Broken-Out Section in SolidWorks: Step-by-Step Guide

Open a window into one drawing view to show what is inside, set the depth so the cut lands where you want it, and keep every drawing revision tracked in Sibe while reviewers mark it up in a browser.

You can open a window into one corner of a drawing view and show the internal geometry underneath it, without cutting the whole model and without touching the part. That is a broken-out section, and on a crowded sheet it is often the only view that reads clearly.

In SOLIDWORKS® 3D CAD it lives entirely in the drawing. The model never changes, so a broken-out section costs you nothing downstream — no configuration, no derived part, no extra file for someone else to check out.

Sibe is a cloud CAD Document Management platform with a native SolidWorks add-in. Drawings you build this way check in and out directly in SolidWorks, every revision is tracked as you go, and a reviewer with no CAD license opens the current sheet in a browser to mark it up.

What a broken-out section is

A broken-out section removes material inside a closed sketch profile, down to a depth you set, on one drawing view. It is a child of the view, so it moves with the view, scales with the view, and disappears if the view does.

Compare that to the alternatives. A full section view cuts the entire model on a plane and gives you a new view. A half section does the same on half the model. A detail view enlarges a region but shows the same outside surfaces you already had. The broken-out section is the only one that leaves the surrounding geometry intact and still shows you what is inside.

When to use one

• Show a threaded hole, boss or internal rib without cutting the whole part
• Expose a bearing seat while the housing around it stays readable
• Save a sheet — no extra view, no extra cut line to chase
• Reveal wall thickness in one spot on a large casting or weldment
• Show wiring or a routed hose inside an assembly cover

Steps to create a broken-out section

1. Open the drawing and click the view you want to modify, so the sketch belongs to that view rather than the sheet.
2. Go to the Sketch tab and draw a closed profile — spline, circle or polygon — around the area you want to expose.
3. Go to Insert > Drawing View > Broken-out Section, or right-click inside the view and pick Broken-out Section from the context menu.
4. Set the depth: choose Through Entire Part, type a distance, or select a model edge, vertex or face as the reference.
5. Turn on Preview and drag the depth handle until the cut lands where you want it.
6. In an assembly view, add fasteners, shafts and other solid hardware to the Excluded components list.
7. Click OK. SolidWorks removes material inside the sketch boundary to the depth you set and hatches the cut faces.

Setting the depth correctly

Depth is measured from the front of the view — the side nearest you — straight back into the model. It is not measured from the sketch plane of the original part, and it is not measured from the model origin. That single fact clears up most of the confusion.

Typing a number works when you know the geometry cold. Everywhere else, pick a reference instead. Click a circular edge on the far side of the bore you want to open, and the depth follows that edge — including when the model changes and the bore moves. A typed 12.5 mm does not follow anything.

Through Entire Part cuts all the way through. On a single part that is usually what you want for a hole callout. On an assembly it will slice everything in the sketch region, hardware included, which is why the excluded components list matters.

Three things that usually go wrong

1. The sketch is not closed, or it belongs to the sheet

If the Broken-out Section command is grayed out or throws an error, the profile is open somewhere. Zoom in on the endpoints; a spline that looks joined at 100% is often two points a fraction apart. Run Tools > Sketch Tools > Check Sketch For Feature to find the gap. The other half of this failure is selecting nothing before you sketch — the sketch then belongs to the sheet, and the command has no view to act on. Click the view first, confirm its border highlights, then sketch.

2. The depth reference is wrong, so the cut lands short or too deep

You get a hatched face with nothing interesting behind it, or you cut clean through a wall you needed. Edit the broken-out section, turn on Preview, and drag the handle rather than guessing. If you typed a value, switch to a model edge on the feature you actually want revealed. A reference survives a design revision; a typed number quietly goes stale and nobody notices until the shop calls.

3. In an assembly, the wrong components get cut

By convention, bolts, pins, shafts and other solid parts are drawn uncut in a section. A broken-out section will happily slice them unless you say otherwise. Open the Excluded components list in the PropertyManager and add every fastener inside the sketch region. Do it while you create the feature — going back later means reselecting each one against a hatched view.

Editing a broken-out section

The feature sits under its parent view in the FeatureManager tree. Right-click it to reach Edit Sketch for the boundary shape or Edit Definition for the depth. Deleting the feature restores the view; deleting the sketch deletes the feature with it. If you need the same cut on a second sheet, copy the sketch and rebuild the feature there — the section itself does not travel between views.

Best practices

• Keep the boundary spline simple — four or five points, not fifteen
• Use a reference edge for depth so the cut follows design revisions
• Limit yourself to one or two broken-out sections per view
• Exclude fasteners and shafts before you click OK, not after
• Add a note when the depth is not obvious from the hatching

Used well, a broken-out section answers a manufacturing question in place, on the view the machinist is already looking at. Used everywhere, it turns a sheet into a patchwork of hatch marks. One clear cut beats three vague ones.

Where Sibe fits

A drawing is only as good as the revision it reflects. The broken-out section you set up against Rev C shows the wrong thing the moment the model moves to Rev D — and the person who most needs to see that is usually the one without a CAD seat.

Sibe is a cloud CAD Document Management platform with a native SolidWorks add-in. Engineers check drawings in and out directly in SolidWorks, and Sibe tracks every version, so the sheet on screen is the current one and the older ones are still there when you need to prove what shipped. Assembly references resolve automatically, so a drawing keeps pointing at the right parts even when they are shared across projects. DWG and DXF files sit alongside the native drawings.

For review, a free public share link or QR code opens the model and its drawings in any browser — no Sibe account, no viewer install. A production manager, a supplier or a client marks up the exact area you cut, and the comment lands against that version. See how that works on the design reviews page, or how approvals lock a released drawing in revision and approval workflow. Setup is live in under 20 minutes.

No servers, no VPNs, no admin hassles. Book a free 20-minute demo or try Sibe free for 14 days — no credit card.