This manual presents the inner — under-the-hood — functioning of FreeCAD's Assembly4 workbench. It is primarily intended for power-users and developers.
The project results from discussions on the FreeCAD forum about an assembly without solver. It has then evolved into a dedicated workbench.
Important Note: Assembly 4 is not compatible with FreeCAD v0.18, and needs FreeCAD >= v0.19.18353
Important Note: Assembly 4 is not compatible with Assembly2+ and Assembly3.
Assembly 4 is available through the FreeCAD Addon Manager. It is called Assembly4 in the addon repository.
It is possible to install this workbench manually into FreeCAD's local workbench directory:
- for Windows:
C:\Users\******\AppData\Roaming\FreeCAD\Mod - for Linux:
~/.FreeCAD/Mod - for MacOS:
~/Library/Preferences/FreeCAD/Mod/
This can be useful for testing local modifications to the workbench, or to remove an old stale version of the workbench. In this case, download the Github FreeCAD_Assembly4-master.zip archive from github.com/Zolko-123/FreeCAD_Assembly4 to a temporary directory, and extract the Zip archive. Then, remove any existing Assembly4 directory from FreeCAD's local workbench directory, and move (or link) the folder FreeCAD_Assembly4-master into the directory containing all FreeCAD addon modules.
The very principle of Assembly4 is that FreeCAD container objects ( of type App::Part or PartDesign::Body) are linked together using the App::Link interface introduced in FreeCAD v0.19. The host parent assembly is also an App::Part type container objects called Model. The parts that are linked can be in the same document as the assembly or an external document, invariably.
Even though an Assembly4 assembly is a standard FreeCAD App::Part type object, it has some particularities:
- it is called Model at creation time
- it contains a group called Constraints at the root
- it contains a Datum Coordinate System called LCS_0 at the root
- it contains an
App::FeaturePythonobject called Variables that can hold assembly-wide variables - a FreeCAD document may contain only 1 Assembly4 Model (but can contain many
App::Partobects)
Thus, a standard FreeCAD App::Part cannot serve as host container for an assembly. But since an Assembly4 Model is also an App::Part type object, it can itself be included into another higher-level Assembly4 Model to form nested assemblies with sub-assemblies and sub-sub-assemblies. There is no limit on the number of levels of such nested assemblies.
Also, since an App::Part container has an own reference coordinate system, each child App::Link instance of an App::Part is positioned in the parent assembly's reference coordinate system by its Placement property. This Placement property can be calculated in several ways:
- manually, by setting the parameters in the Placement property fields
- by the Transform tool, which allows to graphically move the
App::Linkinstance - by the built-in ExpressionEngine, that matches the positions of a coordinate system in the child
App::Partand a coordinate system in the assembly - by an external solver when this feature is implemented
We list here the code that creates various objects used in Assembly4. The purpose is to allow developers to extend the capabilities of these objects, and to create compatible objects. This can also be considered as the API of Assembly4.
Linked parts are placed to each-other by matching their Datum Coordinate Systems (PartDesign::CoordinateSystem, called here-after LCS (Local Coordinate System)). There is no need for any geometry to be present to place and constrain parts relative to each other. LCS are used because they are both mechanical objects, since they fix all 6 degrees of freedom in an isostatic way, and mathematical objects that can be easily manipulated by rigorous methods (mainly combination and inversion).
To actually include some geometry, a body needs to be created, and designed using the PartDesign workbench. To be linked with the previously created model, this body needs to be inside the App::Part container called 'Model'.
The result is the following:
- the part Bielle is placed in the assembly by attaching it's LCS_0 to the LCS_0 of the parent assembly.
- the part Cuve is placed in the assembly by placing its LCS_0 on the LCS_1 of the part Bielle
- the part Bague is placed in the assembly by placing its LCS_0 on the LCS_0 of the part Bielle
- the parts Screw_CHC_1 and Screw_CHC_2 are placed in the assembly by placing their LCS_0 on the LCS_1 and LCS_2 of the part Cuve
Assembly4 commands are accessible from the Assembly menu or the Assembly4 toolbar.
Commands in the menu and the toolbar are activated with relevant selection. If a command you want to use is inactive try to change the selection (with the mouse).
