- 1 Introduction
- 2 Installing
- 3 Getting Started
- 4 Assembling
- 4.1 Keeping the Overview
- 4.2 Constraints
- 4.3 Subassemblies
- 5 Constraint Handling
- 6 Part Lists
- 7 Special Features
- 8 Preferences
- 9 Troubleshooting
The A2plus workbench is an external workbench to assemble different parts in FreeCAD.
This documentation describes A2plus version 0.4.10 or newer.
The A2plus workbench is an addon to FreeCAD. It can easily be installed via the menu Tools → Addon Manager. A2plus is under active development and will get new features frequently. Therefore you should update it regularly using also the menu Tools → Addon Manager. The A2plus code is hosted and developed on GitHub and can also be installed manually by copying it into FreeCAD's MOD directory.
At first switch to the A2plus toolbar in FreeCAD. To create an assembly create a new file in FreeCAD. At first this file needs to be saved. It is recommended (but not necessary) to save it in the same folder of the parts you want to assemble.
Now parts can be added to the assembly by using the toolbar button . The first added part gets a fixed position by default. (You can change this later via the part property DATAfixed Position.)
Parts that are already in the assembly can be cloned with the toolbar button .
To edit a part from the assembly, select it in the model tree and use the toolbar button . This will open the part into a new tab in FreeCAD or switch to its tab if the file is already opened.
To import changes in parts into the assembly click on the toolbar button .
Imported parts will keep their external dependencies and can be edited. For well-defined parts like screws it is however useful that their shape cannot be edited. This can be achieved with the toolbar button that converts the selected part to a static copy of the original part.
Assembling parts is done by adding constraints between parts. After a constraint A2plus will move the parts according to the constraint if possible.
For complex constraints between parts A2plus might fail to solve the constraints. Therefore also have a look at section Troubleshooting for strategies to resolve such cases.
Constraints between parts are added by keeping thekey pressed and selecting an edge or face of two parts. The constraint will be added attached in the model tree to the affected parts.
Keeping the Overview
The more parts you add, the more important it is to keep the overview. A2plus therefore offers these tools to move and view parts:
- To move a part around in the assembly, select it in the model tree and use the toolbar button . When you placed the part where you like it, left-click with the mouse. If the moved part has already constraints the part will be placed accordingly by pressing the toolbar button because this triggers to resolve all constraints of the assembly.
- To show a constraint select it in the model tree and use the toolbar button . This will make the whole assembly transparent and highlight the two things that are connected in the constraint. To go back to the normal view, left-click into the assembly.
- To show only certain parts in the assembly, select these parts in the model tree and use the toolbar button . Alternatively you can hide a certain part by selecting it in the model tree and pressing to toggle its visibility.
- To toggle the transparency view of the whole assembly you can use the toolbar button .
When creating a constraint such a dialog will be displayed after you pressed a constraint toolbar button:
For certain constraints it allows you to modify the constraint direction. With the button you can check in advance if this new constraint can be solved by A2plus. If not, have a look at section Troubleshooting.
A2plus provides the following constraints:
Point on Point
Select a vertex (point) on each part. The toolbar button adds the constraint pointIdentity. It will make the vertices coincident.
Point on Line
Select a vertex (point), or circular edge (will select its center point), or a spherical face (will also select its center point) on one part and an edge on the other part. The toolbar button adds the constraint pointOnLine. It will put the vertex on the edge.
Point on Plane
Select a vertex (point), or circular edge (will select its center point), or a spherical face (will also select its center point) on one part and a plane on the other part. The toolbar button adds the constraint pointOnPlane. The constraint dialog allows you to specify an offset between the point and the plane. This offset can also be flipped between both sides of the plane. If the offset is zero, the constraint will put the vertex on the plane.
Sphere on Sphere
Select either a spherical face or a vertex (point) on both parts. The toolbar button adds the constraint sphereCenterIdent. It will either make the center of the spheres, the center of the sphere and the vertex, or the vertices coincident.
Circular Edge on Circular Edge
Select a circular edge on both parts. The toolbar button adds the constraint circularEdge. 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.
Select either a cylindrical face or a linear edge on both parts. The toolbar button adds the constraint axisCoincident. 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.
Select either a cylindrical face or a linear edge on both parts. The toolbar button adds the constraint axisParallel. The constraint dialog allows you to specify the axis direction. The constraint will make the axes or lines parallel.
Axis on Plane
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 axisPlaneParallel. The constraint will make the axis or line parallel to the plane.
Select a plane on both parts. The toolbar button adds the constraint planesParallel. 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 planeCoincident. 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.
Select a plane on both parts. The toolbar button adds the constraint angledPlanes. 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 centerOfMass. 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.
An assembly can contain other assemblies. They are added like parts by pressing the toolbar button and selecting a *.FCStd file containing an assembly. Such subassemblies can also be edited like parts using the toolbar button . Please assure sure for higher assembly stages that you update the assembly via the toolbar button when there were changes.
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.
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 #PARSTINFO# 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 two times in the assembly it will get QTY 2.
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.
Degrees of Freedom
The button labels every part of the assembly with their 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 View → Panels → Report view.
The degrees of freedom labels can be removed with the button .
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.
The a2plus preferences can be accessed via FreeCAD's menu Edit → Preferences 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 DATAfixed Position 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 for 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 DATAfixed Position set to true. Note that this will in most cases take more time for the calculation of a solution.
- Force fixed position
This sets for all parts in the assembly the property DATAfixed Position to true. Then no calculation is actually performed since all parts will always be fixed to the positions where they were created.
Default solver behavior
- Solve automatically if a constraint property is changed
The solver will automatically be started. The same as turning on the toolbar button .
Behavior 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.
- 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 DATAmux Info. 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 importing 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 color 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 for FEM simulations or 3D-printing if only one solid is allowed. The alternative is to create later a shape of the whole assembly.
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 ).
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.
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 planesParallel constraint set for two planes. Now you want to set for the same planes the planeCoincident constraint and A2plus cannot solve this. Then the constraint directions of planesParallel and planeCoincident are different. Use the same direction for both constraints to fix this.
Most cases of unsolvable constraints occur directly when adding a new constraint. The solution is then to delete the constraint you added the last. A2plus will also propose this.
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 after another that is connected to the changed part. 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.
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 axisCoincident 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 DATAfixed Position 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 DATATip.
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 DATATip. If the tip is not at the feature where you want it, right-click on the feature where the tip should be and choose Set tip. Finally save the part and reload the assembly using the toolbar button .
Repairing Assembly Tree
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.
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 DATAfixed Position set to true or is connected by a constraint to a part with DATAfixed Position set to true, the constraint cannot be solved. The same happens if both parts of the constraint have DATAfixed Position 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 DATAfixed Position set to true. Then assure that you only set constraints to a part which is somehow connected to the fixed part. To visualize these dependencies, see section Assembly Structure.
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 angledPlanes 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 Transform).
Note: Assure that at least one part of the constraint has the property DATAfixed Position set to false.