Assembly3 Workbench/pl

Wprowadzenie
Assembly3 jest zewnętrznym środowiskiem pracy, które jest używane do wykonywania złożeń różnych części zawartych w jednym lub wielu dokumentach. Środowisko to bazuje na kilku zmianach funkcji rdzenia FreeCAD w wersji 0.19 (np. App Link). Dlatego środowisko Assembly3 nie może być używane ze starszymi wersjami programu.

Głównymi cechami Środowiska Assembly3 są
 * dynamiczny/interaktywny solwer. Oznacza to, że możesz przesuwać części myszką, podczas gdy solwer będzie ograniczał ruch. To pozwala na przykład, na połączenie koła z osią i interaktywne poruszanie kołem przy pomocy myszki.
 * łącza. To oznacza, że możesz używać pojedynczej części, np wkrętu, wielokrotnie w złożeniu (w różnych miejscach) bez kopiowania geometrii.
 * łącza zewnętrzne. Możliwe jest posiadanie dokumentu FreeCAD zawierającego tylko złożenie, a nie części. Każda z części może być osobnym plikiem. Pliki mogą znajdować się nawet w bibliotece lub gdziekolwiek indziej w systemie plików. Jedynym wymogiem jest to, że ten plik musi być załadowany, kiedy tworzone jest łącze. Po utworzeniu łącza, plik musi być otwarty to wykonywania aktualizacji łączy dotyczących tego pliku. Assembly3 rozwiązuje to przez otwieranie plików w tle, gdy jest to konieczne.
 * złożenia hierarchiczne. W prawdziwym życiu złożenia mechaniczne mogą składać się z podzłożeń. One mogą składać się z kolejnych podzłozeń, a te z kolejnych, itd.
 * zamrażanie złożeń. Jako, że procesor potrafi zarządzać tylko określoną liczbą wiązań w czasie rzeczywistym, zamrażanie złożeń pozwala na używanie wiązań nawet do wielkich złożeń. Po zamrożeniu ukończonych złożeń lub wiązań, które nie muszą pozostać dynamiczne (np. spawane, skręcane lub klejone części) są one wyłączane z aktualizacji obliczeń i uznawane przez solwer Assembly3 za ustaloną geometrię.
 * Zauważ inne podejścia rozwiązujące ten problem odmiennie, np. Assembly4_workbench_icon.svg Środowisko Assembly4.

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Paski narzędzi
Środowisko Assembly3 zawiera następujące paski narzędzi - stan na rok 2020.

Główny Pasek Narzędzi

 * Assembly3_ToolbarMain.png


 * Główny Pasek Narzędzi zawiera narzędzia, które obejmują najczęściej używane funkcje programu. Skróty klawiaturowe są podawane przez podpowiedzi narzędzi.