These functions are also accessible with the Assembly toolbar:
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: New Model : creates an Assembly4 Model, which is a FreeCAD App::Part called Model and with some extra additions. One document can only contain one Assembly4 Model. -
: New Body : creates FreeCAD PartDesign::Body in an Assembly4 Model or in an App::Part. This Body can then be used with FreeCAD's PartDesign workbench. -
: New Part : creates FreeCAD App::Part in the current document. A document can contain many parts. -
: Insert an External Part : creates a FreeCAD App::Link to an App::Part in another document. Only parts from documents already saved to disk can be used. If there are multiple parts in a document, they can be selected individually. A part can be inserted (linked) many times, but each instance must have a unique name in the assembly tree. If a name already attribuated is given again, FreeCAD will automatically give it a unique (and probably un-user-friendly) name. -
: Place Link : this places a linked part in the assembly to its intended position. This attaches an LCS in the linked part to another LCS in the assembly (called target LCS). This target LCS can be either in the assembly itself (in the Model) or in a sister part already linked. In this case, only LCS at the root of the linked part can be used, and not LCS inside a Body (for example) in the linked part. -
: Fasteners dropdown : Allows to insert screws, nuts and washers from the Fasteners Workbench, and allows to attach them to Assembly4 datum objects, primarily coordinate systems (LCS). If the Fasteners Workbench is not installed, these features are disabled. To install the Fasteners Workbench, go to the menu Tools > Addon Manager > fateners-
: Insert Screw : creates a normed screw from the Fasteners Workbench. The type of screw, diameter and length can be changed in the properties window of the screw.
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: Insert Nut : creates a normed nut from the Fasteners Workbench. The type of nut, diameter and length can be changed in the properties window of the nut. -
: Insert Washer : creates a normed washer from the Fasteners Workbench. The type of washer and its diameter can be changed in the properties window of the washer. -
: Edit attachment of Fastener : allows to attach an object from the Fasteners Workbench — screw, nut or washer — to a datum object in the assembly or a sister part, in the regular Assembly4 manner.
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: New Sketch : creates FreeCAD Sketch in an App::Part (and thus also in Assembly4 Models). This Sketch is unattached, to attach it to an object edit its MapMode in its Placement Property -
: New Datum : this is a drop-down combined menu grouping the creation of all Datum objects:-
: New LCS : creates FreeCAD PartDesign::CoordinateSystem in an App::Part (and thus also in Assembly4 Models). This LCS is unattached, to attach it to an object edit its MapMode in its Placement Property
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: New Datum Plane : creates FreeCAD PartDesign::Plane -
: New Datum Axis : creates FreeCAD PartDesign::Line -
: New Datum Point : creates FreeCAD PartDesign::Point -
: New Hole LCS : creates FreeCAD PartDesign::CoordinateSystem in an App::Part (and thus also in Assembly4 Models) at the center of the selected circular edge. This is therefore only active when a (single) circular edge is selected. This PartDesign::CoordinateSystem is attached to the center of the circle, and is intended to serve as attachment LCS for fasteners. This is the combined function of creating an LCS and attaching it (via MapMode) to a circular edge, and is provided to streamline the workflow.
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: Place Datum : this attaches an existing Datum object in the assembly to another existing Datum object in a linked part. Datum objects of different types can be attached. -
: Import Datum : this imports an existing Datum object from a linked part into the assembly. Precisely, it creates a Datum in the assembly and attaches it to a datum in a sister part of the same type. By default, the same name is given to the imported Datum object. -
: Add Variable : this adds a variable to the Variablesobject in the Model. These variables can be used in any parameter of the document by enteringVariables.HeightorVariables.Length(for example). This is especially useful for assemblies built in a single file, where several parts can be built using the same dimensions. Modifying a variable is done in thePropertieswindow of theVariablesobject. -
: Solve constraints and update assembly : this recomputes all the links and all the placements in the assembly
Assembly4 uses a special and very useful feature of FreeCAD, the ExpressionEngine. Some parameters can be entered through mathematical formulae, that are evaluated by this ExpressionEngine. For Assembly4, it's the parameter Placement of the inserted App::Link object that is calculated, such that 2 LCS - one in the linked part and the one in the assembly - are superimposed.
