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How to Scale an Assembly in SOLIDWORKS

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When working with large assemblies in SOLIDWORKS, it is common to discover late in the project that the final product is either too large or too small. You might need a scaled version for a prototype, a scale model for a customer, a new envelope requirement, or to correct a units mistake (for example, a model created in millimetres that should have been in inches).

Ideally, the overall size of the assembly is estimated and agreed upon early in the design process. However, real projects are rarely perfect. This article explains what SOLIDWORKS can and cannot do when it comes to scaling and walks through practical workflows for scaling an entire assembly without completely breaking your design intent.

Top-Down vs Bottom-Up Design and Why Assemblies End Up Oversize

Generally, there are two main design approaches when working with large assemblies in SOLIDWORKS:

  • Top-down design: The overall assembly and key interfaces are defined first, often using layout sketches, skeleton parts, or in-context references. Individual parts are then created to fit within this framework.
  • Bottom-up design: Individual parts are designed first, then assembled using mates. This is very common when reusing existing parts or when many components are purchased items.

In a bottom-up workflow, it is easy to end up with an assembly that turns out larger or smaller than expected once everything is put together. At that point, it may be tempting to simply “scale the assembly” and be done with it. Unfortunately, SOLIDWORKS does not provide a direct scale command at the assembly level, so you need to use one of the available workarounds described below.

What the SOLIDWORKS Scale Feature Actually Does

SOLIDWORKS includes a Scale feature, but it is only available in part documents (solid or surface models), not in assemblies. You access it from the Features toolbar or from the menu via Insert > Features > Scale (or under Insert > Molds > Scale in some environments). The Scale feature scales the 3D geometry of the part, either uniformly or non-uniformly. It does not change the underlying sketch dimensions or reference geometry definitions; it only changes the resulting body geometry.

The key points about the Scale feature in SOLIDWORKS are:

  • It is available in part/surface documents, not in assembly documents.
  • It scales the geometry only; existing driving dimensions and sketches keep their original numerical values.
  • You can scale about the centroid, the part origin, or a coordinate system.
  • You can scale uniformly (same factor in all directions) or non-uniformly (different factors for X, Y, and Z).

Because the Scale feature does not update the dimension values, it is best thought of as a geometric transformation tool—useful for tasks such as preparing models for export, creating cavities, or resizing neutral/imported geometry—rather than a substitute for a fully parametric, dimension-driven size change.

Can You Scale an Assembly Directly in SOLIDWORKS?

In short, no: there is no native Scale feature that works directly on an assembly file. The Scale PropertyManager is only available when a part document is active, and community and support discussions consistently confirm that assemblies cannot be scaled directly using a built‑in command.

When you need to scale an assembly, you are left with two practical options:

  1. Scale each individual part and rebuild the assembly (recommended for production designs).
  2. Convert the assembly to a multi‑body part and scale that part (useful as a quick what‑if or for export/visualization).

The rest of this article focuses on these two methods and shows how to use the Scale feature carefully so that you do not unintentionally destroy your assembly structure.

Method 1 – Scale Individual Parts and Rebuild the Assembly (Recommended)

From a design‑intent and maintainability standpoint, the most robust way to “scale an assembly” is actually to scale the parts and let the assembly update through its mates and references. This takes more effort up front but keeps the model editable in the future.

When to Use This Method

Use part‑by‑part scaling when:

  • You care about keeping the assembly fully parametric and easy to edit later.
  • You may need different scaled versions of the same product (for example, 1:1, 1:2, 1:5).
  • You want to be able to change features or tolerances afterwards, not just the overall size.

Also consider which components should not be scaled. Standard fasteners, off‑the‑shelf purchased components, and items constrained by real‑world standards usually need to keep their original size. You may decide to scale only some custom parts and adjust the assembly around the unscaled ones.

