A2plus Workbench/de

Einführung
Der A2plus Arbeitsbereich ist ein externer Arbeitsbereich, zum Zusammenbau (Assembly) verschiedener Teile in FreeCAD.

Diese Dokumentation beschreibt die A2plus Version 0.4.47 oder neuer.

Installation
Der A2plus Arbeitsbereich ist eine Erweiterung zu FreeCAD. Er kann einfach mit Hilfe des FreeCAD Addon Managers aus dem  Menü installiert werden. A2plus wird aktiv weiterentwickelt und erhält häufig neue Funktionen. Deshalb solltest Du ihn regelmäßig updaten, ebenfalls mittels des Menüs. Der A2plus Code wird auf GitHub gehostet und weiterentwickelt und kann auch manuell durch Kopieren in das -Verzeichnis von FreeCAD installiert werden.

Einstieg
Wechsele zuerst zur A2plus Werkzeugleiste. Um ein Assembly zu erstellen erzeuge eine neue Datei in FreeCAD. Zuerst muss diese Datei gespeichert werden. Es wird empfohlen (jedoch nicht zwingend notwendig), diese in dasselbe Verzeichnis wie die zusammenzubauenden Teile zu speichern.

Jetzt können Teile durch Verwendung der Schaltflächen oder  zum Assembly hinzugefügt werden. Die Schaltfläche fügt alle Körper aus der ausgewählten Teile-Datei als ein einzelnes Teil zum Assembly hinzu. Wenn Du hingegen die Schaltfläche benutzt, kannst Du auswählen, welches Teil aus der Teile-Datei zum Assembly importiert werden soll. Auf diese Weise kann man zum Beispiel auch nur eine Skizze importieren, welche zur Positionierung anderer Teile verwendet werden kann.

Das zuerst hinzugefügte Teil bekommt eine fixe Standard-Position. (Du kannst dies später über die Teile-Eigenschaft verändern.)

Im Assembly bereits vorhandene Teile können mit der Schaltfläche geklont werden.

Um ein Teil des Assemblys zu bearbeiten, wähle es im Modellbaum aus und benutze die Schaltfläche. Dies wird das Teil in einem neuen Tab in FreeCAD öffnen oder zu dem jeweiligen Tab wechseln, falls die Datei bereits geöffnet ist.

Zum Aktualisieren veränderter Teile klicke auf die Schaltfläche. Die Schaltfläche importiert Teile ebenfalls, jedoch rekursiv über mögliche Subassemblies. Wenn Du eines oder mehrere Teile in FreeCAD's Modellbaum auswählst, dann wird A2plus nachfragen, nur die ausgewählten Teile zu aktualisieren.

Importierte Teile behalten ihre externen Abhängigkeiten und können bearbeitet werden. Für genau definierte Teile wie Schrauben ist es hingegen nützlich, dass ihre Form nicht verändert werden kann. Dies kann erreicht werden mit der Schaltfläche, welche das ausgewählte Teil in eine statische Kopie des Originals konvertiert.

Um das Assembly zu speichern und danach zu schließen kann die Schaltfläche verwendet werden.

Der Zusammenbau
Der Zusammenbau von Teilen erfolgt durch Hinzufügen von Beschränkungen zwischen den Teilen. Nach einer Beschränkung wird A2plus die Teile nach Möglichkeit entsprechend der Beschränkung verschieben.

Um eine Beschränkung zwischen Teilen zu erstellen, halte die Taste gedrückt und wähle jeweils eine Kante oder Fläche von zwei Teilen aus. Klicke dann auf die Werkzeugleisten Schaltfläche der gewünschten Beschränkung. Ein Dialogfeld wird aufgeklappt, das in Abschnitt Beschränkungen beschrieben wird. Die Beschränkung wird in den Modellbaum eingefügt, der an die betroffenen Teile angehängt ist.

Bei komplexen Beschränkungen zwischen Teilen kann A2plus die Beschränkungen möglicherweise nicht lösen. Schau dir daher auch Abschnitt Fehlerbehebung für Strategien zur Lösung solcher Fälle an.

