Padstack Editor 17.4

前言

Padstack Editor 是SPB17.X中出现的新内容。找到的资料都是SPB16.X的，和17.X对不上。以前学了一次Cadence, 用ORCAD画原理图没问题。到了建立焊盘这里，卡住了。以前工作忙，没条件学下去，这次用了3天，弄懂了。

但是找到的资料，是面向新手的。细节上有点疑问和不解。

尝试找一下Cadence17.4中的Padstack Editor的官方文档，找到了。
做个笔记。

文档位置

D:/Cadence/SPB_17.4/doc/pcoms/pchap.html
搜索 ”Pad Editor“，如下:

焊盘用途(种类)

可选的焊盘用途一共12种.

1. Thru Pin

Specifies that the padstack penetrates all layers. This is the default padstack type. You must specify the drill hole parameters for the through padstack type.

Thru Pin 是通孔焊盘，默认的焊盘就是通孔，需要指定钻孔参数。

2. SMD Pin

Specifies that the padstack is for only one layer. You usually use this option for SMT pads.

SMD Pin 是表贴焊盘(只有一面有焊盘)

3. Via

Specifies a plated through hole.

Via 是过孔焊盘（是为了连同不同层的电路连接，而不是为了焊接元件引脚）

4. BBVia

Specifies that the padstack is blind (navigates the surface and internal layers) or buried (traverses internal layers).
When creating a blind or buried padstack, layers to be excluded must have their pads removed. Pad information must exist on a given layer to be considered drilled to that layer. The criterion for connectivity is the existence of a pad definition on the subclass. The connectivity model for any padstack reads all/any type pad information defined in the padstack, and both the model and the add connect command interpret the existence of a pad of any type (thermal, antipad or regular) as a legal layer for a connection. When an outer subclass is missing a regular pad, it is still considered a thru drill when it contains some pad information. If all pad data is missing, then the layer is not considered drilled, and it is a candidate for blind/buried via status. No connection is available on layers with no pad definitions.

BBVia 是盲埋孔焊盘. 高级复杂的多层板才会用到.

5.Microvia

Specifies a blind or buried via as a microvia, defined by the IPC – Association Connecting Electronics Industries as less than or equal to 0.15 mm or 5.91 mils in diameter, with a pad diameter less than 0.35 mm or 13.8 mils formed by laser or mechanical drilling, wet/dry etching, photo imaging, or conductive ink-formation followed by a plating operation.Enables the padstack to be used for HDI features, including advanced DRC. Use on HDI boards where spacing rule sets differ between HDI and conventional blind/buried or core vias. Only applicable to a blind/buried via type, which should be used to represent mechanical drilled vias, such as the core via on an HDI design. The two via types are supported in the Spacing and Same Net Spacing Constraint domains of Constraint Manager.Note: In Allegro PCB Design L, OrCAD, and Allegro PCB Performance option L, a padstack remains classified as a microvia, but any action based upon this padstack type is ignored, as pad_designer is an unlicensed tool. DRC treats microvias as blind and buried vias and uses blind and buried rules for reporting, possibly resulting in more DRCs if the blind and buried rules spacing requirements are larger than those for microvias. If a design with microvia DRCs is opened in a non-microvia tier, those DRCs are maintained and reported as microvia DRCs. Any operations that affect those DRC'ed objects (for example. drcupdate) deletes these DRC and possibly replaces them with a blind and buried via DRC. This DRC model follows the current electrical DRC tiering model.

Microvia 是微通孔焊盘。微的定义是孔内径小于5.91mil, 或焊盘外径小于 13.8mil.

6.Slot

Species a slotted hole.

Slot 是槽型孔

7.Mechanical Hole

Mechanical Hole 是机械孔（是机械孔的一种，和电气无关）

8. Tooling Hole

Tooling Hole 是工装孔（是机械孔的一种，和电气无关）

9.Mounting Hole

Mounting Hole 是安装孔（是机械孔的一种，和电气无关）

7,8,9这3种孔都是机械孔，只是用途上有细微区别，请参考 http://ipc2581.com

10.Fiducial

Specifies a fiducial pad on the beginning or end layer.

Fiducial 是基准焊盘(只在顶层或底层上出现，可以理解成mark点)，给贴片机用的。

11.Bond Finger

Specifies a padstack on one layer, either beginning or end. Select this if you are working with wire bond dies.

Bond Finger 是键合焊盘，给IC设计用的，应用层的PCB用不到。

12. Die Pad

Specifies a padstack for a die on one layer, either beginning or end.