 * [[Image:Assembly Add Existing Part.svg‎‎|32px]] Create assembly: Add an assembly folder
 * [[Image:Assembly New Group.svg‎‎|32px]] Group objects: Group objects
 * [[Image:Assembly New Element.svg‎‎|32px]] Create element: Create element.
 * Import from STEP. This has two settings
 * [[Image:Assembly Import.svg‎‎|32px]] Import STEP files: Import STEP files
 * [[Image:Assembly ImportMulti.svg‎‎|32px]] Import as multi-document: Import as multi-document
 * [[Image:Assembly3_workbench_icon.svg‎‎|32px]] Resolve constraints: Resolve constraints
 * [[Image:Assembly QuickSolve.svg‎‎|32px]] Quick solve: Quick resolve constraints
 * [[Image:Assembly Move.svg‎‎|32px]] Move part: Move parts in 3D, this is specific to Assembly3
 * [[Image:Assembly AxialMove.svg‎‎|32px]] Axial move: Axial move parts in 3D, this is the classical tool available elsewhere in FreeCAD
 * [[Image:Assembly QuickMove.svg‎‎|32px]] Quick move: This will attach the part selected in the tree to the mouse cursor. It will change the position of the part when you click.
 * Often added parts are stacked upon each other in the origin. Use this function to grab a part you can not see.
 * [[Image:Assembly LockMover.svg‎‎|32px]] Lock mover: Lock mover for fixed part. Toggle Button. When this is un-selected you can move the parts that have a "Locked" constraint.
 * [[Image:Assembly_TogglePartVisibility.svg‎‎|32px]] Toggle part visibility: This toggles the visiblity of the selected part on/off.
 * Note that this differs from using space. Using space with selected items from a sub-assembly in the 3D view often does not behave as expected. Use this function in those cases (or shortcut A-Space)
 * [[Image:Assembly Trace.svg‎‎|32px]] Trace part move: Trace part move (TBD)
 * [[Image:Assembly AutoRecompute.svg‎‎|32px]] Auto recompute: Auto recompute. Usually enabled.
 * May be un-selected when repairing constraints or fixing parts where the solver gives a "do not converge" message (e.g. by turning the part 180deg)
 * [[Image:Assembly SmartRecompute.svg‎‎|32px]] Smart recompute: Smart recompute. Usually enabled.
 * [[Image:Assembly AutoFixElement.svg‎‎|32px]] Auto fix element: Element Auto Fixing. Experimental feature in 0.19_pre
 * Element Style. This has two settings
 * [[Image:Assembly AutoElementVis.svg‎‎|32px]] Auto element visibility: Auto element visibility
 * [[Image:Assembly ShowElementCS.svg‎‎|32px]] Show element coordinate system: Show element coordinate system
 * Workplane and origin. Adds a workplane, placement or origin. A part must be selected. This has five settings
 * [[Image:Assembly Add Workplane.svg‎‎|32px]] Add workplane: Add XY workplane
 * [[Image:Assembly Add WorkplaneXZ.svg‎‎|32px]] Add XZ workplane: Add XZ workplane
 * [[Image:Assembly Add WorkplaneZY.svg‎‎|32px]] Add ZY workplane: Add YZ workplane
 * [[Image:Assembly Add Placement.svg‎‎|32px]] Add placement: Add placement
 * [[Image:Assembly Add Origin.svg‎‎|32px]] Add Origin: Add Origin
 * [[Image:Assembly TreeItemUp.svg‎‎|32px]] Move item up: Move selected tree item up
 * [[Image:Assembly TreeItemDown.svg‎‎|32px]] Move item down: Move selected tree item down
 * Allows to sort Parts, Elements or Constraints in the tree. Element roll over (top to bottom and vice versa). Only works for a single selection.
 * [[Image:Assembly ConstraintMultiply.svg‎‎|32px]] Multiply constraint: Multiply Constraint. This can be selected if multiple parts and suitable Elements are present.
 * It is used e.g. to assign multiple fasteners of the same type into multiple holes with one constraint.

Główny Pasek Wiązań

 * [[Image:Assembly3_ToolbarConstraints_1.jpg|700px]]


 * Niektóre narzędzia są w rzeczywistości menu dla kolejnych przyborów.


 * [[Image:Assembly ConstraintLock.svg‎‎|32px]] Locked: Add a "Locked" constraint to fix one or more parts.
 * You must select a geometry element of the part.
 * If you fix a vertex or an edge the part is still free to rotate around the vertex or edge.
 * Fixing a face will completely lock the part.
 * ([[Image:Assembly ConstraintAlignment.svg‎‎|24px]]) Plane Alignment: Add a "Plane alignment" constraint to align planar faces of two or more parts.
 * The faces become coplanar or parallel with an optional distance.
 * ([[Image:Assembly ConstraintCoincidence.svg‎‎|24px]]) Plane Coincidence: Add a "Plane coincidence" constraint to coincide planar faces of two or more parts.
 * The faces are coincided at their centers with an optional distance.
 * [[Image:Part Attachment.svg‎‎|32px]] Attachment: Add an "Attachment" constraint to attach two parts by the selected geometry elements.
 * This constraint completely fixes the parts relative to each other.
 * [[Image:Assembly ConstraintAxial.svg‎‎|32px]] Axial Alignment: Add an "Axial alignment" constraint to align edges/faces of two or more parts.
 * The constraint accepts
 * linear edges, which become collinear,
 * planar faces, which are aligned using their surface normal axis,
 * and cylindrical face, which are aligned using the axial direction.
 * Different types of geometry elements can be mixed.
 * ([[Image:Assembly ConstraintOrientation.svg‎‎|24px]]) Orientation: Add an "Orientation" constraint to align faces of two or more parts.
 * The planes are aligned to have the same orientation (i.e. rotation)
 * [[Image:Assembly ConstraintMultiParallel.svg‎‎|32px]] Multi parallel: Add a "Multi parallel" constraint to make planar faces or linear edges of two or more parts parallel.
 * ([[Image:Assembly ConstraintAngle.svg‎‎|24px]]) Angle: Add an "Angle" constraint to set the angle of planar faces or linear edges of two parts.
 * ([[Image:Assembly ConstraintPerpendicular.svg‎‎|24px]]) Perpendicular: Add a "Perpendicular" constraint to make planar faces or linear edges of two parts perpendicular.
 * [[Image:Assembly ConstraintPointCoincident.svg‎‎|32px]] Point coincident: Add a "Point coincident" constraint to coincide two points in 2D or 3D.
 * [[Image:Assembly ConstraintPointInPlane.svg‎‎|32px]] Point on plane: Add a "Point on plane" to constrain one or more point onto a plane.
 * [[Image:Assembly ConstraintPointOnLine.svg‎‎|32px]] Point on line: Add a "Point on line" to constrain a point onto a line in 2D or 3D.
 * [[Image:Assembly ConstraintPointOnCircle.svg‎‎|32px]] Point on circle: Add a "Point on circle" to constrain one or more points on to a clyndrical surface defined by a cricle.
 * Note that you must select a point (any geometry element can define a point), and then select the circle (or clyndrical surface),
 * after which you can add more points to your selection if you want.
 * [[Image:Assembly ConstraintPointsDistance.svg‎‎|32px]] Points distance: Add a "Points distance" to constrain the distance of two or more points.
 * [[Image:Assembly ConstraintPointPlaneDistance.svg‎‎|32px]] Point plane distance: Add a "Point plane distance" to constrain the distance between one or more points and a plane.
 * [[Image:Assembly ConstraintPointLineDistance.svg‎‎|32px]] Point line distance: Add a "Point line distance" to constrain the distance between a point and a linear edge in 2D or 3D.
 * [[Image:Assembly ConstraintSymmetric.svg‎‎|32px]] Symmetric: Add a "Symmetric" constraint to make geometry elements of two parts symmetric about a plane.
 * The supported elements are linear edge and planar face.
 * [[Image:Assembly ConstraintMore.svg‎‎|32px]] More: Toggle toolbars for more constraints
 * Not really a constraint but a toggle switch to show/hide the Additional Constraints Toolbars.

