3D Clearance Check Settings

The 3D Clearance Check Settings dialog allows you to configure the settings for 3D clearance check. 3D clearances are checked on board design data items and mechanical data. Use the Mechanical Object Organizer to import the mechanical data to check. This dialog is displayed by clicking MCAD > Check > 3D Clearance Check split button > 3D Clearance Check Settings on the eCADSTAR PCB Editor ribbon.

Item	Description
Import parameters	Allows you to import parameters that were previously exported as a 3DCL parameter file (.xml). Browse to the required file in the displayed Open dialog. The settings in the 3D Clearance Check Settings dialog are overwritten by the settings in the imported file.
Export parameters	Allows you to export the settings in the 3D Clearance Check Settings dialog as a 3DCL parameter file (.xml). In the displayed Save As dialog, specify the name and location of the exported file. You can add the exported settings to the 3D Clearance Check Settings dialog by clicking Import parameters.

Rule set

Value		Description
Rule set table		The Rule set table allows you to create up to ten rule sets.
	Rule Set	Specify a unique text string that identifies the check rule set.
	Check	Selected: the associated rule set is used. Not selected: the associated rule set is not used.
Add		Adds a rule set to the bottom of the Rule set box.
Delete		Deletes the rule set that you select in the Rule set box. You can delete multiple rule sets using the Ctrl or Shift keys.

Rule

Value		Description
Rule table		The Rule table allows you to create up to 100 rules.
	Rule	Specify a unique text string that identifies the rule.
	Check	Selected: the associated rule is used. If all relevant parameters are not specified, then this box is made unavailable. Not selected: the associated rule is not used.
	Check (Source)	Specify the source items that are checked in the design.
	Type	Specify the type of source item that is checked in the design. Board outline: Checks the data in relation to the board outline in the active design data. Component: Checks the data in relation to component areas of the specified component in the active design data. Comp.condition: If selected, the Select Condition for Component dialog is displayed when you click "..." in the Name column. The condition names for component selection that are saved in the board are listed in the dialog. If you select a condition name, its name is set in the Name column. Net: Checks the data in relation to the specified net in the active design data. Specify the net in the Select Net dialog. This dialog is displayed when you click "..." in the Name column.
	Name	Specify the name of each source item that is checked in the design. If Board outline is selected in the Type column: specify the board instance name. If Component: is selected in the Type column: specify the reference name in the Select Component dialog. This dialog is displayed when you click "..." in the Name column. If Comp.Condition is selected in the Type column: specify the condition name for component selection that is saved in the board. This is done in the Select Condition for Component dialog. This dialog is displayed when you click "..." in the Name column. If Net is selected in the Type column: specify the net name in the Select Net dialog. This dialog is displayed when you click "..." in the Name column.
	Check (Destination)	Allows you to specify the mechanical data that the source data is checked against. You can also specify clearance values.
	Type	Checks the data in relation to mechanical data.
	Name	Specify the name of the mechanical data that the source data is checked against. You can either type a value in this column, or specify the mechanical data in the Select Mechanical Item dialog. This dialog is displayed by clicking "..." in this column. If there are sub-components of the mechanical data, then they can be selected in this dialog.
	Clearance	Specify the clearance to check between two data items. By default, 0 is specified when you add a row. If this clearance is not met between a source and destination item, then the actual clearance value is shown in the 3D Clearance Check Report dialog, Clearance column. Values are also shown in the Dist.X, Dist.Y and Dist.Z columns to indicate the relevant clearances in the X, Y and Z directions.
Add Rule		Adds a row to the bottom of the Rule box.
Delete Rule		Deletes a rule that you select in the Rule box You can delete multiple rules using the Ctrl or Shift keys.
Add Check (Destination)		For a row that you that select in the Rule box, a rule that contains the settings in the Check (Source) columns is added to the bottom of the Rule box.

Check target

Value		Description
Hole in board		Allows you to add holes in the board as targets.
	Selected	The following items are added as targets: Round holes Slot holes in the board Holes in non-plated through padstacks
	Not selected	The following items are not added as targets: Round holes Slot holes in the board Holes in non-plated through padstacks
Cutout in board outline		Allows you to add cutouts in the board outline as targets.
	Selected	Adds cutouts in the board as targets.
	Not selected	Does not add cutouts in the board as targets.
Mechanical data with no thickness		This setting allows mechanical data that have no thickness to be added as a target.
	Selected	Mechanical data that do not have thickness are added as targets.
	Not selected	Mechanical data that do not have thickness are not added as targets.
Prioritize 3D model		Allows you to specify whether the 3D model or the component area is used when running a check.
	Selected	Uses the 3D model instead of the component area when running a check. Any component to which the 3D model has not been assigned is checked using the component area.
	Not selected	Uses the component area when running a check.