Properties

Edit the units and precision of a drawing by clicking the first icon, labeled Units and precision, at the top of the Drawing properties panel.

Primary

Define the default primary units for the drawing. Edit the format of:

• Units - Default units for the drawing. Choose between: Inches, Inches fractional, Millimeters, and Feet and inches.
• Decimal separator - Default character to use a decimal separator. Choose between: Comma and Period.
• Precision - The precision of all numbers except those listed in the Properties flyout. Choose between: Zero and up to 6 decimal places, or between 0 and 1/256 for fractional numbers.
• Tolerance precision - The precision of geometric tolerances. Choose between: Zero and up to 6 decimal places, or between 0 and 1/256 for fractional numbers.
• Angular precision - The precision of angular measurements. Choose between: Zero and up to 6 decimal places.

Initial drawing with default properties (above) and with Decimal separator set to 'decimal' (below)

• Angular tolerance precision - The precision of the tolerance for an angle. Choose between: Zero and up to 6 decimal places.

Dual

Specify whether or not to show dual dimensions and/or dual units in the drawing. You have the ability to specify the location of the dimension in reference to the view, as well as unit type, precision of decimal places, and the tolerance precision.

• Check Show dual dimensions to display all drawings dimensions in the default document units as well as a second, specified unit. Specify where to display the second dimension, either on top of, or on the bottom of the default units:

  

  

• Check Show dual unit to display the units of the dual dimension; otherwise, just the dimension is shown, without the unit of measurement.
• Dimension location - Specify where to place the dual dimension: on the top or bottom of the initial dimension
• Hole callout location - Select where to place the hole callout dual dimension: top, bottom, left or right of the initial dimension.
• Units - Specify the units for the dual dimension: this list will contain all units of measure except the units specified for the initial dimension label.
• Precision - The precision of the dual dimension. Choose between: Zero and up to 6 decimal places, or between 0 and 1/256 for fractional numbers.
• Tolerance precision - The precision of geometric tolerances. Choose between: Zero and up to 6 decimal places, or between 0 and 1/256 for fractional numbers.

Drawing with Show dual dimensions selected, Show dual unit selected with Units set to 'Inches', and Precision set to '0.12' (two decimal places)

Leading and trailing zeros

Use these settings to format the leading and trailing zeros in lengths.

• Length leading zeros - Select to include leading zeros on lengths.
• Length trailing zeros - Select to include trailing zeros on lengths.
• Length tolerance leading zeros - Select to include leading zeros for tolerances.
• Length tolerance trailing zeros - Select to include trailing zeros for tolerances.

Drawing with Length trailing zeros set on

To access the Dimensions menu, click the second icon in the Drawing Properties panel icon bar.

Use this tab to edit your drawing's font, text height, color, text alignment, text gaps, geometry gaps, and more. Change each option by clicking the drop down menu arrows on the right side of the menu and selecting an option.

• Font - Select the font of choice for dimension text.
• Text height - Select the size of choice for dimension text.
• Color - To edit colors for any drawing entity, click the color block in the Drawing properties panel to access the color dialog:

  

  • Select Palette to choose a color or enter a hex or RGB codes. Use the Mixer panel to drag to a general color area and then enter a specific hex or RGB code.

  • On either the Palette or Mixer panels you are able to click the plus sign under Custom colors to save the currently specified color value as a custom color for later use.

• Arrowhead length - Change the size of arrowheads for dimensions. Arrowhead length can be any value between 0.004 inches and 393.7 inches.
• Arrowhead type - Select no arrowhead, a filled or unfilled arrowhead, or oblique marks.

Drawing with the Color of dimensions set to red, the Font changed to APMONO, the Text height increased to 4.5, and the Arrowhead length set to 4.5000. Second image illustrates 'Oblique' selected as the Arrowhead type.

Gaps and extensions

Use Text alignment, under Gaps and extensions, to specify whether to align the dimension text with either the dimension line, or align it horizontally along the bottom edge of the drawing sheet:

• Align with dimension line - Aligns dimension text with the dimension line, whether vertical or horizontal.

