How to extrude cut in SolidWorks?

Contents

An Extruded Cut removes material from an existing solid body using the shape of a 2D sketch.
Because it is a sketch‑based feature, you must already have at least one solid feature in the part before you can create an extruded cut.

This tutorial explains:

How to create a basic Extruded Cut step by step
What the From (start condition) options do
What the Direction and end condition options do
Useful advanced options: draft, thin feature, selected contours, feature scope
A worked example that compares Up to Next vs Through All – Both

1. Creating a basic Extruded Cut

Create or open a part with an existing solid body.
Extruded Cut cannot be the first feature in a part because there is nothing to remove yet.
Choose a sketch plane or face.
Pick a plane (Front, Top, Right) or an existing planar face where you want to define the cut profile.
Start a sketch.
Click Sketch, then draw the 2D profile of the material you want to remove (rectangles, circles, slots, etc.).
Fully define the sketch with relations and dimensions where practical – it makes edits more predictable.
Exit the sketch.
Start the Extruded Cut feature.
Go to Features > Extruded Cut (or Insert > Cut > Extrude…).
The Cut‑Extrude PropertyManager opens.
Set the From (start) condition.
Choose how the cut starts: from the sketch plane, another face, a vertex, or an offset distance (explained in detail below).
Set the end condition in Direction 1.
Pick Blind, Through All, Up to Next, etc., and enter the depth where needed.
Optionally enable Direction 2.
Turn on a second direction if you need the cut to go both ways from the sketch (with different depths or end conditions).
Adjust options such as Draft, Thin Feature, Selected Contours, and Feature Scope if needed (covered later).
Check the preview and click OK.
Rotate the model to verify the cut behaves as intended.

From

The From options control where the cut starts relative to the sketch.
They are especially important when you’re not sketching directly on the starting face of the cut.

Sketch Plane

The cut starts directly from the sketch plane (or sketch face) and extends in the chosen directions.
This is the most common and simplest option:

Use when the sketch is drawn on the exact face where the cut should begin.
Ideal for simple holes, pockets, and through cuts starting from a flat face.

Surface / Face / Plane

The cut starts from a specified surface, face, or reference plane, instead of the sketch plane itself.
SolidWorks effectively creates a virtual start plane through that selection and extrudes from there.

Useful when the sketch is located on one plane but the cut must start at a different face (e.g., offset geometry).
Maintains design intent: if the reference face moves, the start of the cut updates with it.

Vertex

Starts the cut from a plane parallel to the sketch plane that passes through a selected vertex or sketch point.

Good when you want the start of the cut to line up with a known corner, hole center, or construction point.
Helps avoid manually calculating offsets – the model geometry controls the position.

Offset

Creates the cut starting at a specified offset distance from the sketch plane.
You can flip the direction of the offset with the flip arrow/button.

Use for cuts that must start a fixed distance inside a part (e.g., a pocket that starts 5 mm below the surface).
Very useful when the outer dimensions of the part may change but the offset must remain constant.

Tip: In many designs you can achieve more robust, parametric behavior by referencing faces, planes, or vertices instead of typing static distances whenever possible.

Direction

The Direction 1 (and optional Direction 2) areas define how far and in which direction the cut extends from the start condition.
SolidWorks offers several End Condition types:

Blind

Creates a cut to a specified depth in one direction from the start plane.

Set the Depth value to control how far the cut goes.
Use the Reverse Direction arrow to flip the cut direction.
Best when you truly want a fixed depth that does not depend on surrounding geometry.

Through All

Extends the cut from the start plane through all existing geometry in one direction until it exits the part.

Ideal for holes or slots that must always go completely through the part, even if thickness changes.
Reduces the need to manually edit the cut depth when dimensions change.

Through All – Both

Cuts through all geometry in both directions from the sketch in a single setting (no need to configure Direction 2 separately).

Great when the sketch is positioned mid‑thickness and you want the cut to pass entirely through the part both ways.
Also useful for open profiles (e.g., a line) to create “split” cuts that pass through both sides of a part.

Up to Next

Extends the cut from the start plane to the next face or surface that fully intersects the cut profile.
It stops as soon as the profile is completely cut by a face on the same body.