Den Überblick behalten
Je mehr Teile du hinzufügst, desto wichtiger ist es, den Überblick zu behalten. A2plus bietet daher diese Werkzeuge zum Verschieben und Anzeigen von Teilen:


 * Um ein Teil in der Baugruppe zu verschieben, wähle es im Modellbaum aus und verwende die Werkzeugleistenschaltfläche [[Image:A2p MovePart.svg|24px]]. Wenn du das Teil dort platziert hast, wo es dir gefällt, links-klicke mit der Maustaste. Wenn das verschobene Teil bereits Beschränkungen aufweist, wird es durch Drücken der Werkzeugleistenschaltfläche [[Image:A2p solver.svg|24px]] entsprechend platziert, da dies die Auflösung aller Beschränkungen der Baugruppe auslöst.
 * Um eine Beschränkung anzuzeigen, wähle sie im Modellbaum aus und verwende die Werkzeugleistenschaltfläche [[Image:A2p ViewConnection.svg|24px]]. Dadurch wird die gesamte Baugruppe transparent und die beiden Objekte, die über die Beschränkung verbunden sind, werden hervorgehoben. Um zur Normalansicht zurückzukehren, links-klicke in die Baugruppe.
 * Um nur bestimmte Teile in der Baugruppe anzuzeigen, wähle diese Teile im Modellbaum aus und verwende die Werkzeugleistenschaltfläche [[Image:A2p Isolate Element.svg|24px]]. Alternativ kannst du ein bestimmtes Teil ausblenden, indem du es im Modellbaum markierst und drückst, um seine Sichtbarkeit umzuschalten.
 * Um die Transparenzansicht der gesamten Baugruppe umzuschalten, kannst du die Werkzeugleistenschaltfläche [[Image:A2p ToggleTransparency.svg|24px]] verwenden.
 * Jedes Teil kann mit der normalen FreeCAD Bearbeitung transparent gemacht werden. Manchmal geht jedoch die Transparenzeinstellung für Teile beim erneuten Öffnen der Baugruppe aufgrund eines Fehlers in FreeCAD verloren. Als Ausweichlösung kannst du den Werkzeugleistenknopf [[Image:A2p_Restore_Transparency.svg|24px]] verwenden, um die Transparenzeinstellungen wiederherzustellen.

Beschränkungen
Bei der Erstellung einer Beschränkung wird ein solches Dialogfeld angezeigt, nachdem du eine Schaltfläche in der Beschränkungswerkzeugleiste gedrückt hast:

Bei bestimmten Beschränkungen erlaubt es dir, die Richtung der Beschränkung zu ändern. Mit der Schaltfläche kannst du vorab prüfen, ob diese neue Randbedingung von A2plus gelöst werden kann. Falls nicht, wirf einen Blick auf Abschnitt Fehlerbehebung.

Beschränkungen können durch Ändern der Sichtbarkeit deaktiviert werden. Wähle dazu die Beschränkung in der Baumansicht aus und drücke. Dadurch wird die Eigenschaft umgeschaltet. Eine unterdrückte Beschränkung wird bei der Lösung der Baugruppe nicht berücksichtigt.

A2plus bietet die folgenden Beschränkungen:

Punkt auf Punkt
Wähle entweder einen Knoten (Punkt), Kreis oder Kugel auf jedem Teil. Wenn ein Kreis oder eine Kugel ausgewählt wurde, wird dessen Mittelpunkt für die Beschränkung verwendet. Die Werkzeugleistenschaltfläche fügt die Beschränkung  hinzu, die die Knoten deckungsgleich werden lässt.

Punkt auf Linie
Wähle einen Knoten (Punkt), oder kreisförmig Kante (wählt seinen Mittelpunkt aus), oder eine sphärische Fläche (wählt auch seinen Mittelpunkt) auf der einen Seite und ein Kante auf dem anderen Teil. Die Werkzeugleistenschaltfläche fügt die Beschränkung  hinzu. Dadurch wird der Knoten auf die Kante gesetzt.

