Creating a Drawing

From the Parts list in a Part Studio or Assembly:

Right click on a part, curve, or surface. Select Create drawing of <part, curve, or surface name>.

The drawing will populate it's name based on the existing part, curve, or surface name. You can edit the name of the drawing by clicking on the existing name (outlined in red below) at the top of the Create drawing dialog and typing your preferred name:

Click Suggested views at the bottom of the dialog and then click OK. Four views of the part are inserted into the drawing:

Your template will have centermark extensions turned on by default. To delete a centermark, click to select and press the Delete key. See centermarks for more information on centermark editing options.

From the Parts list in a Part Studio or Assembly:

1. Right click on a part. Select Create drawing of <part>.

   

2. The drawing will populate it's name based on the existing part, curve, or surface name. You can edit the name of the drawing by clicking on the existing name (shown highlighted below) at the top of the Create drawing dialog and typing your preferred name:

   

3. Click Suggested views at the bottom of the dialog and then click OK.

   

• Suggested views - Automates the placement of up to 6 orthographic views: front, top, left, back, bottom, right. If there is MBD data present on the front top and left planes. these views are automatically placed in the drawing sheet and the annotations are displayed in the view. If there is MBD data present in the part, but not in the suggested views inserted into the drawing, they are displayed in the MBD Status panel's Datums and Characteristics tables.

  

• No views - Opens an empty drawing sheet, where the user can select which views to insert. Once users insert a view, If MBD data is present on the view plane being inserted, this data is displayed in the inserted drawing view. Any missing data is displayed in the MBD status panel's Datums and Characteristics tables automatically.

  Your template will have centermark extensions turned on by default. To delete a centermark, click to select and press the Delete key. See centermarks for more information on centermark editing options.

Notes

• Default tolerances are automatically shown on dimensions, with explicit tolerances highlighted; changes in default tolerances are passed down to the drawing when a drawing is updated. See Default Tolerances Library for more information.

• When generating suggested views, top, right, and front views are prioritized. This is based both on which part planes contain the MBD data and the plane where the annotation is located.

  If using first angle projection, the order adapts to the relevant set of views, but the bias remains toward these primary orientations.

• All requirements and tolerances are visible and managed through the MBD Inspection table, streamlining review and documentation.

• Dimensions on hidden lines and section views are automatically shown when those views are added, which aids in the completeness of documentation.

• MBD data units are converted to the drawing units when data populates the drawing views. This includes welds, surface finishes, and geometric tolerances. This ensures consistency across metric and imperial drawings.
• Onshape automatically prevents duplicate annotations when part views are inserted. The user can add reference annotations manually in the drawing after insertion, and as required.

  Duplicate prevention is based on a combination of top/right/front, parent views over children, and view insertion order for manual view insertion cases.

• Composite parts are supported. This ensures MBD data flows correctly into drawings for all part types.

See MBD status for additional information on viewing and using MBD references (annotations and dimensions) in the drawing.

From the Create tab menu:

Click on the plus sign icon , then select Create Drawing:

The drawing will populate it's name based on the existing part, curve, or surface name. You can edit the name of the drawing by clicking on the existing name (shown highlighted below) at the top of the Create drawing dialog and typing your preferred name:

Click OK and the drawing is create without any views (empty).

Import an existing drawing file in .DWG or .DXF format. You are able to import from the Documents page and from within a document.

When importing from the Documents page, a new document is created:

1. Click the Create button in the top left corner of the page:

   Create

2. From the dropdown menu, click Import files...

1. Select the .DWG or .DXF file.
2. Select an owner for the document (if available).
3. Note the new document listed on the Documents page. (The document name is the same as the file name.)

When importing from within a document:

1. Click , then Import.

   

2. Select the .DWG or .DXF file.
3. Note the new tab in your document, with the same name as the file you imported.

A template must be specified at the creation of the drawing, and determines the drawing's starting system variable values, sheet size, border entities, units, standards and other properties.

Onshape owns and provides publicly available templates with names like Onshape ANSI Drawings Templates, Onshape ISO Drawing Templates, and so on. To view the Onshape templates, select the Onshape filter.

You can create your own custom templates. You can also specify whether to create four standard views or begin with no views. To change the background color of a drawing, access the setting under Preferences.

To narrow your search for the desired template, you can use:

• Filters - On the left of the dialog, select a filter (which are similar to the filters found of the Documents page). Select a filter to either narrow the list of templates or order the list:
  • Recently opened - List the templates in the order of most recently used
  • Onshape - List templates provided by Onshape
  • My templates - Display all templates created by you or shared with you by another user (select sub-filter Created by me or Shared with me); these include any .DWT files in documents for which you have read permission.
  • Public - Display all templates made public by other Onshape users
  • Teams and companies - If you belong to a team or company, those names appear in this list; click a name to see available templates
• Standards - Across the top/right of the dialog, select a standards acronym to reduce the list of templates to only those of the selected standards format:
  • All - List templates in all supported standards
  • ANSI - List only ANSI standard templates (American National Standards Institute). Note that these templates configure the drawing for third angle view projection with inch or millimeter dimension units.
  • ISO - List only ISO standard templates (International Organization for Standardization). Note that these templates configure the drawing for first angle view projection and millimeter dimension units.
  • JIS - List only JIS standard templates (Japanese Institute for Standardization).

Only templates of the selected standard and in the selected filter are displayed.

Once you have a drawing (empty or with default views), you can then:

1. Add more views, see Views.
2. Add dimensions, see Dimensions.
3. Add notes, see Notes.
4. If the underlying geometry changes, you might want to update the drawing, see Updating a Drawing.
5. Exporting a Drawing.
6. Add more sheets, see Sheets.