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Onshape is built from the ground up to enable efficient design processes. This section walks you through getting set up in Onshape for the first time, then presents the basic steps to modeling. There are some settings you can make right away to make your modeling more efficient.

Set it and forget it account settingsCopy link

You can set preferences in your Onshape account to mimic the mouse settings of another CAD system. Why not start with a mouse configuration that is already second nature to you? The preferences you set become immediately available in your Onshape account regardless of what device or browser on which you access Onshape.

Example of editting preferences

  1. After signing in to your Onshape account, click the user menu in the top right corner of the window to open the User menu.

    Top Right Corner of window with User Menu circled in orange

  2. Click My account.
  3. On the next page, select Preferences in the left panel.
  4. Select your preferred settings, as follows.
  5. Each setting has its own Save button. If you do not click Save for each change made, the change is not registered.

  6. Units - Select your preferred units. Keep in mind that this setting will be the default for all numeric fields in all of the documents you create. You can override these settings in any numeric field simply by typing the units in the field. (The units will be recalculated and then displayed using your default units.)
  7. Click Save units.
  8. View manipulation - Select the CAD system whose mouse settings you are most comfortable with. (If you opt to keep Onshape's default settings, see Setting Preferences to learn about Onshape's mouse settings.)
  9. Click Save view manipulation settings.

For more information

These are the most relevant settings for your account right now, but for more information on additional settings, see Managing Accounts.

Create a document to hold all your design dataCopy link

Think of Onshape documents as multi-data containers. Not only are you able to sketch, create parts, assemble parts, and create drawings all in one document, but you are also able to store non-CAD data in any document as well: images, non-translated CAD data, PDFs and more. Just about any type of file you want to keep track of can be imported into a document.

Creating a Document

  1. The Onshape landing page (where you find yourself when you sign in) is called the Documents page because it displays a table listing all of the Onshape documents you have access to.

    To access this page from anywhere else in the system, click the Onshape logo in the top left corner of the window (or your company logo if you are part of an enterprise account).

  2. Click Create.
  3. Select Document from the menu.
  4. Give the document a name (in the dialog that opens).
  5. Click OK to create and open the document.

Documents, by default, contain two tabs when created: Part Studio 1 and Assembly 1. Tabs are Onshape's way of allowing you to store more than one type of data together in one place. Look towards the bottom of the window to see the name of the tab. Click a tab to activate it. Each data type is stored in a specific tab type.

Begin part design with a sketchCopy link

A Part Studio is used to define parts and has a Feature list (parametric history) that, when regenerated, produces solid bodies called parts in Onshape.

Part Studio tabs are where you begin creating parts to be later used in assemblies. All parts begin as sketches, using sketch tools, and then, in the same Part Studio, you use feature tools to create solid bodies (called parts) from the sketches. You can create as many Part Studios in a document as you wish, and create as many parts in a Part Studio as you wish. Keep in mind that it's best to limit parts in a Part Studio to only those that are geometrically relevant to each other. For the best performance, parts not geometrically related to each other should be in their own separate Part Studios. So you'll have multiple parts in a given Part Studio only when those parts are geometrically related to each other.

This is similar to multi-body part modeling in other CAD systems, but is much more powerful. One Onshape Feature list has the ability to drive the shape of multiple, actual parts. Each part is able to be instanced multiple times in assemblies and each instance is able to move independently in the assembly.

In a Part Studio, there are two tool sets: Sketch Tools and Feature Tools.

Use Sketch tools to create sketches, the foundation of parts. Use Feature tools to create parts from the sketches. Each feature is recorded in the parametric history that is the Feature list.

Parts created in Onshape always begin with a sketch. The first tool on the toolbar when you create or open a document is Sketch (next to the Undo/Redo icons).

Creating a Sketch

To create a solid (versus a surface) you need a sketch with closed regions. (Onshape automatically shades all closed regions of a sketch.)

  1. Click Sketch.

    A sketch dialog opens.

    Sketch dialog

    Blue highlighted fields require selection in the graphics area

  2. First, select a plane to sketch on (top, front, right).

    You can select the name of the plane in the Features list or the plane in the graphics area.

    Press the N key to orient the sketch plane to normal (if desired).

  3. Click a sketch tool in the toolbar; hover on a tool to see a name and tooltip.
    1. For demonstration purposes, select Rectangle Rectangle Button. Click it in the toolbar or press the shortcut key (G) to toggle the tool on, and press it again to toggle the tool off.
    2. Click in the white space (the graphics area) to set one corner of the rectangle, and click again to set the opposite corner of the rectangle.
    3. Onshape automatically displays dimension text. The dimension text with the box around it is the active one: type a dimension and press Enter (you can always change it). The other dimension becomes active. Type another dimension and press Enter. Note that this must be done with the sketch tool still active. When you select another tool or toggle this tool off (by clicking the tool icon again or pressing the Escape key) the tool is deselected and the dimension fields are inactive. Simply double-click a dimension to activate it again.

      Dimensions can also be deleted; click once on the dimension and press the Delete key. Note that dimensions are only visible when the sketch dialog is open.

  4. Click the checkmark Accept checkmark icon in the corner of the dialog to accept (save) the sketch and close the dialog.