Additional Constraints Toolbars

 * [[Image:Assembly3_ToolbarConstraints_2.jpg|700px]]


 * Możesz je uruchomić przez wybranie ikony '...' na Głównym Pasku Narzędzi.


 * [[Image:Assembly ConstraintPointDistance.svg‎‎|32px]] Point distance: Add a "Point distance" to constrain the distance of two points in 2D or 3D.
 * [[Image:Assembly ConstraintEqualAngle.svg‎‎|32px]] Equal angle: Add an "Equal angle" to equate the angles between two lines or normals.
 * [[Image:Assembly ConstraintPointsSymmetric.svg‎‎|32px]] Points symmetric: Add a "Points symmetric" constraint to make two points symmetric about a plane.
 * [[Image:Assembly ConstraintGeneral.svg‎‎|24px]] Symmetric horizontal: Symmetric horizontal
 * [[Image:Assembly ConstraintGeneral.svg‎‎|24px]] Symmetric vertical: Symmetric vertical
 * [[Image:Assembly ConstraintSymmetricLine.svg‎‎|32px]] Symmetric line: Add a "Symmetric line" constraint to make two points symmetric about a line.
 * [[Image:Assembly ConstraintPointsHorizontal.svg‎‎|32px]] Points horizontal: Add a "Points horizontal" constraint to make two points horizontal with each other when projected onto a plane.
 * [[Image:Assembly ConstraintPointsVertical.svg‎‎|32px]] Points vertical: Add a "Points vertical" constraint to make two points vertical with each other when projected onto a plane.
 * [[Image:Assembly ConstraintLineHorizontal.svg‎‎|32px]] Line horizontal:Add a "Line horizontal" constraint to make a line segment horizontal when projected onto a plane.
 * [[Image:Assembly ConstraintLineVertical.svg‎‎|32px]] Line vertical: Add a "Line vertical" constraint to make a line segment vertical when projected onto a plane.
 * [[Image:Assembly ConstraintArcLineTangent.svg‎‎|32px]] Arc line tangent: Add an "Arc line tangent" constraint to make a line tangent to an arc at the start or end point of the arc.


