Autodesk Inventor Sheet Metal, Frame Generator, Tube & Pipe, Harness Summary
Overview
What sets Inventor apart among manufacturing and equipment engineers are two modules: Sheet Metal and Frame Generator. Sheet Metal is a parametric structure that reflects real-world shop floor practice — flat patterns, K-Factor, Punch Tools — and Frame Generator drops structural shapes and aluminum profiles onto a Skeleton and even aggregates the BOM automatically. This page focuses on the two modules, while Tube & Pipe and Cable & Harness (covered in depth on the assembly side) are summarized only at the points where they physically connect to sheet metal and frames (see 03 for full workflows).
0. Module Selection Flow
If you're unsure which module to reach for, work backward from product form.
| Form | Recommended Module |
|---|---|
| Thin plate (≤ 6 mm) with bending | Sheet Metal |
| Structural shapes, tubes, square tubing | Frame Generator |
| Fluid or gas flow paths | Tube & Pipe |
| Wire and signal routing | Cable & Harness |
| Composite (sheet metal cover + frame base) | Sheet Metal + Frame hybrid |
In practice, the "hybrid" row at the bottom is the most common pattern. Sheet Metal handles skins, covers, and brackets while Frame Generator handles the structural base — that division of labor is the standard.
1. Entering the Sheet Metal Environment
Sheet metal parts have a different structure from regular IPT files. You must enter the dedicated sheet metal environment before stacking features, or the Flat Pattern won't generate properly.
- New → pick the Sheet Metal.ipt template (canonical approach)
- To convert an existing part later:
Environments → Convert to Sheet Metal
2. Sheet Metal Rules — the DNA of Every Sheet Metal Part
All values that govern sheet metal behavior — material, thickness, radius, relief, neutral axis — live in a single Sheet Metal Rule. Menu path: Sheet Metal → Setup → Sheet Metal Defaults (or the wrench icon at the bottom of the ribbon).
| Tab | Items | Field Points |
|---|---|---|
| Sheet | Material, Thickness | Material ties directly to iProperty and Mass aggregation |
| Bend | Bend Radius, Bend Relief (Round/Straight/Tear), Minimum Remnant | Default bend radius = thickness (1t) as a starting point |
| Corner | Corner Relief (Round/Square/Tear), Miter Gap, 3 Bend Intersection | Round is stable for laser cutting; Square for forming |
| Unfold Rule | K-Factor or Bend Table | 0.44 is the baseline K-Factor for mild steel. Tune with shop measurements |
3. Key Sheet Metal Features
Menu path: Sheet Metal → Create.
- Face: base flat plate from a sketch profile
- Flange: adds a perpendicular plate to an edge. Height, angle, radius, and relief are all parameterized
- Contour Flange: creates sheet metal along a profile sketch. Good for U-channels and complex cross-sections
- Lofted Flange: lofts between two sketches. Hoppers, truncated cones
- Contour Roll: rolls a 2D profile about an axis. Cylindrical shells, pipe-shaped sheet metal
- Hem: folds an edge (Single / Rolled / Double / Teardrop)
- Bend: inserts a bend between two existing faces
- Fold: bends a face about a sketch line
- Corner Seam: processes the corner between two plates (Miter / Overlap / Reverse Overlap)
- Cut: cuts holes or outline from a sketch. "Cut Across Bend" option cuts in the developed state
- Punch: iFeature-based punch tool. Simulates Emboss/Lance/Form
- Corner Round / Corner Chamfer: 2D edge chamfers and fillets
4. Flat Pattern
The flat pattern is the input for laser, CNC punching, and bending. Menu path: Sheet Metal → Flat Pattern → Create Flat Pattern.
- After creation, toggle between 3D and 2D with Go to Folded Part / Go to Flat Pattern
- Drawing placement: pick "Flat Pattern" under Sheet Metal View in a drawing view
- Punch Representation: real shape / 2-point Center Mark / 1-point Center Mark. Critical for drawing performance with thousands of punches
- Bend Order Annotation: auto-annotates the bend order on the drawing
When Flat Pattern Fails
The core principles from Autodesk's official guide are as follows.
