Properties

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 panel. 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.

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)

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

• 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 can click the plus sign under Custom colors to save the currently specified color value as a custom color for later use.

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

    

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.

• Text justification - Change the justification of all the Note and Dimension text in the drawing. Choose from Left, Center, Right, or Auto alignment.
• Underline overridden dimensions - Uncheck this box to remove the underline format from all currently overridden dimensions.
• Break dimension by default - Checked by default, this creates a space between overlapping dimension lines. Unchecking it does not change existing dimensions, but determines the default state for dimensions created later.

Use this tab to edit your drawing's text alignment, text gap, geometry gap, extension past line, and to lock the angle of all jogged dimensions to 45 degrees:

• Text alignment - Specify whether to align the dimension text with either the dimension line, or align it horizontally along the bottom edge of the drawing sheet.
• Text gap - Set the measurements of the text gap in the drawing.

• Geometry gap - Set the measurements of the geometry gap in the drawing.
• Extension past line- Set how far the extension line will extend past the text.
• Lock the angle of all jogged dimensions to 45 degrees - Check this box to lock the angle of all jogged dimensions in the drawing to 45 degrees.

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

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

Use these properties to style the chamfer dimensions on the drawing. You can 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; C 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

Changes the Drawing ordinate dimension style.

• ANSI - Displays leading lines from the ordinate dimensions.

• ISO - Displays leading lines from the ordinate dimensions and additional arrows that connect the increasing ordinate values from the origin point.

Drawing with ANSI Ordinate dimension style on the left and ISO on the right

If you use an ANSI or ISO template when creating a new drawing, the ordinate dimension style defaults to ANSI or ISO, respectively.

• Show dimension lines by default - Displays radial and diameter dimension lines inside the circle or arc. By default, this option is checked when creating a drawing with an ISO template, and unchecked when creating a drawing with an ANSI template. Unchecking it does not change existing dimensions, but determines the default state for dimensions created later.

  

  Circular drawing with Show dimension line checked (left) and show dimension line unchecked (right).

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

You can also specify to:

• Hide property placeholder (----, as in the title box)

• Hide property background (gray by default, as seen in the title box)

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

Specify the defaults for all flag notes, including Font, Border shape, and Color.

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

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

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

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

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

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.

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:

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 .

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
• View labels - Specify the font, size, font treatment and color of all view labels

Simplify the geometry shown in the drawing by setting a threshold below which features will be hidden, this setting affects only newly inserted views.

• None - No simplification setting is applied.

• Auto - Default. Finds the best view simplification settings based on the geometry of the part and automatically uses those settings to display the part or assembly.

• Absolute - Enter a number in the length units of the drawing to indicate that any feature smaller than the value will be simplified within the view. If whole parts are smaller than the threshold value, those parts will be missing from the view. This is useful for removing excessive details not needed for drawing purposes (for example, a large number of very small features or components).

• Ratio to studio - Enter a percentage of the size of the Part Studio or Assembly below which the feature will be simplified within the view. If whole parts are smaller than the threshold value, those parts will be missing from the view. This is useful for removing excessive details not needed for drawing purposes (for example, a large number of very small features or components).

• Ratio to part - Enter a percentage of the size of the part below which the feature will be simplified within the view. This setting aims to preserve parts in a view, while simplifying the detail within those parts. This is useful if you intend to ensure all the parts are present to facilitate detailing actions, such as placing callouts.

Specify the thickness and color of lines representing hidden edges, as well as the spacing of the dashes.

Specify the thickness and color of lines representing tangent edges, as well as the spacing of the dashes.

Specify the thickness and color of the exploded lines of the exploded view, as well as the spacing of the dashes.

Specify defaults here for:

• Hatch pattern - Specify the default type and pattern for the hatch marks
• 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, unfilled, or open)
• 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

Specify details here for:

• Detail profile lines - Specify the default line size, color, and style (Phantom, Dashed, or Solid) of the detail profile lines.
• Arrowhead - Specify the default size and arrowhead type (filled, unfilled, or open).
• Detail profile label - Specify the font, font size, style, and color of all detail profile labels.
• Detail profile style - Select In line, Connected, or Leader.
• Detail view profile - Deselect the check box to remove the outline surrounding the Detail view.
• Show detail view profile - Displays the detail view profile.
• Clip border to geometry - By default, the detail view border is displayed. Enabling this option displays the detail view geometry only, without a border.

  

  Original Front view (left), Detail A with Clip border to geometry disabled (middle); Detail B with Clip border to geometry enabled (right).

Specify details here for:

• Show view reference indicator - Show/hide the view reference indicator.
• View reference format - Click the format image to switch the view reference indicator format between line style and arrow style.
• Viewing lines - Specify the default view reference indicator line thickness and color.
• Arrowhead - Specify the default size and arrowhead type (filled, unfilled, or open).
• Viewing line label - Specify the font, size, font treatment and color of all viewing line labels.
• View label prefix - Enter a prefix to display before the view label.
• View label style - Select between A-A and A.
• View label suffix - Enter a suffix to display after the view label.

An Auxiliary view shown in the brown bounding square, the view plane and reference indicator shown in blue, and the label shown in black.

You can also create dimensions or Line to line angular dimensions using the Auxiliary view arrow style as a reference point. Once the Auxiliary view is created, open the Properties panel > Views > Auxiliary views, and select Arrow style as the View reference format. You can then create the angular dimension using the Dimension tool.

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

For drawings of sheet metal flat patterns, specify the following: 

• All bend lines - Adjust the thickness of all bend lines

• Up bend lines - Adjust the style (Solid, Dashed, or Center (default)) and color of the up bend lines.

• Down bend lines - Adjust the style (Solid, Dashed, or Center (default)) and color of the down bend lines.

• Bend tangent edges - Adjust the thickness and color of the bend tangent edges.

• Counterbore/Countersink up - Adjust the style (Solid (default), Dashed, or Center) and color of the Counterbore/Countersink up lines.

• Counterbore/Countersink down - Adjust the style (Solid (default), Dashed, or Center) and color of the Counterbore/Countersink down lines.

• Form tear - Adjust the style (Solid (default), Dashed, or Center) and color of the Form tear lines.

• Form up - Adjust the style (Solid, Dashed, or Center (default)) and color of the Form up lines.

• Form down - Adjust the style (Solid, Dashed, or Center (default)) and color of the Form down lines.

• Form centermarks - Adjust the style (Solid (default), Dashed, or Center) and color of the Form centermarks.

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

• During an export, elements are added to the corresponding layer: Title block, Border frame, or Border zones.
• The Drawing layer will not be included on DWT exports of the drawing.
• The Border frame, Border zone, and Title block layers will be locked when the format is set to Locked.
• The Border frame, Border zone, and Title block layers can have different default color and line thickness.
• The content in the Border frame, Border zone, and Title block layers will be located on specific layers (e.g., BORDER_FRAME, BORDER_ZONES, TITLE_BLOCK) when exported to DWG/DXF.
  • Please notes that older versions of DWG/DXF formats may not fully support layers.
• The title block is not replaced on drawing sheet size changes. However, the border frames and border zones are redrawn at larger/smaller sizes or more or less zones.
• All content on the Drawing layer is never replaced in sheet size changes or sheet format replacements.