Design Settings

The Design Settings dialog allows you to set design values that apply to relevant commands in eCADSTAR PCB Editor. Click Settings in an appropriate command dialog to display the relevant category in the Design Settings dialog. Alternatively, display the Design Settings dialog by clicking Design > Settings > Design or Net / Route > Design Settings > Routing Settings on the eCADSTAR PCB Editor ribbon.

 

 

Dimension Text

Dimension Display

Subtract Parameter

Thermal Relief

Online DRC

Post Check

Cross Probe

Snap

Routing

Dimension Text

Precision (Dimension)

Value	Description
0-5	Specify the number of decimal places for the dimension value.

Precision (Tolerance)

Value	Description
Same as dimension.	Sets the number of decimal places for the tolerance value to be the same as for the dimension value.
0-5	Specify the number of decimal places for the tolerance value.

Zero suppression

Value	Description
Never	Zeros are never suppressed in the dimension value. For example: "0.100" is displayed when the precision is 3.
Decimal only	Zeros are only suppressed in the decimal part of the dimension value. For example: "0.1".
Integer only	Zeros are only suppressed in the integer part of the dimension value. For example: ".100".
Both	Zeros are suppressed for the decimal and integer parts of the dimension value. For example: ".1".

Offset from dimension

Value	Description
Real number equal to or greater than 0.	Specify an offset value from the dimension line to the dimension string.

Font

Value	Description
(Font values)	Select a single byte font for the text that is used to display dimensions.

Character width

Value	Description
Real number greater than 0.	Set the width for text characters (real number equal to or greater than 0). You can also select this from the Font setting dialog. This value refers to the dimensions of the non-displayed box which contains the character, rather than the actual width of the character.

Character height

Value	Description
Real number greater than 0.	Set the height for text characters (real number equal to or greater than 0). You can also select this from the Font setting dialog. This value refers to the dimensions of the non-displayed box which contains the character, rather than the actual height of the character.

  Character spacing

Value	Description
Real number greater than 0.	Set the spacing for text characters (Real number equal to or greater than 0). You can also select this from the Font setting dialog. This value refers to the spacing between the non-displayed boxes which contain the characters, rather than the actual spacing between characters.

 Select font sizes

Value	Description
Select	Displays the Font setting dialog. This contains the text size and spacing criteria that you define for eCADSTAR PCB Editor or Footprint Editor. Select a row in the dialog, and click Apply or OK to apply the settings to the Design Settings dialog. Existing values in the Design Settings dialog are overwritten by the values that you specify.

Origin

Value	Description
(Justification)	Specify the reference point for characters from the following options. The origin is shown as a red point on the image that accompanies each option. Top-Left Top-Center Top-Right Middle-Left Middle-Center Middle-Right Bottom-Left Bottom-Center Bottom-Right

 

 

Dimension Display

Arrow Length L

Value	Description
Real number greater than 0.	Set the length of the arrow "head".

Arrow Angle A

Value	Description
Integer between 1 and 90.	Set the angle of the arrow "head".

Circle diameter D

Value	Description
Real number greater than 0.	Set the diameter of the circle associated with an arrow.

Offset dimension O1

Value	Description
Real number equal to or greater than 0.	Set the offset value shown below for a dimension line.

Offset aux line O2

Value	Description
Real number equal to or greater than 0.	Set the space for starting an extension line from the dimension reference point.

Line width

Value	Description
Real number equal to or greater than 0.	Set the pen width for drawing dimension lines.

Subtract Parameter

Allow isolated figure

Value	Description
Selected	A copper area is generated for an area that becomes isolated as a result of correction.
Not selected	A copper area is not generated for an area that becomes isolated as a result of correction.

Closed area generation

Value	Description
Selected	An area is generated within the target shape, even when the target shape for DRC error avoidance has a loop shape that is created by a closed line.
Not selected	When the target shape for DRC error avoidance has a loop shape that is created by a closed line, an area is not generated within the target shape.

Text viewed as

Value	Description
True shape	The area flood will fill to within the clearance rules of text.
Rectangle	A rectangle is drawn around the extents of the text. This prevents area flood from filling in this area.