Die Pad 是裸焊盘，给IC设计(邦定)用的，应用层的PCB用不到。

焊盘种类小结

应用层的焊盘有10种(1~10)
IC设计的焊盘有2种(11~12)

焊盘形状(几何图形)

焊盘形状共9种。

1.Circle

Requires a diameter.

圆形焊盘，需要给定一个直径

2.Square

Requires a width.

正方形焊盘，需要给定一个宽度

3.Oblong

Requires width and height.

椭圆长方形焊盘，需要给定宽度和高度

4.Rectangle

Requires width and height.

纯长方形焊盘，需要给定宽度和高度

5.Rounded Rectangle

Requires width, height, and a corner radius. You can select one or more corners. By default, all four corners are selected.

长方形圆角焊盘，需要给定宽度，长度，圆角半径。4个圆角的半径可以单独指定(可以指定每个角是否为圆角，默认是4个角都是圆角)

6.Chamfered Rectangle

Requires width, height, and length of the chamfers. You can select one or more corners. By default, all four corners are selected.

长方形倒角焊盘。需要给定宽度，长度，倒角边长。可以指定每个倒角的长度。默认4个倒角长度都是一样的。

7.Octagon

Requires width.

正八边形焊盘，需要给定宽度。

8.Donut

Requires a inner and outer diameters. You can use this geometry for fiducials and mounting holes where contact with a chassis ground may be required. This pad geometry uses a different connectivity model (touch vs. connect point) from all other pad geometries.

环形焊盘，需要给定内径和外径。

9.n-Sided Polygon

Requires diameter and number of sides. This can be used in applications related to vectoring of pad figures when exporting artwork data for manufacturing (Stream data).The number sides must be even.

正多边形焊盘，需要给定直径和边数，边数必须是偶数。

设置焊盘数值的单位和精度

做一个贴片焊盘的步骤

假设这个贴片焊盘的size = 1.2mm * 0.2mm

选择焊盘类型(表贴焊盘)，焊盘形状（长方形）

孔的类型
表贴焊盘没有孔，选择为NONE

Secondary Drill / Drill Symbol / Drill Offset 页面对于表贴焊盘都不可操作。

Design Layers

Design Layers 页面用来填写焊盘尺寸，焊盘位置偏移，正片规则焊盘尺寸，散热焊盘尺寸，负片焊盘尺寸，焊盘禁止区尺寸。

Layer Name

Layer Name: Displays all the layers of your padstack, with the corresponding Regular Pad, Thermal Relief, Anti Pad and Keep Out definitions. You can edit any of the white fields. Begin and End layers are the outer layer pads: in a .brd file, the Top and Bottom; in an .mcm file, Surface and Base. Default internal is used for through-hole inner layer pad data.

Layer Name ：padstack所在层的名称。

对于表贴焊盘，可在的层为顶层或底层。

Regular Pad

Regular Pad: Specifies a positive pad with a regular shape flashed on positive layers only. Through hole pads require regular pad geometries be defined for every board layer. Surface mount pads require only Top and related Top mask information. Non-standard shaped pads are available as pad shapes and as pad flashes.

Regular Pad 是正片焊盘

Thermal Pad

Thermal Pad: Specifies either a positive or a negative pad. A positive thermal relief connects pins to a positive copper area or to an embedded plane that prevents heat from concentrating near a pin or via during the unsoldering process. The thermal relief definition also may connect a pad to a copper area created on a routing layer, such as an external shield.
A positive plane thermal relief comprises a “spoked wheel” pattern, which combines the regular positive pad, void areas, and tie bars, the latter two of which are defined in the Shape Parameters dialog box.
A negative thermal relief is defined by a flash symbol used to connect pins to a negative copper area. The thermal relief may be plotted as a regular pad flash combined with the thermal values used as the shape-to-pad clearance.

Thermal Pad 是散热焊盘

Anti Pad

Anti Pad: Specifies a negative pad (clear, surrounded by black), where the size and type determine pad flashes for negative planes, or pad sizes for clearances when specified in positive shape parameters. Used to disconnect pins from a surrounding copper area.

Anti Pad 是负片焊盘

Keep Out

Keep Out: Specifies an area around pad in which placing ETCH/CONDUCTOR, vias, or other symbols are restricted.

