Detail Options Specific to 3D Mode
The following Detail options are specific to 3D mode.
ang_unit_trail_zeros
yes*, no
Determines if trailing zeros (ANSI standard) are kept when angular dimensions are shown in deg/min/sec format.
Default and Available Settings:
• yes*—Trailing zeros are kept.
• no—Trailing zeros are removed.
ang_unit_lead_zeros
yes*, no
Determines if leading zeros are kept when showing angular dimension in degree format. This is to support ASME Y14.5 standard.
• yes*—Leading zeros are kept.
• no—Leading zeros are removed.
arrow_length_ratio
0.600000*, <user-defined value>
Sets the length of leader line arrow heads as 0.6 * calculated text height.
arrow_width_ratio
0.200000*, <user-defined value>
Sets the width of the leader line arrow heads as 0.2 * calculated text height.
arrow_style
Controls the style of the arrow head for all detail items that appear with arrows.
Default and Available Settings:
• filled*—The arrow head appears filled.
• open—The arrow head appears open.
• closed—The arrow head appears closed.
attach_sym_height_ratio
0.600000*, <user-defined value>
Sets height of leader line slashes, integral signs, and boxes.
attach_sym_width_ratio
0.200000*, <user-defined value>
Sets width of leader line slashes, integral signs, and boxes.
excl_annotations_of_excluded
yes*, no
Determines whether to exclude annotations that are children of excluded features.
excl_annotations_of_deleted
yes, no*
Determines whether to exclude annotations that are children of deleted features.
excl_annotations_of_section
yes*, no
Determines whether to exclude standalone annotations that are children of section features when the section is not active and not shown.
excl_annotations_of_suppressed
yes, no*
Determines whether to exclude annotations that are children of suppressed features.
default_ansi_ord_dim_aligned
yes*, no
Specifies whether ordinate dimensions are aligned with the baseline dimension when you create or edit dimensions with the Detail option ord_dim_standard set to std_ansi.
default_sketcher_hatch_spacing
Sets the spacing between hatching lines in closed areas within a sketch.
Default and Available Settings:
• relative*—The spacing between hatch lines is calculated based on a scale value relative to the sketch outline.
• 0.1<value—The spacing between hatch lines is set based on a model unit value.
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When you create a drawing from the part that contains a sketch feature, the spacing between hatching lines defined by this option also reflects in the drawing.
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default_thickness_dim_prefix
NONE*, <user-defined value>
Defines the default prefix value for thickness dimensions.
default_thickness_dim_suffix
THICK*, <user-defined value>
Defines the default suffix value for thickness dimensions
dim_leader_length_ratio
1.500000*, <user-defined value>
Sets the length of the dimension leader lines when the leader arrows are outside the witness lines.
dot_diameter_ratio
default*, <user-defined value>
Sets the diameter of dots in a leader line. If set to default, uses value set for arrow_width_ratio proportional to text height.
gtol_indicator_attached
yes*, no
Specifies whether to attach the plane and feature indicators to the GTOL frame, or to leave a gap.
• yes*—Attaches the GTOL frame to the plane and feature indicators.
• no—Shows a gap between the GTOL frame, and the plane and feature indicators.
gtol_secondary_value_precision
round*, truncate
Controls the precision of secondary unit value of GTOLs, when dual_dimensioning Detail option is set.
Default and Available Settings:
• round*—The secondary unit values of GTOLs are rounded.
• truncate—The secondary unit values of GTOLs are truncated.
leader_elbow_length_ratio
1.500000*, <user-defined value>
Determines the length of the leader elbow for model and draft datums.
minimum_angle_dimension
If the angle between the references is less than the value defined in the detail option, the references are assumed to be parallel. When you create a driven dimension annotation, a linear dimension is created between the references. For example, if the value of the angular value between the references is 3 and the value of the detail option is 4, a linear dimension is created between the references.
If the angle between the references is more than the value defined in the detail option, an angular dimension is created between the references. For example, if the value of the angular value between the references is 5 and the value of the detail option is 4, an angular dimension is created between the references.
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If you open a model created in Creo Parametric 4.0 M070 and earlier, the Detail option value is set to the current value of the configuration option minimum_angle_dimension.
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set_datum_leader_length_ratio
2.070000*, <user-defined value>
Determines the default length of the leader for a draft set datum and model set datum.
show_hidden_quilt_sket_pnt_axes
no*, yes
Specifies the display of axes that are defined by geometry points located in the sketch associated with the hidden quilts.
Default and Available Settings:
• no*—Axes defined by sketch points are hidden with the layer, along with the quilt associated with the sketch.
• yes—Displays axes defined by sketch when the quilt associated with the sketch is hidden with layer.
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• This detail option does not affect the visibility of axes that are automatically created at the center points of cylindrical surfaces of the quilt.
• These axes are shown or hidden with the associated quilt.
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text_height
calculated*, <user-defined value>
Sets default text height for text. The default value is calculated based upon the size of the model envelope when the annotation is created.
visible_annotations_scope
Active model only*, all
Displays the annotations of sub model, active model, or both for non_mbd combination state in an assembly.
• Active model only*—Displays the annotations of the active model in an assembly.
• all—Displays the annotations of the active model and sub model in an assembly. This works only for non_mbd combination states.
wf_inch_solid_dtl_setup_file
Sets the path to the file that contains the default model values for pre Creo inch models. If you do not set this option, the system uses the 3d_inch.dtl detail file for new inch models, sets ord_dim_standard to std_ansi, iso_ordinate_delta to no, and symbol_font to legacy.
wf_metric_solid_dtl_setup_file
Sets the path to the file that contains the default model values for pre Creo metric models. If you do not set this option, the system uses the 3d_inch.dtl detail file for new metric models, sets ord_dim_standard to std_iso, iso_ordinate_delta to yes, and symbol_font to legacy
witness_line_delta_ratio
0.600000*, <user-defined value>
Sets the extension of the witness line beyond the dimension leader arrows.
witness_line_offset_ratio
0.300000*, <user-defined value>
Sets offset between a dimension line and object being dimensioned. This may be visible only when plotting (and on screen plot). Also controls the size of the line break at the intersection of witness lines.