Connect to temporary net in component

Value	Description
Selected	Objects that overlap the area to be generated are placed in the same net as the area.
Not Selected	Objects that overlap the area to be generated are handled as targets for DRC error avoidance, and the area is corrected.

Merge distance

Value	Description
Real number equal to or greater than 0.	Specify the distance for which target objects are merged into one object to prevent DRC errors. This is measured between the center points of objects.

Minimum area

Value

Description

Real number equal to or greater than 0.

For new template areas, this setting allows you to specify the minimum area of copper that is generated, by default. If the area of the copper area is less than the specified value, then it is not generated. Specifying a minimum area for template areas allows you to prevent isolated copper areas being generated. If you specify "0", then a minimum area is not defined. If you do not specify a value, then this field is set to "0". Note To set the minimum area of an existing template area, specify a value in the Template Parameters Dialog, Minimum area field. Template areas are created on conductor layers using the Area Fill (Polygon), Area Fill (Rectangle) or Area Fill (Circle) command. Select ON in the Template area field.

 

Gap correction

This setting controls the minimum width of the spacing when the clearance of two objects overlaps and creates a gap.

Value	Description
Selected	When figures are subtracted, the Min. spacing setting within the area fill is maintained. This is shown in the following example. Min. spacing set to 0.2mm Min. spacing set to 0.4mm If Gap correction is selected, then the Min. spacing box is made available.
Not selected	When figures are subtracted, the gap between the area fills is not changed.

Min. spacing

Select whether the clearance within the same area fill uses a rule, or the minimum spacing that you specify.

Value	Description
Rule	The clearance within the same area fill is specified using the rule in the Rule Editor Dialog. The Specified value box is made unavailable.
Specified value	The Specified value box is made available. The value that you enter in this box is used as the minimum spacing within the same area fill.

Specified value

Value	Description
Real number equal to or greater than 0.	When Min. spacing is set to Specified value, enter a value to set the minimum spacing within the same area fill. If you enter "0", default rule specified in the Rule Editor Dialog is used.

Min. width correction

This setting controls the minimum width of a copper pour area between objects, such as two components, or a component and the edge of the template area. It allows you to maintain a minimum width value for these gaps by changing the minimum width value, Min. width. Set this in the Rule Editor Dialog or in the Specified value box below.

Value	Description
Selected	If the Min. width value for gaps within the same area is not sufficient because of the track width used to create the area, then the Min. width value is maintained by changing it for the gap. This is illustrated below using increasingly large Min. width values. Set to 0.1mm: the width between components and the edge of the template area is above the minimum width. Therefore, no changes are made. Set to 0.3mm: the width between components and the edge of the template is below this minimum width. Therefore, changes are made to increase the minimum width of the copper pour area in the positions marked below. Set to 1.0mm: the width between components and the edge of the template is below this minimum width. Therefore, changes are made to increase the minimum width of the copper pour area in the positions marked below. Note In this example, small triangular sections remain because Allow isolated figure is selected in the Template Parameters Dialog. If Min. width correction is selected, then the Min. width box is made available.
Not selected	When figures are subtracted within the same area, the Min. width value of tracks is not changed.

Min. width

Value	Description
Rule	The minimum gap width specified in the Rule Editor Dialog is set as the minimum clearance.
Specified value	The Specified value box is made available. The value that you enter in this box is used as the minimum gap.

Specified value

Value	Description
Real number equal to or greater than 0.	If Min. width is set to Specified value, then enter a value for the minimum gap width. If you enter "0", then the default clearance rule specified in the Rule Editor Dialog is used.

Thermal Relief

Number of lines

Value	Description
Integer greater than or equal to 0, and less than or equal to 12.	Specify the number of thermal lines to be generated.

Track width

Value	Description
Real number equal to, or greater than 0.	Specify the track width of the thermal line to be generated.

Track start angle

Value	Description
Real number equal to or greater than 0, but smaller than 360.	Specify the start angle of the thermal track to be generated.

Additional Spacing

Value	Description
Real number equal to, or greater than 0.	Specify a value for extra spacing between the thermal lines. This is additional to the spacing that is set in the design rules.

Pin

Value	Description
Selected	Thermal lines are generated between both through hole pins and surface mount pins that are in the same net as the conductor area to be generated.
Not Selected	Thermal lines are not generated between either through pins or surface mount pins that are in the same net as the conductor area to be generated.