 * [[Image:Assembly ConstraintSketchPlane.svg‎‎|32px]] Sketch plane: Add a "Sketch plane" to define the work plane of any draft element inside or following this constraint.
 * Add an empty "Sketch plane" to undefine the previous work plane.
 * [[Image:Assembly ConstraintLineLength.svg‎‎|32px]] Line length: Add a "Line length" constrain the length of a non-subdivided Draft.Wire.
 * [[Image:Assembly ConstraintEqualLength.svg‎‎|32px]] Equal length: Add an "Equal length" constraint to make two lines of the same length.
 * [[Image:Assembly ConstraintLengthRatio.svg‎‎|32px]] Length ratio: Add a "Length ratio" to constrain the length ratio of two lines.
 * [[Image:Assembly ConstraintLengthDifference.svg‎‎|32px]] Length difference: Add a "Length difference" to constrain the length difference of two lines.
 * [[Image:Assembly ConstraintLengthEqualPointLineDistance.svg‎‎|32px]] Length Equal Point Line Distance: Add a "Length Equal Point Line Distance" to constrain the distance
 * between a point and a line to be the same as the length of a another line.
 * [[Image:Assembly ConstraintGeneral.svg‎‎|24px]] ( [[Image:Assembly ConstraintEqualLineArcLength.svg‎‎|32px]] )Equal Line Arc Length: Add an "Equal Line Arc Length" constraint to make a line of the same length as an arc.
 * [[Image:Assembly ConstraintMidPoint.svg‎‎|32px]] Mid point: Add a "Mid point" to constrain a point to the middle point of a line.
 * [[Image:Assembly ConstraintDiameter.svg‎‎|32px]] Diameter: Add a "Diameter" to constrain the diameter of a circle/arc.
 * [[Image:Assembly ConstraintEqualRadius.svg‎‎|32px]] Equal radius: Add an "Equal radius" constraint to make two circles/arcs of the same radius.
 * [[Image:Assembly ConstraintPointsProjectDistance.svg‎‎|32px]] Points project distance: Add a "Points project distance" to constrain the distance of two points projected on a line.
 * [[Image:Assembly ConstraintEqualPointLineDistance.svg‎‎|32px]] Equal point line distance: Add an "Equal point line distance" to constrain the distance
 * between a point and a line to be the same as the distance between another point and line.
 * [[Image:Assembly ConstraintColinear.svg‎‎|32px]] Collinear: Add a "Collinear" constraint to make two lines collinear.


 * Paski Narzędzi Wiązań będą głównym interfejsem używanym podczas składania części.
 * Są one domyślnie wyszarzone, i zostają aktywowane gdy przynajmniej jedna ściana, linia lub punkt części jest wybrana.
 * Ogólnie wybierasz Elementy, które powinny zostać połączone a następnie wybierasz typ wiązania.
 * Ramki w różnych barwach oznaczają różną charakterystykę wiązań:
 * czy to 2D/3D albo czy więcej niż dwa Elementy mogą zostać dodane.
 * Dokładny opis znajduje się w Wiki na Githubie.

Pasek Narzędzi Nawigacji

 * [[Image:Assembly3_ToolbarNavigation.jpg|100px]]


 * Theses functions are useful when working with an assembly with a hierarchy of linked external files


 * [[Image:Assembly_GotoRelation.svg‎‎|32px]] Go to relation: Select the corresponding part object in the relation group
 * [[Image:LinkSelect.svg‎‎|32px]] Select linked object: Select the linked object
 * [[Image:LinkSelectFinal.svg‎‎|32px]] Select linked final: Select the deepest linked object

Measurement Toolbar

 * [[Image:Assembly3_ToolbarMeasurement.jpg|150px]]


 * The Measurement toolbar adds functions to measure the distance or the angle between two objects


 * [[Image:Assembly MeasurePointDistance.svg‎‎|32px]] Measure points: Add a "Measure points" to measure the distance of two points in 2D or 3D.
 * [[Image:Assembly MeasurePointLineDistance.svg‎‎|32px]] Measure point to line: Add a "Measure point to line" to measure the distance between a point and a linear edge in 2D or 3D.
 * [[Image:Assembly MeasurePointPlaneDistance.svg‎‎|32px]] Measure point to plane: Add a "Measure point to plane" to measure the distance between a point and a plane.
 * [[Image:Assembly MeasureAngle.svg‎‎|32px]] Measure angle: Add a "Measure angle" to measure the angle of planar faces or linear edges of two parts.


 * There is no function to measure a radius or diameter.
 * The measurement tools survive part changes, e.g. the distance between edges of a cube when the cube is re-sized.
 * As the constraints the calculations are done in real time and updated upon any change. Behind the scenes, the function is very similar to the constraints. The distance or angle is calculated between Elements in the same way as for constraints. The display in the tree works in the same way.

As usual you can modify the tool bars and add or remove single tools. Be sure to check the menu Assembly3 for functions that may not be present in the tool bars.

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Wiązania
Projektant używa wiązań by uzyskać określony efekt relacji dwóch części. Sztuką jest wybranie właściwych wiązań dla najlepszego poradzenia sobie z danym problemem. Każdy usunięty stopień swobody w teorii powinien być usunięty tylko raz między dwoma obiektami, ale w praktyce wiele narzędzi CAD tworzy nadmiarowe kombinacje wiązań, często kompensowane przez skomplikowane algorytmy, a czasami nie. Assembly3 używa algorytmów do wykrycia i kompensacji nadmiarowych wiązań, ale zdecydowanie one nie są jeszcze dojrzałe. Dlatego w praktyce Assembly3 by uniknąć problemów należy być świadomym jak wiele stopni swobody (DOF) zostało użytych i które mogą być jeszcze zablokowane przez wiązania. Żadna część nie powinna być połączona przez wiązania używające więcej niż 6 stopni swobody.