Behaves like a local “Through To” condition – the cut stops at the first qualifying wall.
If the sketch intersects the thickest region of the part, it may behave similarly to a full Through All.
Excellent when you want the cut to adapt automatically as intermediate geometry moves.

Up to Vertex

Extends the cut to a plane parallel to the sketch plane that passes through a selected vertex or sketch point.

Useful when a drawing or design calls out a cut ending exactly at a particular corner, point, or intersection.
Avoids having to maintain a dimension if that point moves with design changes.

Up to Surface

Extends the cut until it reaches a selected surface or face.

Use for cuts that must terminate on a curved or non‑planar surface, or on a specific face of another feature.
Preferable to Blind when the terminating face can move; the cut updates to follow that face.
Works with both solid faces and surface bodies (with some limitations if the surface is smaller than the cut profile).

Offset from Surface

Extends the cut to a distance offset from a selected face or surface.
The sign of the offset controls whether the cut stops before or beyond the reference surface.

Ideal for maintaining a constant clearance or wall thickness relative to another face.
Combines the robustness of geometry‑based termination with a controllable gap.

Up to Body

In a multibody part or an assembly feature, this option extends the cut from the sketch plane to a selected body.

Very robust for tooling, mold, or fixture design where one body is cut up to the shape of another.
References the whole body instead of individual faces, so it often survives geometry changes better than Up to Surface.

Mid Plane

Extends the cut equally in both directions from the sketch plane by half of the specified depth.
The sketch plane becomes the middle of the cut.

Great for keeping features centered on a main reference plane.
Helps maintain symmetry around the origin or primary planes.

Depth

The Depth parameter is used by end conditions such as Blind and Mid Plane. It specifies:

For Blind: total distance from the start plane in that direction.
For Mid Plane: total thickness of the cut (half applied to each side of the sketch plane).

Draft On/Off

Without draft, the side faces of the cut are perfectly parallel.
Turning Draft On adds a taper angle to the side faces of the cut.

Use draft for manufactured parts that require taper for release (e.g., molded or cast parts).
The Draft outward option flips the direction of taper.
Direction 1 and Direction 2 can have different draft angles if needed.

Direction 2

Direction 2 allows you to apply a second, independent end condition from the same sketch in the opposite direction.

You can choose a different end condition in Direction 2 (for example, Blind one way and Up to Surface the other).
Depth, draft, and termination can be configured independently for each direction.
Especially powerful when your sketch lies in a mid‑plane and the geometry on each side of the plane behaves differently.

2. Additional useful options

Thin Feature

The Thin Feature option lets you use open or closed sketches to create thin‑walled cuts with a specified wall thickness.
Instead of cutting the full area of the sketch, SolidWorks creates a “slot” or “channel” based on the sketch and the thickness.

Excellent for creating slots or grooves from a single line or arc.
Can add thickness in one direction, both directions, or symmetrically about the sketch.
Can be combined with draft and both directions for quite complex cuts.

Flip side to cut

When using closed profiles, SolidWorks needs to know which side of the sketch to remove material.
The Flip side to cut option inverts the side that is removed.

Use when the preview shows material being removed on the wrong side of the sketch region.
Critical when using mid‑plane or “through all both” conditions on centrally located sketches.

Selected Contours

If your sketch has multiple closed regions (multi‑contour sketch), you don’t have to create separate sketches for each cut.
The Selected Contours box lets you pick specific regions to cut while leaving others unused.

Reduces sketching time by letting you reuse a single sketch to create different features.
Helps keep models simpler and easier to edit by avoiding unnecessary duplicated sketches.

Feature Scope (multibody and assembly cuts)

In multibody parts and assembly features, Feature Scope controls which bodies or components are affected by the cut.

All bodies / All components – the cut is applied everywhere it intersects.
Selected bodies / Selected components – only the chosen bodies/components are cut.
Auto‑select – allows SolidWorks to automatically pick intersecting bodies, which you can override when needed.

Using Feature Scope correctly is essential to avoid unintentionally cutting “through everything” in complex multibody or assembly designs.

3. Worked example

This example builds a simple multibody block and then uses different end conditions to illustrate how Up to Next and Through All – Both behave.
Dimensions are not critical for the concepts, but they are included for clarity.

