• Overview
• The Framework
  • GeoFeature
  • Property Link
  • GUI Selection
• Topological Name Generation
  • Object Identification
  • Element Mapping
  • New Makers in TopoShape
  • String Hasher
  • Element Map Versioning

Current FreeCAD uses generic type + index as the topological names of various geometry elements, such as Face1, Edge2, and Vertex3. The indexing order of the elements is determined by the CAD kernel, OCCT, which is consistent during document save and restore. However, when the model is edited, i.e. when new geometry elements are added or removed, the element indices are rearranged/reused, and there is no easy way of tracking which one is which after the modification.

There has been other attempts trying to solve this problem, e.g. here, here, and here And various research papers posted in the forum, such as this. They all served as great inspirations leading to the solution presented here, which is offered as a general framework that is

• fully backward compatible, meaning that you can save your model in new version of FreeCAD and still able to open it in older version of the software. You will loose all new style topological naming of the model, obviously. But your link properties continues to work; and,

• automatic, with very little code modification of existing workbench, because the framework resides in the core, and other workbench get the benefit through various property links which are enhanced. When you open models created in older version of FreeCAD, it automatically gains the benefit of the new topological naming feature after recompute.

The framework deals with abstract geometry element name mapping, and name reference auto update. The core does not know or care how the topological names are generated and mapped. It provides necessary ground works for other modules to generate stable topological names. At the time of this writing, Sketcher.SketchObject can now provide a complete stable topological naming, and both Part and PartDesign have full implementation of the topological name generation.

In the current FreeCAD core, the interface class that describes a geometry shape is called ComplexGeoData. It has been extended to include an optional ElementMap, with the following new APIs in both C++ and Python,

• setElementName(element,name, postfix=None, overwrite=False). It is used to assign a new name to an element with optional postfix, e.g. setElementName('Edge1','e1'). An element can have multiple names, but a name can only be associated to one element. You can overwrite existing mapping by the overwrite parameter. The purpose of postfix is to make it easy for the caller to form meaningful names, such as use the postfix to identify operation, and mark modifications. More importantly, as the name gets longer, ComplexGeoData allows the caller to compress the name using string hash, but it will ensure that the postfix remains the same, for more advanced applications like deducing modified elements, etc. More details about string hashing will be given in later section.

• getElementName(name,reverse=False). Returns the original element name by the given name, or, the other way around if reverse is true.

The entire element map is also exposed to C++ with set/getElementMap(), and as writable attribute called ElementMap in Python.

When exposed to Gui.Selection, ComplexGeoData uses a special prefix to mark the mapped element. Currently, ; is chosen as the prefix. When calling setElementName(), the special prefix is optional, and will be stripped away before storage, same for getElementName(). More details about the involvement of Gui.Selection will be given later.

ComplexGeoData does not know or care the content stored in the map. It is up to the inherited geometry classes to provide the semantic meaning of the content. These APIs also make it possible for other core classes to work their magic to provide seamless upgrade. Here is how it works,

GeoFeature, the core geometry document object class, now provides a few convenient method (getElementName(), resolveElements()) to let other query the element map in its associated PropertyComplexGeoData. After GeoFeature detects any element name changes in its onChanged() method, it will signal all its dependent objects to update their geometry element references.

PropertyLinkSub, PropertyLinkSubList, and PropertyXLink are the only properties in the core that can carry geometry element reference information. Other objects that use those properties are free to choose which type of element name to store as reference, either the original or the mapped one. Behind the scene, they will keep a shadow copy of both the original and mapped element reference (if there is one) each time they are assigned a new reference. When updating, if and only if there exists a shadow copy of the mapped element reference, will it auto updates its original index based element reference.

Let's take an example, say, a compound with a mapped reference F1 -> Face1. When the user assigns the reference Face1 to a PropertyLinkSub, it will immediately query the element map, and stores a shadow copy of both F1 and Face1. When you updates a compound, say rearrange the order of its children, its element name will surely change. Assume the compound has updated the mapping for F1 to Face10. When PropertyLinkSub is asked to update its reference, it will query the current element mapping for F1, and obtained the updated reference Face10, and then update the user assigned value from Face1 to Face10 automatically.

