SOLIDWORKS Tips: How to Create Planes in SOLIDWORKS

HOW TO ADD 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.

SHORTCUT FOR CREATING PLANES IN SOLIDWORKS

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.

OFFSET PLANES

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.

PERPENDICULAR PLANES

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.

ANGLED PLANES

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.

PARALLEL PLANES

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.

SELECTING EDGES, VERTICES & OTHER PLANES

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.

TANGENTIAL PLANES

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.

ENDPOINT PLANES

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.

CREATE A PLANE PARALLEL TO THE SCREEN

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.

CAN YOU CREATE PLANES IN AN ASSEMBLY?

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?

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 support@solidsolutions.ie and one of our certified SOLIDWORKS Engineers will be in contact.