A2plus Workbench/zh-hans

Introduction
A2plus工作台是外部工作台，用于在FreeCAD中的不同零件组装成一个装配体.

本文档介绍了A2plus 0.4.33或更高版本的使用.

Installing
A2plus工作台是FreeCAD的插件. 可以通过菜单轻松安装. A2plus正在积极开发中，并将经常获得新功能. 因此，您还应该使用菜单定期对其进行更新. A2plus代码是在GitHub上托管和开发的，也可以通过将其复制到FreeCAD的MOD目录中进行手动安装.

入门
首先，切换到FreeCAD中的A2plus工具栏. 要创建装配体，请在FreeCAD中创建一个新文件. 首先，该文件需要保存. 建议（但不是必需）将其保存在要装配的零件的同一文件夹中.

现在，可以使用工具栏按钮或将零件添加到装配体中. 按钮将所选文件中的所有实体作为单个部分添加. 使用按钮时，您可以选择将文件的哪个实体作为零件导入. 默认情况下，第一个添加的零件会固定在一个固定位置. (您可以稍后通过零件属性对其位置进行改变. ) 可以使用工具栏按钮复制装配中已经存在的零件. 要编辑部件中的零件，请在模型树中选择它，然后使用工具栏按钮. 这将在FreeCAD中将零件在新选项卡中打开，或者如果文件已经打开，则切换到其选项卡. 要将零件中的更改导入到部件中，请单击工具栏按钮.

导入的零件将保留其外部依赖性，并且可以进行编辑. 但是，对于像螺丝这样定义明确的零件，阻止对其进行编辑很有用. 这可以通过工具栏按钮实现，该按钮可将所选零件转换为原始零件的静态副本.

要保存装配体并随后将其关闭，可以使用工具栏按钮.

装配
通过在零件之间添加约束来完成零件的组装. 约束后，如果可能，A2plus将根据约束移动零件. 对于零件之间的复杂约束，A2plus可能无法解决约束. 因此，也可以参考故障排除部分中有关解决此类情况的策略.

通过按住键并选择两个零件的边或面来添加零件之间的约束. 约束将附加在模型树中，并添加到受影响的零件.

保持追踪
添加的零件越多，跟踪就越重要. 因此，A2plus提供了以下工具来移动和查看零件：


 * 要在装配体中移动零件，请在模型树中选择它，然后使用工具栏按钮[[Image:A2p MovePart.svg|24px]]. 将零件放置在所需位置时，用鼠标左键单击. 如果移动的零件已经具有约束，则将通过按下工具栏按钮[[Image:A2p solver.svg|24px]]进行相应放置，因为这将触发以解决装配体的所有约束.
 * 要显示约束，请在模型树中将其选中，然后使用工具栏按钮[[Image:A2p ViewConnection.svg|24px]]. 这将使整个装配透明，并突出显示通过约束连接的两个对象. 要返回普通视图，请在组件中单击鼠标左键.
 * 要仅显示装配中的某些零件，请在模型树中选择这些零件，然后使用工具栏按钮[[Image:A2p Isolate Element.svg|24px]]. 或者，您可以通过在模型树中选择某个零件并按来切换其可见性来隐藏该零件.
 * 要切换整个装配体的透明度视图，可以使用工具栏按钮[[Image:A2p ToggleTransparency.svg|24px]].
 * 使用正常的FreeCAD编辑可以使每个零件透明. 但是，有时由于FreeCAD中的错误，在重新打开装配体时零件的透明度设置会丢失. 解决方法是，可以使用工具栏按钮[[Image:A2p_Restore_Transparency.svg|24px]]恢复透明度设置.

约束
创建约束时，按下约束工具栏按钮后将显示一个对话框: 对于某些约束，它允许您修改约束方向. 使用按钮 您可以预先检查是否可以用A2plus解决这个新约束. 如果不是，请查看故障排除部分.

A2plus提供下列约束:

点对点
在每个零件上选择一个顶点 （点）. 点击工具栏按钮添加约束，它将使顶点重合.

点对线
选择一个零件上的顶点（点）或圆形边（将选择其中心点），或一个球面面（也将选择其中心点），另一零件上的边. 工具栏按钮 添加约束. 它会把顶点移动到边的上面.

点对面
选择一个零件上的顶点（点）或圆形边（将选择其中心点），或一个球面面（也将选择其中心点）和另一个零件上的平面. 点击工具栏按钮添加约束. “约束”对话框允许您指定点和平面之间的偏移. 此偏移也可以在平面的两侧之间翻转. 如果偏移为零，则约束将顶点放置在平面上.

球面对球面
在两个部分上选择球形面或顶点（点）. 工具栏按钮添加了约束. 它将使球的中心，球的中心与顶点或顶点重合.

圆边对圆边
在两个零件上选择圆形边. 工具栏按钮添加了约束. 约束对话框允许您指定边缘之间的偏移. 该偏移量也可以翻转. 您还可以设置约束方向并锁定零件的旋转. 如果偏移量为零，则约束将使边缘同心于同一平面.

轴约束
在两个部分上选择圆柱形面或线性边. 工具栏按钮 24px添加了约束. 约束对话框允许您指定轴方向. 该对话框还允许您锁定零件的旋转. 约束将使轴或线重合.

轴平行
在两个零件上选择圆柱形面或线性边. 工具栏按钮添加了约束. 约束对话框允许您指定轴方向. 约束将使轴或线平行.

轴对面平行
在一个零件上选择圆柱面或线性边，在另一部分选择一个平面. 工具栏按钮添加了约束. 约束将使轴或线平行于平面.

轴对面法线
在一个零件上选择圆柱面或线性边，在另一零件选择一个平面. 工具栏按钮添加了约束. 约束将使轴或线垂直于平面.

面平行
在两个零件上选择一个平面. 按下工具栏按钮添加约束. 约束对话框允许您指定约束方向. 约束将使平面平行.

面对面
在两个零件上选择一个平面. 按下工具栏按钮添加了约束. 约束对话框允许您指定约束方向和平面之间的偏移. 该偏移量也可以翻转. 如果偏移量为零，则约束将使平面重合.

平面角
在两个零件上选择一个平面. 点击工具栏按钮添加约束. 约束对话框允许您指定平面之间的角度. 约束将使平面首先平行，并设置指定的角度.

重合中心
在两个零件上选择闭合的边或平面. 点击工具栏按钮添加约束. 约束对话框允许您指定边或平面之间的偏移. 该偏移量也可以翻转. 您还可以设置约束方向并锁定零件的旋转. 如果偏移量为零，则约束会将边或平面置于同一平面中.

子装配体
装配体可以包含其他装配体. 通过按下工具栏按钮，然后选择包含装配体的文件，可以像零件一样添加它们. 也可以使用工具栏按钮像零件一样编辑这些子装配体. 请确保在更高的装配阶段中，当发生更改时，可以通过工具栏按钮更新装配.

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 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.

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:

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.

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.

Avoiding Accented Characters
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

This is the dragging animation using the example assembly:



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:

The command means, we change the placement property Rotation.Angle of the part get got previously as "starWheel". This property gets the angle as radian. The function radians from the library math converts the angle from degree to radian.

The property Rotation.Angle 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 angle but  PositionShift 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 with all possible placement commands.

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