Step-by-Step: Scaling a Part with the Scale Feature

For each part that should be resized:

  1. Open the part in its own window.
  2. Decide whether to use configurations.
    For many workflows it is best to create a new configuration (for example, Default, Scale_0_5, Scale_2_0) so that both the original and scaled versions coexist in a single file. SOLIDWORKS allows scale feature parameters (X, Y, Z factors) to be configuration‑specific, which fits this pattern well.
  3. Insert the Scale feature.
    Use Insert > Features > Scale (or Insert > Molds > Scale depending on your toolbar layout) to open the Scale PropertyManager.
  4. Choose what to scale.
    In a single‑body part, the only body is selected automatically. In a multi‑body part, you can select one or more bodies from the graphics area or the Solid Bodies folder.
  5. Set the “Scale about” reference.
    You can scale about:

    • Centroid – each body scales about its own center of mass.
    • Origin – the global part origin is used as the reference.
    • Coordinate system – any user‑defined coordinate system can be used as the base point.

    For single‑body parts, any of these can work, but for multi‑body parts (especially those derived from assemblies), using the Origin or a well‑chosen coordinate system usually preserves relative positioning better.

  6. Choose uniform or non‑uniform scaling.
    • Uniform scaling applies the same scale factor in all directions.
    • Non‑uniform scaling lets you enter independent scale factors for X, Y and Z.
  7. Enter the scale factor.
    • A factor > 1 enlarges the model (for example, 2.0 to double the size).
    • A factor < 1 reduces the model (for example, 0.5 for half size).
  8. Rebuild and save the part, then return to the assembly.
  9. Update the assembly configuration.
    If you used part configurations, set each component instance in the assembly to the correct configuration corresponding to the desired scale.

Remember that the Scale feature does not change your dimension values or sketches—only the resulting body geometry. If you want both the geometry and the driving dimensions to scale in a coordinated way (for example, for a fully parametric “family of sizes”), you may want to drive key dimensions using equations and global variables instead of relying solely on the Scale feature.

Method 2 – Save the Assembly as a Multi‑Body Part and Scale It (Quick Check)

When the priority is speed—for example, to quickly evaluate how a scaled version of the assembly fits within a larger system, or to create a scaled model for export—you can convert the assembly into a multi‑body part and apply a single Scale feature to that part. This is essentially the approach you described originally and is widely recommended as the fastest way to scale an entire assembly in SOLIDWORKS.

The trade‑off is that you lose mates and component structure in the scaled file, so future design edits are less convenient. For quick checks and one‑off deliverables, however, this method is very effective.

Option A – Save Assembly as Part (All Versions)

In all supported versions of SOLIDWORKS, you can do the following:

  1. Open the assembly that you want to scale.
  2. Use File > Save As, then change the file type to Part (*.sldprt).
    In the Save As options, choose how much detail to carry over (for example, All components, Exterior faces, or similar options depending on version). This creates a part file with multiple solid bodies, each corresponding to a component from the assembly.
  3. Open the new part. You will see a multi‑body part with an entry in the FeatureManager tree representing the imported assembly geometry.
  4. Apply the Scale feature to all bodies:
    1. Use Insert > Features > Scale.
    2. Select all solid bodies (from the graphics area or the Solid Bodies folder).
    3. Set Scale about = Origin (recommended for multi‑body parts coming from assemblies).
    4. Enable Uniform scaling and enter the desired factor.
  5. Click OK to apply the scale and save the part.

This approach gives you a single multi‑body part representing the scaled assembly. It is great for tasks like export to STEP/IGES/STL, collision checks, or sharing a simplified “dumb” representation with customers or suppliers without exposing all internal details.

Option B – Use “Make Multibody Part” (SOLIDWORKS 2024 and Newer)

Starting in SOLIDWORKS 2024, there is a new command specifically for converting assemblies to multibody parts: Tools > Make Multibody Part. This gives you more control over what gets transferred and allows you to maintain an optional link back to the original assembly so that updates propagate forward.

With an assembly open:

  1. Go to Tools > Make Multibody Part.
  2. In the PropertyManager, choose what to include (solid bodies, surfaces, axes, planes, coordinate systems, materials, etc.).
  3. Decide whether to break the link or keep it so that changes in the assembly update the multibody part.
  4. Click OK. The new multibody part opens in its own window, with a Make Multibody Part feature at the top of the tree.
  5. Apply the Scale feature to all solid bodies in the multibody part just as in Option A.

This method is particularly useful if you need a scaled representation that stays synchronized with an evolving assembly design, because you can regenerate the multibody part as the assembly changes.

