Projects, parts, and the model tree¶

N3XD organizes each project in a tree:

Project  ->  Assemblies  ->  Parts  ->  Bodies / Sketches  ->  Features

A project always contains an assembly and has a stable project_id in its URL (/p/<project-id>). The id is immutable and separate from the project name.
An assembly contains parts and can also contain other assemblies. The tree shows assemblies that are not placed elsewhere at the top level. Each sub-assembly appears under its parent and remains editable there.
A part is a modeled component with an ordered history of features and the sketches those features use.
A body is one solid. A part can contain several bodies, for example, to support multi-material printing.
A sketch is a separate object that can be used by several features, such as an extrude followed by a pocket.
Features are the operations in a part's history. When you edit an earlier feature, N3XD recomputes everything that follows it.

The tree panel¶

The tree shows origin elements (planes and axes), parts, bodies, sketches and features. From the tree, you can:

Rename items inline.
Toggle visibility. Visibility is a view setting and is not saved in the document.
Identify operations at a glance. Each history row uses the icon of the toolbar button that created it, so you can scan a part's history without reading every name.
Read a feature's rebuild status from its icon: ok, warning, failed, unresolved_reference, suppressed or stale.
Preview a feature's main parameter. Selecting it shows a small, read-only summary beside the row, such as a fillet radius, extrude distance or hole size. N3XD does not roll back the model, so the preview stays responsive even on large models. Press Escape or click away to dismiss it.

Groups¶

A group is a folder that helps organize the tree. It has no position or effect on the model, so you can put hundreds of bolts behind one row instead of filling the panel. Select the rows you want (Ctrl-click to add to the selection), open the command palette with ++f1++ and choose Group Selection. The new group appears collapsed and shows how many items it contains.

Rename a group by clicking its name, like any other row.
The eye icon hides or shows everything in it at once.
Selecting the group row selects all its members, so a group is also how you act on a set of parts at once.
Drag a part, instance or sub-assembly row onto a group to put it in; the × on a member row takes it out again. A part belongs to at most one group.
Ungroup (the icon on the group row) removes the group and leaves every part exactly where it was.

Groups can contain children of only one assembly, so all selected rows must belong to the same assembly. A group is not a sub-assembly: creating one does not move anything, and mates, exports and simulations ignore groups.

Dragging in the tree¶

Use drag and drop to link, copy or reorder items. Drop an item in the same container to reorder it. Drop it in a different container to create a linked copy that follows its source. Hold Ctrl (or Cmd) while dropping to make an independent copy instead. The original item stays where it is, and a label on the target row explains what the drop will do.

Features can be reordered within their part's history. Two kinds of gaps appear: a solid line marks a position that leaves the model unchanged, while a dashed red line marks a valid position that changes the part (for example, moving a fillet after a shell or a boss before the hole it fills). Drop a feature on a red line to rebuild the part; N3XD explains what changed, and you can undo the move with Ctrl+Z. A gap with no line is not allowed by the history. The feature brings its own sketch along, but a profile shared by two features stays where it is. You cannot reorder features while moving the rollback bar or editing a feature, because those actions move the cursor used for the check. Hover over the row to see which action is blocking reordering. Alt+↑ and Alt+↓ move between positions that do not change the model, and tell you which positions they skipped.
Parts reorder inside their assembly. Drop one on another assembly's row to derive it there (a linked part that tracks the source), or Ctrl-drop an editable copy. Deriving keeps the source in place and removes no mates.
Sketches dropped on another part's row derive there; Ctrl-drop gives a static copy. Ctrl-dropping onto its own part copies it within the part. A copy or a derived sketch keeps its mirrors, offsets and patterns. Projected geometry stays linked to its source body only within the same part.
Assemblies dropped on another assembly become sub-assemblies. The row appears under its parent (-> name) and expands so you can edit it in place. You can place the same assembly in several parents because N3XD stores its contents once; an edit through any row updates every placement. Hold Ctrl while dropping to make a deep copy. An assembly cannot be placed inside itself or one of its own sub-assemblies.
Sub-assembly and instance rows dropped on another assembly move that placement. The definition is untouched and the placement keeps its identity, so mates naming it survive. Moving a row that sits inside another sub-assembly edits that parent definition, so every copy of it updates.
To un-nest, drag a sub-assembly row onto the Move to project root strip at the bottom of the tree. It returns to the top level with the pose it had inside its parent. Only the last placement can be moved out; while it is still placed elsewhere the strip stays away, since removing that row would just delete it.

Deleting an assembly also deletes its nested sub-assemblies, at every level, and their parts. N3XD asks first and lists what will be deleted. If a sub-assembly is also placed elsewhere, it stays in the project and returns to the top level when its last placement is removed.

Derived parts and sketches show a link icon. If the source changes, the item is marked stale and offers a refresh action. Dragging an already-derived item creates a copy, because N3XD does not derive from another derived item.

When an upstream feature fails, everything depending on it is marked blocked or stale rather than failing silently. See History and revisions for stepping back through the history.

A project's URL (/p/<project-id>) is its share link. To choose what the link allows, select Share on the project card in your dashboard and choose:

Read & write (default): anyone with the link can open and edit alongside you.
Read only: they can open, inspect, measure and export, but every edit is refused. A Read-only badge shows in their toolbar.
Public view: anyone with the link can look at the model without signing in. Use this option to show a design to someone who does not have an account.
No access: the link stops working and the project disappears from the dashboards it had reached.

Changes take effect immediately, including for people who already have the project open. You can use this setting to revoke access as well. Only the owner can change sharing, and the owner always keeps access.

Set User settings → Application → Default link sharing to choose what links allow for projects without their own setting. For example, you can make new projects read-only or private by default. The share dialog highlights projects with a different setting. You cannot set Public view as the default; choose it for individual projects instead.

What a public-view visitor sees¶

Public-view visitors see the model with its materials and the model tree. They can orbit, zoom, switch between shaded and wireframe, and open your saved viewpoints. They also appear in the participant list, so you can present the model to them live. Visitors appear as Guest and see other participants as anonymous.

Their toolbar shows a View only label and the participant list. Visitors have no editing tools, import or export controls, downloads, AI assistant or access to your other projects. The server enforces these limits; the controls are not merely hidden. If you change the project's sharing mode, existing public links stop working within about half a minute.

Rollback¶

Rollback suppresses every feature after a chosen point. Use it to insert or edit earlier history, then move forward again. Assembly mates survive rollback through checkpoint caching. N3XD saves the rollback position with the project, so it restores the bar when you reopen the project. You can place the bar on a sketch or a feature. When it is on a sketch, the model includes everything before that sketch, just as it does while you edit the sketch.

Pick up the rollback bar to highlight the drop targets in that part's history. Only the part you picked it up from responds, and the tree stays still while you drag. This keeps the target gap in place. Drop the bar above the first row to place it before the entire history. The part then builds nothing, and the next sketch or feature you add goes at the start of the history. Select × on the bar to roll forward again.