Configuration Options for Assembly

Assembly Design > Using Assembly > Configuring Creo Parametric for using Assembly > Configuration Options for Assembly

accessory_window_display

docked*, undocked

Docked—Displays a component in an accessory window embedded in the graphics window.

Undocked—Displays a component in a stand alone accessory window.

add_offset_to_constraint_comp

no*, yes

Adds offset dimensions, during dragging operations, to Distance or Angle Offset constraints initially created without offsets.

advanced_intersection

no*, yes

Controls the scope of available options in the Intersect tab of feature tabs that remove material in an assembly.

no—Enables basic functionality.

yes—Allows setting display level for individual components and selecting Family Table instances to intersect.

allow_copy_with_ext_refs

Allow a part with external references to be mirrored copy. Note that any features of the original component that are dependent become independent.

allow_direct_ref_to_layout_file

Allows referencing a layout file through the layout feature. For full update control, it is recommended to reference the copied layout geometry and not the layout file.

allow_freeze_failed_assy_comp

no*, yes

Allows freezing failed assembly components.

allow_mfg_in_assem_mode

yes, no*

Allows you to open a manufacturing model in assembly mode.

yes—Adds the Open in Assembly mode option to the list in the File Open dialog box when you click the arrow next to Open.

allow_package_children

all*, feature, none

Sets allowances of features to reference packaged components. After you set this option, it takes effect immediately in the current session.

all—Allows both feature and component placement references

feature—Allows only geometric feature references

none—Disables both feature and component placement references

allow_redo_intersections

yes, no*

yes—Displays the ReIntersect command in the ASSY FEAT menu.

allow_ref_scope_change

all*, environment, model

Defines the accessibility of reference control settings at the application level and model level.

• Application level—On the Assembly page of the Creo Parametric Options dialog box, set the External Reference Control options.

• Model level—Open the Reference Creation Control dialog box. Click

File > Prepare > Model Properties. Click change in the Reference and Backup line.

all—Reference control settings are accessible in all places.

environment—Reference control settings can only be changed at the application level.

model—Reference control settings can only be changed at the model level.

After you set this option, it takes effect immediately in the current session.

allow_save_as_instance

no*, yes

Allows the option to save a copy of the active model as a family table instance.

animate_explode_states

yes*, no

Yes—The transition between explode states is animated.

assem_placement_ignore_units

no*, yes

yes—Enables an automatic update of model units when placing a model whose unit settings are different from the assembly unit settings. The unit settings of the placed model update to those of the assembly.

no—Disables automatic unit update.

assemble_module_in_rep

Representative Module Variant*, specified representation

Sets the default representation of a module when it is assembled in a configurable assembly.

Specified representation—Set one of the following options:

• Last Stored

• Current Configuration

• Master Rep

• Exclude

• Graphics Rep

• Geometry Rep

• Light Graphics Rep

auto_assembly_with_notebooks

yes*, no

Controls automatic assembly.

yes—Enables automatic assembly.

no—Disables automatic assembly.

auto_constr_always_use_offset

yes, no*, never

Controls whether the Automatic constraint creates offsets.

yes—Automatic constraint always creates an offset, Distance constraint.

no—Automatic constraint snaps Coincident Align or Mate if surfaces are within tolerance.

never—Use Coincident as the default constraint type.

auto_constr_offset_tolerance

0.5*

Sets the tolerance for creating an offset dimension. When the distance is less than the tolerance multiplied by the component size, the offset is set as coincident.

auto_eval_current_cnfg_rule

Provides or prevents the automatic evaluation of the Current Configuration simplified representation and any other simplified representation containing a rule with the NOT_IN_CUR_CONF condition. The evaluation occurs when the configurable product is retrieved or regenerated.

