- 易迪拓培训,专注于微波、射频、天线设计工程师的培养
怎样设置一个局部的布线约束？
录入：edatop.com 点击：
各位大侠，因为主处理芯片BGA封装，需要走比较细的线，而其它部分又想把线及间距拉大点，局部能单独设置布线约束吗?谢谢！
constraint area
谢谢二楼！问题是不知道给怎么设置constraint area?希望哪位大侠能不吝赐教！谢谢！
How to set up a constraint region in 16.2.
Lets say we want to create a spacing region:
Open constraint manager and create a Spacing Rule set for the constraint region.
1. Open Constraint Manager on the board file.
2. Select Spacing > All Layers worksheet
3. RMB on the Objects and select Create Spacing CSet
4. Type the name of Spacing CSet and change the pin to pin constraints that allow
pin to pin spacing for the 'special' component.
Now create a region and assign a spacing CSet to the region.
1. In Constraint Manager, select Region > All Layers
2. RMB > Create Region
3. Give a name to the region, and select Ok.
4. On the Region worksheet, select the region that you just created, and assign
the Spacing CSet that you had created in the previous step. The rules of the
spacing CSet are automatically taken over by the Region.
Now create a Shape on Constraint Area subclass and assign the region rules to it.
1. On Allegro, Select Shape > Polygon or Rectangular.
2. In the Options panel on the Right hand side, select the Class as Constraint
Region > All.
3. From the drop down in the options panel, select the Region you had defined in
the previous step.
4. Draw the rectangle or polygon around the component.
setup->constraints,在弹出对话框内的constraints areas单击add按钮，在电路板上做出需要做约束的区域，单击add对话框下面的attach propperty,shape按钮，在FIND中选择SHAPE，单击刚刚做好的约束区域，在弹出的EDIT PROPERTY对话框的AVIAILABLE PROPERTY中选择NET PHYSICAL_TYPE并添加属性，单击APPLY完成。
接下来在setup->constraints,在弹出对话框内的PHYSICAL RULE SET中设置物理属性，再到physiacl RULE ASSIGNMENT TABLE中将刚刚建好的规则分配给你做好的约束的区域就OK了
