Documentation

Steel Frame & Weldments — User Guide

The same Help that ships inside the add-in (version 1.3.2). Product page · Autodesk App Store

Quick Workflow

Find the tools. Run Weldments from Utilities > Add-Ins. A Weldments tab appears in the Design workspace with three panels: Create (Frame, Member, Gusset, End Cap), Modify (Notch, Miter, Trim / Extend, Tab / Slot) and Manage (Manage Library, Profile from Sketch, Delete Profile, Cutting List, Info).
Sketch the member centerlines. Use sketch lines/arcs, or select model edges. Keep the sketch visible while selecting.
Create the main frame first. Use Create > Frame. Select the primary rails/posts as Group 1, choose the profile, then add more groups for braces, diagonals, arcs, or different profiles.
Check the live preview. The preview uses the same temporary BRep trim pipeline as the final build. If a corner looks wrong, fix group order, trim type, or profile orientation before clicking OK.
Add plates and joints. Use Gusset for reinforcement plates, End Cap for closed profile ends, and Tab / Slot for self-fixturing laser-cut tube joints.
Export fabrication data. Use Cutting List for the on-screen table, CSV, and PDF cut sheet.

Recommended for drawings: leave Create each member as a component on in Frame. Fusion Drawing and BOM can then balloon members, gussets, and end caps as separate parts. Component mode is slower on large frames, but better for deliverables. A Part or Assembly design does not allow the child components this option needs — the Frame dialog says so, and members are created as root bodies instead; use a Hybrid design when you want component output.

Frame Command

What a Frame group means

Field	Meaning
Group path	The selected centerline edges for this group. A group must be one connected chain/loop or one parallel set — Frame refuses edges that would cross mid-span (X), touch another edge's middle (T), overlap, branch at a vertex where 3 or more edges meet, or sit disconnected and not parallel. Such an edge simply will not highlight when you try to pick it; put it in another group. There is no fixed edge-count limit.
Profile	Standard, family, and size used for every member in the group. Only standards ticked as visible in Manage Library appear here.
Orientation	Anchor, rotation, offset X/Y, and flip are applied to this group only. They also affect how this group touches earlier groups. Sections are placed with their X axis parallel to the ground plane of the document (XZ in a Y-up document, XY in a Z-up one — Preferences > General > Default modeling orientation); a member that runs straight up takes its section orientation from the horizontal member it meets at a node (or from its sketch plane), so the posts and rails of a wall frame drawn with an RHS 80x40 share the same orientation and miter cleanly. Miter corners are cut through the real outer and inner corners of the two sections, so members anchored at their top or bottom edge, or two widths joined by a corner override, still close. Left/right anchors shift a member to the side that depends on the direction its line was drawn in.
Corner default	Same-group corners use End Miter, End Butt1, or End Butt2.
Trim type	How this group's members are cut wherever they yield — at End Butt corners, and also where the group butts or copes onto an earlier group. Simple cut is a flat end cut; Coped cut notches the yielding member by the target body. The field is shown only while Corner default is End Butt1/End Butt2, but the last value stays in force, so set it there first if a Miter group's braces must be coped onto earlier groups.

Group order and priority

Rule	Result
Groups table	Every group of the frame is listed with its edge count. Click a row to edit that group; the icons below the list add a group, remove the selected group, or move it up or down. A new group starts with the current group's profile size and its own empty selection.
Change priority later	Move a group up to make it the keeper at its joints, or down to make it yield. You do not have to re-select the edges.
Earlier groups win	Group 1 is highest priority. Group 2 trims to Group 1. Group 3 trims to Groups 1-2. Later groups should not cut earlier groups.
Use separate groups	Put primary rails/posts, face braces, cross braces, arcs, and different profiles into separate groups when they are different structural roles.
Do not overpack a group	Do not put unrelated crossing diagonals, branches, and rails into the same group just to select them faster. That creates ambiguous same-group corner rules.
Arcs and curves	Curved members can be selected in Frame and appear in Cutting List with path length, chord, radius, sweep, rise, inside/outside radius, and section depth when data is available.