Creo Parametric does not evaluate simplified representation rules by default unless they contain the condition NOT_IN_CUR_CONF.

auto_place_max_number

Sets the default for the Number of positions displayed in Auto Place dialog box in the Assembly page of the Creo Parametric Options dialog box. Type a different number in the box.

auto_update_simprep_rules

yes, no*

yes—Newly created simplified representations defined by filters are updated each time you retrieve or regenerate a model.

autoplace_single_comp

yes*, no

Assembling components with an interface automatically places the component at the first position satisfying the interface definitions.

boolean_associative_placement

yes*, no

Update the Boolean feature according to the placement of the modifying component in Boolean operations.

boolean_copy_datums

yes, no*

Copy datum planes from the modifying component to the modified model as part of the Boolean operation.

boolean_copy_quilts

yes*, no

Copy quilts from the modifying component to the modified model as part of the Boolean operation.

boolean_default_operation

model_type*, add_bodies, merge, cut, intersect

Sets the default Boolean operation.

• model_type—Determines the default feature by the type of model. In Assembly sets the default to merge, in Part sets the default to add_bodies.

• add_bodies—Sets the default Boolean feature to Add Bodies.

• merge—Sets the default Boolean feature to Merge.

• cut—Sets the default Boolean feature to Cut.

• intersect—Sets the default Boolean feature to Intersect.

boolean_discard_modifying

yes, no*

Delete the modifying components after a Boolean operation.

boolean_feat_update_state

auto*, manual, no_dependency

Determines updates to the Boolean feature when the original models change.

• auto—New Boolean features are created with automatic update settings.

• manual—New Boolean features are created with manual update settings.

• no_dependency—New Boolean features are created with no dependency settings.

boolean_transfer_refs

yes, no*

Transfer all references from the modifying components to the resulting Boolean feature.

can_snap_to_missing_ref

yes*, no

Enables snapping to missing references while using the drag-and-drop operation for component placement.

check_interface_criteria

yes, no*

Determines if Check Interface Criteria is selected by default in the Placement Preferences dialog box.

yes—The option is selected by default.

no—The option is not selected.

check_same_assy_parts

yes*, no

Determine whether to permit different names for different part occurrences or not in the mirror subassembly user interface.

child_of_layout_backup_update

notify, manual, auto*

Sets the default update state for a feature referencing geometry from the layout feature.

notify—Displays an icon next to the feature icon to notify that the source layout is updated and is in session.

manual—Allows manual update of the feature.

auto—Automatically updates the feature when the source layout is updated and in session.

chooser_size_filter_default

Sets the default size for the Component Chooser size filter as a percentage of the assembly size.

cnfg_ref_control_add_comp

all, pg, tagged*, none

Sets the specified shared geometry reference control conditions to the newly added components in a configurable module.

all—all components

pg—publish geometry

tagged—tagged components

none—Allows assembling a new module to CSA.

cnfg_ref_control_new_comp

all*, pg, tagged, none

Sets the specified shared geometry reference control conditions to newly created configurable modules if template models were not used.

all—all components

pg—publish geometry

tagged—tagged components

none—Allows creating a new module without a template.

cnfg_ref_control_plcmnt_new_comp

all, tagged *, interfaces, none

Sets the specified shared placement reference control conditions to newly created configurable module if template models were not used.

all—all components

tagged—tagged components

interfaces—components with interfaces

none—Allows creating a new module without a template.

combined_views_customization

yes*, no

yes—Combined views can be ordered, included, or excluded on the Combined Views bar. A saved thumbnail preview image is available when the pointer hovers over the combined view tab, and the configuration of the Combined Views bar is saved to the model.

no—The Combined Views bar cannot be customized and the combined views are not saved to the model.

comp_angle_offset_eps

Specifies the angle epsilon when the selected surface is equal or greater than the epsilon (in degrees). An angle offset constraint is created.

comp_assemble_start

default*, constrain_in_window, package, move_then_place

Adjusts the position of a component during placement.

default—Displays the component being placed outside the assembly.

constrain_in_window—Displays the component being assembled in a separate window.

package—Attaches the component being assembled to the pointer. Move the component to the required location, click, and open the Placement tab to place the component.

move_then_place—Attaches the component being assembled to the pointer. Move the component to the required location, click, and select references to place the component.