Punkt auf Ebene
Wähle einen Knoten (Punkt), oder kreisförmige Kante (wählt seinen Mittelpunkt aus), oder eine sphärische Fläche (wählt auch seinen Mittelpunkt) auf einem Teil und eine Ebene auf dem anderen Teil. Die Werkzeugleistenschaltfläche fügt die Beschränkung  hinzu. Im Dialogfeld Beschränkung kannst du einen Versatz zwischen dem Punkt und der Ebene angeben. Dieser Versatz kann auch zwischen beiden Seiten der Ebene umgedreht werden. Wenn der Versatz gleich Null ist, setzt die Beschränkung den Knoten auf die Ebene.

Kugel auf Kugel
Wähle entweder ein kugelförmiges Fläche oder einen Knoten (Punkt) auf beiden Teilen. Die Werkzeugleistenschaltfläche  fügt die Beschränkung  hinzu. Sie bewirkt, dass entweder das Zentrum der Kugeln, das Zentrum der Kugel und der Knoten oder die Knoten deckungsgleich werden.

Circular Edge on Circular Edge
Select a circular edge on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify an offset between the edges. This offset can also be flipped. You can furthermore set the constraint direction and lock the rotation of the parts. If the offset is zero, the constraint will put the edges concentric in the same plane.

Axis Coincident
Select either a cylindrical face or a linear edge on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify the axis direction. The dialog allows you furthermore to lock the rotation of the parts. The constraint will make the axes or lines coincident.

Axis Parallel
Select either a cylindrical face or a linear edge on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify the axis direction. The constraint will make the axes or lines parallel.

Axis on Plane parallel
Select either a cylindrical face or a linear edge on one part and a plane on the other part. The toolbar button adds the constraint. The constraint will make the axis or line parallel to the plane.

Axis on Plane normal
Select either a cylindrical face or a linear edge on one part and a plane on the other part. The toolbar button adds the constraint. The constraint will make the axis or line normal to the plane.

Axis on Plane angle
Select either a cylindrical face or a linear edge on one part and a plane on the other part. The toolbar button adds the constraint. The constraint will at first make the axis parallel to the plane. Then you can adjust the angle for the axis in the appearing constraint settings dialog.

Plane Parallel
Select a plane on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify the constraint direction. The constraint will make the planes parallel.

Plane on Plane
Select a plane on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify a constraint direction and an offset between the planes. This offset can also be flipped. If the offset is zero, the constraint will make the planes coincident.

Plane Angular
Select a plane on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify an angle between the planes. The constraint will make the planes at first parallel and the set the specified angle.

Coincidence at Center of Mass
Select either a closed edge or a plane on both parts. The toolbar button adds the constraint. The constraint dialog allows you to specify an offset between the edges or planes. This offset can also be flipped. You can furthermore set the constraint direction and lock the rotation of the parts. If the offset is zero, the constraint will put the edges or planes into the same plane.

Subassemblies
An assembly can contain other assemblies. They are added like parts by pressing the toolbar button and selecting a  file containing an assembly. Such subassemblies can also be edited like parts using the toolbar button. Please make sure for higher assembly stages that you update the assembly recursively via the toolbar button when there were changes.

Constraint Handling
Possible constraints for a selection are displayed in the toolbar and the Constraint Tools dialog by enabling the corresponding buttons. The Constraint Tools dialog is opened via the toolbar button. It is intended to stay open to be able to add quickly several constraints to the assembly.

Existing constraints can be edited by selecting them in the model tree and then either double-clicking on it or using the toolbar button. This opens the Constraint Properties dialog.

Constraints can be temporarily suppressed by selecting them in the model tree and changing the tree element property.

Constraints can be deleted either by selecting them in the model tree and pressing or by selecting a part with constraints in the model tree and using the toolbar button.

All constraints can be resolved at any time with the toolbar button. If the toolbar button is turned on a resolve is automatically done after every edit of a constraint.

The toolbar button affects the constraint that was added most recently. It flips the constraint direction.

Part Lists
To create part lists of assemblies, the different parts of the assembly must get part info that can be read by A2plus. This is done by editing the part using the toolbar button. In the opened part press the toolbar button and a spreadsheet with the name #PARTINFO# is created.

The structure of the spreadsheet is like this:



Fill out the grey fields with info you have and want to have in the final parts list.