Via

Value	Description
Selected	Thermal lines are generated between vias that are in the same net as the conductor area to be generated.
Not Selected	Thermal lines are not generated between vias that are in the same net as the conductor area to be generated.

 

 

Online DRC

This section allows you to specify targets for the Online DRC command. This command allows you to automatically check clearances while making changes to a design. See Executing DRC while Editing a Design. The Online DRC section is displayed by clicking Report > Design Rule Checking > Online DRC split button > Online DRC Settings on the eCADSTAR PCB Editor ribbon. Alternatively, select Online DRC split button > Online DRC Settings on the status bar.

 

 

Check Components

Value	Description
Selected	Routing patterns and components are checked.
Not Selected	Only routing patterns are checked. Components are not checked.

Pin Shape

Value	Description
Selected	Clearances of pin shapes on the component are checked.
Not Selected	Component pins are not checked. Clearances of component areas are checked.

Component Position

Value	Description
Selected	Components are checked for the violation of limits on placement side, and placement angle.
Not Selected	The limits on the placement side and placement angle are not checked.

Component placement (manhattan length)

Value	Description
Selected	In a High Speed environment, the manhattan length of pin pairs is checked. Note In Constraint Browser, the actual routed length of the pin pair is checked, rather than the manhattan length. This value is shown in the Actual column, in the High Speed Routing Tab, Pin Pair Length section.
Not Selected	In a High Speed environment, the manhattan length of pin pairs is not checked.

Resist check

 

 

Value	Description
Selected	If selected, then the clearance from resist objects is applied that is set in the Rule Editor Dialog: Non Conductor Tab when adding a copper area. This is done when the Online DRC command is toggled on or off. By default, existing copper areas are not affected.
Not Selected	The clearance from resist objects is not applied when adding a copper area. By default, existing copper areas are not affected.

For same net

Value	Description
Selected	The clearance from resist objects is maintained when routing patterns are edited. However, the following are not checked: Pins. Leads from vias. Resist objects included in a routing pattern.
Not Selected	For a pattern that overlaps with a resist object, lines and areas are not checked that are in the same net.

Via check for same net

Value	Description
Selected	Vias are added or edited while maintaining the clearance from other vias in the same net.
Not Selected	Vias in the same net are not checked with each other.

Hole to hole

Value	Description
Selected	Vias are not added in positions where via holes in the same net cannot keep the via hole clearance.
Not Selected	Vias are not added in positions where via land shapes overlap each other.

Allow stack via

Value	Description
Selected	A via can be added just above or below the via in the same coordinate position, in the same net. Vias cannot be added that have a From-To combination which violates the via combination restriction.
Not Selected	Vias are added while maintaining the clearance from other vias in the same net.

Post Check

This section allows you to specify the parameters for the Post Check command. It is displayed by clicking Report > Design Rule Checking > Post Check split button > Post Check Settings on the eCADSTAR PCB Editor ribbon. Alternatively, select   Post Check split button > Post Check Settings on the status bar. The Post Check command allows you to  allows you to automatically check clearances after you make changes to a design on the canvas. See Executing DRC while Editing a Design.

 

 

Show DRC results after check

Allows you to specify whether DRC errors are displayed immediately after making a change to a design.

Value	Description
Selected	DRC errors are displayed immediately after making a change to a design.
Not selected	DRC errors are not displayed immediately after making a change to a design.

Check Components

Allows you to specify whether DRC errors are displayed immediately after making a change to a design.

Value	Description
Selected	Routing patterns and components are checked.
Not selected	Only routing patterns are checked. Components are not checked.

Cross Probe

For an object that is displayed on the canvas using the Auto Send command, or by clicking a component in the Component Selector dialog, Reference Designator section list. This section allows you to specify its position and size. It is displayed by clicking Design > Cross Probing > Auto Send split button > Cross Probing Settings on the eCADSTAR PCB Editor ribbon. Alternatively, click Auto Send split button > Cross Probing Settings on the status bar. You can also display this section by clicking Cross Probe Settings in the Component Selector dialog.

