If you are making basic models in SolidWorks then you may not have to use any reference geometry aside from the provided Default Planes (Top, Right, and Front), the Coordinate system, and the Origin. But as you proceed to make complex designs, you will realize that it becomes very difficult, if not impossible to do so with the default reference geometries. Reference geometries not only help a lot in the creation of your design but sometimes they make that design possible. If used properly, they can save a lot of time. In this article, we are going to tell you about all the reference geometries available in SolidWorks, what they are, what they are used for, and how you can use them.

Reference geometry includes Plane, Live Section Plane, Axis, Coordinate System, Point, Centre of Mass, Bounding Box, Grid, Ground Plane, and Mate Reference. Reference Geometries can be found under the Reference Geometry toolbar in the Features Tab. They can also be accessed via Insert -> Reference Geometry.

Plane:

Planes are used for sketching and for creating features such as Lofts, Sweeps and Revolves. Most of the time, planes are required in the Mirror command. You can use planes to create a Section View of a model or for a neutral plane in a Draft feature. They can be used as references for defining Coordinate Systems’ direction, and for establishing feature direction in Patterns, Extrudes, Wraps, Move Face, and a lot of other features. Also used as references for Mates in Assemblies.

You can use up to three references to create a plane. There are several combinations of entities that can be used to create a new plane. Some combinations include a single face or offset to a face/plane, a line/edge/axis and a point/vertex, a face/plane and a point/vertex, two faces/planes, and three points. You can also create a plane parallel to your screen. To let you know if your combinations are correct or not or if additional references are needed, a message will always be shown under the Message menu.

Planes that you create are automatically sized to either the geometry on which they are created or to the bounding box of the model geometry. You can move and change the plane’s size by clicking on it and dragging the handles.

Axis:

Axes are commonly used for Revolved features and Circular Patterns. Used for aligning and positing parts in an Assembly. Used in Move/Rotate Component for Move Along Entity and for facilitating various Mates. Axes are used in creating Planes and in creating Sketch geometry. Similar to planes, they can also be used as references for establishing feature direction in Extrudes, Drafts, Move Face, Patterns, and for defining Coordinate Systems’ direction.

Axis can be created using a line or an edge, or from the intersection of two planes, or using 2 points/vertices, from a Cylindrical/Conical face, or by using a point and a face/plane.

Tip: SolidWorks also makes Temporary Axes automatically for every cylindrical and conical face present in the model.

If the Temporary Axes are not visible go to the drop-down symbol present along with the View icon and select the View Temporary Axes button. If it’s still not showing make sure the View icon is not suppressed.

If any of the Reference Geometries (Planes, Axes, Coordinate Systems, Points, Live Section Planes, or Centre of Mass) that you created are not visible, check if they are selected in this View toolbar and make sure the View icon is not suppressed.

Live Section Plane: 

Live Section Planes allows you to dynamically section models using any plane. You can move, rotate, and resize the section plane while you work with your model. A triad is provided to move and rotate the Live Section Plane to section the model from different angles and positions. Right-click on the plane’s edges in the graphics area and select the Show Triad icon to access the triad. You can display multiple Live Section Planes at the same time. Unlike the Section View which sections the whole model irrespective of the size of the plane, the live section plane only sections the model according to the size of the plane. You can resize the plane by clicking on it and dragging its handles.

In the FeatureManager design tree, you will find the Live Section Planes folder, which stores all Live Section Planes. You can use features like Instant 3D at the same time while you are using the Live Section Plane making it a very useful tool for direct editing.

Coordinate System

You may have found yourself in a situation where you want to scale your part with respect to a point other than the default Origin. Or maybe you wanted to calculate the center of mass or moment of inertia with respect to another location other than Origin because you made the part at the wrong position or orientation. Or maybe you need this information relative to a mounting point.

When this is the case, new coordinate systems can be created and used to show this information. Coordinate systems are exceptionally useful for use with the Measure and Mass Properties tool.  These can also be made to help in the designing process or to facilitate assembly Mates.

Point

Used in creating Sketches, and Coordinate Systems. You can create several types of reference points to use as construction objects.

A point can be created as the center of a circle/arc, as the center of a face, from the intersection of 2 lines/curves/arcs, or by projecting a point on a plane.