Corner and trim options

Option	Use when
End Miter	Two same-group members meet on a shared miter plane. Frame falls back to a butt where a miter cannot work: at any corner between two different groups, and at same-group corners sharper than about 20 degrees.
End Butt1	One same-group member should run through and the other should butt into it. Butt1 and Butt2 choose opposite members.
End Butt2	Same as Butt1, but the run-through side is reversed.
Simple cut	The butting member gets a flat planar end cut.
Coped cut	The butting member is trimmed by the real body it touches. Use this for round tubes, hollow sections, and joints that need body contact rather than a simple plane.
Weld gap	Adds a controlled gap at treated joints. Keep 0.00 mm for flush preview/build.
Allow extension	Lets lower-priority straight members extend to the trimming boundary before being cut. Use it for braces/diagonals that stop short of the target body but should still make contact.
Apply corner treatment	Turns automatic joint solving on/off. When off, members are created from raw sweeps without miter/butt/cope treatment.
Merge collinear segments	Combines end-to-end collinear selected edges into one member. Turn it off if each sketch segment must stay a separate physical piece.

Corner override (one corner of this group)

Corner default and Trim type apply to every corner of the group. Use Corner override (this group) when a single corner must differ, instead of splitting the group in two.

Expand Corner override (this group). It appears once the group has two or more corners. A cross marker is drawn at every corner this group takes part in: grey = can be overridden, orange = already has its own style, cyan = the corner being edited.
Click a member near the corner you want. The nearest marker turns cyan.
Set Corner and Trim type for that corner. Leave either on Use group default to keep the group setting for that one.

An override reaches only this group's members at that corner; members of other groups keep their own group default. Overrides are saved with the frame, travel with the group when you reorder or delete groups, and are reloaded when you edit the frame.

Edit an existing frame

Run Frame.
In Edit frame, select any body created by the Frame command. A body from the Member command is not accepted — edit that one with Member.
The saved groups, profiles, orientations, and options are loaded, and the centerline sketches are switched back on so their curves can be re-selected.
Change the settings and click OK. The previous frame is replaced by the rebuilt frame. Clicking OK without changing anything leaves the frame exactly as it was — unless the centerline sketch moved since the build (a changed dimension, a dragged point): Frame notices that, says so in the Edit frame hint, and OK rebuilds the frame from the new sketch with the same profiles and options. That is the way to update a frame after editing its sketch; nothing has to be re-entered.
Tab/Slot joints, gussets, and end caps recorded on this frame are un-built with it and re-applied to the rebuilt members automatically. Items you deleted by hand stay deleted. If one cannot be re-applied, Frame lists it after the build — create that item again.

Profiles and Library

Built-in sectionsOver 600 sizes in 35 families across four standards. EN/DIN: IPE, HEA, HEB, UPN, equal and unequal L, T, RHS, SHS, CHS, round tube, and flat/square/round bar. ANSI/AISC: W, C, equal and unequal L, HSS, Pipe, and flat/square/round bar. JIS: H, C, STKR square/rectangular tube, STK pipe. I and channel sections are drawn with their real root fillets, channels also with their tapered inside flange faces, and hollow sections with real inside and outside corner radii.

Aluminium extrusionT-slot 20, 30, 40 and 45 series, V-slot 20 series, C-Beam 40x80, and imperial 80/20 10 and 15 series (1010, 1020, 1030, 1515, 1530, 3030). Each size is the real extruded outline — slots, X core, and centre bore — so coped joints, notches, and end caps follow the true wall instead of a plain box.

Custom profilesUse Profile from Sketch to capture a closed sketch section (lines, arcs, and circles) and reuse it in Frame or Member — this is the way in for any section the parametric families cannot describe (cold-formed and bent-plate shapes, sections with angles other than 90°, proprietary extrusions). Inner loops are kept, so a section with holes stays hollow at coped joints. Splines and ellipses are approximated as polylines. File the section under a new family or an existing custom one — a family that already holds standard sections is refused.