 

 

Cross Probe

Item		Description
Select only		If an object is selected from outside of the canvas, then its position and size are not changed when highlighted on the canvas.
Centering		If an object is selected from outside of the canvas, then it is highlighted in the center of the canvas. Its size is not changed.
Adjust		If an object is selected from outside of the canvas, then you can specify its size when highlighted on the canvas. This is done using the Adjust ratio (%) box. If Adjust is selected, then this box is made available.
	Adjust ratio (%)	Specify a zoom ratio using an integer between 1 and 100, where 100 is fully zoomed in. This box is made available when Adjust is selected.

Snap

Allows you to configure the Snap function (2D View mode only) in eCADSTAR PCB Editor. This function is used to snap to existing objects on the canvas when running a command. When the position of an object on the canvas is identified, the "Flag" icon is displayed and the cursor is snapped to its coordinates. When the Snap command is toggled on, the following icon is displayed at the cursor position: . This section of the Design Settings dialog is displayed by clicking the Snap split button on the status bar and then selecting Snap Settings.

Snap

Value		Description
Only allow snap point selection		Allows you to specify whether a snapping position must be identified before a relevant command can be run.
	Selected	The relevant command cannot be executed unless a snapping position is identified.
	Not Selected	The relevant command can be executed, regardless of whether a snapping position is identified.
Multiple Pad/Padstack reference points		For a non-circular pad or padstack, this setting allows you to snap only to its center, or to the vertices and mid points of its segments, as well as to its center.
	Selected	For a non-circular pad or padstack, you can snap to its center, as well as to its vertices and the mid points of its segments. These snap points are illustrated below for a rectangular padstack.
	Not Selected	For a non-circular pad or padstack, you can snap only to its center. This snap point is illustrated below for a rectangular padstack.

Arc

Allows you to snap to the middle point, center point or corner point of an arc.

Value	Description
Middle point	If selected, then a flag icon is displayed at the middle point of the arc, and the cursor is snapped to it.
Center point	If selected, then a circle is displayed at the center point of the arc. This enables you to select this position when executing a command.
Corner point	If selected, then a flag icon is displayed at the corner of the arc or tangent arc. This marks the position a vertex would be if the arc was a 90 degree corner. The cursor is snapped to it.

Target layer

Allows you to specify the layer for which the Snap function applies.

Value		Description
Visible layer		The Snap function applies to objects on the visible layer.
Specify layer		The Snap function applies to objects on the layer that you select in the Layer box in the Target layer group. If selected, the Layer box is made available.
	Layer box	Specify the layer for which the Snap function applies.

Objects

Allows you to select the type of object on the canvas for which the Snap function applies.

Value	Description
Type	Select the type of object for which the Snap function applies. The following types of object can be selected. All Pad Padstack Line Area fill / Meshplane Area (Component/Height limit) Hole

Routing

Snap between pins

Value	Description
Selected	Route candidates are displayed between pins, and the rubber band is snapped when the cursor is placed over it.
Not Selected	No route candidate is displayed between pins.

Snap to center

Value	Description
Selected	The route is snapped only to the center between pins.
Not Selected	The route is selected from multiple candidates to be snapped between pins

Space indicator

Value	Description
Selected	A routing space is displayed as a guideline. The space is defined by referencing the following items in sequence: Route to route design rule stack for a different net. Rules by area. Undefined clearance class in the clearance class for signals. The clearance class for the board.
Not Selected	The routing space is not displayed.

No net routing

Value	Description
Selected	Tracks that are not connected to a net can be added on the canvas. This allows you to add a track, and then add a net to it at a later time.
Not Selected	Tracks that are not connected to a net cannot be added to the canvas.

Wide track snap mode

When joining tracks of different width, this setting allows you to specify whether they are snapped to their centers, or to either the center or outline of the narrower track.

Value	Description
Center	When snapping between tracks of different width, the tracks are snapped to their center lines. This is illustrated below.
Outline	When snapping between tracks of different width, the widest track can be snapped to the outline of the narrower track. This is illustrated below. When Outline is selected, you can also snap to the center lines of the tracks.

 

 

Trunking (Advanced)

Routing Parameters

Auto minimize crossed connection

Value	Description
Selected	The order of routes in the trunk is automatically changed so that the number of intersecting unconnected routes at end points is minimized.
Not Selected	The order of routes in the trunk is not changed.