In the assembly or subassembly use the toolbar button. It will ask you if you want to iterate recursively over all subassemblies. Click on Yes. This creates a new spreadsheet with the name #PARTSLIST#. It contains the info from the different #PARTSINFO# spreadsheets of the parts in a list like this:



The position (POS) is automatically set according to the appearance of the parts in the model tree. The top level part will get POS 1.

The quantity (QTY) is automatically calculated from the assembly. If a parts is twice in the assembly it will get QTY 2.

If you have updated a part info you can refresh the parts list by pressing the toolbar button again.

For subassemblies you can also create an info spreadsheet using the toolbar button. When you create or update the parts list of the main assembly this info will be used if you click on No for the question if you want to iterate recursively over all subassemblies. Then the different parts are not in the parts list but only the subassemblies.

Assembly Structure
The toolbar button  creates an HTML file with the structure of your assembly. The file will by default be created in the folder of your assembly file. The structure looks like this one:

Degrees of Freedom
The button labels every part of the assembly with its degrees of freedom. Furthermore it outputs a list with all parts and their dependencies. The list is output into FreeCAD's widget Report view. If this widget is currently not visible, it can either be shown by right-clicking into an empty part of the FreeCAD toolbar area and then choosing it in the appearing context menu or with the menu.

The degrees of freedom labels can be removed by clicking the button again.

Part Labels
The button labels every part of the assembly in the 3D view with its name. The part labels can be removed by clicking the button again

Shape of whole Assembly
Sometimes it is necessary to have the whole assembly combined as one shape. This shape can then for example be used for 3D printing in the Mesh workbench or for drawings in the TechDraw workbench. It is created using the toolbar button. The shape is by default not made visible. Use the same toolbar button to update the shape in case of changes in the assembly.

Convert absolute Paths to relative Ones
With the menu you can convert absolute paths of imported parts to relative ones.

Preferences
The a2plus preferences can be accessed via FreeCAD's menu and there in the section A2plus. You can set the following options:

Default solving method

 * Use solving of partial systems : The solver begins with a part that has the property set to true and a part constrained to it. All other parts are not calculated. If a solution could be found, the next constrained part is added to the calculation and so on.
 * Use "magnetic" solver, solving all parts at once : The solver tries to move all parts at once in direction to a part that has the property set to true. Note that this will in most cases take more time for the calculation of a solution.
 * Force fixed position : This sets the property to true for all parts in the assembly. Then no calculation is actually performed since all parts will always be fixed to the positions where they were created.

Default solver behaviour

 * Solve automatically if a constraint property is changed : The solver will automatically be started. The same as turning on the toolbar button [[Image:A2p ToggleAutoSolve.svg|24px]].

Behaviour when updating imported parts

 * Recalculate imported parts before updating them : All parts of the assembly, including subassemblies, will be opened in FreeCAD to be reconstructed using values from spreadsheets. This feature is designed to construct fully parametrically. Note: This feature is very experimental and not recommended for important projects. Known problems:
 * The assembly can be destroyed because of wrong references to topological names in parts
 * Master spreadsheets can get broken when they are edited while a referenced part file is already closed. This can crash FreeCAD.


 * Enable recursive update of imported parts : Opens all subassemblies recursively to update them.


 * Use experimental topological naming : While importing parts to the assembly an algorithm generates topological names for each subelement of the imported shape. The topological names are written into the . When an imported part needs to be updated, these topological names are used to update the subelements of the constraints. So assemblies get more robust against volatile subelement numbers of FreeCAD. Note: This increases file sizes and calculation time during import of parts. If topological naming should be used it has to be activated before the assembly is created.


 * Inherit per face transparency from parts and subassemblies : Use colour and transparency settings from imported parts. Note: This feature is very experimental and not recommended for important projects.


 * Do not import invisible shapes : This will hide invisible datum/construction shapes. Note: No constraints must be connected to datum/construction shapes in higher or other subassemblies. Otherwise you can break the assembly.


 * Use solid union for importing parts and subassemblies : All imported parts will directly be put together as union. This feature is useful for FEM simulations or 3D-printing if only one solid is allowed. The alternative is to create a shape of the whole assembly later on.