Keep Out 是焊盘周围的禁止层区域

对于一个焊盘，正片规则焊盘(Regular Pad) / 散热焊盘(Thermal Pad) / 负片焊盘(Anti Pad) 只能选一种。
即一个焊盘是正片焊盘或散热焊盘或负片焊盘的一种。不可能是3种焊盘类型的组合。

但是这3个参数都要填写，参数不能缺(不要空在那里)，让cadence根据焊盘实际用途来选择这3种焊盘中的一种。

每个焊盘都有禁止层（Keep Out）

填写正片焊盘参数

点击正片焊盘格点，然后在下方出现的焊盘形状列表中选择焊盘形状，然后填写焊盘参数。

填写剩下的焊盘参数

填写散热焊盘(Thermal Pad) / 负片焊盘(Anti Pad) /禁止区域(Keep out), 填写步骤和正片规则焊盘(Regular Pad)一样。

可以在填好的正片焊盘格点选择右击菜单 => Copy, 然后在其他格点右击菜单 => Paste, 这样快一些。

正片焊盘的尺寸比元件数据表上的尺寸大0.2mm
散热焊盘尺寸可以和正片尺寸一样。
负片焊盘尺寸比正片焊盘大0.1mm
禁止层尺寸比负片大0.2mm

焊盘参数都填好的样子

Mask Layers

Mask Layers 是掩膜层，也就是阻焊区域参数和锡膏区域参数。

将正片规则焊盘的参数拷贝粘贴到顶层阻焊和顶层锡膏参数格点中。
顶层锡膏参数和正片规则焊盘是一样的，
顶层阻焊参数比顶层锡膏参数大0.1~0.2mm。
填好的掩膜层参数如下：

FILMMASK_X COVERLAY_X 层参数是可选的，不用填写。

做好的焊盘参数预览

如果发现自己填写的焊盘参数不对，可以去前面几个TAB页进行修改

保存填好的焊盘参数为磁盘文件

焊盘文件名称中不能包含’.'字符，可以用d来代表‘.’
焊盘命令要能见名知义（通孔/表贴焊盘? 焊盘形状? 顶层/底层? 焊盘尺寸? …）, 方便自己后面做封装时，选择合适的焊盘文件。

保存到磁盘上的焊盘文件的样子

通孔焊盘的例子

做一个圆形通孔焊盘，拿一个1/4W的插装电阻用的焊盘为例。
可知 d = 0.54mm

单位选mm, 精度2位。

选择焊盘种类为通孔，焊盘形状为圆形。

钻孔参数 : 钻孔形状为圆形, 外径填写0.56mm(比 d = 0.54mm 大0.2mm)

背钻和沉头/埋头孔参数不用填。

钻孔符号的焊盘选圆形，名称为d(自己随意命名)，钻孔直径为0.56mm.

钻孔偏移不用改，就为默认的0，0

设计层
这里和前面做表贴的参数填写方法一致。
不同点是还要填写底层参数(因为通孔在底层和顶层都有焊盘，而表贴焊盘只在一面有焊盘)

值得注意的是，设计层的尺寸必须要大于钻孔层尺寸，就是在钻孔层尺寸上，加上焊盘的边(手工焊接的焊盘边)，否则只有钻孔，没有焊接的环边。
从左边的预览也可以看出来，如果设计层尺寸和钻孔层尺寸一样，做出来，只是一个孔，而不是焊盘。

将设计层尺寸改的比钻孔层大，e.g. 加0.2mm, 在预览中，就能看到，做出的东西是一个焊盘(有孔，有环形焊边)，如下

具体焊盘的焊接环边填多少合适，可以参考AD的焊盘尺寸。或者参考手头的已有AD工程，
因为在AD的封装制作中，焊盘尺寸直接指定的，并不需要单独先制作焊盘封装。

也可以参考前辈同学写好的焊盘参考建议，e.g 如下

1mm = 39.3mil
0.1mm = 3.9mil
12mil = 12 / 3.9 = 3 * 0.1 = 0.3mm
所以焊接环边的宽度，至少要宽度为0.15mm才行。要在钻孔直径上至少加0.3mm.

我这里就不改了，就按照钻孔直径 + 0.2mm算.

掩膜层
阻焊尺寸和锡膏尺寸也要比钻孔尺寸大。
其中阻焊尺寸要大于锡膏尺寸。

执行检查

出现警告报错提示框
看提示，默认内层要填东西。将顶层参数都拷贝过来填入默认内层。

再检查，没有错误了。

存盘保存成焊盘文件。

具体焊盘是否做的合适，需要做封装，做板子，打样后看看效果。不行就再调整。但是 SPB17.X开始独有的Padstack Editor的用法，基本就是这样。

总结

大厂的软件自带的帮助文件(本地文档，官网文档)做的比较详细(原因:用户多，收费, 有需求将文档做细做全，减少人工技术支持的成本)。

对于新手，在找到教程或资料时，如果有疑问的时候，可以参考一下官方资料，对细节会有新的认识。不至于只能被动吃前辈同学们已经嚼碎然后吐出来喂给大家的的零食。

我们在看官方文档和做实验的过程中，也许能发现一些新的细节。即使发现不了，对习得的技能也理解的比较深刻。