In normal use, the ExpressionEngine of an App::Link object is hidden, it must be shown as in the following screenshot:
The syntax of the ExpressionEngine is the following:
If the LCS belongs to the parent assembly:
LCS_parent.Placement * constr_LinkName.AttachmentOffset * LinkedPart#LCS_link.Placement ^ -1
If the LCS belongs to a sister part:
ParentLink.Placement * ParentPart#LCS_parent.Placement * constr_LinkName.AttachmentOffset * LinkedPart#LCS.Placement ^ -1
- ParentLink is the name of the App::Link of the sister part in the assembly
- ParentPart is the name of the App::Part that the previous ParentLink refers-to
- LCS_parent is the LCS in the parent part (can be either the assembly itself or a sister part in the assembly)
- constr_LinkName is a FeaturePython object with a conventional name
- LinkedPart is the App::Part's name that the inserted App::Link refers-to
- LCS_link is the LCS in the linked part
To each part inserted into an assembly is associated an App::FeaturePython object, placed in the 'Constraints' group. This object contains information about the placement of the linked object in the assembly. It also contains an App::Placement, called 'AttachmentOffset', which introduces an offset between the LCS in the part and the LCS in the assembly. The main purpose of this offset is to correct bad orientations between the 2 matching LCS.
Note: These constraints are not really constraints in the traditional CAD sense, but since App::FeaturePython objects are very versatile, they could be expanded to contain real constraints in some (distant) future.
Taking a closer look at the fields contained in an App::FeaturePython object associated with the part 'Bague'. The small button under the cursor opens the dialog that allows to edit the parameters of the Attachment Offset
Dialog that opens when clicking the previous small button, and permitting to edit the parameters of the App::Placement called 'AttachmentOffset' in the constraint associated with a link, and allowing relative placement of the link -vs- the attachment LCS
The basic workflow for creating a part is the following:
- Create a new document, create a new 'Model' with the macro 'new_Model'. This will create a new App::Part called 'Model' with the default structure
- Create or import geometries in bodies (
PartDesign::Body) - Create LCS with the macro 'new_ModelLCS', and place them wherever you feel they're useful. Use the MapMode to attach the LCS
- Save part (only saved parts can be used currently). If necessary, close and re-open the file
- Repeat
The basic workflow for creating a part is the following:
- Create a new document, create a new 'Model'
- Create a new sketch with the 'new_ModelSketch' macro. Attach it to whatever is useful, and draw the skeleton of the assembly, placing vertices and lines where useful
- Create new LCS (with the new_ModelLCS macro) and place them on the correct vertices of the sketch (using MapMode)
- Save document
- Import a part using the 'link_Model' macro. It will place your part with its LCS_0 to the LCS_0 of the assembly. You should give it a recognisable name.
- Select the link in the tree, and execute the macro 'place_Link'. Select the LCS of the part that you want to use as attachment point, select the part that you want it to be attached, and select the LCS in that part where you want the part to be attached. Click 'Apply'.
- If the placement corresponds to your needs, click 'Ok', else select other LCS / Part until satisfied
- If the part is correctly paced but badly oriented, select the corresponding constraint in the 'Constraints' folder, select the property 'Offset', and modify its parameters. Click 'Apply'. Repeat until satisfied
The previous method allows to assemble parts within a single level.
But this workbench also allows the assembly of assemblies: since there is no difference between
parts and assemblies, the 'Insert External Part' allows to chose a part that has other parts linked to it.
The only difference will be for the coordinate systems in the inserted assemblies: in order to be used
with Assembly 4, a coordinate system must be directly in the root 'Model' container, meaning that a
coordinate system inside a linked part cannot be used to attach the assembly to a higher-level assembly.
Therefore, in order to re-use a coordinate system of a part in an assembly, a coordinate system must be created at the root of the 'Model', and the placement of this coordinate system must be 'copied' over from the coordinate system that the user wants to use. This is done by inserting a coordinate system and using the 'Place LCS' command, which allows to select a linked part in the assembly and one of it's coordinate systems: the 2 coordinate systems — the one at the root of 'Model' and the one in the linked part — will always be superimposed, even if the linked part is modified, allowing the placement of the assembly in a higher level assembly using a linked part as reference. It sounds more complicated than it actually is.
LGPLv2.1 (see LICENSE)