• Horizontal - Aligns all dimension text with the horizontal bottom edge of the drawing sheet.

Drawing with Text alignment set to Horizontal, and Text gap and Geometry gap set to 0.75, and Extension past line increased to 1.5

Chamfer dimension

For information on using the tool, see Dimensions, Chamfer dimension.

Use these properties to style the chamfer dimensions on the drawing. You are able to specify:

• 45 degree style - Select either a Note or a Dimension to appear
• 45 degree content - Angle x Length; Length x Angle; Length x Length
• Non 45 degree style - Dimension; Note
• Non 45 degree content - Angle x Length; Length x Angle; Length x Length
• Length precision - Number of digits in the length value
• Angle precision - Number of digits in the angle value

To access the properties for Annotations, click the third icon at the top of the Drawing properties panel. From there you are able to edit the font, text height, arrowhead length and type, and color of each annotation type in your drawing: You have the ability to supply defaults for all annotations at once, or Notes, Callouts, Datums, Geometric tolerances, Surface finish symbols, Weld symbols, Hole callouts, and Bend notes (for sheet metal) separately.

The properties for each drawing annotation entity are similar and explained below. Any properties specific to an annotation type are explained under that subheading, following this section.

• Font - Select the font of choice for each annotation type.
• Text height - Select the size of choice for each annotation type.

• Color - To edit colors for any annotation entity, click the corresponding color block to access the color dialog:

  

  • Select Palette to choose a color or enter a hex or RGB codes. Use the Mixer panel to drag to a general color area and then enter a specific hex or RGB code.

  • On either the Palette or Mixer panels you are able to click the plus sign under Custom colors to save the currently specified color value as a custom color for later use.

Notes

Specify the defaults for all note properties, including Font, Text height, and Color.

Note that all exported drawings will, by default, no longer contain Drawing and Sheet Property placeholders ("----").

Callouts

Specify the defaults for all callouts, placed in space or attached to geometry, including Font, Text height, and Color.

The callouts in the drawing correspond to the Item No. column in the BOM

Datums

Specify the defaults for all datum properties, including Font, Text height, Datum size (the size of the triangle), and Color.

Geometric tolerances

Specify the defaults for all geometric tolerances, including Font, Text height, and Color.

Surface finish symbols

Specify the defaults for all surface finish symbols, including Font, Text height, and Color.

Weld symbols

Change the standard for the Weld symbol at the bottom of the Annotations menu. This menu changes the default standard for the Weld symbols used in the drawing. This standard is separate from the standard of the drawing and does not change that. For example, for an ANSI standard drawing you could change this setting and use all ISO Weld symbols in your drawing.

Bend notes

Change the formatting for bend notes attached to sheet metal views, including font, text height and color. Bend notes come into the drawing from the bend specifications made in the Part Studio:

Hole callouts

Change the formatting for hole callouts attached to sheet metal views, including font, text height and color. Hole callouts are applied to a drawing of a sheet metal flat pattern through the Dimensions dropdown menu, Hole callout tool .

To access the Views menu, click the fourth icon at the top of the Drawing properties panel. In this menu, you are able to edit your drawing's projection angle, the color and thickness of your drawing's visible edges, tangent edges, hidden edges, cutting lines, arrowheads, view labels and more.

The properties for each drawing view are similar and explained below. Any properties specific to a view type are explained under that subheading, following this section.

• Arrowhead: size and type - Select the size and type of arrowhead to use, choose from: filled or unfilled
• Labels: View, Cutting line, and Detail circle - Select the font, size, and font treatment (apply bold and/or italic), and color for each label type

Color - To edit colors for any annotation entity, click the corresponding color block to access the color dialog:

• Select Palette to choose a color or enter a hex or RGB codes. Use the Mixer panel to drag to a general color area and then enter a specific hex or RGB code.