 * Note: Jeśli solwer spotka kombinację której nie może rozwiązać, wyrzuci błąd. Jest bardzo trudno solwerowi znaleźć co spowodowało problem, więc zwykle z tego wyrzuconego błędu nie będzie jasne gdzie jest ten problem. W skomplikowanych złożeniach może to prowadzić do uciążliwego poszukiwania problemu. Niestety nie ma prostego sposobu na uniknięcie tego. Jednak przydatna jest pełna świadomość jak działa system (np. zobacz Elementy poniżej), używanie komunikatywnych nazw dla wszystkich biorących udział komponentów i dodawanie kolejnych wiązań tylko gdy solwer już rozwiąże dotychczasowe złożenie. Bardzo przydatnym do wyśledzenia problemu jest funkcja "Menu kontekstowe/Deaktywuj" każdego z Wiązań.

Wiązania Assembly3 określają ograniczenia pozycji lub orientacji pomiędzy dwoma Elementami. Niektóre wiązanie działają nawet więcej niż z dwoma Elementami. Elementem może być ściana, linia lub krawędź lub punkt części. Ogólnie wiązania definiowane są przez wybranie żądanych Elementów i późniejsze wybranie wiązania z paska narzędzi Wiązań.

Other
 * Fixes 6 DOF, leaves 0 DOF:
 * Lock: The lock constraint fixes all DOFs for a face. It should be used for one base part in each assembly. You may also want to enable the "MoveLock" function (in the tool bar) so that the part can not be moved accidentially. Normally it does not matter which face/line/point you use to fix a part. Also note that the lock is only valid for the direct assembly, i.e. in case of a sub-assembly the parent assembly would still require a locked part on its own.
 * Attachment: Makes both elements coordinate systems equal for all axes. This is computation wise the most inexpensive function and should be used where ever possible. Note that you could use the element properties to compensate for offsets and angles if the two elements are not perfectly aligned.
 * Fixes 5 DOF, leaves 1 DOF:
 * Plane Coincident: fixes Tx,Ty,Tz, Rx,Ry. Only Rz is free. There remains the rotation around the normal passing through the ‘‘center of the plane’’.
 * Fixes 4 DOF, leaves 2 DOF:
 * Axial Alignment: fixes Tx,Ty, Rx,Ry. Only Tz, Rz are free. There remains the rotation around the axis of the shape and the translation along this same axis. Two PointOnLine constraints (if the two points are different) give the same result. The '‘Colinear'’ constraint too.
 * PointOnLine: This eliminates the translation and rotation along the normals to the reference line. Only the translation and rotation along the line axis is allowed.
 * Fixes 3 DOF, leaves 3 DOF:
 * Same Orientation: fixes Rx,Rz,Rz. All T's remain free.
 * Points Coincident: fixes Tx,Ty,Tz. All R's remain free.
 * PointOnPoint constraint eliminates the 3 translations.
 * Plane Alignment: fixes Tz, Rx,Ry. In plane motion and Rz. This eliminates the translation along the normal to the reference plane and the two rotations around the axes of this plane.
 * Fixes 2 DOF, leaves 4 DOF:
 * Multi Parallel: fixes Rx,Ry. all T's and Rz remain. This eliminates the two rotations around the axes of the reference plane.
 * Fixes 1 DOF, leaves 5 DOF:
 * Points in Plane: Fixes Tz. This eliminates the translation along the normal to the reference plane.
 * Points Distance: fixes the distance between the Element origins.
 * This gives you more freedom than Points in Plane
 * Points on Circle: fixes Tz and partially Tx,Ty. Freezes the point translation (or several points) on a circle or disk area. You must pick the circle second. This leaves all rotations free and gives limited translation in the circle reference plane.

'': Note: In the following list Tx,Ty,Tz and Rx,Ry,Rz are used to describe translations and rotations about the reference coordinate systems of the involved Element's. This is not always exact or fully defined, e.g. when a line is involved it is not defined if it runs in X, Y or any angle in betweeen. The system is used for bevity and easy comparison in favour of a correct but more complex definition. So Z is generally the normal direction of any faces involved. Please feel free to modify this with a better approach with improved readability.''

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Elementy
Elementy są specyficznym terminem w środowisku Assembly3 i ważne jest zrozumienie Elementów by zrozumieć jak Assembly3 powinno być używane.

