent continuous. Shape = App.ActiveDocument.Shape.Shape [visibleG0,visibleG1,hiddenG0,hiddenG1] = Drawing.project(Shape) print "visible edges:", len(visibleG0.Edges) print "hidden edges:", len(hiddenG0.Edges) Everything was projected on the Z-plane: print "Bnd Box shape: X=",Shape.BoundBox.XLength," Y=",Shape.BoundBox.YLength," Z=",Shape.BoundBox.ZLength print "Bnd Box project: X=",visibleG0.BoundBox.XLength," Y=",visibleG0.BoundBox.YLength," Z=",visibleG0.BoundBox.ZLength Different projection vector [visibleG0,visibleG1,hiddenG0,hiddenG1] = Drawing.project(Shape,App.Vector(1,1,1)) Project to SVG resultSVG = Drawing.projectToSVG(Shape,App.Vector(1,1,1)) print resultSVG

The parametric way
Create the body App.ActiveDocument.addObject("Part::Box","Box") App.ActiveDocument.Box.Length=100.00 App.ActiveDocument.Box.Width=100.00 App.ActiveDocument.Box.Height=100.00 App.ActiveDocument.addObject("Part::Box","Box1") App.ActiveDocument.Box1.Length=90.00 App.ActiveDocument.Box1.Width=40.00 App.ActiveDocument.Box1.Height=100.00 App.ActiveDocument.addObject("Part::Box","Box2") App.ActiveDocument.Box2.Length=20.00 App.ActiveDocument.Box2.Width=85.00 App.ActiveDocument.Box2.Height=100.00 App.ActiveDocument.addObject("Part::Cylinder","Cylinder") App.ActiveDocument.Cylinder.Radius=80.00 App.ActiveDocument.Cylinder.Height=100.00 App.ActiveDocument.Cylinder.Angle=360.00 App.activeDocument.addObject("Part::Fuse","Fusion") App.activeDocument.Fusion.Base = App.activeDocument.Cylinder App.activeDocument.Fusion.Tool = App.activeDocument.Box1 App.activeDocument.addObject("Part::Fuse","Fusion1") App.activeDocument.Fusion1.Base = App.activeDocument.Box2 App.activeDocument.Fusion1.Tool = App.activeDocument.Fusion App.activeDocument.addObject("Part::Cut","Shape") App.activeDocument.Shape.Base = App.activeDocument.Box App.activeDocument.Shape.Tool = App.activeDocument.Fusion1 Gui.activeDocument.Box.Visibility=False Gui.activeDocument.Box1.Visibility=False Gui.activeDocument.Box2.Visibility=False Gui.activeDocument.Cylinder.Visibility=False Gui.activeDocument.Fusion.Visibility=False Gui.activeDocument.Fusion1.Visibility=False
 * 1) Create three boxes and a cylinder
 * 1) Fuse two boxes and the cylinder
 * 1) Cut the fused shapes from the first box
 * 1) Hide all the intermediate shapes

Insert a Page object and assign a template App.activeDocument.addObject('Drawing::FeaturePage','Page') App.activeDocument.Page.Template = App.getResourceDir+'Mod/Drawing/Templates/A3_Landscape.svg'

Create a view on the "Shape" object, define the position and scale and assign it to a Page App.activeDocument.addObject('Drawing::FeatureViewPart','View') App.activeDocument.View.Source = App.activeDocument.Shape App.activeDocument.View.Direction = (0.0,0.0,1.0) App.activeDocument.View.X = 10.0 App.activeDocument.View.Y = 10.0 App.activeDocument.Page.addObject(App.activeDocument.View)

Create a second view on the same object but this time the view will be rotated by 90 degrees. App.activeDocument.addObject('Drawing::FeatureViewPart','ViewRot') App.activeDocument.ViewRot.Source = App.activeDocument.Shape App.activeDocument.ViewRot.Direction = (0.0,0.0,1.0) App.activeDocument.ViewRot.X = 290.0 App.activeDocument.ViewRot.Y = 30.0 App.activeDocument.ViewRot.Scale = 1.0 App.activeDocument.ViewRot.Rotation = 90.0 App.activeDocument.Page.addObject(App.activeDocument.ViewRot)

Create a third view on the same object but with an isometric view direction. The hidden lines are activated too. App.activeDocument.addObject('Drawing::FeatureViewPart','ViewIso') App.activeDocument.ViewIso.Source = App.activeDocument.Shape App.activeDocument.ViewIso.Direction = (1.0,1.0,1.0) App.activeDocument.ViewIso.X = 335.0 App.activeDocument.ViewIso.Y = 140.0 App.activeDocument.ViewIso.ShowHiddenLines = True App.activeDocument.Page.addObject(App.activeDocument.ViewIso) Change something and update. The update process changes the view and the page. App.activeDocument.View.X = 30.0 App.activeDocument.View.Y = 30.0 App.activeDocument.View.Scale = 1.5 App.activeDocument.recompute

Accessing the bits and pieces
Get the SVG fragment of a single view ViewSVG = App.activeDocument.View.ViewResult print ViewSVG Get the whole result page (it's a file in the document's temporary directory, only read permission) print "Resulting SVG document: ",App.activeDocument.Page.PageResult file = open(App.activeDocument.Page.PageResult,"r") print "Result page is ",len(file.readlines)," lines long"

Important: free the file! del file Insert a view with your own content: App.activeDocument.addObject('Drawing::FeatureView','ViewSelf') App.activeDocument.ViewSelf.ViewResult = """       """ App.activeDocument.Page.addObject(App.activeDocument.ViewSelf) App.activeDocument.recompute del Shape,ViewSVG, resultSVG That leads to the following result:



Templates
FreeCAD comes bundled with a set of default templates, but you can find more on the Drawing templates page.