- Always start from a Sheet Metal template
- Use Face / Flange / Contour Flange instead of a generic Extrude
- Rip only when converting a Solid to sheet metal
- A zero bend radius prevents unfolding. Minimum 0.1 mm
- When three or more Flanges meet at one vertex, resolve with Corner Seam or Three Bend Corner
Sheet Metal → Flat Pattern → Export Flat Pattern As DXF. It's the standard format sent to laser shops. Bend info is conventionally attached as a separate PDF drawing.5. Sheet Metal DFM (Design for Manufacturability)
Keeping process constraints in mind before modeling keeps downstream operations clean. t denotes sheet thickness.
| Item | Empirical Minimum |
|---|---|
| Hole-to-bend distance | ≥ 3t |
| Minimum Flange height | 4t (including relief) |
| Minimum bend radius | Aluminum 1t, mild steel 1–2t, stainless 2–4t |
| Max Boss Depth | 3t |
| Tab-to-slot tolerance | +0.1–0.2 mm (laser) |
Tips for Choosing K-Factor
K-Factor is the position ratio of the neutral axis (the unstrained layer) in the sheet. It varies with material, thickness, bend radius, and process (air bending / bottoming / coining).
| Condition | Empirical K-Factor |
|---|---|
| Mild steel air bend, R ≈ t | 0.38 – 0.44 |
| Aluminum air bend, R ≈ t | 0.33 – 0.40 |
| Stainless steel air bend | 0.44 – 0.50 |
| Coining (bottom pressing) | Around 0.50 |
Punch Tool and iFeature
Forming operations like Emboss, Lance, Louver, and Dimple are reproduced with a Punch Tool (iFeature-based).
- New iFeature: design the punch shape in a sheet metal IPT →
Manage → Extract iFeature - Store in a shared library, then drag and drop into other sheet metal parts
- Use drawing Punch Representation options to balance drawing speed and readability
6. Frame Generator Overview
A module dedicated to structural shape design for machine bases, equipment frames, and safety fences. It drops Content Center profiles onto a Skeleton (frame centerlines), automates end treatments (Miter/Notch/Trim), and aggregates the BOM. Menu path: Design → Frame → Insert Frame.
Standard Workflow
- Skeleton Layout: Draw frame centerlines as a 3D Sketch or 2D Sketch (can reference edges of other parts)
- Insert Frame: Select a section from Content Center → place it along the Skeleton lines
- End Treatments: Handle ends with Miter, Notch, or Trim
- Frame Member List (BOM): Lengths and quantities are aggregated automatically
Frame Generator File Structure
Running Insert Frame causes Inventor to auto-generate the following files internally.
- Frame Assembly (.iam): the overall frame sub-assembly. Named "Frame0001" by default
- Frame Member (.ipt): each member, reflecting the profile plus end treatments
- Skeleton (.ipt): optionally separated into its own file
These files have strong name dependencies on each other. Renaming even one breaks the links, so always move or rename them in bulk via Vault Rename or Design Assistant.
7. Skeleton Design Strategy
The heart of Frame Generator is the Skeleton. Manage structural centerlines in a separate .ipt or inside an .iam sketch, and build frames referencing it. With this separation, changing the Skeleton alone updates the entire frame.
- Adding Bend (corner fillet) in the 3D sketch lets Frame Generator auto-miter
- If the company has standard heights and spans, declare them as User Parameters so the Skeleton scales parametrically
- Separating Sub-Assembly skeletons from the top-level Skeleton massively improves manageability in large equipment
8. End Treatments
End treatments mirror how the members are processed on site.
| Treatment | Description | Use |
|---|---|---|
| Miter | Cuts two frames at a specified angle (usually 45°) and joins them | Square frame corners |
| Notch | Cuts a frame to match the profile of another | T-joints, cross beams |
| Trim/Extend to Face | Trim or extend to a specified face | Floor plate joins |
| Trim to Frame | Trims to another frame's cross-section | Mutual tube intersections |
| Lengthen/Shorten | Adjust length by value | Clearance, fine adjustment |
| Reuse | Reuse a previous end treatment | Bulk processing of repetitive structures |
9. Custom Notch & Secondary Features
When the standard notch profile doesn't match the real geometry, you can publish a Custom Notch Profile.
- Edit the profile part → add a notch area sketch in the Body Sketch
- Run the Author tool → assign that sketch to the Optional Notch Profile
- Publish to Content Center
- Select that profile during Notch in Frame Generator
Secondary Features
When adding Hole, Fillet, or Chamfer on top of a Frame Member, enable "Maintain geometry through end treatments". Without it, features disappear when the Skeleton changes. Example: keeping a slot at the end of a leg for a panel slide after mitering.
10. Frame BOM and Material Optimization
Frame members are automatically grouped into a sub-assembly ("Frame" = sub-assembly structure).