Pomocne jest myślenie o Elementach jako ogólnym określeniu dla 'wybieralnej pozycji' części, np. ściany, krawędzi, okręgu lub narożnika czy innego punktu. Pozycje które wybierasz aby związać je są tymi Elementami. W drzewie folderu Assembly znajdują się trzy podfoldery. Oprócz "Parts" i "Constraints" jest tam folder nazwany "Elements", który jest pusty tak długo jak nie ma dodanych żadnych wiązań. Podczas dodawania wiązania, samo wiązanie dostanie dwa (lub więcej) listki, są one wybranymi "Elementami". Dodatkowo zostają one dodane do folderu "Elements", który jest po prostu listą wszystkich Elementów użytych w złożeniu. Dobrym pomysłem jest zmiana ich nazw (przyciskiem F2), szczególnie w większych złożeniach.

Spójrzmy na przykład
 * Stwórz nowy plik i z środowiska Część dodaj prostopadłościan i walec. Ustawimy walec na prostopadłościanie. Najpierw utwierdzimy część bazową, w naszym przypadku prostopadłościan. Wybierz dolną ścianę prostopadłościanu i wybierz wiązanie "Locked" (pierwsza ikona na pasku Wiązania). Wybierz górną ścianę walca i górną ścianę prostopadłościanu. Następnie wybierz wiązanie "Plane Coincident". W tym momencie walec zostanie przesunięty na prostopadłościan i w drzewie, pod "Constraints", zostanie dodany nowy listek z dwoma węzłami podrzędnymi. Dodatkowo te same węzły podrzędne zostały dodane pod "Elements". Jeśli twój walec jest w środku prostopadłościanu zamiast na prostopadłościanie, poprawmy to najpierw: wybierz węzeł podrzędny pod "Constraints", który wskazuje na ścianę walca i przy pomocy kliknięcia prawym przyciskiem myszy wybierz w menu kontekstowym "Flip Part". Teraz walec jest już ustawiony na prostopadłościanie.

Kluczową rzeczą do zrozumienia jest to, że wiązanie działa na łączach do Elementów z listy w folderze drzewa "Elements". To pozwala na utrzymywanie nienaruszonej struktury wiązań podczas zmiany części. To jest bardzo trudne do zrozumienia bez przywołania przykładu.

Spójrzmy ponownie na powyższy przykład
 * Uwaga: upewnij się, że dodałeś wiązanie "Lock" to prostopadłościanu, bo inaczej przykład będzie wyglądał myląco
 * W oknie CAD wybierz inną ścianę prostopadłościanu. W tej chwili pracujemy tylko w widoku drzewa. Przesuń się myszą do drzewa, w miejsce gdzie prostopadłościan powinien zostać wybrany. Przeciągnij prostopadłościan do folderu "Elements". Upuść go na nazwę "Elements", a nie w żadne inne miejsce folderu - później zobaczymy dlaczego. Powinieneś zobaczyć kolejny Element dodany do listy "Elements". Teraz w folderze "Constraints" wybierz węzeł podrzędny dla ściany prostopadłościanu w wiązaniu "Plane Coincident" i usuń go. Wiązanie będzie pokazywać znak wykrzyknienia, ponieważ brakuje mu jednego Elementu. Zauważ, że usuwając Element w Wiązaniu nie usunęliśmy go z listy. Jest tak ponieważ wiązanie było tylko łączem do Elementu na liście. Teraz weźmy nowododany Element w liście "Elements" i przeciągnijmy go na wiązanie "Plane Coincident". W tym momencie walec przesunął się na drugą zaznaczoną ścianę Może być konieczne ponowne wybranie "Flip Part" z menu kontekstowego, jeśli walec znów znajduje się w środku prostopadłościanu.

The example showed that without removing the constraint we can change the Elements that are used for the constraint. The same way we can move the cylinder to a totally different part. After playing around with this example a bit more, you will note some additional things as
 * If you rename an Element in the list, the name will be changed in all Constraints.
 * you can use one Element in the list in several constraints.
 * You can use the Property Window of an Element to add Offsets. In the example this could move the cylinder around on the cube face.
 * you can use the "Show Element Coordinate System" button in the main toolbar to see what 'ContextMenu/Flip Part' and 'ContextMenu/Flip Element' are doing. Be sure to look what happens in the Property Window.
 * you can add a constraint in a totally different order: First add some Elements to the 'Elements List' (naming is useful, e.g. "Cube Top Face" or "Cube Front Face"), then add a constraint without selecting anything - it will be an empty constraint. Then drag Elements from the 'Elements' list. The result is the same than what we did in the first example. After doing that exercise the nature of how constraints work with Elements should be clear.
 * you can change an existing constraint between existing elements by just select a different item in the PropertyWindow/ConstraintType property.

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Compatibility
Assembly3 was inspired by Assembly2, but it is not compatible with it. If you have older models made in Assembly2, you should stay with FreeCAD 0.16 and use Assembly2 there.

New models developed with Assembly3 should only be opened and edited with this workbench.

