Drawing Module

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 is very limited, so the scripting API is more interesting. Here follow 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 import FreeCAD import Part import Drawing

App.ActiveDocument.addObject("Part::Box","Box") App.ActiveDocument.Box.Length=100.00 App.ActiveDocument.Box.Width=100.00 App.ActiveDocument.Box.Height=100.00
 * 1) Create three boxes and a cylinder

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
 * 1) Fuse two boxes and the cylinder

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 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'
 * 1) Cut the fused shapes from the first box
 * 1) Hide all the intermediate shapes

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 ViewSVG That leads to the following result:



General Dimensioning and Tolerancing
Drawing dimensions an toleranecs are still under development but you can get some basic functionality with a bit of work.

First you need to get the gdtsvg python module from here (WARNING: This could be broken at any time!):

https://github.com/jcc242/FreeCAD

To get a feature control frame, try out the following:

import gdtsvg as g # Import the module, I like to give it an easy handle ourFrame = g.ControlFrame("0","0", g.Perpendicularity, ".5", g.Diameter, g.ModifyingSymbols("M"), "A", g.ModifyingSymbols("F"), "B", g.ModifyingSymbols("L"), "C", g.ModifyingSymbols("I"))  Here is a good breakdown of the contents of a feature control frame: 

The parameters to pass to control frame are:
 * 1) X-coordinate in SVG-coordinate system (type string)
 * 2) Y-coordinate in SVG-coordinate system (type string)
 * 3) The desired geometric characteristic symbol (tuple, svg string as first, width of symbol as second, height of symbol as third)
 * 4) The tolerance (type string)
 * 5) (optional) The diameter symbol (tuple, svg string as first, width of symbol as second, height of symbol as third)
 * 6) (optional) The condition modifying material (tuple, svg string as first, width of symbol as second, height of symbol as third)
 * 7) (optional) The first datum (type string)
 * 8) (optional) The first datum's modifying condition (tuple, svg string as first, width of symbol as second, height of symbol as third)
 * 9) (optional) The second datum (type string)
 * 10) (optional) The second datum's modifying condition (tuple, svg string as first, width of symbol as second, height of symbol as third)
 * 11) (optional) The third datum (type string)
 * 12) (optional) The third datum's material condition (tuple, svg string as first, width of symbol as second, height of symbol as third)

The ControlFrame function returns a type containing (svg string, overall width of control frame, overall height of control frame)'''

To get a dimension, try out the following:

import gdtsvg ourDimension = linearDimension(point1, point2, textpoint, dimensiontext, linestyle=getStyle("visible"), arrowstyle=getStyle("filled"), textstyle=getStyle("text")

Inputs for linear dimension are:
 * 1) point1, an (x,y) tuple with svg-coordinates, this is one of the points you would like to dimension between
 * 2) point2, an (x,y) tuple with svg-coordinates, this is the second point you would like to dimension between
 * 3) textpoint, an (x,y) tuple of svg-coordinates, this is where the text of your dimension will be
 * 4) dimensiontext, a string containing the text you want the dimension to say
 * 5) linestyle, a string containing svg (i.e. css) styles, using the getStyle function to retrieve a preset string, for styling the how the lines look
 * 6) arrowstyle, a string containing svg (i.e. css) styles, using the getStyle function to retrieve a preset string, for styling how the arrows look
 * 7) textstyle, a string containing svg (i.e. css) styles, using the getStyle function to retrieve a preset string, for styling how the text looks

With those two, you can proceed as above for displaying them on the drawing page. This module is very buggy and can be broken at any given moment, bug reports are welcome on the github page for now, or contact jcc242 on the forums if you post a bug somewhere else.

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

Extending Drawing Module
Some notes on the programming side of the drawing module will be added to the Drawing Documentation page. This is to help quickly understand how the drawing module works, enabling programmers to rapidly start programming for it.