comp_assemble_with_interface

default_multi*, default_single, from_list, none

Options for placing a component with configured interfaces.

default_multi—You can automatically place multiple instances of the component using a configured interface.

default_single—You can automatically place a single instance of a the component using a configured interface.

from_list—The Select Interface dialog box opens before the Component tab opens. Select the interface for component placement from the list and then specify multiple or single placement.

none—Place components without using interfaces.

comp_normal_offset_eps

10.000000*

Specifies the angle epsilon. When the angle between the selected surfaces is equal or less than epsilon (in degrees), a normal constraint is created. The expected value should be positive or zero. A negative value is stored as an absolute value.

comp_offset_dec_places

Sets the default number of decimal places (0-10) to display in the offset column of component placement.

comp_placement_assumptions

yes*, no

Sets the default for Allow Assumptions in the Placement tab during component placement.

yes—Allow Assumptions is selected by default.

no—Allow Assumptions is not selected.

comp_placement_legacy_move

yes*, no

Shows the legacy Move tab in the Component Placement tab.

yes—The Move tab is displayed.

no—The Move tab is not displayed.

comp_ret_angular_increment

1*, integer from 1 through 10

Controls the resolution of components selected for a shrinkwrap feature or for external or outer component selection.

The resolution is controlled by the density of angle increments. 1 gives a 90° increment, 2 gives a 45° increment and so on until 10 which gives a 1° degree increment. In most instances a value of 1 is sufficient. A higher value selects more components that are not completely external.

comp_rollback_on_redef

yes*, no

Controls whether the system rolls back the assembly when you redefine a component.

comp_snap_angle_tolerance

0-90, 30*

Specify the angle tolerance for snapping while freeform dragging components being assembled.

comp_snap_dist_tolerance

0.1*,0-1

Specify the distance tolerance for snapping while freeform dragging components being assembled. Relative to the size of the component being assembled.

constraint_reference_redefine

keep_constrait_type*, reset_constraint_type

Defines the behavior when choosing a new reference for an existing constraint during component placement.

keep_constrait_type—Adjusts the component’s position to keep the same constraint type.

reset_constraint_type—Automatically changes the constraint type to keep the position of the component.

convert_to_wf3_replace

no*, yes

Updates legacy designs to use Wildfire 3 Replace functionality.

copied_feat_refs_update_state

auto*, manual, notify, no_dependency

Sets the update state for newly created geometry backups for feature references.

auto—Automatically updates the geometry backups for features when the reference model is updated and in session.

manual—Allows manual update the geometry backups for features when the reference model is in session.

notify—Displays an icon next to the feature geometry backup icon to notify that the reference model is updated and is in session.

no_dependency—Sets the geometry backups for features to no dependency.

copied_place_refs_update_state

auto*, manual, notify, no_dependency

Sets the default for newly created copy feature placement references.

auto—Automatically updates the feature placement reference when the reference model is updated and in session.

manual—Allows manual update of the feature placement reference when the reference model is updated and in session.

notify—Displays an icon next to the feature placement reference icon to notify that the reference model is updated and is in session.

no_dependency—Sets the feature placement reference to no dependency.

copy_geom_update_pre_2000i_dep

yes—Flags independent copy geom features in a pre-2000i model as modified when retrieved into Creo Parametric. This enables you to save the model immediately to update the model’s copy geom dependency information. This information has changed in Release 2000i for improved interpretation of references in Pro/PDM and Pro/INTRALINK.

After you set this option, it takes effect immediately in the current session.

create_temp_interfaces

yes, no*

Allow creation of temporary component interfaces based on previous assembly instructions.

def_comp_ref_ctrl_exception

copy*, prohibit

Sets the default for newly created components to allow or disallow referencing entities forbidden by reference control settings.

def_multiple_backup_prompt_num

100*

Sets the number of components or features selected before a confirmation message appears when you create or delete backups.

def_obj_feat_refs_to_backup

non_permitted*, all, other_models, none

Sets the default to control the level of feature references backup for newly created models.

non_permitted—Backup only references created despite restrictions to referencing external components.