Notice the sketch is listed in the Features list on the left side of the window; by default the name is 'Sketch 1'.

You can rename everything you create in Onshape: in an open dialog, click the name and a pencil appears to the right. Click the pencil to edit the field. Otherwise, you can right-click on the sketch (or feature) in the Features list and select Rename from the context menu that appears. Specify a new name and and press Enter.

Sketch context menu

For more information

For more detailed information about sketching and tools, see Sketch Basics.

You can also take a self-paced learning course on sketching here: Starting a Sketch.

Create solid partsCopy link

Parts (solid bodies) are created by selecting a sketch region (closed curves indicated by shading). By contrast, surfaces are created by selecting a curve. In Part Studios, you can create more than one part at a time.

Extruding a surface

To create a part:

  1. Select the Extrude tool Extrude icon in the toolbar.
  2. At the top of the open dialog, select Solid.
  3. Select the shaded region of the rectangle.
  4. Accept the defaults for the remaining fields in the dialog.
  5. Click the checkmark Accept checkmark icon to accept the actions and close the dialog. (To dismiss the dialog without accepting the actions, click Red X.)

To create more than one part, use an additional Extrude feature, select Solid, and then New in the dialog box:

Example of multiple Extrude

Notice the part listed in the Parts list at the bottom of the Feature list on the left: Part 1. Onshape uses cross-highlighting to help you locate features and sketches involved in a part. Try this: Click the part in the graphics area and see what becomes highlighted in the Feature and Parts lists:

Selection of Graphics

Selecting a face of the part in the graphics area causes the Extrude feature and the Part name to be highlighted in the Features and Parts lists, respectively

Now try selecting something in the Feature or Parts list and notice what else is highlighted:

Selection of Feature/Part

Selecting the sketch name in the Features lists causes the sketch to be highlighted in the graphics area

Each sketch and feature created are stored parametrically in the Feature list on the left side of the window. You can go back and edit any feature or sketch listed in the feature list.


  • Use the 's' key to display your shortcut feature toolbar (with the sketch dialog closed). (Remember you can customize this toolbar through your account settings).
  • Use Shift+E to open the Extrude dialog.
  • Click Help menu icon and select Keyboard shortcuts to access the list of all keyboard shortcuts within Onshape.

For more information

For detailed information about using Onshape's Feature tools to create parts, see Feature Basics.

You can also take a self-paced learning course on creating parts here: Starting a Part.

Start part design by importing a partCopy link

You may have a part or assembly from another system that you want to import into Onshape. Onshape allows the import of files from many systems, but note that when imported, models lose their parametric history. However, Onshape supplies powerful direct editing tools so you can modify parts post-import. You can also use in-context modeling to use the imported model as a reference for the creation of additional parts.

To learn about all your options for importing files from another CAD system, see Importing Files.

Once you have imported your design, open the document or Part Studio with the model in it and begin using Onshape's direct editing tools to modify it:

Modifying a Fillet

For more information

For more detailed information on importing, see Importing Files. For information about in-context modeling, see Modeling In-Context.

You can also take a self-paced learning course on importing parts here: Importing a Part.

Onshape provides functionality for assembling parts in Assembly tabs and creating drawings in Drawings tabs.

Assemble partsCopy link

An Onshape Assembly is a tab type that is used to define the structure and behavior of an assembly. Each Assembly has its own Feature list that contains Instances (of parts and sub-assemblies), Mates, and Mate connectors.

An Assembly contains instances. An instance is a reference to either a part defined in a Part Studio, or to a sub-assembly defined in another Assembly. Instead of creating and inserting commonly used parts, like nuts and bolts, you can instance desired standard content and either replicate it in the assembly, or create patterns using the one instance. This keeps the Assembly from getting cluttered and bogged down by too many unnecessary parts.

Mates are used to position instances and to define how they move.

It's important to understand how Onshape Mates differ from mates in other CAD systems. In older CAD systems, mates are low-level assembly constraints, for example, making two planar faces coincident. As a result, positioning two instances usually requires two or three mates.

In Onshape, mates are high-level entities. There is only one Onshape mate between any two part instances, and the movement (degrees of freedom) between those two instances is embedded in the Mate. For example, a single Mate in Onshape can define a pin slot relationship and may also include movement limits as well.

Create drawings with a bill of materialsCopy link

You create drawings directly from a part or Part Studio, or even Assembly in Onshape. Simply select the entity (part name in a Part Studio or an Assembly or Part Studio tab) right-click and select Create drawing. You have the opportunity to select a drawing template, and then the drawing is created within a new Drawing tab in your document. For more information on drawings, see Drawing Basics.

To insert a bill of materials, click the Bill of materials icon in the toolbar Insert BOM icon. For more information on inserting a bill of materials, see Insert BOM.

Organizing dataCopy link

It is important to remember that Onshape documents are not files; they are containers that can include parts, assemblies, drawings, imported data and basically anything you need for your project. Although you are able to (and sometimes should) have one part per document, we recommend that you keep all project-related data in one document. Anything you plan on reusing across multiple projects should be in its own document. You are able to link from one document to another in order to cross-use data from one document in another document.

For more information on how best to organize your data within Onshape, check out our Onshape Fundamentals: Data Management (opens in new tab) learning pathway.