Although they may have similar tools, Assembly3 is not compatible with A2plus nor Assembly4. Models created with these workbenches should be opened only with their respective workbench.

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Testing
The Assembly3 Workbench is under development and is not yet available (April 2020) through the Addon Manager, but it is expected that this will happen at some point.

You can test it in two ways:
 * A special fork of FreeCAD made by realthunder; see FreeCAD_assembly3 releases. This fork is based on a particular commit of the master branch of FreeCAD, but it also has additional features currently not present in the master branch. Due to this fork being based on a particular development snapshot, it does not have the latest features merged daily to the master branch.
 * The development AppImage; this is based on the current master branch, and includes the dependencies needed for working with Assembly3 such as the SolveSpace solver.

Since the AppImage only works for Linux, for Windows users at the moment the only option to test Assembly3 is the first option (realthunder's fork).

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Get Started
There are many ways to create an assembly with Assembly3. Here is the most simple one you can do.


 * Assembly3_Example-GettingStarted.jpg
 * Final Result of the Getting Started Example. In the image the Assembly3 Worksbench is selected, so its multiple toolbars are visible. Note that the vertical "TabBar" left of the tree view is an AddOn Workbench that is not contained in standard FreeCAD (but can be installed with the Addon-Manager).


 * Create a new FreeCAD file
 * Select assembly Workbench. Select CreateAssembly (first icon)
 * Select Part Workbench and add a cylinder and a cube
 * Save the file with any filename you like. Close and open and the file.
 * The tree view should look like this


 * Now Draw&Drop with the mouse both Cylinder and Cube onto the Parts folder. They are moved into that folder.
 * That is the quickest way. Please note that a better way is to open the Context menu on both and select ContetxMenu/LinkActions/MakeLink. This adds two link files. Then Drag/Drop the link files to the Parts folder. For simple cases like this it does not really matter.
 * Click both top surfaces of Cylinder and Cube (keep Ctrl pressed)
 * Select assembly Workbench. Select "PlaceCoincident" from the Constraint Toolbar.
 * Now the parts should be joined into each other and your tree should look like this

We omitted one important step that should be done in larger assemblies: locking a base part. That means define one part that should not be moved by constraints. In your case we use the cube for that: Done. If you like you can move the "Locked" constraint upwards in the tree. Use the "MoveItemUp" button on the Main Toolbar for that.
 * Right click "_Element" (any of the two) and select "Flip Part".
 * Now the Cylinder should be on top of the box. If the whole thing is upside down, go back and select "Flip Part" on the other Element.
 * Select the lower face of the cube. Only the lower face, not the whole cube.
 * select the "Lock" constraint from the constraint tool bar
 * The finished assembly tree should look like in the image above

Note: all new external files must be saved, closed and re-opend at least once, so that Assembly3 can find it. Without doing that FreeCAD can not give a file handle to the Assembly3 Workbench and it can not find the new part. When all parts are in the same file, you should save and re-open the file.

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Add an Offset
Assembly3 does not offer Offset with the constaints in the way the A2plus Workbench or other CAD tools do. Instead it offers a more general and flexible system to add offsets translations but also angles.


 * Add the offset in the properties of one Elements of a Constraint.
 * you can choose which one of the two you want to use.

Example:
 * Add 2 cubes to an assembly and select their side faces.
 * select "PlaneCoincident". The cubes will be attached inside each other.
 * select one Element and ContextMenu/Flip Part. The cubes will be attached side-by-side.
 * select one Element property Offset/Position/Zz and set to 5mm. The cubes will be 5mm apart.
 * Test with other axes or the angle/axis fields. Also verify that you get the same result when using the other Element.

This is the same approach for all other constraints.

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Solve a Solver Failure
This often happens when parts are over-constraints, i.e. more than 6 DOF are locked.

The easiest way to find the problem is to click relevant constraints in the tree and select ContextMenu/Disable and re-calculate. It is helpful to know the last added constraints before the solver failed and just undo them.

Note: as Assembly3 tries to compensate for over-constraint parts behind the scenes, sometimes the problem is just triggered by a new constraint but the root cause is somewhere different. Before deleting all and starting again, remember that you can re-use Elements. If you named them you can identify the required elements and re-build the constraints without using the 3D view at all. See Elements seciton above.

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Replace a part or rename a filename
When a part is removed or when a filename changes, the assembly breaks, it can not longer be solved and the solver will issue the message "Inconsistent constraints". The solver marks invalid Elements and Constrains with a question mark in the tree.