Trunk corner style

Value	Description
Octagonal	The corner that is added at a right angle is chamfered at 45 degrees.
Orthogonal	The corner that is added at a right angle is not changed.
Curved	The corner that is added at a right angle is filleted into an arc.

Trunk width change style

Value	Description
Chamfer	The angle of the route connecting to the via pattern or rule area is set to 45 degrees. The following image shows a route connecting to a via pattern. The following image shows a route connecting to a rule area.
Square	The angle of the route connecting to the via pattern or rule area is set to 90 degrees. The following image shows a route connecting to a via pattern. The following image shows a route connecting to a rule area.

Guide Parameters

End routing area

Value	Description
Selected	The termination routing area is displayed during routing.
Not Selected	The termination routing area is not displayed during routing.

Twist arrow

Value	Description
Selected	An arrow indicating the optimum entry direction that minimizes intersecting unconnected lines is shown at the snapping destination.
Not Selected	The optimum snap direction is not shown.

Snap axis

Value	Description
Selected	Axes are displayed from the center of the leading source and the snapping destination.
Not Selected	The snap axis is not displayed.

Active snap

Value	Description
Selected	When the cursor is placed near the snap axis, the cursor is automatically snapped to the axis.
Not Selected	Even if the cursor is placed near the snap axis, the cursor is not snapped to the axis.

Single click finish on snap line

Value	Description
Selected	When the target symbol is displayed, clicking the snap axis finishes the routing process. The target symbol is displayed when you can accept routing within Snap distance.
Not Selected	Clicking the snap axis does not finish the routing process.

Snap axis length

Value	Description
Small	The snap axis is set to have a short length.
Medium	The snap axis is set to have a medium length.
Large	The snap axis is set to have a long length.

Snap distance

Value	Description
Small	The snap axis is set to have a narrow recognition range.
Medium	The snap axis is set to have a medium recognition range.
Large	The snap axis is set to have a wide recognition range.

Simple trunk view

Value	Description
Selected	The trunk being routed is displayed in a simplified view (only the trunk outline is displayed).
Not Selected	The trunk being routed is displayed in a detailed view (the trunk outline and its inner routes are displayed).

Composition parameters

Angled tracks tolerance

Value	Description
Real number between 0 and 1.0.	Specify the tolerance angle for judging during composition whether or not the routes are parallel.

Spacing tolerance

Value	Description
Real number between 0 and 1.0.	Specify the tolerance for judging during composition whether or not the specified clearance is given between the parallel routes.

Via pattern tolerance

Value	Description
Real number between 0 and 25.4.	Specify the tolerance that is referred to for judging during composition whether the vias are in a group of via patterns.

Ignore via pattern

Value	Description
Selected	Vias are ignored during composition and only a trunk routing pattern is generated.
Not Selected	Vias are also trunked.

Bus Route

Allows you to configure the guide parameters that are used by the Bus Route command.

End Routing Area

Allows you to specify whether an end routing area is added around the destination pins.

Value	Description
Selected	An end routing area is added around the destination pins. This allows you complete the bus routing within a specified distance from the destination pins, rather than at a set, close distance. The Distance from target field is made available, and allows you to specify this distance. In the following image, End Routing Area is selected. The bus routing can be completed from this position.
Not Selected	An end routing area is not added around the destination pins. This means that you must complete the bus routing at a set, close distance form the destination pins. The Distance from target field is made unavailable. In the following image, End Routing Area is not selected. The bus routing can be completed from this position.

Distance from target

This field is made available when End Routing Area is selected. It allows you to complete the bus routing within the distance that you select from the destination pins.

Value	Description
Small	Allows you to complete the bus routing when the bus outline is close to the destination pins.
Medium	Allows you to complete the bus routing when the bus outline is a medium distance from the destination pins.
Large	Allows you to complete the bus routing when the bus outline is a long distance from the destination pins.

Twist arrow

Value	Description
Selected	An arrow is displayed at the routing destination on the canvas that indicates the optimum entry direction for completing the end routing. The recommended direction minimizes the number of intersecting signals. This is illustrated below.
Not Selected	The arrow that indicates the optimum entry direction for completing the end routing is not displayed on the canvas.

