Import and export¶

Import¶

To import a file, open Manage in the sidebar. In the panel that opens, choose a format and upload the file.

To open an entire .n3xd file instead, choose Manage → Load project. This replaces the project on screen rather than merging its contents. If the file has an id that already belongs to you, N3XD asks what to do: choose Replace to overwrite your project, or Import as copy to open the file with a new id. If the id belongs to another account, you can only import the file as a copy.

A few things worth knowing:

• N3XD always stores models in millimetres. STEP and IGES files are normalized on import, and the import feature records the source-unit scale. STL does not reliably specify units, so N3XD assumes the file uses millimetres. You can correct the scale after importing it.
• An STL is drawn from its own triangles and is never re-meshed or simplified. Edges sharper than 30° stay crisp, while finely faceted curves are shaded smoothly.
• Those sharp edges, and the borders of any gaps in the mesh, become the part's edges. They are drawn like the edges of any other part, and you can select and measure them. They cannot be used by features such as fillet, or be projected into a sketch.
• N3XD parses STEP, IGES and STL files in a sandboxed subprocess with resource limits. This prevents malformed files from hanging or crashing the backend, and oversized uploads are rejected.
• N3XD can try to heal imported geometry by sewing faces, running ShapeFix or converting a shell to a solid. It also reports best-effort validity checks.

Adding standard components¶

You can add bolts, washers and other standard parts from the component library instead of modeling them again for each project. Open Manage → Import and switch to Add. A browser opens over the model with the public catalog, your published library and a search box that matches names, descriptions, tags and authors.

The catalog includes three categories: Fasteners (hex bolts and nuts, socket head cap screws, and plain washers), Profiles (aluminium T-slot rails, slot nuts and button head screws), and Bearings (deep groove ball bearings). Bearings are simplified: their bore, outside diameter and width match the catalog dimensions, but their balls and cages are not modeled.

When you select a component, choose its size first. Standard components use one parametric model with a configuration for each size. For example, choosing "M6" and "20" selects the M6x20 configuration, and the part is named after that configuration. A rail uses two size options: its series and cut length, such as 4040 and 1000. Components with only one size dimension offer a single list.

Use Target to choose where to add the component: an existing assembly or a new one. N3XD selects a target based on the current tree selection. If nothing is selected and the project has one assembly, it uses that assembly, so adding a bolt does not create a separate assembly by default.

N3XD inserts the component as a derived part that is locked to the revision you selected. As a result, later catalog updates do not change a model you have already built. The component's parameters stay in the catalog project instead of being copied into yours.

The tab only appears when you are signed in, since the library lives there.

Derived and linked parts¶

Instead of a deep copy, you can derive a part from an existing part or body, in the same or another project. A derived part starts from a snapshot of its source and stays editable, so you can add features on top of it.

Open Manage → Import, switch to Derive, and choose a part or sketch under Source. Source project starts on the current project, so deriving from another part of the model you have open needs no extra step; switch it to pull from a different project. Components published to a library or the public catalog live under Add instead. N3XD snapshots the source geometry into the current project and inherits the source parameters (clashing names get an _imported suffix), so expressions keep resolving.

Target picks where the result lands, always inside the current project. Deriving a part creates a new part, so the target is an assembly (or a new one). Deriving a sketch can add it to an existing part, create a new part in a chosen assembly, or start a new assembly with a part in it. The target starts on whatever the tree selection implies, so selecting a part and deriving into it works without touching the field.

You can also derive by dragging in the model tree: drop a part on another assembly, or a sketch on another part (hold Ctrl to copy instead). See Projects and the parts tree.

Each derived part keeps a link back to its source, in one of three modes:

• Follow latest (default): tied to the source revision it was taken at. If the source moves on, the part is flagged stale and Refresh re-snapshots it and pulls the updated parameters.
• Locked: pinned to the snapshot revision, never refreshed.
• Broken: the link is severed and the snapshot becomes an independent frozen base.

A derived part is not live-linked: a follow-latest part in another project updates only when you refresh it, since the rebuild never reaches into the source project. A source in the same project is the exception and re-snapshots automatically when it rebuilds. The tree shows a link badge, a jump-to-source icon on hover for cross-project links, and a stale or broken indicator.

Export¶

Open Manage in the sidebar to export a model. Each tab uses the same layout: choose a format, adjust its settings, then select what to export from the tree of assemblies and parts. The tree mirrors the sidebar, so you can export the whole model, one assembly or one part.

• 3D model (STEP / STL / 3MF): STEP resolves the full parametric history to B-Rep. For STL, adjust the facet tolerance with the Mesh quality slider. 3MF keeps each part as a separate object and preserves its colour and material. Select All to export the whole model, an assembly row to export that assembly with its placements, or a part row to export that part in its own coordinates.
• Image (PNG): capture the viewport in the browser at 1x, 2x or 4x with MSAA and a transparent, white or theme background. Select All to capture the whole viewport. Select a part or assembly to hide the rest temporarily while N3XD captures it. The camera re-frames the selection from the current direction so it fills the image, unless you pick a saved view. Visibility and camera are restored afterwards.

The CAM and Slice tabs use the same tree. In the Slice tab, select an assembly row to set up and download G-code for the whole assembly as one plate (see Slicing and printing). CAM setups remain part-specific.

You can batch-export configurations to create one file per configuration in a single archive.