Manage LibraryShow/hide standards, edit the naming patterns, and import or export the library as CSV. A CSV needs the columns standard, family, type, size plus one column per parameter (h, b, tw, tf, t, od, d); importing merges the rows in and can create new standards and families. Sketch-captured and aluminium extrusion profiles are exported too, as rows of type custom with their outline in a geometry column (JSON — leave it untouched in Excel), so the CSV is a complete backup and moves your profiles to another machine.
The library you edit lives in your user folder (%APPDATA%\VanThanBK\Weldments\profiles.json on Windows, ~/Library/Application Support/VanThanBK/Weldments/ on macOS): an add-in update never touches it and only adds the sizes that are new in the shipped library.

Delete ProfileRemove one size, a whole family, or a whole standard. There is only one library, so this deletes built-in standards too, and a deleted built-in entry stays deleted through updates. It is permanent — there is no Undo; to restore the shipped defaults delete profiles.json from your user folder (see Manage Library) and restart the add-in — so export a CSV backup from Manage Library first. Deleting the last size also removes its family, and deleting the last family also removes its standard.

Gusset Command

Gusset creates a plate between two support faces. It is intended for reinforcement plates after your members already exist.

Input	How to use it
Support faces	Select two planar or cylindrical support faces. For rectangular/tube frames, select the real side/top face that defines the plate direction, not a distant face hidden behind the joint.
Triangular	Uses two support-leg lengths and one outside diagonal.
Polygonal	Uses the same support legs but flattens/chamfers the outside point to create a polygonal plate.
Length on face 1 / face 2	Leg length measured along each selected support face. Default 150 mm each.
Outer chamfer	Polygonal only: the fraction of each leg used to cut the outside corner (0.05 to 0.85, default 0.25).
Thickness	Plate thickness. Thickness location can be centered or shifted to one side.
Flip thickness side	Reverses which way the positive and negative thickness sides point when the plate lands on the wrong face.
Corner relief	Moves the inside corner away from the physical intersection to avoid a sharp internal corner.
Offset along corner	Moves the plate along the support intersection line without changing its shape.
Name	Body/component name. It is regenerated from the current size (`Gusset-Tri-150x150x6`) every time you change Profile, a leg length, or Thickness, so type your own name last — a later size change overwrites it.
Create as component	Creates the gusset as its own component for Drawing/BOM.
Edit gusset	Select an existing gusset body and OK rebuilds it from saved data.
After a frame edit	Gussets are rebuilt automatically on the new members when you edit the Frame or Member they sit on. You do not have to re-pick the support faces or run Gusset again.

Curved supports: cylindrical faces are supported and the plate is coped for contact. For general freeform curved faces, create/select a clear planar reference face or a cylindrical support face; ambiguous curved intersections can produce more than one possible plate direction.

Plates follow their members: if a frame edit removes the member a plate sat on, that gusset or end cap is deleted with it, without a message. A plate you deleted by hand is not brought back.

End Cap Command

End Cap creates plates on selected closed-profile end faces.

Option	Meaning
End faces	Select planar closed-profile end faces. Hollow profiles can use the internal opening when the selected face exposes it.
Thickness	Cap plate thickness. Default 6 mm.
Outward	Adds the cap outside the member.
Inward	Places the cap inward and trims the member by cap thickness.
Internal	Fits the cap inside a hollow profile using the inner loop when available.
Internal inset	Internal placement only: how far inside the end face the cap sits. 0 keeps it flush with the opening.
Offset type	Thickness ratio insets the cap by a fraction of the profile wall thickness — 0.5, the default, is half a wall. It needs a hollow section: a solid section has no wall to measure, so the ratio does nothing there. Use Offset value for an exact distance on any section.
Reverse offset	Reverses the offset direction when the preview grows/shrinks the opposite way you need.
Corner treatment	None, Chamfer, or Fillet on the cap outline. A positive corner size is required.
Name prefix	Prefix for the created bodies/components. Caps are numbered `EndCap-01`, `EndCap-02`, and so on.
Cap outline	On members built from a library RHS/SHS/CHS or flat section with a square end, the outline comes from the library section, not from the edges of the face you pick — so an end where a Tab/Slot slot or a notch has already cut material away still caps square and complete. Custom sketch profiles and mitred ends follow the picked face outline.
Edit end cap	Select an existing end cap and OK rebuilds it from saved data.
After a frame edit	End caps are rebuilt automatically on the new member ends when you edit the Frame or Member they sit on. Only the plates on the frame you edited are touched.