all—Backup all references.

other_models—Backup all references to other models.

none—Backup no references.

def_obj_place_refs_to_backup

non_permitted*, all, other_models, none

Sets the default to control placement references backup for newly created models.

non_permitted—Backup only references created despite restrictions to referencing external components.

all—Backup all references.

other_models—Backup all references to other models.

none—Backup no references.

def_obj_ref_ctrl_exception

copy*, prohibit

Sets the default for newly created models to allow or disallow referencing entities forbidden by reference control settings.

default_comp_geom_scope

all*, pg, none

Set the specified Shared Geometry reference control conditions to newly added components.

default_comp_module_geom_scope

tagged*. all, pg, none

Sets the specified Shared Geometry reference control conditions to modules being added to a configurable structure.

default_comp_scope_setting

all*, none, subassemblies, skeleton_model

Set the specified accessible reference control conditions to newly added components.

default_comp_skel_geom_scope

all*, pg, none

Set the specified Shared Geometry reference control conditions to newly added Skeleton components.

default_comp_skel_scope_setting

all*, none, subassemblies, skeleton_model

Set the specified Shared Geometry reference control conditions to newly added Skeleton components.

default_ext_ref_scope

all*, none, skeleton, subassembly

Set default scope for externally referenced models.

all—Create references to any component.

none—Cannot create references to other models.

skeleton—Create references only to skeleton and layout models of the high-level subassembly.

subassembly—Create references to components inside the same subassembly.

default_geom_scope

all*, pg_if_exists, pg_only

Sets the default value for geometry available for external reference selection by other models.

all—Allow external references to any geometry.

pg_if_exists—Allow external references to only published geometry if it exists in a model (if it does not exist, allow external references to any geometry.

pg_only—Allow external references to only published geometry.

default_obj_constraints_scope

all*, interfaces, none

Set the specified Shared Placement reference control conditions to newly created models if template models were not used.

default_obj_module_constr_scope

all*, tagged, interfaces, none

Sets the specified Shared Placement reference control conditions when creating new modules for configurable structures when template models were not used.

default_obj_module_geom_scope

all*, tagged, pg, none

Sets the specified Shared Geometry reference control conditions when creating new configurable modules without a template.

default_object_geom_scope

all*, pg, none

Set the specified Shared Geometry reference control conditions to newly created models if template models were not used.

default_object_scope_setting

all*, none, skeletons, subassemblies

Selects the default condition for reference control in a new object.

all—Reference any model. This is the way the system works today. The user may freely create external references to any component in an assembly.

none—Reference no other models. This will not allow any models other than the model being created, and those that exist below it on its branch, to be externally referenced.

skeletons—A new component may reference the Skeleton model of the assembly that the component belongs to. If a Skeleton model is being created, it may reference the skeleton model of the Assembly above the one that it belongs to.

subassembly—Allow external references to the model being created, the models which will exist below it, any peer models that the model being created might have, and models below them.

default_placement_scope

all*, intrf_if_exists, intrf_only

Default value for Component Placement Reference filter.

all—Allow all geometry to be used as component constraints.

intrf_if_exits—Allow only component interfaces to be used for component constraints, if they exist. If not, any geometry is allowed.

intrf_only—Allow only component interfaces to be used for component constraints.

default_ref_current_module_vrnt

yes*, no

Allow references only to the current module variant.

dim_inactive_components

shaded_only*, always, never

Sets the display of inactive components in an assembly.

shaded_only—Inactive shaded components display in the default appearance and phantom transparency. Assigned colors are ignored and non-shaded components are ignored.

always—Inactive components display in the default color in all display styles. Shaded components in the default appearance, non-shaded components display in the default geometry color.

never—There is no change in the display of inactive components.

direct_child_of_layout_update

notify*, manual, auto

Sets the default update for a feature directly referencing the layout model through a layout feature.

notify—Displays an icon next to the feature icon to notify that the source layout is updated and is in session.

manual—Allows manual update of the feature.

auto—Automatically updates the feature when the source layout is updated and in session.