Step 1 – Extrude1: Base block

Create a new part.
On the Front Plane, sketch an 85 mm × 85 mm square, coincident with the origin.
Create an Extruded Boss/Base:
- From: Sketch Plane
- End condition: Mid Plane
- Depth: 30 mm
This produces a centered block 30 mm thick.

Step 2 – Extrude2: Add a larger pad on one side

On the back face of the square block, start a new sketch.
Sketch a rectangle 250 mm × 115 mm, positioned as desired.
Create another Extruded Boss/Base:
- From: Sketch Plane
- End condition: Blind
- Depth: 10 mm
You now have a thicker region on one side of the original block.

Step 3 – Cut‑Extrude1: Compare Up to Next vs Through All – Both

On the Right Plane, start a sketch.
Sketch a 25 mm × 15 mm rectangle, and make one corner coincident with the top edge of Extrude1.
Create Cut‑Extrude1 from this sketch.
Set Direction 1 and Direction 2 end conditions to Up to Next.
Observe the preview:
- The cut travels until it hits the next face that completely intersects the profile in each direction.
- In some directions it may stop in the thicker pad (Extrude2), in others it may stop at the side face of the original block.
Now change both directions to Through All – Both and watch the preview again:
- The cut now passes completely through all geometry in both directions until it exits the part.
- You can clearly see the difference between “stop at the first wall” (Up to Next) and “go through everything” (Through All – Both).

Step 4 – Cut‑Extrude2: Up to Next acting like Through All – Both

Start another sketch on the Right Plane and draw the same 25 mm × 15 mm rectangle.
Constrain the rectangle:
- Make the center point horizontal with the origin.
- Make the center coincident with the back edge of Extrude1.
Create Cut‑Extrude2 using this sketch and set both Direction 1 and Direction 2 to Up to Next.
Because the sketch now intersects the thickest part of the model on both sides, the cut travels until it passes through all the relevant walls.
In this configuration, Up to Next effectively behaves like Through All – Both.

Step 5 – Verifying behavior with additional geometry

To further prove how Up to Next works, an additional boss can be inserted so that it lies in the path of the cut:

If that new boss becomes the first surface to fully intercept the cut profile, Up to Next will stop at its face.
If it does not fully intersect the profile, the cut continues to the next qualifying face beyond it.

The final result and a side view of the cut on the extra boss (if added) illustrate how Up to Next is sensitive to which faces are actually intersected by the sketch profile.

4. Best practices and design intent tips

Prefer geometry‑aware end conditions where possible.
Use Through All, Up to Surface, Offset from Surface, or Up to Body instead of fixed Blind depths when the termination is tied to other geometry.
This reduces the need for manual updates when the model changes.
Use Mid Plane for symmetric parts.
For features that should stay centered, sketch on a main reference plane (Front/Top/Right) and use Mid Plane end conditions to keep the model symmetric.
Keep sketches simple and reusable.
Use multi‑contour sketches with Selected Contours instead of creating many separate sketches for each cut.
Control which bodies are cut in multibody parts.
Always check the Feature Scope area to ensure you are cutting only the intended bodies or components.
Use draft where manufacturing requires it.
For molded, cast, or machined parts that need taper, add draft directly in the cut feature so the design and manufacturing intent stay linked.

5. Troubleshooting common Extruded Cut issues

The cut appears on the wrong side of the sketch.
Use Flip side to cut or reverse the direction arrow.
The cut doesn’t go all the way through the part.
Check the end condition – you may be using Blind or Up to Next where Through All or Through All – Both is needed.
Up to Surface or Offset from Surface gives an error.
Make sure the reference surface or face completely covers the projected area of the cut profile.
If the face is too small or highly irregular, create a larger reference surface or use Up to Body instead.
Up to Body fails with “unable to extrude up to selected body”.
The selected body must fully intersect the cut’s path. Extend the sketch or adjust geometry so the body properly lies in the cut direction.
Unexpected bodies get cut in a multibody part.
Open the feature definition and review the Feature Scope settings. Switch from All bodies to Selected bodies and explicitly choose only the bodies that should be affected.

By understanding the From options, end conditions, and advanced controls like Thin Feature, Selected Contours, and Feature Scope, you can create Extruded Cuts in SolidWorks that are not only correct today but also robust against future design changes.