- Frame BOM: the Length column is mandatory. It flows directly into the drawing's Parts List
- Mass / Cost: aggregated automatically when you set material density in iProperty
- Save Nested BOM: preserves hierarchy. Useful for sub-level quoting
- Cut length rounding: apply Round-off rules to match shop cutting tolerances
Cautions When Editing Frame Members
- Use Change Member to batch-replace profile and material. Changing them manually one by one breaks relationships
- Reuse End Treatment: with a single drag, apply a repeated treatment pattern
- Don't shorten or delete Skeleton lines after Insert Frame. Deleting them leaves the member in a Sick state that's hard to recover
- Separate sub-frames: Split functionally distinct frames (base, upper structure, safety fence) into sub-assemblies to keep iProperty and Lifecycle independent
11. Tube & Pipe — Interface Points with Frames
The full Tube & Pipe workflow, Style management, Auto Route, and Connection Point rules are in 03. Here we focus only on physical interfaces with sheet metal and frames.
- Support brackets: For routing piping along a frame, connect a sheet metal bracket to the Frame Member via Notch/Cut. Design the bracket as a separate sheet metal part
- Pipe clamp library: Register in a custom Content Center library and place by bundle
- Isometric Drawing: Select the Pipe Run directly from an IDW Base View and dimension with Auto-dimension Pipe Run. For spool drawings, split IPN scenes across sheets
→ See also: /cad-tips/inventor/assembly-content (Tube & Pipe Style and Auto Route)
12. Cable & Harness — Interface Points with Frames
The Harness module is also covered in 03. The interfaces with frames and sheet metal are as follows.
- Cable tray (sheet metal): Create a U-shaped tray with Contour Flange and define interior Segment paths with a 3D Sketch
- Cable fixing bracket: Place a sheet metal bracket on top of a Frame Generator member and use it as a start/end point for Harness Segments
- Enter the Bundle Diameter accurately in Segment Properties so bracket slot sizes and interference checks are meaningful
→ See also: /cad-tips/inventor/assembly-content (Harness Authoring, RefDes, Wire List)
13. Drawing Tips Shared by Sheet Metal and Frames
Sheet metal and frame drawings differ subtly from general machined-part drawings. Everything in 04 still applies, but the following items matter especially.
- Sheet metal drawings: Place the Flat Pattern as a Sheet Metal View and auto-annotate the bend order
- Include DXF: Laser shops only need DXF, but bend order, grain direction, and deburring scope must be called out on the PDF drawing
- Frame drawings: Since the Frame BOM auto-populates the Parts List, always include Length and Cut Length columns. State the cutting round-off too
- Weld symbols: Use ISO 2553 to differentiate fillet, groove, and plug welds. Get size, length, and pitch (@) right
- Heat Number tracking: Add material Heat Number to the BOM (Custom iProperty) for pressure vessels and safety-related frames
- Surface Treatment: Plating, painting, anodizing, etc., go in Title Block notes or a dedicated table
→ Drawing fundamentals: /cad-tips/inventor/drawing-presentation/
14. Industry Application Notes
- Conveyor frames: Define centerlines and heights as User Parameters on the Skeleton → use iLogic to auto-generate length variants. Break long members in drawings with Break View
- Automation equipment base: Frame Generator + sheet metal cover hybrid is the standard pattern. Use Lofted Flange and Contour Flange for covers
- Jigs/Fixtures: Sheet metal + frame hybrid is common. Derive the workpiece to adaptively position clamps and pins
- Plant pipe support structures: Design pipe racks in Frame Generator → lay Tube & Pipe on top. Interference Check is mandatory
15. Common Mistakes
- Starting Extrude in a regular IPT for plate thickness, then converting to sheet metal → Flat Pattern failures become routine
- Entering 0 for Bend Radius → unfolding is impossible at all
- Redefining Sheet Metal Rules per part → flat pattern lengths vary for the same shop
- Renaming or moving Frame Generator files → destroys Skeleton linkages with almost no recovery
- Deleting Skeleton lines → the member remains in a Sick state
- Repeating End Treatments manually → Reuse does it in a few clicks
- Not checking Maintain Geometry on Secondary Features → work is lost when the Skeleton changes
- Managing frame material only through Parameters → Mass/Cost aggregation is inaccurate. Also set iProperty Material
Field Checklist
- Sheet metal parts were started from the Sheet Metal template
- Sheet Metal Rules reference a single master in the company Style Library
- K-Factor is tuned to shop measurements, or a Bend Table is applied
- Bend reference options during Flange creation match shop practice
- After Flat Pattern creation, DXF export is possible
- DFM criteria like hole-to-bend distance and minimum flange height are met
- Frame Generator Skeleton is isolated as a separate part or sketch
- Frame files were not renamed or moved (or only via Vault Rename)
- Secondary Features have "Maintain geometry" enabled
- Frame BOM Length, Material, and Mass aggregate correctly
- Custom Notch profiles are published to Content Center and shared
- Interfaces where piping or harness meets the frame (brackets, trays) are modeled as separate sheet metal parts