disp_symb_name_in_symb_rep

yes*, no

Displays the names of components in symbolic representations.

dont_show_symbol_nodes

yes, no*

Filter out relations and parameters when viewing parent/child information in the Reference Viewer.

enable_advance_collision

yes, no*

Enables using advanced collision detection.

enable_assembly_accuracy

yes*, no

Accuracy modification for assembly objects.

enable_dragdrop_on_components

all and confirm*, all, reorder

Enables drag and drop operations for components and features in the Model Tree.

all and confirm—Displays a message window to confirm the restructure operation.

all—Allows you to reorder and restructure features and components using drag and drop in the Model Tree.

reorder—Allows you to only reorder features and components in the Model Tree using drag and drop. Restructure is not allowed.

enable_implied_joints

yes*, no

Allow underconstrained components as mechanism connections.

enable_insep_asm_operations

yes*, no

Exposes all inseparable assembly operations, make inseparable, embed, extract, make separable, and creating an embedded component.

erv_show_external_only

yes, no*

Controls the objects displayed in the Reference Viewer.

yes—Displays only objects with external references.

no—Displays all objects.

exec_prog_on_assem_retr

yes, no*

Execute Program for models during assembly retrieval.

explode_animation_max_time

1.0*, positive real value

Sets the maximum duration, in seconds, of an explode animation.

fail_ref_copy_when_missing_orig

yes*, no

When using a copied geom feature or a backed-up external reference with the Design Manager, and the reference is missing in the original, then the copied geom feature will:

yes—fail

no—freeze and not update

fast_highlight

Toggles fast highlight and standard highlight of selected assembly components during spin, pan, and zoom operations. Applies for models in the Wireframe, Hidden Line, No Hidden Line, and Shaded modes.

yes (default)—Fast highlight. Selected components, annotation features, datum curves, and cables associated with the selected components are highlighted and displayed during spin, pan, and zoom operations. Datum planes of selected components are not automatically highlighted unless specifically selected.

no—Standard highlight. Datum planes of selected components are automatically highlighted.

feat_references_to_backup

non_permitted*, other_models, none

Sets the backup of newly created feature references.

non_permitted—Backup feature references created despite an initial restriction.

other_models—Backup feature references to other components.

none—Do not backup feature references.

References to geometric bodies are not backed up.

fix_refs_to_intersections

yes, no*

Sets remnant removal ability for the ReIntersect command in the ASSY FEAT menu.

yes—You can remove remnants.

no—You cannot remove remnants.

force_upd_assem_mp_in_simp_rep

use_stored*, yes, no

Toggles the update of top-level assembly mass properties on regeneration according to simplified representation definitions.

use_stored—Mass properties are calculated or not calculated according to the following situations:

• Mass properties are calculated for the subassembly on regeneration when all components on the same level have accessible mass property data.

• Mass properties are not calculated for the subassembly on regeneration when not all the components on the same level have accessible mass property data.

yes—Mass properties for all components is recalculated and stored.

no—Mass properties are recalculated for subassemblies with components modified in simplified representations, but not stored.

The regeneration status is always green.

generate_viewable_on_save

yes, no*

Controls automatic generation of Creo View MCAD .pvz files when you save a model.

grv_default_view

references*, dependencies

Sets the default view of the Reference Viewer dialog box.

hide_pre_creo4_reps

maintain_master*, yes, no

Controls the availability of legacy simplified representations in the user interface.

maintain_master—Use Master, Exclude, Automatic, Default Envelope, and User Defined simplified representations.

When excluded components are retrieved on demand, they are retrieved in Automatic representation.

yes—Use Automatic, Default Envelope, and User Defined simplified representations.

no—Use Master, Exclude, Automatic, Geometry, Assembly, Graphics, Symbolic, Light Graphics, Boundary Box, Default Envelope, and User Defined simplified representations.