The reason why we keeps a shadow copy of the unmapped reference is because the user is free to choose to store the new mapped name as well. Say, it stores F1 in the above example, then no user visible update will happen. But PropertyLinkSub will still keep the shadow copy of the unmapped reference up to date behind the scene. When saving, PropertyLinkSub will store this up-to-date unmapped reference just like before, so that the old version FreeCAD can still open the document, and every links inside works as expected. PropertyLinkSub will also save the user assigned value, if and only if it is a new mapped name, so that when restoring in the new FreeCAD, it stays the same. The old version FreeCAD will simply skip it.

You may be wondering why can't we just hide the whole mapped element reference name behind the scene, and only assign the original element name to PropertyLinkSub, and let the core works its magic to keep it up-to-date. There are cases where you'll prefer a constant reference name. For example, The new sketch export feature allows you to export any private geometry element of a sketch, including the external edges. Sketch will use the new mapped reference name for linking to external edges, and then use the SHA1 hash of the link reference as the element name for export. The stability of the mapped name ensures the stability of the export, as well.

When you call Gui.Selection.getSelectionEx(), it will return the geometry element selection in the SubElementNames attribute of its returned value. My Link branch FreeCAD went through major upgrade to bring you full object hierarchy information through this SubElementName field, as a . separated string. For example, when you selects a face of a PartDesign Pad feature, SubElementNames will give you something like, Pad.Face1. Now, it is further extended to include any mapped element name found, as well, like, Pad.;F1.Face. The ; is used here to mark the following name as a mapped element name instead of an object name. The mapped element name is not obtained by Gui.Selection directly, but by the object's view object. Just like the current FreeCAD relying on the view object's getElement() function to return the selected element name Face1, it now returns ;F1.Face1 if the mapping is found. As a result, when you hover your mouse over some geometry element in the 3D view, you will now see the new mapped element reference in status bar.

By default, calling Gui.Selection.getSelectionEx() will automatically walk down the selected object hierarchy, and resolve the final object, and its selected geometry element index based reference, so that any existing workbench sees exactly what they expect. New code can pass an additional parameter resolve, set to 2 to see the mapped reference name, or 0 to see the entire object hierarchy. That's how a PropertyLinkSub can be assigned a mapped geometry reference.

It may seems that we have yet to enter the main topic, considering the fact that the title of this article is called Topological Naming, and we haven't actually talked about it. However, let me assure you the utter importance of the ground works described above. Because, only when you actually tries to implement a full working solution, will you realize that it is now difficult to implement some seemingly straight forward operations, like copy and paste. Because, ironically, in order to have a stable topological naming, it has to include object identification. But copy and paste generates new objects, with new identification, and thus, will completely change all existing topological naming. In other word, it is useless to copy topological names. We have to rely on old style type+index to re-generate all mappings, and re-establish all property links. Without the framework above, it just won't work.

Now, we are going to talk about the actual topological name generation, which I consider to be fairly standard, most of which follows some of the research papers out there.

Each document object in FreeCAD will now be assigned an integer identification number that is unique within its owner document. UUID is not really useful here, when objects can be freely copied and pasted from other documents, which may be a copy by themselves. There is no uniqueness guarantee outside of the object's document. A simple integer is simpler, cheaper, much easier to manipulate.

Part.TopoShape has a new public member variable called Tag that is used to link a shape to its owner object. When the shape is generated by code, the user is free to assign any integer value to Tag. The rule is that, zero Tag disables automatic element mapping. When mapping an element from another shape with a different Tag, it will append the Tag into the mapped element name.

TopoShape now offers a helper method to map the same geometry element from other TopoShape instance into itself.

mapSubElement(shape, op=None)

op is an optional string to insert before the mapped element name. In Python, TopoShape's sub-shape attributes will all use mapSubElement to transfer the element mapping from the owner shape to its sub-shapes. For example, run the following code in FreeCAD Python console,

import Part,pprint
cube = Part.makeBox(10,10,10)
cube.Tag = 1
cube.ElementMap
{}

pprint.pprint(cube.Face2.ElementMap)
{'Edge5': 'Edge1',
 'Edge6': 'Edge2',
 'Edge7': 'Edge3',
 'Edge8': 'Edge4',
 'Face2': 'Face1',
 'Vertex5': 'Vertex1',
 'Vertex6': 'Vertex2',
 'Vertex7': 'Vertex3',
 'Vertex8': 'Vertex4'}

As you can see, cube itself does not have any element mapping, because it is a primitive shape, and thus, all its element can be considered as fixed. To enable sub-shape element mapping, set the Tag to non-zero, and you can see how sub-shape cube.Face2 maps the original cube's element name into its own elements. In the returned dictionary, the key is cube's original element name, and the value is the sub-shape's element name. The element mapping will be generated by all sub-shape accessors, like Solids, Wires, etc.