Snap axis

Value	Description
Selected	Axes are displayed at 45-degree increments from the center of the end routing destinations. All fields in the Snap axis section are made available.
Not Selected	The snap axes are not displayed. All fields in the Snap axis section are made unavailable.

Active snap

Value	Description
Selected	When you place the cursor near a snap axis, it is automatically snapped to it.
Not Selected	The cursor is not snapped automatically to the snap axis when placed near it.

Single click finish on snap line

Value	Description
Selected	If the target symbol is displayed on a snap axis, then clicking the snap axis finishes the routing process. The target symbol is displayed when you can accept routing within the value specified in the Snap distance field, in this section.
Not Selected	Clicking a snap axis does not finish the routing process.

Snap axis length

Allows you to specify the length of the snap axes.

Value	Description
Small	The snap axis is set to have a short length. This is the average track width multiplied by ten.
Medium	The snap axis is set to have a medium length. This is the average track width multiplied by twenty.
Large	The snap axis is set to have a long length. This is the average track width multiplied by forty.

Snap distance

Allows you to specify the distance from the snap axes at which you can snap to them.

Value	Description
Small	You can only snap to the snap axes when the cursor is half of the medium distance away from them.
Medium	You can snap to the snap axes when the cursor is a medium distance away from them.
Large	You can snap to the snap axes when the cursor is twice the medium distance away from them.

Shielding

Snap

Value	Description
Selected	When a shield is generated, pins, vias and area fills around the shield pattern are connected by lines.
Not Selected	When a shield is generated, nothing is snapped from the shield pattern.

Delete isolation

Value	Description
Selected	Shield patterns are deleted that have become isolated because of shield generation.
Not Selected	Shield patterns that have become isolated because of shield generation are not deleted.

Fillet corner

Value	Description
Selected	Bends in lines are generated as arcs.
Not Selected	Bends in lines are generated as vertices.

Shape around pin

Value	Description
Contour	A shield pattern which follows the shape of the pad is generated around the pin or via.
None	No shield pattern is generated around the pin or via.

Minimum track length

Value	Description
Real number equal to or greater than 0.	A shield pattern longer than the specified value is generated. (Specify the lower limit value of the shield pattern cut by an obstacle.)

Shield merge

Value	Description
Selected	If selected, shield signals are merged into appropriate, existing connections on the board, if possible.
Not Selected	Shield signals are not merged into existing connections on the board.

Teardrops

Teardrops

Maximum Length ratio

Value

Description

Real number equal to or greater than 1.0.

Specify the maximum value for the length ratio of the teardrop. This is the ratio between its length and width, as illustrated below: Length ratio = L / (R1 / 2) This value is used by the Reinforce command when you create teardrops. If DRC errors are produced, then this value is automatically adjusted down to the Minimum length ratio value. If teardrops cannot be created using the Minimum length ratio value, then an error is reported by the Reinforce command. Note If you specify a value in the Minimum length ratio box that is greater than the Maximum length ratio, then the Maximum length ratio value is automatically increased to this value.

Minimum length ratio

Value

Description

Real number equal to or greater than 1.0.

Specify the minimum value for the length ratio of the teardrop. This is the minimum ratio between its length and width, as illustrated below: Length ratio = L / (R1 / 2) If the Minimum length ratio value for teardrops is not met, then the length of the teardrop is extended automatically to include the next segment of the track. If this value is still not met, then the teardrop is not created. Note Teardrops are not extended in this way for tracks connected as follows. Tracks connected to non-circular pads, including square pads or pads with a cut land. Tracks connected to outside the center of a circular pad. If teardrops cannot be created by the Reinforce command without producing DRC errors, then the Maximum length ratio value is automatically adjusted down to this value. If teardrops cannot be created using this value, then an error is reported by the Reinforce command. Note If you specify a value in the Minimum length ratio box that is greater than the Maximum length ratio, then the Maximum length ratio value is automatically increased to this value.

 

Minimum line width ratio

Value	Description
Real number greater than 1.0.	Specify the minimum value for the ratio between the widest and narrowest widths of the teardrop. A teardrop is created when the following condition is satisfied: Widest width (R1) / Narrowest width (R2) >= Minimum line width ratio. This is illustrated below.