User interface settings

 * Show constraints in toolbar : If this option is not used, the toolbar buttons for the different constraints are not visible to save space in the toolbar. New constraints can still be set using the Constraint Tools dialog (toolbar button [[Image:A2p DefineConstraints.svg|24px]]).
 * Use native file manager of your OS : If this option is used, you get the file dialog of your OS when selecting files for assemblies.

Storage of files

 * Use relative paths for imported parts : Uses relative file paths to the part files.
 * Use absolute paths for imported parts : Uses absolute file paths to the part files.
 * All files are in this project folder : All project files have to be in the specified folder. It doesn't matter if they are in subfolders of this folder. Note: No file is allowed to exist several times in the folder (e.g. in different subfolders). This option is helpful to work on different machines because then one only has to copy the project folder.

Troubleshooting
Sooner or later you will get the problem that A2plus cannot solve the constraints you set. To overcome this, there are different strategies:

Using the Conflict Finder Tool
This is the safest method when you have several constraints because this tool attempts to solve one constraint after another until it finds the conflicting constraint. Then you can go on with the other strategies to resolve the identified constraint. The tool is called using the toolbar button.

Checking Constraint Direction
Sometimes constraints seem to be consistently defined but they can nevertheless not be solved. An example: Assume you have a constraint set for two planes. Now you want to set for the same planes the constraint and A2plus cannot solve this. Then the constraint directions of and  are different. Use the same direction for both constraints to fix this.

A2plus offers to automatically check the right direction for all constraints of the assembly using the toolbar button.

Deleting Constraints
Most cases of unsolvable constraints occur directly when adding a new constraint. The solution is then to delete the constraint you added last. A2plus will propose this, too.

Sometimes the deletion strategy is the only one, for example when you edited a part in FreeCAD so that faces or edges connected to constraints are missing. You should then delete one constraint that is connected to the changed part at a time. Use the toolbar button after every deletion to see if you reached a solvable state.

When you got an assembly that can be solved, add step by step the constraints you need.

Moving Parts
In some cases the solver only needs better start values to solve the constraints. Take for example the case that you have an axle part and a wheel part. You add a constraint and get no info that the solver failed but the parts are not moved accordingly and in the Report view widget of FreeCAD you see "REACHED  POS-ACCURACY :0.0". A solution for this is to move the parts closer to that position you like to get by the constraint.

Note: Assure that at least one part of the constraint has the property set to false.

Setting the Tip Property
If you miss some features of your part after the import to an A2plus assembly, check the property.

A2plus imports bodies of parts with all their features up to the tip feature. This is sensible because setting the tip to a certain feature means that all features behind the tip should not appear in the final part. So if you miss a part feature in A2plus, open the part via the toolbar button, then select a body and look at its property. If the tip is not at the feature where you want it, right-click on the feature where the tip should be and choose. Finally save the part and reload the assembly using the toolbar button.

Repairing Assembly Tree
If you cannot see a clear reason why some constraints cannot be resolved, you can try to use the toolbar button. This will resolve all constraints and re-group then again under the different parts.

Migrating old A2plus assemblies
Assemblies created with A2plus older than March 2019 do not show the correct icons for imported parts and have obsolete properties. These assemblies can be migrated to A2plus version 0.4.35 and newer using the menu. After doing this, you must save and reopen your assembly file.

Avoiding Accented Characters
This strategy is not necessary for Windows.

On some operating systems you can get problems if the file names or the file paths of parts or the assembly contain accented characters. Therefore avoid such characters and also special characters in general.

Fixing Position
This strategy is no longer necessary for assemblies created with A2plus 0.3.11 or newer because A2plus issues now a warning for missing fixed positions.

When you set a constraint between two parts and no part has the property set to true or is connected by a constraint to a part with  set to true, the constraint cannot be solved. The same happens if both parts of the constraint have set to true.

Then A2plus outputs the info about the failed solution, but sometimes you only see that the parts are not moved accordingly and in the Report view widget of FreeCAD you see "REACHED POS-ACCURACY :0.0". This means the solver finished without errors but it could actually not solve the constraints.

Therefore check that at least one of your parts in the assembly has set to true. Then assure that you only set constraints to a part which is somehow connected to the fixed part. To visualise these dependencies, see section Assembly Structure.