One cap per end: with a single end face selected, creating a cap on an end that already has one replaces it, whatever you changed. Select several end faces at once and each face simply gets a new cap, so re-capping an already-capped end that way stacks a second plate — edit those ends one at a time. Gusset replaces its plate in the same way, but only when the two supports, profile, leg lengths, thickness, thickness location, flip thickness side, and offset along the corner all match; change any one of those and you get a second plate at the same joint.

Tab / Slot Joints

Tab / Slot adds a self-fixturing tab on one member and a matching through-wall slot on the other (laser-cut tube workflow). Pick the tab member, then the slot member. Both must be members created by Frame or Member — the command reads each member's stored centerline, so an imported or native Fusion body is refused. Each pick is captured and its highlight cleared straight away, so read the Tab: / Slot: line under the pickers to confirm what is held, and click a Select box again to swap a member. Any profile with real material at the joint works: square/rect tube, round tube, flat bar, angles, channels, and custom profiles from sketch.

The tab member's end should already sit at the slot member's wall. On square/rectangular tube and flat bar, an end buried more than about 2.5 mm past the wall is refused — cut it back with Trim / Extend first. On round tube and on open sections (angle, channel, I, T, custom from sketch) a buried end is not caught, so trim it back yourself. The members may meet square or at an angle, up to about 75 degrees off the wall normal; a shallower brace is refused because the joint stops making fabrication sense.

Input	How to use it
Tab position	Which wall of the tab member carries the finger. Auto takes the first placement that lands on real material, Center needs material on the member's own centreline (solid bar, an I-beam web, a tee stem) and is not available on round tube, Side 1 / Side 2 pin it to one wall, and Both sides makes two tabs and two matching slots in one operation.
Tab width	Width of the finger across the wall. Default 12 mm. Keep it inside the flat part of the face, clear of the tube corner radii.
Tab thickness	Thickness of the finger. Default 4 mm, filled in from the member's wall thickness for rectangular, square and round tube and for flat bar. Angles, channels, I-sections and custom sketch profiles are not in the library that way, so the dialog warns you and you type the thickness yourself.
Tab length	Flush with wall (default) ends the tab level with the far side of the wall it passes through. Custom length reveals a length field (default 10 mm); a value that does not reach the slot member's wall is rejected.
Rotate tab 90 deg	Turns the finger a quarter turn in the member's own section, so it grows out of the other pair of walls. Use it when the tab aims at open air, or to put the tab on the wide face instead of the narrow one.
Slot cut	Square through wall cuts square and elongates the hole for an angled tab (any tube laser). Angled with tab follows the tab for a constant gap all round (needs a 5-axis or bevel-head laser).
Slot clearance (per side)	Fit clearance added to each side of the hole. Default 0.15 mm; 0.1–0.2 mm suits most tube lasers. Cutting services compensate kerf themselves, so this is fit only.

On hollow tube the tab extends one of the tube's walls (a curved strip of the wall on round tube) — keep it clear of the corner radii, and away from high-stress joints: it locates parts for welding, the weld still carries the load. The preview draws the tab in orange and the slot cut in red; if the pair cannot make a joint, an orange line says why, and nothing changes until you click OK.

Each joint is grouped in the timeline as TabSlot:<n> and recorded on the document, so it is re-applied automatically after a Frame or a Member edit rebuilds either member. If the rebuilt members no longer meet, a Frame edit reports which joint could not be re-applied; a Member edit drops it without a message, so check that the TabSlot:<n> group is still in the timeline. Either way, fix the members and create that joint again. Deleting a TabSlot:<n> group by hand removes the joint for good and it is no longer tracked.