• On either the Palette or Mixer panels you are able to click the plus sign under Custom colors to save the currently specified color value as a custom color for later use.

All views

Specify defaults here for all view types: Section views, Detail views, Break views, and Flat pattern views:

• Projection angle - Specify which projection to use
• Visible edges - Specify the thickness and color of lines representing visible edges
• Tangent edges - Specify the thickness and color of lines representing tangent edges
• Hidden edges - Specify the thickness and color of lines representing hidden edges
• View labels - Specify the font, size, font treatment and color of all view labels
• Exploded lines - Specify the width and color of the exploded lines of the exploded view

Section views

Specify defaults here for:

• Hatches - Specify the default line size and color for hatch marks
• Cutting lines - Specify the default line size and color for cutting lines
• Arrowhead - Specify the default size and arrowhead type (filled or unfilled)
• Cutting line label - Specify the font, size, font treatment and color of all cutting line labels

 

In the illustration above, the hatches of the section view were changed to a gold color (which is propagated to the detail view as well) and the arrowhead on the cutting line was increased in size

Detail views

Specify details here for:

• Detail circle lines - Specify the default line size and the color of the detail circle lines
• Arrowhead - Specify the default size and arrowhead type (filled or unfilled)
• Detail circle label - Specify the font, size, font treatment and color of all detail circle labels

In the illustration above, the detail circle line was changed from 0.13mm to 0.50mm and the detail circle label was changed from black to teal

Break views

Specify the default line thickness and color for break lines.

In the illustration above, the break line thickness is 0.50mm and the color is blue

Flat pattern views

For drawings of sheet metal flat patterns, specify the default line thickness, of all bend lines and the colors for up bend lines and down bend lines.

In the illustration above, all bend lines have a value of 0.50mm and the up bend lines have a red color specified

To access the Construction geometry menu, click the fifth icon at the top of the Drawing properties panel. In this menu, you are able to edit the color and thickness of your drawing's centerlines, as well as the style, color, and thickness of the drawing's virtual sharps. Use the Part Studio sketches section to edit the format of sketches brought into the drawing.

• Created in drawing - Specify defaults for construction geometry you create in the drawing:
  • Centerlines - Specify the default line size and color.
  • Centermarks - Specify the default line size and color.
  • Virtual sharps - Specify the visual treatment for all virtual sharps as Centermark or Edge extension, shown below, respectively:
  • Lines and splines - Specify the default line size and color for all lines and splines added to the drawing.
• Part Studio sketches - Specify defaults for the geometry brought in as a Part Studio sketch.

The illustration above shows the selections made in the dialog for construction geometry; the image to the right shows the virtual sharps are purple and edge extensions

To access the Formats menu, click the sixth icon at the top of the Drawing properties panel. This menu enables / disables selection of objects in a drawing's border frame, border zone, and title block. The default for a new drawing is Locked; you are not able to immediately select objects in the title block, border, or border zones.

Drawings should have this property initially set to unlocked; so the user is able to select objects in the titleblock or border.

If field values change, the content of the titleblock updates when the title block is locked.

If you move an entity to the titleblock, border, or border zone, and the Format is locked, you must move the entity back to Drawings in order to edit it.

• Locked - Lock or unlock the title block to disallow editing or allow editing.
• Border frame - Specify the color and thickness of the drawing's inner border
• Border zone - Specify the color and thickness of the labels inside the drawing's border zone
• Title block - Specify the color of lines and content of the title block, and the thickness of the lines

In the title block and border, entities in gray inherit their values from document data or properties. However, right-click on an entity to access the context menu for that entity. Select Edit note to edit the entity. Hover over a field (or click on it) to see what the corresponding property is. You have the ability to delete the field (property) and insert your own text if you wish. Use the Insert drawing property icon in the Note edit box to insert a different property:

This illustration shows a field in the title block being edited (select Edit note from the context menu), and a new field being inserted via the Insert drawing property command

To access the Tables menu, click the last icon at the top of the Drawing properties panel. You are able to make changes for Bill of Material (BOM) tables as well as all other tables, like Hole tables, you create in your drawing.