Choosing the Right “Scale About” Option for Multi-Body Parts

When you scale a multi‑body part created from an assembly, the choice of “Scale about” reference is critical. It determines how the bodies move relative to each other during the scaling operation.

In the Scale PropertyManager, the most important input is:

  • Scale about – Centroid, Origin, or Coordinate system.

If you select the Origin, the entire model is scaled about the global part origin. If a user‑defined coordinate system exists, you can select it to scale around that reference instead—useful when you want the scaled assembly to stay aligned to a particular physical reference, such as a mounting interface or packaging coordinate system.

The option to scale the multi‑body part about the Centroid is usually best avoided when your multi‑body part comes from an assembly. The following image illustrates why.

When “Scale about: Centroid” is used on a multi‑body part, each body scales about its own centroid. Because the bodies do not share a common reference point, their relative positions can shift as they grow or shrink, effectively “pulling apart” the assembly. Since mates do not exist in the part environment, there is nothing to keep those bodies together in the same way they were in the original assembly. Scaling about the Origin (or a carefully placed coordinate system) keeps the bodies aligned and avoids this disruption.

Uniform vs Non-Uniform Scaling

After choosing the base point, the next critical choice in the Scale feature is whether to use Uniform scaling or Non‑uniform scaling.

Uniform Scaling (Most Common Case)

Uniform scaling is the simple case in which every linear dimension is multiplied by the same factor. This is what you typically want when you say “half‑scale model” or “double‑size version.” For example:

  • A uniform scale factor of 2.0 doubles all lengths; areas increase by a factor of 4, and volumes by a factor of 8.
  • A uniform scale factor of 0.5 halves all lengths; areas become one quarter, and volumes one eighth of the original.

In the Scale PropertyManager, this is done by leaving Uniform scaling checked and entering a single scale factor.

Non-Uniform Scaling (X, Y, Z Factors)

In rare situations, you may need to scale the model differently along each axis—for example, to create a visually stretched prototype or to compensate for anisotropic shrink in a specific manufacturing process.

To do this, clear the Uniform scaling checkbox and enter independent scale factors for X, Y, and Z. For instance, you could scale only in the Y direction by using scale factors such as:

  • X = 1.0
  • Y = 0.5
  • Z = 1.0

In the example referenced by the image below, the same multi‑body part has been scaled only in the Y direction with a scale factor of 0.5, effectively compressing the model along that axis while leaving X and Z unchanged.

Be cautious with non‑uniform scaling in engineering contexts: it distorts shapes and angles and usually invalidates any detailed tolerances, fits, or analysis results unless it is part of a very specific, well‑understood workflow.

Best Practices and Practical Recommendations

  • Prefer parametric resizing when possible.
    If you can, resize your design by changing key dimensions, equations, or configurations. Use the Scale feature primarily for imported geometry, legacy models that are difficult to edit, or special cases like cavity creation.
  • Use part‑by‑part scaling for production assemblies.
    Scaling each part and rebuilding the assembly is more work, but it preserves editability and allows you to keep certain components unscaled (fasteners, purchased items, standard hardware).
  • Use a multi‑body part for quick checks and exports.
    Converting an assembly to a multi‑body part and scaling it is fast and convenient for visualization, export (for example, to STL, STEP), or sharing simplified geometry. Just remember that this file is not a fully parametric assembly anymore.
  • Scale about a common reference (origin or coordinate system).
    When scaling multi‑body parts derived from assemblies, avoid scaling about each body’s centroid. Instead, scale about the origin or a deliberately placed coordinate system to keep bodies from drifting apart.
  • Use configurations to manage multiple scales.
    Store different scale factors in configurations when you need several variants (full‑size, half‑scale, etc.) in the same file. SOLIDWORKS supports configuration‑specific scale parameters, so you can manage different scales cleanly.
  • Be careful with analysis and mass properties.
    Scaling geometry changes volume and mass (if material density is defined). If you are running FEA or using mass properties, treat the scaled model as a different design and re‑evaluate loads, boundary conditions, and material definitions accordingly.

By understanding how the SOLIDWORKS Scale feature works and choosing the right workflow—either scaling individual parts or using a multi‑body part as an intermediate—you can resize assemblies in a controlled way while preserving as much of your design intent and future editability as possible.

 

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