How to Insert and Trace an Image in SOLIDWORKS

Contents

Use Sketch Picture when you want to place a photo, scan, logo, or drawing on a SOLIDWORKS sketch plane and trace it into editable sketch geometry. The reliable workflow is to insert the image in a part sketch, scale the picture from a known dimension, trace the important contours, and then fully define the resulting sketch.

A picture can help reproduce an outline, create a concept model, or reconstruct simple geometry when no CAD file is available. It does not make a photograph dimensionally accurate by itself. Perspective, lens distortion, and an unknown scale can all introduce error, so use a straight-on image and verify the final dimensions against a drawing or physical measurement.

What You Need Before Tracing

A part document with an open 2D sketch.
A clear still image such as JPG, PNG, BMP, GIF, TIFF, WMF, or PSD.
At least one known dimension visible in the image or measured from the real object.
A suitable sketch plane that matches the view shown by the picture.

Choose a front, top, or side image taken as square to the object as possible. A perspective photograph is useful for visual reference but poor for precise tracing. If the existing default planes do not match the required orientation, first learn how to create a reference plane in SOLIDWORKS.

SOLIDWORKS documents Sketch Picture for part sketches. Pictures cannot be inserted into an assembly sketch through the same workflow, and Sketch Picture options are unavailable for sketches created in the context of an assembly. Create or edit the traced profile in the part instead.

How to Insert a Sketch Picture

1. Start a Sketch

Open a part, select the plane or planar face that matches the image view, and begin a sketch. Orient the view normal to the sketch plane so the image is not visually skewed.

2. Open Sketch Picture

With the sketch active, click Sketch Picture on the Sketch toolbar or choose Tools > Sketch Tools > Sketch Picture. Browse to the image file and click Open.

This is different from inserting an OLE object with Insert > Object. An OLE object can display an external file, but it is not the recommended underlay for this tracing workflow. Clipboard paste behavior can also vary by source application, so importing the file through Sketch Picture is more predictable.

3. Position and Rotate the Picture

Drag the picture to place it near the sketch origin. Use the handles or the Sketch Picture PropertyManager to adjust position, width, height, and rotation. Keep the aspect ratio locked unless you know that the source image itself is stretched. Changing width and height independently can distort circles, angles, and hole spacing.

Reference image prepared for insertion and tracing in SOLIDWORKS — Figure 1 – Reference image prepared for tracing.

Scale the Picture Before Tracing

When a Sketch Picture is inserted, SOLIDWORKS displays a scale tool over the image. Use it before creating geometry:

Move the left endpoint of the scale tool to one end of a known distance in the image.
Move the right endpoint to the other end of that known distance.
Enter the real measurement in the Modify dimension box.
Confirm the value and check another known dimension if one is available.

The image and scale tool resize together. Scale from the longest reliable dimension you can identify because a small placement error has a larger percentage effect on a short reference. After scaling, disable the scale tool if it obstructs the tracing area.

Do not assume the entire photograph is accurate because one length matches. An angled camera can make one region appear larger than another. For production work, treat the image as an underlay and apply authoritative dimensions to the sketch.

How to Trace the Image Manually

1. Trace Functional Geometry First

Begin with geometry that controls fit and function: straight edges, centerlines, hole centers, circles, symmetry, and major radii. Use lines and arcs for manufactured geometry rather than approximating every pixel with splines. Reserve splines for genuinely freeform outlines.

Keep the first pass simple. Too many short entities make the sketch hard to constrain and edit. If the outline is symmetric, trace one side and mirror it instead of tracing both sides independently.

SOLIDWORKS sketch picture with outline and hole locations traced — Figure 2 – Outline and important hole locations traced over the picture.

2. Add Relations

Add horizontal, vertical, tangent, concentric, equal, midpoint, and symmetry relations where they describe the real design intent. Relations make the traced geometry stable and reduce the number of dimensions needed.

For a freeform contour, add only the spline controls required to reproduce the shape. The guide to fully defining a spline in SOLIDWORKS explains how to control a spline without adding unnecessary points.

3. Dimension the Sketch

Add dimensions from real measurements, a supplier drawing, or another authoritative source. Do not round unknown hole locations until the sketch looks plausible and then treat those values as exact. A traced photograph is not a replacement for inspection or a controlled drawing.

If you need to revise existing values, follow the workflow for changing dimensions in SOLIDWORKS parts. Continue until the important geometry is fully defined and the remaining degrees of freedom are intentional.

Traced SOLIDWORKS sketch geometry prepared for scaling and dimensioning — Figure 3 – Traced sketch geometry prepared for final constraints and dimensions.

4. Hide the Picture and Inspect the Profile

Hide or move the picture temporarily and inspect the sketch by itself. Look for gaps, duplicate entities, tiny segments, unintended overlaps, and contours that do not close. Use repair tools where necessary before creating a feature.

Once the profile is clean, create the required feature. If the traced outline represents an opening or engraved area, see how to create an extruded cut in SOLIDWORKS.

Finished SOLIDWORKS model created from traced sketch geometry — Figure 4 – Finished model created from the traced and dimensioned sketch.

Using the Autotrace Add-In

Autotrace converts selected raster areas into sketch geometry. Enable it through Tools > Add-Ins, then select Autotrace. Insert the image with Sketch Picture and open the second page of the Sketch Picture PropertyManager.

Select a rectangular, polygonal, freehand, or color-based area.
Click Begin Trace.
Adjust brightness, contrast, color tolerance, and recognition tolerance.
Preview the traced geometry and click Apply.
Exit the Sketch Picture PropertyManager to create editable SOLIDWORKS sketch geometry.

Autotrace works best with high-resolution, high-contrast line art and uniform colors. Official guidance recommends at least 300 dpi. It is less effective on photographs with shadows, reflections, textured backgrounds, or soft edges. Even a successful automatic trace normally needs simplification, relations, and dimensions afterward.

Common Problems

Sketch Picture Is Unavailable

Confirm that a sketch is open in a part document. The command is not available for an assembly-context sketch. If you are working from an assembly, open or edit the component part and create the sketch there.

The Picture Is Distorted

Keep the aspect ratio locked and start from an image taken perpendicular to the object. If circles in the real part appear elliptical in the photo, the camera angle or lens has distorted the reference. Find a better image rather than forcing the sketch to match it.

The Traced Size Is Wrong

Return to the Sketch Picture PropertyManager and scale the image from a known length before tracing. If geometry has already been created, you can scale the sketch in SOLIDWORKS as a controlled correction, but you must review dimensions, relations, and external references afterward.

Autotrace Creates Too Many Segments

Crop the source image, increase contrast, isolate one region, and trace only the functional boundary. Manual lines, arcs, and circles are often cleaner for mechanical parts than a dense automatic outline.

The Image Does Not Load

Verify that the file opens normally outside SOLIDWORKS and convert it to a standard PNG or JPG if necessary. Animated formats are not supported. Very large TIFF files are also subject to a 4096 by 4096 resolution limit in Sketch Picture.