You add a louver, a lance, or a drawn cutout to a SolidWorks sheet metal part, flatten it, export DXF, and the cuts that should appear in the flat layout are either missing or positioned wrong. The forming tool placed correctly in the bent part. The flat pattern shows the footprint outline but not the cut geometry. The laser operator can’t nest from this file.
This happens because of how SolidWorks models forming tool geometry — and the fix depends on which features are actually in play.
How SolidWorks Forming Tools Work
A forming tool in SolidWorks is not a cut feature. It is a push feature — it displaces material to create a formed shape (louver, lance, bridge, drawn cutout) without removing metal. The forming tool adds geometry to the sheet metal part by deforming the material surface. It does not punch a hole; it pushes material to a new shape.
When SolidWorks unfolds a sheet metal part to its flat pattern, it reverses the bends and develops the part geometry. For bent flanges, this is straightforward: the bend radius and K-factor determine the developed length, and SolidWorks computes the flat geometry from the bent geometry.
Forming tools are different. The geometry underneath a forming tool — the face being deformed — is excluded from the unfolding calculation. The unfold engine treats the formed region as a black box and does not attempt to compute what the pre-formed flat should look like for that zone. This exclusion zone is exactly what causes feature geometry to disappear or shift in the flat pattern DXF.
SolidWorks explicitly documents this behavior: the flat pattern for features created with forming tools shows the forming tool outline in its flat-state projected position but does not reconstruct the individual geometry elements that the forming operation created. The flat pattern is showing you the forming tool’s footprint, not its internal geometry.
What Actually Disappears — Lances and Louvers
Consider a lance: a cut-and-formed tab where the sheet is slit on three sides and the resulting flap is bent. In the bent part, you see the slit opening and the displaced tab. In the flat pattern, what should appear is the slit lines and the cut geometry before forming.
What SolidWorks shows depends on how the lance was modeled:
Using the built-in SolidWorks Forming Tool library (lance from the Design Library): The flat pattern shows the forming tool footprint in its projected position. The slit lines — the actual cut path for the laser or punch press — are often absent or simplified into the footprint boundary. The operator sees a closed rectangle where they need an open slit.
Using a custom forming tool with a Stopping Face defined correctly: The stopping face determines where the tool placement anchors to the sheet surface. If the custom forming tool was designed with cut geometry modeled at the stopping face level (the flat interface between tool and sheet), those cuts appear in the flat pattern. SolidWorks projects the stopping-face geometry onto the sheet in its flat-state position. This works when the forming tool was built this way — but the Design Library tools generally were not.
Relief cuts added as separate features on the sheet metal part (not inside the forming tool body): These are independent Extruded Cut features in the feature tree. They appear correctly in the flat pattern in all cases.
The key distinction: cuts and holes defined inside the forming tool body may not appear in the flat pattern. Cuts and holes defined as separate features on the sheet metal part always appear correctly.
The Unfold/Fold Workaround
For forming tools where the flat-state cut geometry is critical — lances that need precise slit positioning, louvers where the laser needs to cut before the press forms — the Unfold/Fold workflow gives you explicit control.
Step 1: Unfold the specific bend
Instead of relying on the automatic flat pattern, use Insert > Sheet Metal > Unfold to manually unfold specific bends. Select the fixed face and the bends you want to unfold. This places the unfolded geometry in the 3D part file as a real state.
Step 2: Add cuts in the unfolded state
With the part unfolded (still a 3D feature in the tree), add sketch-based Extruded Cut features in the unfolded state. These are real features — they survive folding and appear in all configurations.
Step 3: Fold back
Use Insert > Sheet Metal > Fold to re-fold the same bends. The cut features you added in the unfolded state are now present in both the folded and flat-pattern representations.
The cut geometry now appears correctly in the DXF export because it’s a native feature, not geometry inside a forming tool body.
The tradeoff: This workflow is manual. For a part with 10 unique forming tool instances, adding the cut geometry manually for each is time-consuming. For a panel with 200 louvers, it’s impractical by hand — see the 200-louver section below.
The 200-Louver Problem
A stainless enclosure panel with a grid of 200 louvers. The designer wants the flat pattern DXF to show the slit cut lines so the laser/punch operator knows where to cut before the forming station. The forming tools place correctly in the bent model. The flat pattern shows 200 footprint outlines but no slit cut lines.
This is the scenario where teams hit the forming tool limitation at production scale. Options, ranked by practical value:
Option 1 — Model slits as separate Extruded Cuts, patterned (best for new parts)
Create one louver with the forming tool AND an Extruded Cut for the slit, then apply a Linear Pattern to both features simultaneously. The pattern drives both features from the same driving dimension. The Extruded Cut is independent of the forming tool, so it appears in the flat pattern. This is the correct approach for any part that will go into production.
The critical detail: the pattern must drive both the forming tool instance and the cut instance, keyed to the same reference geometry. If the forming tool and the cut are in separate patterns, they drift out of alignment when the pitch changes.
