Overlooked But Useful SOLIDWORKS Tool: Mirror

Cut down modeling time and increase efficiency using the Mirror command.

In this tutorial, we will be exploring how to use the Mirror tool, which allows users to copy sketches, features and bodies across a sketched line or plane.

Mirror Feature icon, which is found in the features toolbar.

Of all the many tools available in SOLIDWORKS, the Mirror tool is one of my absolute favorites. I would be hard pressed to find another tool that’s as powerful and time-saving as this one is. If the model you are working on is symmetrical in nature, mirroring sketches and features means that you only need to do half the work. 

Let’s look at a few situations in which the Mirror tool can be used.

The most basic way to use the Mirror tool is within a sketch. Let’s say we need to create a simple part with a square bolt pattern, like this:

A simple part made simpler with the Mirror sketch tool.

Starting with the base part, let’s make a sketch for the bolt pattern. Without the Mirror tool, we would have to make each of the four circles and fully define them. But, with the Mirror tool, we only have to make and define one circle. 

In the sketch, let’s create the circle on the top left and fully define it. Next, we need some lines to act as mirror tools. Because our part and therefore the holes, are symmetric, we need to make sure that these lines are exactly in the middle of the face. Let’s make two lines, one vertical and one horizontal, and make sure they are construction lines. Our sketch should look like this:

The first circle acts as a seed for the Mirror tool.

We are now ready to use the Mirror Entities tool. This can be found in the Sketch toolbar, or by clicking Tools > Sketch > Mirror. Once we activate the tool, we see the Mirror PropertyManager. There are only three parameters here: Entities to Mirror, Copy, and Mirror About. Select the defined circle in the Entities to Mirror field and the vertical construction line in the Mirror About field. Leave the Copy option selected; otherwise, our original circle will disappear. 

The Mirror sketch tool FeatureManager.

Once all the parameters are filled, we should see a preview of the mirrored circle in our sketch. Press the green checkmark and exit the tool. Now, we need two more holes on the bottom half of our sketch. Open the Mirror Entities tool once more. 

Now, let’s select our original circle as well as the mirrored circle on the right-hand side for the Entities to Mirror and the horizontal construction line in the Mirror About field. 

The original circle, as well as the newly mirrored instance, are now the seeds.

We now should see a preview of the two circles on the bottom half of the sketch. Press the green checkmark again and we have our four circles, which are ready to be cut as holes.

Four fully defined circles, which are ready for a Cut Extrude.

Now, I know what you may be thinking. Did we really save that much time? For a simple sketch like this, it may have been quicker to simply create and define the circles without the Mirror tool. And although that may be true for this instance, this same principle works for far more complicated sketches as well. Also, using the Mirror tool future-proofs the sketch.

Let’s say that we need to change the dimensions of the sketch. Instead of them being dimensioned one inch from the edges, now we need them to be 1.5 inches away. If we had made the circles one by one instead of with the Mirror tool, we would have to change that dimension on each of the circles. But if the sketch entities are mirrored, the mirrored parts will follow any dimensional changes made to the original entity. So, the three mirrored circles will also now be 1.5 inches away from the edges. 

Changing dimensions of the seed circle also changes the dimensions of the mirrored ones.

Features, such as a Boss or Cut Extrude, can also be mirrored. Let’s look at another way to create this part. Instead of mirroring the circles in the sketch, we will make the hole with only the first circle, like so:

One hole is cut as its own feature.

Now we have a Cut Extrude feature in the design tree of the single hole. We can now use the same mirroring technique we used before, but on the feature level. For this, we will be using planes instead of construction lines as our mirror tools. Because the part is symmetrical, we will use the Front Plane and the Right Plane as these tools. If you are working with a more complicated part, however, you will need to create new planes using the Reference Geometry tool.

The Front Plane and Right Plane are our Mirror planes.

Open the Mirror feature, which is found in the feature toolbar or by clicking Insert > Features > Mirror. Outside of a sketch, the PropertyManager looks a bit different.

The PropertyManager on the Feature level.

Let’s fill out the parameters, just as we did before. Select the Right Plane for the Mirror Face/Plane and the Cut-Extrude1 feature in the Features to Mirror tab. We should see the preview just as we did before. Press the green checkmark and now we have a Mirror feature in the design tree.

The seed feature mirrored about the right plane.

We can now repeat this process for the bottom holes, just as we did with the previous example. Again, with this part, this may not be the best way to do this. But it shows how to use the Mirror feature, which has more of a role in more complicated parts. 

The Mirror feature can also be used to mirror different bodies across a face or plane. Obviously, this requires a multibody part, so I would encourage anyone unfamiliar with those to learn about them outside of this tutorial.

Say we want to mirror this cube about the right plane, the one that is visible in this picture:

A body to mirror about the right plane.

Let’s open the Mirror feature one last time and select the Right Plane as the Mirror Face/Plane. Now, we will click the dropdown arrow and expand the Bodies to Mirror tab. Simply select the cube in the graphics area. Make sure the Merge Solids box is unchecked, as these two bodies will not touch each other. Check the preview and press the green arrow.

The Mirror tool will also mirror bodies about planes.

We now have two cubes and a multibody part.

A multibody part made with the Mirror feature.

These were three very simple examples of when you can use the Mirror tool. However, I would encourage every user to explore the other capabilities of this tool, as there are many that weren’t covered in this tutorial.