[技术文章]Assigning Constraints [复制链接]

上一主题下一主题查看指定楼层

离线nuoan

一级逆天

性别:: 人妖

发帖: 20

金币: 3

提示：会员销售的附件,下载积分 = 版块积分 + 销售积分只看楼主倒序阅读使用道具 0楼发表于: 2017-11-18

PCB设计软件安装包汇总-点击这里所有版本软件都有了

Assigning constraints to your design allows you to easily control and verify
critical design areas. Constraint types include clearance, routing, and high-speed
rules that can be assigned to nets, layers, classes (collection of nets), groups
(collection of pin pairs), or individual pin pairs. You can also assign a default set
of design rules that apply to all objects not having a unique rule.
In this lesson:
Ÿ Setting default clearance rules
Ÿ Setting net clearance rules
Ÿ Setting conditional rules
Restriction
This tutorial requires the Advanced Rules (for the Conditional Rules section) and
General Editing licensing options.
To determine whether you can proceed:
Ÿ On the Help menu, click Installed Options.
Preparation
If it is not already running, start PADS Layout and open the file named
previewnet.pcb found in the \PADS Projects\Samples folder.
Setting Default Clearance Rules
You can define clearance, routing, and high-speed rules for each level of the
design rule hierarchy.

Setting default clearance rules
The Clearance area of the Clearance Rules dialog box contains a matrix of PCB
design data. You can specify values for each or all data types in the matrix.
1. Setup menu > Design Rules > Default button.
2. Clearance button.
3. Click All (in the upper-left corner of the Clearance matrix) to set a global
default clearance value.
4. In the Input Clearance Value dialog box, type 8 and click OK.
5. In the Trace Width area, type 6 in the Minimum box, type 8 in the
Recommended box, and type 12 in the Maximum box.
6. Type 12 in the Same Net and Other clearance text boxes, with the exception
of Trace to Crn box. Set this box to 0.
7. Click OK.
Set default routing rules
To avoid routing on the plane layers, remove them from the Selected routing
layers as defined in the routing rules. The Layer Biasing area of the Routing
Rules dialog box contains a list of selected routing layers. This list lets you
specify which layers are permitted for routing.
1. Routing button.
2. In the Layer biasing area, in the Selected Layers list, select the Ground
Plane, press and hold Ctrl and click Power Plane to add them to the selection.
3. Click Remove to prevent routing on the plane layers.
4. Click OK to close the Routing Rules dialog box.
5. Click Close to close the Default Rules dialog box.
Setting net clearance rules
You can assign net-specific clearances that take precedence over the default
rules previously entered.
1. Net button.
2. Scroll through the Nets list. Ctrl+click to select +5V, +12V, and GND. The
three selected nets appear beside Selected, under the rule type buttons.
3. Click the Clearance button to set the same clearance rules for all three nets.
4. In the Clearance Rules dialog box, click All (in the upper-left corner of the
matrix) to set a global clearance value.
5. In the Input Clearance Value dialog box, type 10 as the global clearance and
then click OK.
6. In the Trace Width area, type 10 in the Minimum box, type 12 in the
Recommended box, and type 15 in the Maximum box.
7. To complete the definition, click OK in the Clearance Rules dialog box.
8. Click Close to close the Net Rules dialog box.
See also: PADS Layout Help for details about defining other Hierarchy rules.
Setting conditional rules
When two nets require a specific clearance between each other (to avoid adverse
effects on the circuitry), you must define a conditional rule. An example of a
conditional rule might be the Underwriters Laboratories (UL) requirements of
segregating primary, secondary, and ground nets when alternating current is
directly connected to the PCB. You can assign conditional rules between most
components of the design rule hierarchy. Conditional rules can exist between
nets, nets and classes, classes and pin pairs, nets on a specific layer, and so on.
To assign a net-to-net conditional rule:
1. Conditional Rules button.
2. In the Source Rule Object area, click Nets.
Result: A list of nets appears in the Source Rule Object list.
3. Select net +5V.
4. In the Against Rule Object area, click Nets.
Result: A list of nets appears in the Against Rule Object list.
5. Select net +12V.
6. Click Create to define the conditional rule. The new rule appears in the
Existing Rule Sets area.
7. In the Current Rule Set area, type 25 in the Object to Object box.
8. Close all of the open dialog boxes.
Result: The rule you just created will keep all objects pertaining to the +5V
and +12V nets 25 mils apart.
9. Do not save a copy of the design.