Rotating Parts
This strategy is no longer necessary for assemblies created with A2plus 0.4.0 or newer because A2plus rotates the parts now automatically a bit in the background to get a sufficient start angle for the solver.

The solver often fails for the constraint if the two selected planes have currently an angle of 0° or 180°. (The parts are not moved accordingly and in the Report view widget of FreeCAD you see "REACHED POS-ACCURACY :0.0".) A solution for this is to rotate one part by a few degrees using FreeCAD's transform feature (right-click on the part in the model tree and select in the context menu ).

Note: Assure that at least one part of the constraint has the property set to false.

Animation
A2plus offers animations via dragging and via Python scripts.

Dragging
Dragging animations are interactive since you trigger it by dragging a part of the assembly. To get these kind of animations:
 * 1) Fully constrain the part whose movement or rotation should be animated
 * 2) Click on the toolbar button [[Image:A2p MovePartUnderConstraints.svg|24px]]. This enables the dragging mode.
 * 3) Click on the desired part in the assembly.
 * 4) Now you can move the mouse and the part will follow the movement of the mouse within the defined constraints.
 * 5) To end the dragging mode, left click in the assembly or press ESC.

Here is an example assembly to try out the dragging animation: A2p_example-for-dragging-animation.FCStd



Scripting
Despite the dragging mode offers nice interactive animations, they are sometimes not precise enough for screencasts or videos. Scripted animations have the advantage that they animate movements and rotations in a defined way. You can for example rotate a part by exactly 10° back and forth. The following examples use an assembly where a part should be rotated. If you try to animate this using the dragging mode, you will see how hard it is to get a back and forth rotation that you can e.g. show your boss in a presentation. With the interactive example script, however, this is an easy task.

A scripted animation works usually this way:
 * 1) The assembly is fully constrained
 * 2) The script changes a parameter, for example the position or rotation angle of a part
 * 3) After the parameter change, the assembly constraints are solved
 * 4) Step 2. and 3. are repeated to get the animation

It is also possible to change instead of a placement parameter a constraint, for example the distance between 2 planes.

Simple Script Example
The simplest way to script an animation is a non-interactive animation that follows a defined movement. Here is an example: First download this assembly file: A2p_animated-example.FCStd and also this Python script: A2p_animation-example-script.py.

This is the content of the script and the lines beginning with a '#' describe what the different script lines do:

To use the script to perform the animation, we must
 * 1) Open the assembly file in FreeCAD.
 * 2) Open the script file in FreeCAD.
 * 3) Click on the toolbar button [[Image:Menu_Std_DlgMacroExecute_fr_02.png|24px]] to execute the script (also called macro).
 * 4) Change to the tab of the assembly to see the rotation.

To practice, just change something in the script and execute it afterwards. For example increase step to 5.

This is the result of the example animation:



Interactive Script Example
The first script example demonstrated how to create an animation without any user feedback. For most applications you need to interact with the animation. For example the interesting issue in the example is to see how the driving pins cross the center groove of the wheel. To have a closer look you might present this detail to your colleagues or boss. Therefore you need an interactive solution.

This can be done by using a custom animation dialog with a slider. By moving the slider you can set the rotation angle and therefore rotate back and forth at interesting position.

We use the same assembly file: A2p_animated-example.FCStd and this Python script: A2p_animation-example-script.py.

This is the content of the script to get the interactive animation dialog:

The dialog defined in the script looks like this:



Script Commands
To understand the script syntax better, here is some command info:

Here we change the placement property of the part get got previously as. This property gets the angle as radian. The function from the library  converts the angle from degree to radian.

The property uses the current placement axis of the part (in our example the X-axis). To rotate the part e.g. around the Z-axis one can set the rotation axis (before calling the rotation command) using the command:

Instead of rotating, parts can also be moved. To change for example the placement in Y-direction of the wheel, the command would be:

In this case we would not define the variable but  that we change on every loop run.

There are different ways to set the placement of a part. Some are documented here. Unfortunately there is no list (yet) with all possible placement commands.

This is an A2plus-specific command. It solves the assembly constraints of the assembly we previously got as. The option specifies if FreeCAD should store every change in the undo/redo stack. For large animations you might therefore set it to.