Use this value to retain on demand behavior for excluded components.

ignore_all_ref_scope_settings

yes, no*

Controls whether object-specific reference scope settings are ignored or not. Environment scope settings are still enforced.

ignore_export_geom_declaration

yes, no*

Ignore export geometry settings.

individual_child_update

yes*, no

Allows update control for individual children of a layout feature when the layout feature updates.

intf_out_pvs_recipe_file

<install_Dir>....\Common Files\F000\text\prodview\export_LWG.rcp

Sets the Creo View MCAD recipe file for export to PVS format. You can use a recipe file (*.rcp) for Windchill 9.0 and later releases. For more information on recipe files, search the Creo View MCAD Help.

keep_model_in_open_window

yes, no*

Controls whether a model is displayed in the main window when its accessory window is open.

keep_publish_geom_in_footer

yes*, no

Disables moving a Publish Geometry feature outside the Footer folder.

yes—Publish geometry feature cannot be moved outside of the footer.

no—Publish geometry feature can be moved outside of the footer.

mass_property_calculate

by_request*, automatic, report_outdateness_only, check_upon_save

Sets when to calculate mass properties.

• by_request—Calculates mass properties only on user request.

• automatic—Calculates mass properties on regeneration.

• report_outdateness_only—Shows a notification when mass properties are outdated.

• check_upon_save—Prompts on save if mass properties are not calculated.

model_allow_ref_scope_change

yes*, no

Change the scope settings of components.

modeltree_show_gen_of_instance

yes*, no

Displays the generic name as an extension of the instance name in the Model Tree and other model name lists.

modify_offset_during_comp_drag

yes, no*

Allows modifying the offset dimension of component constraints when moving a component being placed.

module_variant_cross_refs

yes, no*

Allows references between module variants in a module.

mp_calc_level

assembly_only*, all_models

Specifies the level of mass properties calculations for assemblies and parts.

assembly_only—Calculates mass properties for the assembly and reports them along with the summary of assembly components.

all_models—Calculates mass properties of all models in the assembly and reports them along with the summary of assembly components, details of assembly components, and the summary of bodies included. When the report is longer than 2,000 characters, it is not shown on screen, a *.m_p file is written to your working directory. Models with no calculated mass properties (quilts, no geometry, or zero density) are not included in the report.

multiple_skeletons_allowed

no, yes*

Allows or restricts multiple skeletons.

new_cg_update_state

notify, manual, auto*

Sets the update, relative to the source model, for newly created copy geometry features.

notify—Displays an icon next to the copy geometry feature icon to notify that the source model is updated and is in session.

manual—Allows manual update of the copy geometry feature.

auto—Automatically updates the copy geometry feature when the source model is updated and in session.

new_layout_feature_update_state

notify*, manual, auto

Sets the update relative to the source layout for newly created layout features.

notify—Displays an icon next to the layout feature icon to notify that the source layout is updated and is in session.

manual—Allows manual update of the layout feature.

auto—Automatically updates the layout feature when the source layout is updated and in session.

new_wf5_simp_rep_ui

yes*, no

Choose the new or old method to create and edit simplified representations.

The new method is a Component Chooser where you preview the simplified representation as you select its components from the Chooser Model Tree. In the old method, you select components from the Graphics Window or main Model Tree. No preview is available in the old method.

yes—Displays the new method.

no—Displays the old method.

notify_missing_ref_model

yes*, no

Provides notification when a feature with automatic or manual update control has a missing reference model.

open_simplified_rep_by_default

yes, no*, specified representation name

Determines the representation to retrieve when you retrieve models.

yes—Open the Open Rep dialog box when you retrieve a model.

no—Retrieves the master representation. When the default representation is not the same as the master representation, the assembly is retrieved in the default representation.

