Trimech-Main-Site-Group-Navigation Trimech-Main-Site-Group-Navigation Trimech-Main-Site-Group-Navigation Solid-Solutions-Group-Navigation Javelin-Group-Navigation Solid-Print-Group-Navigation 3DPRINTUK-Group-Navigation Trimech-Enterprise-Solutions-Group-Navigation Trimech-Enterprise-Solutions-Group-Navigation Trimech-Advanced-Manufacturing-Group-Navigation Trimech-Staffing-Solutions-Group-Navigation
With over 35 years of experience, the TriMech Group offers a comprehensive range of design, engineering, staffing and manufacturing solutions backed by experience and expertise that is unrivalled in the industry. The TriMech Group's solutions are delivered by the divisions and brands shown here, use the links above to visit the group's websites and learn more.

SOLIDWORKS Tips: How to Create Planes in SOLIDWORKS

Wednesday July 26, 2023 at 8:00am

By default, every SOLIDWORKS Part and Assembly file has a Top, Front, and Right plane, each centred on the origin.

As a designer, it is essential that you know how to create planes in SOLIDWORKS to enable you to model more complex geometry. Fortunately, the process is straightforward and intuitive.

So, let’s guide you through how to create new planes in SOLIDWORKS.


Each plane is effectively infinite in two directions, but has visible edges for viewing and selection.

Adding planes in SOLIDWORKS is achieved using the Plane wizard.

The Plane wizard can be accessed via Features > Reference Geometry > Plane on the command manager or via Insert > Reference Geometry > Plane from the drop-down menu.

Up to three references can be selected in order to define a new plane. These references are listed as First, Second, and Third within the Plane command.

Just as in a sketch, planes must be fully defined. The property manager must be showing Fully Defined in green at the top before you can accept the command and create the plane.

You might need to select up to three references to create the plane that you want, but usually only one or two selections are necessary – it is only when you have selected points or vertices that you will need all three references.


The quickest way to create planes in SOLIDWORKS is to select a vertex of a plane, hold CTRL and drag the corner into the rough position.

Then specify any references and distances.

Which Plane References Should I Use?

Let’s explore some of the reference variations we can use when creating a new plane.


Whether we select a flat face or an existing plane, we get a preview of a new plane being created parallel to it, with a numerical offset that we can vary.

The direction of which can be reversed by ticking the Flip Offset option.

Be sure to select both references before modifying the offset value.


Here we have selected the left face and the vertical edge on the left corner – but no settings in the Primary reference plane were modified before selecting the secondary reference.

You can see that the system is automatically showing the new plane as perpendicular to the face and coincident to the straight edge.


We could then activate the angle option relative to the face, and then effectively rotate the plane about the straight edge.

This maintains a logical order for selecting references.


It’s important to note that there are many combinations of selections that are valid, but each combination will affect the design intent of your model.

For instance, you can have a plane parallel to a face and have the offset specified by selecting a point or vertex on the model geometry.

If the earlier geometry is edited, then the plane will update its position.


If you select a straight edge, line or axis, and a vertex you will get something like this.

If you pick three vertices or sketch points.

If you pick any two planes or flat faces, the system will give you a new plane halfway between the two.


Choosing an existing plane or flat face and a cylindrical face will default to offering you a new plane that is perpendicular to the flat face or plane, and tangent to the cylindrical face.

However, you could choose the angle option and then rotate the new plane around the cylindrical face.

This is great if you are making a keyway into the side of a shaft. Create a sketch on the plane and make an extruded cut into the shaft to make the recess for the key.

You can then edit the timing of the cam or gear by editing the angle of the plane.


If you want to make a sweep feature, you can draw the path sketch and then create a plane on the end of it using the line and the endpoint.

Create your profile sketch on that plane.


This option is very rarely used, but you should know that it is at least possible… Here we can select a single point or vertex and using the parallel to screen option.

It’s helpful, but purely depends on the viewing angle you are in at that moment in time. So, accurate? Hmm.


You bet! You can also make planes inside an assembly in a similar way via Reference Geometry > Plane.

But do be aware that if you make an assembly-level plane using any of the components as references, then that plane can only update after those components (and their mates) have been rebuilt.

This could cause your system to run slowly, depending on what you have selected.

Looking for More Tips?

Sign up to our CPD-accredited training courses.

It doesn’t matter whether you’re a complete beginner or are intimately familiar with CAD, our friendly and expert trainers are ready to help you get the most out of SOLIDWORKS, either online or in a classroom local to you.

We also have a load of free SOLIDWORKS tutorials across our site, or you can check out our YouTube channel for more tips and tricks.

Don’t forget, with a SOLIDWORKS subscription, you can contact our expert Technical Support team to help you out with new commands and modelling tips.

Call us on 01926 333 777 or drop an email to and one of our certified SOLIDWORKS Engineers will be in contact.

Related Blog Posts

3 Easy Ways to Make Your Renders More Realistic wi
Learn how to add realism quickly in SOLIDWORKS Visualize with these 3 top tips!
Calculating the Trajectory of a Cricket Ball with
Can SOLIDWORKS Motion help to improve your bowling accuracy?
The Best Way to Work Efficiently with Windows File
Discover how to use Enterprise Item Numbers and auto-naming to enhance your workflow.

 Solid Solutions | Trimech Group