Although the Part primitive shape does not have element map by default, the user (or Python code) can assign customized names that are persistent, so can the generic Part::Feature object. Be careful though, if you change the element name of a feature, all its dependent feature may change their element name, too, which may invalidates the element reference inside some link properties. You should choose a fixed rule to generate element names in your derived classes.

import Part
doc = App.newDocument('test')
cube = doc.addObject('Part::Box','cube')
shape = cube.Shape.copy()
shape.setElementName('Face1','F1')
cube.Shape = shape
doc.recompute()
doc.save('test.fcstd')
App.closeDocument('test')
doc = App.openDocument('test.fcstd')
doc.getObject('cube').Shape.ElementMap
{'F1': 'Face1'}

TopoShape offers several new maker method that utilize this element mapping. In C++, all of the new maker function name starts with makE, such as makECompound, makEWires, etc. All new maker code is implemented in a new source file called TopoShapeEx.cpp. In Python, however, the changes are made by change the C++ code of existing method, so that existing Python feature can get the benefit without any python code modification.

There two categories of maker functions. The first category of makers do not modify any existing elements. Instead, it generates new elements by simply combining input lower level elements. They are,

• makECompound, exposed to Python using both Part.makeCompound and Part.Compound constructor.
• makEWires, exposed to Python as a new method in Part.Shape named makeWire, and also as Part.Wire constructor. This function accepts list or compound of unsorted edges. And will automatically connects the edges to form one or more wires (as compound)
• makECompSolid, exposed to Python as Part.CompSolid constructor

All of these method do not really generate new element names, but only map existing element names, although, it may append the tags of the input shape to avoid name conflict.

The following code demonstrate how makECompound maps the input shape elements into the new compound shape. For name Edge10;:T1:6, the trailing ;:T is the marker for tag. The following 1 is the actual tag, and :6 is the source element name length. 6 means the first five characters, i.e. Edge10.

import Part,pprint
cube = Part.makeBox(10,10,10)
cube.Tag = 1
cube2 = Part.makeBox(10,10,10,App.Vector(10,0,0))
cube2.Tag = 2
compound = Part.makeCompound([cube,cube2])

pprint.pprint(compound.ElementMap)
{'Edge10;:T1:6': 'Edge10',
 'Edge10;:T2:6': 'Edge22',
 'Edge11;:T1:6': 'Edge11',
 'Edge11;:T2:6': 'Edge23',

 ...
 
 'Vertex7;:T2:7': 'Vertex15',
 'Vertex8;:T1:7': 'Vertex8',
 'Vertex8;:T2:7': 'Vertex16'}

The Sketcher now uses TopoShape::makEWires to create its public geometry wires and map its internal geometry element names. Too see the effect, create any sketch, and type the following command in the console.

pprint.pprint(App.ActiveDocument.Sketch.Shape.ElementMap)

{'g1;SKT': 'Edge1',
 'g1v1;SKT': 'Vertex1',
 'g1v2;SKT': 'Vertex2',

 ...

}

The second category of maker relies on OCCT's BRepBuilderAPI_MakeShape and its derivatives to construct the shape. And TopoShape relies on this class to provide the shape history information, specifically, the mapping from the input geometry elements to the newly generated or modified elements in the resulting shape. The details of the mapping algorithm can be found here

As you will find out after reading the Topological Naming Algorithm, the generated element names are going to be very long. And as we add more histories to the model, the length of a new element name will quickly go out of control. To deal with this problem, a new object is introduced, StringHasher. It allows you to transform any string into an integer ID. SthringHasher.Threshold controls how the strings are stored. If Threshold is positive, and the string length goes beyond this value, the original string content will be discarded, and only persists the crypto hash of the string, currently SHA1. If Threshold is non-positive, then it will keep the string as it is. The returned integer ID is guaranteed to be unique within its owner StringHasher object.

Every Document now has a default StringHasher object accessible through Document.Hasher. ComplexGeoData also has an attribute named Hasher which is initially None. Simply assign the Document.Hasher to it, or, if you want, create a new one by App.StringHasher(). ComplexGeoData.setElementName() will encode the mapped element name if there is a Hasher available.