Cutting List and PDF

Cutting List reads all recognized Weldments members, gussets, and end caps in the active design. It lists physical pieces, not selections: a member that a crossing brace has cut right through is counted as the two bars you actually have to saw.

Output	Contents
On-screen table	Grouped item number, quantity, profile/size, long/stock length, short-point length for skew cuts, and end-cut summary.
Long / short point	The long/stock length is the longest point of the piece; the short-point length is the shortest distance between the two end cuts, and each end offset is how far that end's short point sits back from its long point. Square cuts leave these cells empty because both lengths are the same, and a coped end has no planar cut face, so that piece reports the stock length only.
Tab / Slot ends	An end carrying a self-fixturing tab is listed as `tab` instead of a cut angle, or `tab x2` when the joint was placed on both sides. This appears in the on-screen table and the CSV; in the PDF it appears in the cut list table only for pieces that carry no details text, and the member cut sheets always dimension a tabbed end by its cut angle.
Totals	The last row of the on-screen table totals the length of every row, plates included, so it is not a bar-stock figure. The CSV `TOTAL MEMBERS` row and the PDF title block's `Members` length count members only; the title block's `pcs` figure counts every piece, plates included.
Cut angle convention	Choose face angle (a square cut is 90 degrees) or saw setting (a square cut is 0 degrees). The same convention is used by the table, CSV, and PDF.
CSV	One header row, then one row per item: item number, profile, standard, family, size, long/stock length, short-point length, both end offsets, width, thickness, both end cuts, quantity, and a details column. The end-cut headers carry the angle convention you chose. Two summary rows follow the data — `TOTAL MEMBERS` (member length and member count) and `TOTAL ALL PCS` — so skip the last rows when importing the file into another tool.
PDF overview	Viewport-based model overview with item balloons.
PDF cut list table	A table under the overview, continued on more pages when needed, with item, quantity, type, profile/size, length, width, thickness, and a last column holding the end cuts — or, when the piece has extra data such as curve or long/short lengths, those details instead. Long text is shortened to fit the column; the CSV holds the full text.
Member cut sheets	Two projected views of each unique member, final length/path length, long/short-point dimensions where required, and visible end-cut angles.
Arc members	Path length, chord, center radius, sweep angle, rise, inside/outside radius, and section depth/OD when the arc metadata is available.
Gussets	Plate outline with leg dimensions, thickness, and significant corner angles.
End caps	Plate outline with length, width, thickness, and significant corner angles.

Slotted members: members are also grouped by how many Tab/Slot holes they carry, because they are different laser parts. Two rows can therefore look identical in every printed column and still be listed separately — the difference is the number of slots.

Non-circular curves: the cut list reports path length and available curve data. For exact fabrication templates of arbitrary splines, use the model or export a DXF/template from Fusion.

Section size on curved members: the section depth/OD, and the inside/outside radius derived from it, are read from the profile size name. Imperial pipe and round-bar names (for example PIPE 1/2 STD) and custom profiles can give a wrong value here. Check it against the model before ordering bent stock.

AI Control with MCP

Weldments includes a local Model Context Protocol server for approved AI clients. It exposes eight fixed tools: weldments_get_status, weldments_list_profiles, weldments_list_sketch_paths, weldments_get_selection, weldments_list_items, weldments_create_frame, weldments_create_gusset, and weldments_create_end_caps. Everything else stays manual: Tab / Slot, Miter, Notch, Trim / Extend, per-corner overrides, Cutting List export, and editing an item that already exists are not available to the AI.

Open Fusion, open a Design document, and start Weldments.
Configure the AI client to launch Contents/mcp_server/run_weldments_mcp.cmd on Windows or Contents/mcp_server/run_weldments_mcp.sh on macOS.
Use weldments_get_status first. For face-dependent geometry, select the intended faces in Fusion before asking the AI to create a Gusset or End Cap.
Close any open Fusion dialog before asking the AI to build. Frame, Gusset, and End Cap requests are rejected while another Fusion command is running.

