Allegro绘制PCB流程

2019-07-14 07:23发布


单位换算 1mil = 0.0254 mm 1mm = 39.3701 mil 默认情况下我们更倾向于使用mil单位绘制PCB板。   1 新建工程,File --> New...   --> [Project Directory] 显示工程路径   --> [Drawing Name] 工程名称,Browse...可选择工程路径   --> [Drawing Type] 工程类型,绘制PCB板选择Board,封装选择Packagesymbol   2 设置画布参数,Setup --> Design Parameters...   --> [Design]       单位为Mils,Size为other,2位精度,       Width与Height分别代表画布的宽高       LeftX与LowerY代表原点位置坐标   点击Apply使修改生效   --> [Display]       勾选Gridon, 打开SetupGrids...       将Non-Etch和AllEtch中的所有Spacing设为1mil=0.0254mm   3 设置库路径,Setup --> User Preference...   将所有绘制好的元件封装复制到同一目录下,方便设置库目录,   --> [Paths]       --> [Library] 指定modulepathpadpath parampath psmpath到封装所在目录   4 绘制板框,Add --> Line   Class:SubClass = Board Geometry:Outline   5 倒角,Manufacture -->Dimimension/Draft --> fillet   倒角半径(Radius)参考:100mmx100mm板倒角100mil~200mil   分别点击倒角的两条边完成倒角   6 设置允许布线区,Setup --> Areas --> RouteKeepin   Class:SubClass = Route Keepin:All   一般情况,RouteKeepin距离板框0.2mm(8mil)~0.5mm(20mil)     方法2:使用Z-Copy命令,Edit-Z-Copy       选择Class:SubClass=RouteKeepin:All,       Size选择Contract向内缩进,Offset填充20mil,       点击板框完成复制,此方法亦使用步骤7   7 设置允许元件摆放区,Setup --> Areas --> PackageKeepin   Class:SubClass = Package Keepin:All   一般情况,PacakgeKeepin与RouteKeepin大小一致     方法2:使用Z-Copy命令   8 放置机械安装孔,Place --> Manual   --> [Advanced Settings] 勾选Library   --> [Placement List]       --> [Mechanical symbols] 选上需要使用的机械安装孔,敲坐标放置     注:使用“选择多个元件,右键Align components”对齐元件。   9 设置层叠结构,Setup --> Cross-section   双层板按默认设置,从上到下依次为:表层空气,铜走线Top层,玻璃纤维介质层,铜走线Bottom层,底层空气   多层板需要做相关层添加[FIXME]   10 导入网表, File --> Import -->Logic...   --> [Cadence] 选择Designentry CIS(Capture),Always,Importdirectory选择网表文件路径    导入完成后File--> Viewlog...查看导入错误信息,确保0 errors,0warnings   11 放置元器件,Place --> QuickPlace...   选择Placeall components,点击place完成自动放置   检查Unpalcedsymbol count显示状态,确认未放置的元件为0     注:有关元器件突出板框外的KC DRC问题 <--- 删除该DRC       Display --> Waive DRCs --> