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How to Scale a Part in SolidWorks?

There are times when we may need to apply a scale to a part. It can either be done to increase or decrease the size of the model. In SolidWorks, scaling is done with help of the Scale feature. You can apply the scale at any point in your workflow but be advised that if you want to change the scale in the future, you may find yourself in the need to rebuild most of the sketches and features created after scaling has been done. But since it doesn’t affect any of the features present in the Feature Tree above the Scale Feature, we recommend using the Scale feature at the very end after you have done completing your part. Scaling can also be done using the Design Table. But, we will leave that method for another time.

Tip: Scaling an assembly directly is not possible as of yet in Solidworks. You can save your assembly as a part file and then apply the scale to it.

1. Go to Insert -> Features -> Scale or select the Scale tool present in the Features Tab.

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2. Under Scale Parameters, Select all the combinations of solid or surface bodies either from the graphics area or from the Solid Bodies/ Surface Bodies folder present in the Feature Tree. In Scale about, there are 3 options available:

  • Centroid: The scaling is done according to the center of mass of your solid body/surface.
  • Origin: The scaling will be done according to the origin point of the part file. (Recommended, read on to know why.)
  • Coordinate System: You can select a different coordinate system that you have previously defined to scale your part along.

3. Select Origin and then enter the Scale Value.

A scale value of greater than 1 increases the size and less than 1 decreases the size. The Scale value of 1 does not change the geometry.

3. Click Ok and your part should now be scaled. A Scale feature will appear in the Feature Tree.

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The Scale feature scales only the geometry of the model. It does not scale dimensions, sketches, or reference geometry. To temporarily restore the model to its unscaled size, you can rollback (recommended) or suppress the Scale feature.

In Scale About, it is highly recommended to either select the Origin or Coordinate system (if you have an additional Coordinate system) when scaling multiple bodies. Selecting Centroid may have adverse effects if there are multiple bodies selected for scaling and can result in misalignment of the part. Take a look at what happens when Centroid is used instead of Origin in the above example.

You can see that the model is scaled but the wheels went into each other. It’s because SolidWorks scales each and every Body (either solid or surface) individually based on their individual centroids, hence causing this mess.

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Non-Unifrom Scaling

In rare cases, you may need to scale the body differently along every axis. For that, SolidWorks got you covered with its Uniform Scaling Option.

Uncheck the Uniform Scaling option and enter scale values for all the axes individually. Look at the end result when a scaling value of 3 for the X-axis, 0.5 for the Y-axis, and 1 for the Z-axis is selected.