• BOM tables - Specify default values for Onshape bill of material tables, including:
  • Line thickness - Specify the default thickness of the BOM table lines.
  • Font - Specify the default font type for BOM tables inserted in the drawing.
  • Header row text - Specify the default font size, font treatment, and color for the header row.
  • Content row text - Specify the default font size, font treatment, and color for the content rows.
• Hole tables - Specify default values for Onshape hole tables, including:
  • Line thickness - Specify the default thickness of the hole table lines.
  • Font - Specify the default font type for hole tables inserted in the drawing.
  • Header row text - Specify the default font size, font treatment, and color for the header row.
  • Content row text - Specify the default font size, font treatment, and color for the content rows.
  • Indicator style - Select a standard for the hole indicator: ANSI or ISO.
  • Indicator arrowhead - Enter or select a size for the indicator arrowhead.
  • Indicator lines - Select a thickness and a color for the lines.
  • Tags - Specify characteristics of the text for the hole tags: font, size, formatting (bold, italic, or none), and color.
• Revision tables - Specify default values for Onshape revision tables, including:
  • Line thickness - Specify the default thickness of the revision table lines.
  • Font - Specify the default font type for tables created in the drawing.
  • Title row text - Specify the default font size, font treatment, and color for the table title row.
  • Header row text - Specify the default font size, font treatment, and color for the table header row.
  • Content row text - Specify the default font size, font treatment, and color for the table content rows.
  • Revision callout - Specify the default shape of the callout, the number of characters, and the font, size, color, and treatment.
• Tables - Specify default values for tables you create in the drawing, including:
  • Line thickness - Specify the default thickness of the lines in all tables created in the drawing.
  • Font - Specify the default font type for tables created in the drawing.
  • Title row text - Specify the default font size, font treatment, and color for the table title row (if applicable).
  • Header row text - Specify the default font size, font treatment, and color for the table header row (if applicable).
  • Content row text - Specify the default font size, font treatment, and color for the table content rows.

Edit the cells of the table separately from the table properties by clicking in the empty area of a cell to open the Cell edit panel:

Edit the text in any cell separately from the table properties by double-clicking on text in the table:

In Onshape, you have the ability to change the properties of a drawing by importing a drawing template you have already created by using the feature at the bottom of the Drawing properties panel (shown below outlined in blue). You can also use the Lock drawing properties checkbox to prevent them from being accidentally edited.

To update properties from an existing Onshape drawing template, open the Drawing properties panel.

Click the Select a DWT icon to the right of Update properties from a template...to open the Select a DWT dialog box:

To select a DWT from the current document

1. Click at the top of the dialog.
2. Type in the Search files bar to find a file, or select one from the list below it.
3. To import a DWT from your desktop, click Import...at the bottom of the dialog box, select the file you wish to import, and click Open.

Use the three icons at the top of the dialog, under Other documents, as explained below:

View released items - Click the View released items icon to list all released items for you to choose from.

Create version - Click the Create version icon to open the Create version dialog box:

Adjust the name and/or description of your version, and click to create the version, or to open the Properties dialog:

Adjust the properties of your version, click to apply your changes, or click to apply the changes and close the Properties dialog.

Click to close the Properties dialog without applying any changes.

Version graph - Click the Version graph icon to select a different version of the document from the version graph.

To select a DWT from other documents

1. Click at the top of the dialog.
2. Use the Search bar, or click one of the options below it, to select a DWT from another document in Onshape.

My Onshape - Select a DWT from a document in your Onshape.

Recently opened - Select a DWT from your recently opened documents.

Created by me - Select a DWT fr om documents created by you.

Shared with me - Select a DWT from documents shared with you.

3. To import a DWT from your desktop, click Import...at the bottom of the dialog box, select the file you wish to import, and click Open.

After you import a drawing template, the properties will automatically update.