Specific name of a representation type—Retrieves the model in the specified representation. When the specified representation does not exist, the default representation is retrieved.

package_constraints

update*, freeze, disallow

Controls the behavior of partially constrained components. You cannot build children from them.

update—updates components if assembly changes

freeze—does not move components if assembly changes

disallow—does not allow packaged components in the assembly

package_ref_alert

yes, no*

Controls whether the system displays a confirmation prompt whenever you select a placement reference to a packaged component.

place_comp_use_mate_align_type

yes, no*

Controls the display of Mate and Align for a Coincident constraint where applicable.

placement_references_to_backup

non_permitted*, all, other_models, none

Controls the level of newly created placement backups in session.

non_permitted—Only placement reference created despite an initial restriction will be backed up.

all—All placement references to other models are backed up.

other_models—Placement references to other components will be backed up.

none—Do not backup placement references.

placement_rep_by_default

Sets the simplified representation to be retrieved when assembling a component. By default, the simplified representation specified in the open_simplified_rep_by_default configuration option is retrieved. You can enter a user-defined simplified representation name or one of the default representations. The specified simplified representation is retrieved when the component is assembled.

preserve_comp_color_in_preview

yes, no*

Defines the color of the component during placement.

yes—The component retains its color during placement.

no—The component displays in yellow preview color until fully constrained.

ref_control_allow_exceptions

yes*, no

Allows references not permitted when the default_ext_ref_scope configuration option is set to none.

ref_scope_copy_color

[0–255], [0–255], [0–255]

Specifies the default color used to display out-of-scope references that are allowed as local copies. The three decimal values in the range from 0 through 255 specify the level of red, green, and blue (in this order) in the resulting color. The models that are out-of-scope and available for copying are displayed in the user-specified color when geometry items are selected for reference.

ref_scope_copy_color_change

yes*, no

Enable or disable changing the color of prohibited external references that are allowed for backup. When set to yes, the color of out-of-scope prohibited references will change to the user-specified color during reference selection.

ref_scope_no_pick_to_copy

yes, no*

Disable or enable selection of external references not allowed for backup in the External Reference Control dialog box.

ref_scope_no_pick_to_prohibit

yes*, no

Disable selection of external references that were prohibited in the External Reference Control dialog box.

ref_scope_prohibit_color

[0-100], [0-100], [0-100]

Set the default color of prohibited external references by providing three RGB values. The three decimal values in the range from 0 through 100 specify the level of red, green, and blue (in this order) in the resulting color.

ref_scope_prohibit_color_change

yes*, no

Enable changing color of prohibited external references during selection.

regen_data_sharing_ref_models

yes*, no

Defines whether reference models of data sharing features are regenerated.

regen_int_mdls_on_retr

yes, no*

To specify if models that are intersected by assembly features are regenerated during assembly retrieval.

regen_notebook_w_assem

yes*, no

Notebook is automatically regenerated when the assembly is regenerated. After you set this option, it takes effect immediately in the current session.

regen_simp_retrieve

yes, no*

Regenerates component placement definition when retrieving an assembly simplified representation.

yes—Model regeneration is available upon retrieval.

no—Model regeneration is not available upon retrieval.

When set to yes, this configuration option impacts retrieval performance.

remember_replaced_components

yes*, no

yes—Preserves the dependency to the current outgoing component when you replace a component with an unrelated or interchange component. Allows you to break the dependency between the assembly and the interchange assembly in the Reference Viewer.

no—Removes the dependency to the current outgoing component. The option to break the dependency between the assembly and the interchange assembly in the Reference Viewer becomes unavailable.

replace_comp_name_method

transfer*, remove, preserve

Sets the naming convention used when replacing components.

Evaluation Rule Order and Configuration Options

The following five configuration options set the default order for evaluation rules when you replace unrelated components and use a reference pairing table for interchange assemblies. Set the order of one rule relative to other evaluation rules with an number from 1-5. The default value for all options is disable.

Option	Description
replace_interface_rule_order	Uses a predefined matching interface in the replacement operation.
replace_samename_rule_order	Uses a component with the same name in the replacement operation.
replace_history_rule_order	Uses history evaluation in the replacement operation.
replace_sameparam_rule_order	Uses the same parameters in the replacement operation.
replace_sameid_rule_order	Uses the same ID in the replacement operation.

replace_history_rule_order

disable*, 1, 2, 3, 4, 5

Sets the order for reference tagging of the History evaluation rule. Use this option when creating a reference pairing table for an interchange assembly or for replacing unrelated components.