Option 2 — Two-configuration approach (best for existing parts)
Create a “Flat_for_DXF” configuration: suppress all forming tools in this config, then add sketch-based Extruded Cuts representing the cut paths at the forming tool positions. This configuration exists only for flat pattern export — the production model stays in the “Formed” configuration.
The limitation: you now maintain two feature definitions. When the louver count or position changes, you update both. This is viable for parts that don’t change often; it becomes a maintenance problem for parts that evolve through many revisions.
Option 3 — Rebuild the forming tool with stopping-face cuts
Rebuild the louver forming tool with the slit cut geometry modeled into the forming tool body at the stopping face level. When SolidWorks places this tool, the cut geometry projects onto the sheet surface. This works correctly when well-built, but requires rebuilding the forming tool model — which is usually not in the Design Library tools you received with SolidWorks.
If your shop uses the same forming tools repeatedly across many parts, this is worth the one-time investment: rebuild the tool correctly, save it to your Design Library, and all future parts that use it get the correct flat pattern automatically.
Option 4 — Post-process the DXF
Accept that the flat pattern DXF has only footprint outlines, and add the slit geometry programmatically in a post-processing step. This is the approach some shops take when they have a fixed forming tool type and a large volume of parts: the post-processor knows the geometry of the louver slit and inserts it at each forming tool footprint center point in the DXF.
The risk: if the forming tool placement angle or depth varies across parts, the post-processor needs to handle those variations. It works well for a fixed, standardized louver on a standard pitch.
What the DXF Looks Like — Each Approach
When you batch export DXF files from a SolidWorks assembly, the flat pattern DXF reflects exactly what the flat pattern configuration contains:
| Approach | Flat pattern DXF shows |
|---|---|
| Default forming tool (Design Library, no extra cuts) | Forming tool outline (footprint), no internal slit geometry |
| Forming tool + patterned Extruded Cut | Forming tool outline + slit geometry as separate sketch entities |
| Two-config (forming suppressed) | Only slit cut geometry — clean cut layout, no forming footprint markers |
| Rebuilt forming tool with stopping-face cuts | Forming tool outline + cuts merged into same profile |
For laser cutting, the two-config approach or a rebuilt forming tool produces the cleanest output: the operator’s nest program needs the cut path as a clean contour, not a footprint marker boundary that may or may not define the actual cut path.
For waterjet cutting — which cuts and then re-forms in a press brake — see the guide on DXF file preparation for waterjet cutting for lead-in geometry and tolerance requirements. The forming tool positioning considerations apply there as well.
Layer Control in the DXF Export
Once you have the correct flat pattern geometry, DXF entity export settings determine which entities land on which layers. For sheet metal parts with forming tool geometry:
- SHEETMETAL-PART — outer boundary of the flat pattern (the profile the laser or waterjet cuts)
- BENDS — bend lines (the scored or marked lines that guide the press brake operator)
- FORMING — forming tool outlines (visible for reference, not for cutting)
Keeping forming tool outlines on a separate layer from cut geometry matters for shops that share DXF files between laser, waterjet, and press brake operations. Each operator’s machine reads only the layers relevant to their step. If forming tool footprints land on the same layer as the cut profile, the laser or nest software may attempt to trace the footprint as a cut path — producing incorrect nest programs.
CadShift handles this layer assignment automatically during batch DXF export — the layer structure is configured once and applied consistently across every flat pattern in the assembly, without per-file manual layer assignment.
The Flat Pattern Configuration and K-Factor
There is one more issue specific to parts where you use a “Flat_for_DXF” configuration with forming tools suppressed. SolidWorks flat pattern dimensions depend on the K-factor being consistent for the material and gauge. If the K-factor or bend deduction source is configuration-specific in the Sheet Metal feature, the “Flat_for_DXF” config may inherit a different value than the production configuration — producing a flat pattern with correct geometry but wrong developed length.
Before using any DXF configuration for production, verify that the Sheet Metal feature’s K-factor is driven at the global model level (or from the gauge table), not by configuration-specific overrides. The forming tool issue and the K-factor issue are related: both stem from flat pattern state being one possible representation of the part, where the driving parameters need to be unambiguously defined for the manufacturing state.
For parts where multiple bodies each have their own flat pattern — a common scenario in weldment assemblies where sheet metal components are modeled as separate bodies — see our guide on multi-body DXF export and per-body orientation for how to manage the flat pattern states across a multi-body part file.
Geometry Patterns That Cause Related Failures
The forming tool flat pattern issue is one of several sheet metal failure modes that are non-obvious and underdocumented. Our post on SolidWorks sheet metal geometry patterns that fail covers the related cases: lofted bend parallel-plane requirement, the non-developable surface error on compound-curve flanges, and the K-factor hierarchy (material > Sheet Metal feature > gauge table) that determines which value actually drives the flat pattern when settings conflict.
If the holes in your flat pattern appear as ellipses rather than circles — a separate but similar issue — the cause is holes drilled in the bent state without the Unfold/Fold workflow. The guide on holes drilled in the bent state covers that specific failure mode and how to reconstruct circular holes in the flat pattern.