The bridge accepts loopback connections only, uses a random per-session token, exposes no arbitrary script execution, and requires an active Weldments license or trial for model changes. It starts whenever Weldments starts and cannot be switched off on its own; it listens on 127.0.0.1 only and stops when you stop the add-in in Utilities > Add-Ins. See Contents/mcp_server/README.md for client configuration examples.

Manual Modify Tools

Command	Use
Member	On the Create panel, not Modify. Places or edits a single swept member, independent of Frame groups.
Miter	Miter exactly two members that meet at a corner. Both must have been created by Weldments (they store their axis) — use Notch for other bodies. Weld gap leaves a gap between the two mitered faces.
Notch	Cope the selected members around the bodies they intersect. Leave Keep cut-against bodies on to keep the tool bodies, or turn it off to consume them. Weld gap cuts the member back from the bodies it copes around; with a gap set, the cut-against bodies are always kept.
Trim / Extend	Pick Mode: Trim cuts the member at a planar face or construction plane and drops the offcut (Flip kept side keeps the other piece instead); Extend grows the member end out to the plane and works only on members created by Weldments. Weld gap leaves the end short of the plane. Several members can be trimmed to one plane in a single run.
Tab / Slot	Add a self-fixturing tab on one member and a matching through-wall slot on the other. See Tab / Slot Joints.

License and Access

A free 3-day trial starts automatically the first time you use a Weldments tool (an internet connection is required to activate it). All tools are available during the trial.
Buying on the Autodesk App Store unlocks the add-in through Autodesk Entitlement when you sign in to Fusion.
If you received an activation code, open Info, paste the code, and click OK.
Info is always available and shows current status, Autodesk account, App ID, and privacy links.
Updates: Info also shows the newest build published by VanThanBK — an early-access build can be offered there before the App Store finishes reviewing it. Download latest version opens the download in your browser for licensed users (bought on the App Store, or granted access by the publisher); unzip and replace the add-in folder, then Stop and Run it in Utilities > Add-Ins. Without a license the button takes you to the App Store page.
Without a license or an active trial, every button stays on the ribbon but shows This Weldments feature requires a license and closes instead of opening. Info keeps working so you can check status or enter a code.

Website: Steel Frame & Weldments

Privacy: Privacy policy

Troubleshooting

Symptom	What to check
A brace cuts the wrong member	Put the main frame in earlier groups and the brace in a later group. Do not put braces and rails into one same-priority group unless that is intentional.
Butt direction is reversed	Switch End Butt1 and End Butt2 for that group. For same-group corners, these choose opposite run-through members.
Butt1/Butt2 changes nothing	The corner is between two groups. There the earlier group always runs through, and neither Butt1/Butt2 nor Corner override changes that (an override can still change the trim type there). Move the group up or down to change which member survives.
An edge will not select in Frame	It would break this group's shape (crossing, T-touch, overlap, a 3-edge branch, or a disconnected non-parallel run). Add a new group and select it there.
A standard is missing from Frame	Open Manage Library and re-tick it under Visible standards. Hiding a standard only removes it from the Frame and Member lists; it is still shown in Profile from Sketch and Delete Profile.
Coped preview looks heavy	Coped preview uses real BRep edge data. Complex hollow/round profiles can show more edges than a simple line preview, but it matches the final body more closely.
Member stops short	Enable Allow extension when a later straight member should grow to an earlier group before trimming.
Tab / Slot says the tab aims at open air	There is no wall of the slot member where the tab lands (the open side of a channel, past an angle leg). Move the joint onto a real wall, tick Rotate tab 90 deg, or change Tab position.
Tab / Slot says the end is buried in the other member	Cut the tab member back to the wall with Trim / Extend, then run Tab / Slot.
Fusion Drawing is hard to balloon	Use Create each member as a component in Frame, and create gussets/end caps as components.
Large frame is slow	Component mode and BRep preview do more work. Build primary groups first, keep sketches clean, and split very large structures into logical frames.