Common Operations

Create a Simple Assembly with a Constraint

• Start FreeCAD and create a new document
• Switch to the Part workbench and create a Cube and a Cylinder
• Switch to the Assembly3 workbench, click to create a new assembly
• Select both the Cube and the Cylinder and drag them into the new assembly
• Select any face of the Cylinder or Cube, and click to activate part manual movement. Click any arrow to drag the Cylinder on top of the Cube, press the ESC key to leave part movement (Alternative: right-click Assembly in the tree view and click Finish editing)
• Select the top face of the Cube and (while holding the CTRL key) select the bottom face or edge of the Cylinder and then click to create a plane coincidence constraint.
• Finally, click to solve the constraint system.

You can click to enable auto-solving with any changes in constraint.

After a new constraint is created, the selected elements will be highlighted in red. You can easily change the color of individual constraining elements under its view object property page. Or, set the color of the entire constraint by changing the color of constraint object itself. Make sure you set the OverrideMaterial view property to True.

In case you find that the constraining element highlight obscure the assembly 3D view, you can enable the Auto Element Visibility feature by clicking . When enabled, all constraining elements will be hidden by default. You can reveal them by selecting any constraint or constraint element object in the tree view.

Now, save this document with whatever name you like.

Create a Super Assembly with External Link Array

We are going to build a multi-joint thing using the above assembly as the base part.

• Create a new document, and save it to whatever name you like. Yes, you need to save both the link and linked document at least once for external linking to work, because PropertyXLink need the file path information of both document to calculate relative path.
• Make sure the current active 3D view is the new empty document. Now, in the tree view, select the assembly we just created previously, and then hold on CTRL key and right click the new document item in the tree view, and select Link actions -> Make link. A Link will be created that brings the assembly into the new document. You probably need to click Fit content button (or press V,F in 3D view) to see the assembly.
• Select the link in the tree view, and change the ElementCount property to four. Now you have four identical assemblies.
• Create a new assembly, and then drag the link object into it.
• Select any face of any Cube, click and click any arrow to drag to spread out the parts. Click the edges of the movement sphere to turn the part. Press Esc to leave part movement.
• Select any face of the left most Cube in 3D view, and click to lock the left most sub assembly.
• Orient the parts whatever you like. Select two face from any two assembly, and create a plane coincidence constraint. If you've enabled auto recompute, then the two assembly will now be snapped together
• Do the same for the rest of the parts.

Now that we've made this multi-joint thingy, try to save this document, and FreeCAD will ask if you want to save the external document, too. If you answer yes, then FreeCAD will take care of ordering, and save the external document first before linking document.

Close both documents. Open the multi-joint assembly document, FreeCAD will automatically open any externally referenced documents, too. If you close the external document while leaving the linking document open, all externally linked object will vanish from 3D view. Open external document again and the objects will re-appear. This allows you to easily swap in a replacement document for whatever reason. But, it demands the replacement document having an object of the same internal name as the original linked one. You can of course, easily re-assign the link to any other object in the opened documents. Just use the property editor, click the edit button of LinkedObject property. In the editor window, select the desired document in the drop list, and then select the desired object. But now, you need to make sure the new linked object has the same element interface, or else the constraints will be broken.

A few more words about link array. Assembly3 normally treats any object added to its part group as a stand alone entity that can be moved as a whole. However, it has special treatment for a link array object. Each array element will be treated as separate entities, that can be constrained and moved individually. If you actually want to add the array as an integral part, simply wrap the array inside a dummy assembly without any constraint, and add that assembly instead into the parent assembly.

By the way, the Draft workbench now has two variation of link array, the LinkArray and LinkPathArray, which provide the same functionality as Draft Array and PathArray, but use link to provide duplicates. Those link arrays, by default, do not show individual element in tree view. You can still access each element through subname reference as usual. Having less objects can improve document saving and loading performance. It is particularly noticeable if you have large amount of array elements. You can, however, show the array element at any time by toggle property ShowElement. Once the elements are visible, they can be moved independently by change their placements.

Add/Modify Element and ElementLink

It is quite easy to directly create a new constraint as shown above, with all involved Element and ElementLink being taken care of for you by Assembly3. It is also straightforward to manually add new or modify existing Elements and ElementLink. Simply select a geometry element in 3D view, and its corresponding owner object will be selected in the tree view (Remember to turn on Sync selection option in tree view as mentioned before). You can then drag the selected item to the ElementGroup of an Assembly to create a new Element, or to a Constraint to add an ElementLink. You can modify an existing Element or ElementLink by simply dragging the item onto an existing item of Element or ElementLink. Checkout this tutorial for demonstration.

Part Move

Assembly3 has extensive support of manual movement of nested assembly. In 3D view, select any geometry element (Face, Edge) that belongs to some assembly, and click to activate part dragging. The dragger will be centered around the selected geometry element. In case of multi-hierarchy assemblies, you will be dragging the first level sub-assembly of the top-level assembly. If you want to drag intermediate sub-assembly instead, add that assembly as the second selection (CTRL select) before activating part move.

If you have enabled , any movement of the sub-assembly will cause the parent assembly to auto re-solve its constraints, as shown below. Because there are too many degree of freedom left, hence many possible solutions of the constraint system, the movement of the multi-joint assembly is jerky. Besides, the part move command is very complicated, and probably need a lot more work to make it perfect. In case when the parts are moved such that they stuck in some invalid position, as you can see from the screen cast below, simply CTRL+Z to undo the movement. Every time you release the mouse button, a transaction will be committed, so that you can undo/redo the previous mouse drag. You can also temporary bypass recomputation by holding CTRL key while dragging.

Import External Assembly

In some cases, it will be easier to distribute your multi-hierarchy assembly as a single self-contained document. FreeCAD core provides a convenient command to help with this otherwise not so trivial task. Simply right-click any item in the document you want to distribute, and select Link actions -> Import all links, and that's all. Click to see if every thing is okay. You can of course selectively import any object you want. Simply right click that item and select Link actions -> Import link.