One way to solve this is to just delete all invalid constraints and elements, import the new part and redo everything. But there is a better way:


 * Rename a file
 * Use a file manager and copy the file you want renamed. Then give the new name to the copy.
 * Open the copy in FreeCAD. The assembly and the old file should also be open
 * Select the old object in the tree and click to change the propery "Linked object" (it does contain the old filename)
 * A list dialog will open containing all open parts. It shows the filenames and objects of each part. The old part and object is selected. Locate the renamed part in the tree and select the same object in the new part. Then confim the selection.
 * Delete the old part in the tree. Also the file can be deleted now.
 * Constraints and elements of te old part became invalid. Open the constraint or Elements list in the tree. Then sequentially
 * select each element surface on the new part. An item in the tree will be highliged.
 * Take that item and drag&drop it over the old element (either in the element list or in one of the constraints where it was used). That element should become valid.
 * Repeat the procedure for the remaining elements. Often a single element is enough to allow Assembly3 to identify the remaining elements of the part automatically.
 * If an element was assigned to the wrong surface by accident, just repeat with the correct surface.
 * Change the object name in FreeCAD, if desired


 * Replace a part with another part
 * which is simular enough to the original part that the original constraints still make sense, of course
 * Delete the old part in the tree. Also the file can be deleted.
 * Constraints and elements of te old part became invalid. Open the constraint or Elements list in the tree.
 * Select an element surface on the new part. An item in the tree will be highliged.
 * Take that item and drag&drop it over the old element (either in the element list or in one of the constraints where it was used). That element should become valid.
 * repeat the procedure for the remaining elements.
 * If an element was assigned to the wrong surface by accident, just repeat with the correct surface.
 * Change the object name in FreeCAD, if desired

''Notes ''
 * They are not as complicated as it may seem here. After 2-3 times they should become second nature and feel really easy to do.
 * Its not only usually ways quicker than deleting and re-doing constraints, its also safer because an element could have been used in a parent assembly. Deleting the original would destroy that link, re-assingning would keep it.
 * Also this procedure becomes really quick and easy to do if constraints and elements are named. There is no guessing where the surfaces should be dragged&dropped to because the names tell it (see Tips & Tricks).

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Tips & Tricks

 * Using hierarchical assemblies helps in avoiding solver issues and keeping you model fluid. You can freeze a subassembly with one click and save CPU resources easily (use the context menu in the tree). When loading an assembly Assembly3 does not need to open external files for frozen subassemblies which keeps the tree compact.
 * Is very helpful to make it a habit to name the elements and constraints. Use the key to do this quickly in the tree. You will find the tree sorting tools in the main toolbar very useful. An assembly with fully named constraints and elements is very easy to understand for other people or for oneself when looking at an older file.
 * Examples for constraint names for a table could be "Align_FrontLegs", "Align_FrameBottom-LegTops" and element names could be "Leg1_Top" or "TableTop_Front", "TableTop_Left".
 * Please note that once external files are opened by an assembly its not possible easy to close them again without closing the assembly. Since the assembly keeps open those files in the backgound, the tab may disappear but the file remains visible in the tree. If you have several layers of subassemblies it becomes close to impossible to close single files. This behaviour may change, but until then a possible approach could be to regulary use the commands File/Save All and File/Close All to clean up the tree before working on another sub-assembly.
 * ''Example: consider you have a large CNC machine with a main assembly and a subassembly for each module. Once you have the main assembly open it may open literally hundreds of files down to a single ball bearing. Before working on the subassembly of the electronics cabinet of the machine it is a good idea to save and close all files to get an empty tree. Then open just the subassembly for the electronics cabinet. This will open all file it needs but ony those.
 * Using external files makes it easier to re-use a parts or do part versioning with systems like git or subversion. The workflow in FreeCAD with Assembly feels quite the same as with files that have all parts in the same file. For exchanging files often with other parties, single files might be more convenient.
 * Multiply linked parts. If you added a link into the assembly, it will have a property value named "Element Count", default 0. If you set this to 3 you get 3 instances of that part. They will be added into a subfolder and can be used like fully separte parts. Use this feature to keep the data footprint of your file low, because the part is saved only once. Each instance only contain the differences.
 * Insert multiple parts, e.g. Screws, with one click. Check out the Assembly3 Wiki on the Github site. This is not only a stunning function (even a bit magic), but really really useful.


 * Using the TabBar Workbench speeds up working with assembly. This adds a Toolbar with one button for each workbench. You can sort the toolbar and can put it where every you want it. Many people put it vertically on the left side just beside the tree view. Of you have Assembly3, Part, PartDesign and other often used workbenches close to the top switching between them becomes extremely easy.

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Links

 * App Link object that makes Assembly3 work.
 * FreeCAD_assembly3 repository and documentation.
 * Assembly3 preview, big discussion thread.
 * Test tutorial for Assembly 3 WB by jpg87.
 * Current Assembly Status
 * External workbenches
 * Old Assembly project development plan, to get acquainted with the history of the issue.