Every SolidWorks tutorial on flat pattern views shows the same thing: open a sheet metal part, drag the flat pattern from the View Palette into a drawing. That works perfectly when you have one part and one drawing. It doesn’t help when you have an assembly with twelve sheet metal components and you need all the flat patterns in a single drawing document.

The assembly case has two complications that the single-part case doesn’t. First, the View Palette shows assembly-level views, not individual part views — so the flat pattern doesn’t appear there. Second, when you insert from the assembly, SolidWorks shows views relative to the assembly coordinate system, not the part’s sheet metal orientation. Knowing which insert path to use for each scenario saves the frustration of inserting views that display the wrong orientation or can’t locate the flat pattern at all.

Adding a Flat Pattern View From a Part File

The simple case first, because it’s the baseline and the assembly workarounds build on it.

Open the sheet metal part (not the assembly that contains it). Open a new or existing drawing. In the View Palette on the right side of the screen, look for the flat pattern in the view list. It appears at the bottom of the standard orientation thumbnails as “Flat Pattern.” Drag it onto the drawing sheet to place it.

If the View Palette doesn’t show the part’s views, click the dropdown at the top of the View Palette and select the open part document. The palette updates to show that document’s available views.

Two situations where the flat pattern doesn’t appear in the View Palette:

The Flat-Pattern1 feature is suppressed. SolidWorks suppresses the flat pattern feature when you switch to certain configurations — particularly configurations set up for 3D modeling or welding where the sheet metal shouldn’t unfold. Check the feature tree in the part: look for Flat-Pattern1 and confirm it’s not suppressed (suppressed features appear in light gray). If it is suppressed, right-click and Unsuppress it, or activate a configuration where it isn’t suppressed before inserting the view.

The part has no Sheet-Metal feature. If the part was built using Boss-Extrude + Shell rather than the sheet metal toolset, SolidWorks doesn’t recognize it as sheet metal and produces no flat pattern feature. The part needs to be rebuilt with sheet metal features or converted with Insert > Sheet Metal > Convert to Sheet Metal before a flat pattern view is possible. This conversion path works in simple cases and fails on complex geometry — see how SolidWorks creates flat patterns and where the unfold algorithm breaks down for when conversion is viable.

Adding a Flat Pattern View From an Assembly Drawing

This is the case the tutorials skip.

You have an assembly drawing open — the assembly is the model reference, and you’ve already placed the isometric and orthographic views. Now you want to add flat pattern views for each sheet metal component without opening separate part files.

The View Palette won’t help here. When the drawing’s active model is the assembly, the palette shows assembly views only. Sheet metal parts inside the assembly don’t expose their flat patterns through the assembly’s view set.

Method: Insert > Drawing View > From Part/Assembly

Go to Insert > Drawing View > From Part/Assembly (or Model View from the Drawing toolbar). The dialog opens, showing the currently open documents. Navigate using the Browse button to the specific sheet metal part file (the .sldprt) — not the assembly. Select it.

The Model View PropertyManager opens on the left. In the Orientation list, scroll past the standard views (Front, Top, Right, etc.) and select Flat Pattern. This option only appears if the part has an unsuppressed flat pattern feature.

Click on the drawing sheet to place the view.

If you need flat patterns from multiple parts in the same drawing, repeat this for each part. This is tedious for assemblies with many sheet metal components — which is where multi-sheet drawings or a batch DXF workflow becomes the better approach.

Alternate method: Use the View Palette with a part open in another window

Open the sheet metal part file in a separate SolidWorks window (not the assembly — the specific part file). Switch to your assembly drawing. In the View Palette dropdown, select the open part document. The palette now shows that part’s views including Flat Pattern. Drag the flat pattern into the drawing.

This is slightly faster than the Insert dialog approach, especially when you’re working through multiple parts and want to see the view thumbnails before placing.

Multi-Sheet Layout for Assembly + Flat Patterns

The practical pattern for assembly drawings that include flat patterns:

  • Sheet 1: Assembly views (isometric, front, top) with BOM table and balloon callouts.
  • Sheets 2–N: One sheet per sheet metal component with the flat pattern view, relevant detail views, and the part’s bend table or k-factor note.

This keeps the assembly drawing intact as the primary communication document while providing fabrication-ready flat pattern drawings for each component. The drawing file references both the assembly (for sheet 1) and the individual parts (for subsequent sheets) — SolidWorks handles this without issue.

To add a sheet, right-click any sheet tab at the bottom of the drawing and select Add Sheet. On the new sheet, the active model can be different from sheet 1: use Insert > Drawing View > From Part/Assembly to set the new sheet’s views to the specific part file.

Multi-Body Sheet Metal Parts

If a sheet metal part contains multiple bodies — for example, a part with two distinct flat patterns representing different piece parts — each body has its own flat pattern feature in the tree.

When you place a flat pattern view from this part, SolidWorks inserts the flat pattern for the active sheet metal body. To get the flat pattern for a different body, you need to either use different configurations (where each config has a different body active) or use the Flat Pattern view with the specific body selection that the View PropertyManager exposes in the Reference Geometry rollout.

The multi-body case is more reliably handled by exporting each body’s flat pattern as a separate DXF directly from the part file rather than through the drawing. The multibody DXF export workflow and how body orientation affects the output covers the body-by-body export path and the handed-part problem in detail.

DXF Export From a Drawing Flat Pattern View

Once a flat pattern view is placed in the drawing, you can export it to DXF via two paths:

Right-click the view > Export > DXF/DWG. This exports the selected view to DXF, but it exports the drawing view region — which may include drawing border, annotation notes, title block elements, and dimension annotations that overlap the flat pattern geometry. Not useful for sending to a laser cutter that expects clean part geometry.

Export the part directly via File > Save As > DXF. From within the part (not the drawing), this produces a clean flat pattern DXF with only the part geometry, bend lines, and any features you’ve configured in the export options. The drawing view is useful for review, but for fabrication output the direct part export is cleaner.

The DXF export options that matter — entity types, bend line layers, chord deviation for splines, whether countersinks appear as circles or cross-hairs — are set per-part in File > Save As > Options and don’t persist between SolidWorks sessions by default. For a team workflow where these settings need to be consistent across all parts, the API fix for persisting DXF export settings prevents the misconfiguration that happens when someone exports on a machine where the options haven’t been set. The DXF entity export settings that actually affect flat pattern quality explains which settings to standardize and why.

When Drawings Aren’t the Right Path

Drawing-based flat pattern views are useful for documentation — for the drawing packet that goes to an internal reviewer or a supplier who needs to understand the part in context. They’re the right tool when someone needs to look at the flat pattern alongside the bent part, see the bend table, or review the full dimension set.

They’re not the right tool when you need to produce DXF files for a CNC laser table, plasma cutter, or waterjet that expects a clean flat outline with bend lines on a separate layer. For that case, batch DXF export from an assembly — which extracts flat patterns from every sheet metal component and outputs them as separate named files — is faster and produces cleaner output than placing views in drawings and exporting one by one. CadShift automates this process from within SolidWorks, pulling part numbers, quantities, and materials from the BOM and embedding them as file names and DXF layer metadata.

The drawing view is for human review. The direct DXF export is for machine input. Most assembly-to-fabrication workflows eventually use both.