Target

Surface mount pin

Value	Description
Selected	Teardrops are generated on surface mount pins.
Not Selected	Teardrops are not generated on surface mount pins.

Through hole pin

Value	Description
Selected	Teardrops are generated on through hole pins.
Not Selected	Teardrops are not generated on through hole pins.

Via/Pad

Value	Description
Selected	Teardrops are generated in the via/pad.
Not Selected	Teardrops are not generated in the via/pad.

Via Spirals

This section allows you to configure the settings for spiral vias.

Angle start

Value	Description
An integer between 0 and 359.	Specify the start angle between the track and the first via. Note 0 degrees is horizontal, at the 3 o'clock position.

Angle increment

Value	Description
An integer between 0 and 359.	For the angle of the track to be connected to the second and subsequent vias that are generated: specify the amount by which this angle is incremented, compared to the previous track. The angle is incremented counter-clockwise from the 3 o'clock position.

Track length

Value	Description
Real number equal to, or greater than 0.	Specify the minimum distance between consecutive vias. The distance is the center-to-center spacing in each via.

Lengthen

This section allows you to specify the settings that are used by the Lengthen command. For the lengthening that is added to a routing pattern, select the meander mode and edge style, and specify the maximum size and minimum space. The specified settings are overridden by the settings in the Lengthening tab, in the Constraint Browser: Signals section, Signals tab or Constraint Browser: Signals section, Classes/Groups tab for a selected E-Net or E-Net class.

Meander mode

Value	Description
Accordion	Lengthening is added to a selected routing pattern using the accordion style. This is illustrated below for the square edge style. Specify the "Maximum size" and "Minimum space" settings shown above using the Max. size and Min. space fields, respectively, in this section.
Trombone	Lengthening is added to a selected routing pattern using the trombone style. This is illustrated below for the square edge style. Specify the "Maximum size" and "Minimum space" settings using the Max. size and Min. space fields, respectively, in this section.

Edge style

Value	Description
Square	The angle of the segment end of the lengthen pattern is set to 90 degrees. This is illustrated below for the Accordion meander mode. This is illustrated below for the Trombone meander mode.
Chamfer	The angle of the route segment end of the lengthen pattern is set to 45 degrees. This is illustrated below for the Accordion meander mode. This is illustrated below for the Trombone meander mode.
Semicircle	The shape of the route segment end of the lengthen pattern is set to an arc. This is illustrated below for the Accordion meander mode. This is illustrated below for the Trombone meander mode.

Max. size

Value	Description
Real number equal to or greater than 0.	Set the maximum length applied between parallel routes when lengthening a routing pattern. This is illustrated below for the Accordion meander mode. This is illustrated below for the Trombone meander mode.

Min. space

Value	Description
Real number equal to or greater than 0.	Set the minimum space applied between parallel routes when lengthening a routing pattern. This is illustrated below for the Accordion meander mode. This is illustrated below for the Trombone meander mode.

Re-lengthen at the end of interactive operations

Value	Description
Selected	For signals that have length constraints set, the lengthening patterns are reapplied after interaction with the signals in the design. This maintains the integrity of the lengthening pattern, and ensures that the length constraints are met. In a High Speed environment, this is done at the end of the following operations. Manual routing Moving tracks Trunk routing Interactive lengthening using the Lengthen command. Re-lengthening occurs only if Push Aside is selected in the Lengthen dialog, and other tracks are actually pushed.
Not selected	For signals that have length constraints set, the lengthening patterns are not reapplied after interaction with the signals in the design.

 

This dialog is used by the following commands.

Linear Dimension (Single)

Linear Dimension (Series)

Linear Dimension (Parallel)

Linear Dimension (Increment)

Dimension Line (Diameter)

Dimension Line (Radius)

Leader Dimension (Polygonal Line)

Angle Dimension (Angle)

Angle Dimension (Arc Length)

Area Fill (Polygon)

Area Fill (Rectangle)

Area Fill (Circle)

Cutout (Polygon)

Cutout (Rectangle)

Cutout (Circle)

Reshape

Fillet

Chamfer

Merge

Divide

Subtract

Offset

Add Route

Move Track

Unroute

Lengthen

Regulate Trunk

Reinforce

Generate Shield

Chamfer Route

Fillet Route