Introduction

Sketch Driven Pattern is a modeling tool used to copy geometry in irregular layouts.

Unlike rectangular or circular patterns, this method does not rely on distances or angles. Instead, the position of each instance is controlled by points defined in a sketch.

In Autodesk Inventor, the command can duplicate:

• Features
• Solid bodies
• Surface bodies

The position and orientation of the copies are controlled by two main inputs:

Sketch center points (2D or 3D)
These define where each new instance will be placed.

Faces or surfaces
These can control the orientation of the duplicated geometry.

The geometry created by Sketch Driven Pattern can be used not only in part modeling, but also as reference geometry in assemblies to create associative component patterns, similar to rectangular or circular patterns.

Workflow

The workflow depends on whether you want to copy features or solid bodies.

Patterning Features

Typical steps are:

1. Start the command:
   3D Model → Pattern → Sketch Driven
2. Select the operation mode: Features
3. Choose the features to duplicate.
4. Select the sketch that contains the points defining instance locations.
5. Define the base point of the pattern.
6. (Optional) Activate Variable Orientation and select faces or surfaces to control orientation.
7. (Optional) Select the bodies used in the operation.
8. (Optional) Change the geometry creation method.
9. Confirm the operation with OK or Apply.

Patterning Bodies

The workflow is similar:

1. Start the command:
   3D Model → Pattern → Sketch Driven
2. Select operation mode: Solids
3. Select the solid bodies to duplicate.
4. Select any work features that should also be duplicated.
5. Choose the sketch that defines the instance points.
6. Define the base point.
7. Select the copy mode for the solids
   (Join or New Solid).
8. (Optional) Activate Variable Orientation and select faces or surfaces.
9. (Optional) Adjust the geometry creation method.
10. Confirm the operation.

Important Things to Pay Attention To

Risk of Duplicate Geometry

If a Sketch Center Point is located exactly at the position of the base geometry, Inventor may create a second instance in the same place.

This duplication may not be visible in the model, but it can cause problems later with:

• Bill of Materials (BOM)
• Associative assembly patterns
• Content Center components

To avoid this issue, convert the center point into a regular Sketch Point (dot).

Correct Positioning

Inventor automatically recognizes the reference of an object at its geometric center.

If a base point is not defined manually, instances may be placed incorrectly or the geometry may not appear as expected.

For reliable results, always define a clear base point.

Controlling Orientation

By default, all instances keep the same orientation as the original geometry.

However, orientation can also be controlled using faces or surfaces.

Inventor compares:

• the direction of the face assigned to the instance
• the direction of the face assigned to the base geometry

Based on this comparison, Inventor calculates a transformation and rotates the instance relative to the original geometry.

This makes it possible to create patterns that follow curved or angled geometry.

When using this method, it is important to also define the base reference surface, so Inventor can correctly calculate the transformation.

Base Point Options

The base point cannot be a Sketch Center Point.

Possible base point references include:

• Sketch Point (simple dot)
• Work Point
• Vertex of existing geometry
• Characteristic geometry point (grip)

One Driving Sketch

All instance positions are controlled by one sketch containing Sketch center points.

Two approaches are possible.

2D Sketch

Used when all instances are placed on a single plane.

3D Sketch

Used when instances must be located in different planes or in space.

A 3D sketch can be created in several ways:

• Independent 3D geometry
• Geometry included from multiple 2D sketches
• A mix of both methods

Associative Patterns for Components

Sketch Driven Pattern can also help automate assembly modeling.

Geometry created in a part file using this pattern can be used as reference geometry in an assembly to create associative component patterns.

Possible references include:

• Solid bodies or features
• Surface bodies
• Work points

This method speeds up component insertion and ensures the assembly stays fully associative.

Multi-Body Modeling and Derived Parts

Associative assembly patterns can also be created using derived parts.

When a derived component is created from a multi-body part, Inventor can include:

• Solid bodies
• Sketches
• Surface bodies
• Work features

This allows the Sketch Driven Pattern to be recreated in the derived part using the same driving sketches or reference points.

Any modification in the original multi-body part will automatically update the derived part and the assembly.

Another workflow is to create the Sketch Driven Pattern directly in the multi-body part, insert that part into the assembly, and set it as a reference component.

This approach keeps the geometry and relationships available for positioning while excluding the part from:

• BOM calculations
• Weight calculations

Practical Advice

To avoid problems when using Sketch Driven Pattern:

• Always define a base point.
• Convert Sketch Center Point to Sketch Point if they coincide with the base geometry.
• When using surfaces to control orientation, also select the base surface.
• Place all instance control points in one sketch (2D or 3D).
• If the model does not update after changing references, run
  Manage → Update → Rebuild All.
• Keep all input geometry fully constrained and clean.

Example Applications

Welded Fence

Charles designs small steel structures. A client asked for a visualization of a fence before production. Because decorative elements required irregular spacing between posts, Sketch Driven Pattern helped quickly distribute the elements and prepare the design proposal.

3D Printed Accessory

Peter produces 3D printed board-game accessories. A particular game used modular board segments that connected like puzzle pieces. To stabilize the board, he designed connectors and locking features. Sketch Driven Pattern allowed him to duplicate these features at different positions and angles across the board.

Industrial Installation

Lucas designs industrial installations where many components—connectors, transitions, and handles—appear in multiple locations. Using Sketch Driven Pattern lets him automate placement while keeping the design fully parametric and easier to update.

CNC Machined Part

Michael manufactures complex CNC parts. For a custom strainer design, he needed to distribute multiple holes across a curved surface. By using Sketch Driven Pattern, he could parameterize the design and simplify the creation of the machining program.

Summary

Sketch Driven Pattern is a powerful modeling tool in Autodesk Inventor for creating layouts that are difficult or impossible with standard pattern commands.

It allows engineers to control both:

• Position of instances using Sketch Center Points
  
• Orientation using surfaces

The feature has been available since Inventor 2017, and improvements introduced in Inventor 2026 increased its reliability and geometric accuracy.

When used correctly, Sketch Driven Pattern can greatly speed up the modeling of complex parts and assemblies while keeping the design fully parametric.

• Author
• Recent Posts

Kacper Suchomski

Autodesk Expert Elite | CAD/CAM Consultant at Mech-Design Kacper Suchomski

Kacper Suchomski is an Autodesk Expert Elite & Mentor with over eight years of experience in CAD design and production implementation. As the founder of Mech-Design, he helps engineers and manufacturers turn innovative ideas into manufacturable, production-ready solutions.

Latest posts by Kacper Suchomski (see all)

• How Engineers Use Sketch Driven Pattern in Autodesk Inventor - 16 March 2026
• Intent-Driven Design in Autodesk Fusion: What Changed in 2026 - 8 February 2026