You can also create multiple reference points that are a specified distance apart along edges, curves, or sketch segments.  Select the entity and create the reference points by clicking on the Along Curve Distance icon.

Centre of Mass

To determine the coordinates of the Center of Mass of the part, click on Mass Properties in the Evaluate tab of the Command Manager. There you will find a lot of information as well as the Center of Mass Coordinates. But sometimes you may need to use the Centre of Mass as a reference (say in a sketch or for a feature). That is why there is a Centre of Mass option available in Reference Geometry. The position of the Center Of Mass point updates automatically when the model’s center of mass changes.

You can create Measurement Sensors that reference the Centre of Mass point. You can measure distances and add reference dimensions between the Center Of Mass point and entities such as vertices, edges, and faces but you cannot create driving dimensions from it. However, you can create a Center of Mass Reference point (by right-clicking on the Centre of Mass feature present in the Feature Manager Tree), and use that point to define driving dimensions.

Bounding Box

The Bounding Box is the smallest box in which the body fits. Bounding Box can help you determine the length, width, and height of the stock required for the body. This helps you to know how much space is required for packaging or shipping the product. Bounding Box can be created for any type of solid, surface, or sheet metal body.

You can create a bounding box for a multibody or single body part. You can also create a bounding box for any cut list item in a cut list. The bounding box is represented by a 3D sketch and is based on the X-Y plane by default.

For parts, bounding box dimensions are available in the File > Properties > Configuration Properties tab. For cut lists, the overall dimensions of the bounding box appear in the Cut-List Properties dialog box. You can also use these dimensions in a Bill of Materials or other annotations.

Grid System

This feature creates multiple copies of your sketch and places them a specified distance apart. Distance between individual sketches can be customized under Grid Control. The grid system is useful when creating welded structures. Or you can use the Grid System tool to create a layout for large structures and assemblies.

• The original sketch that you created is replicated for each level in the structure.
• Reference planes are created for each level.
• Sketch points are added to all projected intersections of the grid lines and levels of the structure.
• A 3D sketch is created that acts as a support between each level in the structure.
• A surface is created that relates to the elevations of all grid lines.
• Balloons are added in the sketch to identify the grid items and help with their orientation.

Mate Reference

You may have noticed that when you bring an item (such as bolts, screws, nuts, gears, etc.) from the Solidworks Libray Toolbox, they snap to their places and the mates get applied automatically. You can also achieve this in your models and components with the help of Mate Reference.

Initialize the Mate Reference and under Primary Reference Entity:

• Select a face, edge, vertex, or plane for the Primary Reference Entity. The entity is used for potential mates when dragging a component into an assembly.
• Select a Mate Reference Type (such as concentric or tangent for a Circular face or coincident, tangent, or parallel for a face/plane) and a Mate Reference Alignment (aligned, anti-aligned, or closest) to define the default mate for the reference entity. In the case of Circular Edge, both concentric and coincident mates are applied whenever possible.

The same can be done for the Secondary Reference Entity and Tertiary Reference Entity if multiple reference mates are needed. In the FeatureManager design tree, the mate references will be added to the MateReferences Folder.

Now, whenever you drag that component on a face (either circular or a planar face) or edge if Reference Mates are defined, they will automatically be applied. If the alignment of a component needs to be reversed, press the Tab key one time on the keyboard.

Take a look at what happens when we bring our part in which we previously selected a circular edge in the Mate Reference closer to a cylindrical face. Since the alignment was wrong we pressed the Tab key once to reverse the direction. They get snapped together and if you click to place the part you will notice that a concentric and a coincident mate have been automatically applied.

Now that you know how to apply and use Mate References you will be able to save a lot of time by not having to repeatedly mate commonly used components together.

Ground Plane

When you insert a Published asset into the assembly, the asset’s ground face snaps to the assembly’s Ground Plane.

Ground Planes are only available in assemblies. You can define multiple ground planes in a single assembly but can have only one ground plane active at a time. In the FeatureManager design tree, all your Ground Planes are stored in the Ground Planes folder.

Ground Plane can be defined from Insert > Reference Geometry > Ground Plane. For assemblies that have an existing ground plane, right-click the Ground Planes folder in the FeatureManager design tree, and click Insert Ground Plane to add more Ground Planes.