TopoShape inherits the Hasher from ComplexGeoData. When you assign a TopoShape containing a Hasher to a PropertyPartShape, the hasher will be persisted to the document. The string inside the Hasher is reference counted. By default, only used string will be persisted. You can change that behavior by setting attribute StringHasher.SaveAll to True. ComplexGeoData will only hash the element name if there is at least a separator ; found in the middle of the name. TopoShape will auto append this separator when mapping element from other shapes with a non zero tag.

To see the effect of the string hasher,

import Part,pprint
cube = Part.makeBox(10,10,10)
cube.Tag = 1
cube.Hasher = App.StringHasher()
cube.Hasher.Threshold=10

cube.setElementName('Edge1','A_LONG_ELEMENT;NAME')
'#1'

cube.setElementName('Edge2','SHORT;NAME')
'#2'

pprint.pprint(cube.ElementMap)
{'#1': 'Edge1', '#2': 'Edge2'}

pprint.pprint(compound.Hasher.Table)
{1: '724be94858dd7faa13ce515d46fc6849616b1a44', 2: 'SHORT;NAME'}

compound = Part.makeCompound(cube)

pprint.pprint(compound.ElementMap)
{'#1;:T1:2': 'Edge1',
 '#2;:T1:2': 'Edge2',
 'Edge10;:T1:6': 'Edge10',
 'Edge11;:T1:6': 'Edge11'

...

}

As you can see, the first element name exceeds the threshold, so Hasher.Table stores the SHA1 hash of the assigned element name. To use the StringHasher more effectively, you should use StringHasher.getID() for both string lookup or ID creation. The returned value is a StringID object that is reference counted.

hasher = App.StringHasher()
id = hasher.getID("abcde")

# Note that the number after '#' is a hex number
print str(id)
'#1'

print id.Value
1

print id.Data
abcde

id2 = hasher.getID(1)

print id.isSame(id2)
True

Each document now has a new property named UseHasher to control be hashing behavior. Part workbench features will check this property to decide whether to hash the generated element names. It is by default on. When you manually set this property to False, the document will touch every geometry feature inside, and you'll need to recompute the entire document to get the updated element map.

The default StringHasher.Threshold is zero, meaning that all string will be stored in the table without crypto hashing. This is because the original string content is important to trace back modeling history. Tracing back history is not need to maintain a stable element reference, however, it is useful in other applications, such as view provider element color mapping.

There is one more important details that is handled inside ComplexGeoData and TopoShape. Most of the shape building involves multiple steps. To make it maker API user to use, we do not demand only hashing in the very last modeling step, which means that it is possible to hash more than once from the input shape element name to the final result shape element mapped names. However, if we hash element names in the intermediate steps, where the shapes produced are not persisted, it is possible to have lost the string ID when restoring the document, causing unwanted element name change. To prevent this, each entry in the element map inside ComplexGeoData will keep an array of every historically used string ID references that are involved in generating that map entry. And the arrays are persisted along with the element map. However, tests shows that the persisted form of this string IDs often gets quite long, often longer than the element name itself. Future development may explore the possibility to reduce file size by simply set Hasher.SaveAll to True, and discard all the intermediate string ID references.

As you can see from the description so far, as well as the naming algorithm, the element name generation is a very delicate process. It can be affected by many factors, such as whether the user turns on the hasher, the hasher threshold, how the feature assigns the primary element name, the TopoShape name generating algorithm, and of course, OCCT's maker's mapping logic that TopoShape relies on to obtain the shape history. Any change of these factors may result in significant changes in the generated element names, and can potentially break existing element references.

To prepare for this possibility, we add a new API to GeoFeature to report its element map version. It returns a string that is persistent. Derived features can choose to override it to store its own version. In fact, it is very important for any geometry feature to change the version number if there is any change in its shape building logic. The default implementation will return something as below,

1.4.70100.1.40
| |   |   | |
| |   |   | --If use hasher, then this is the hasher threshold
| |   |   |
| |   |   --ComplexGeoData algorithm version, now is 1
| |   | 
| |   --OCCT version
| |   
| --TopoShape algorithm version, now is 4
|
--1 means using the same hasher as the document's, or else 0

Any geometry feature can simply append their own version (if any) behind this.

When a document is restored, PropertyPartShape will compare the persisted version string with the current one, and mark the feature for recompute if it is changed. It will also inform any link property that has element reference to this feature to reset its shadow copies, similar to what happens when an geometry feature object is copied and pasted.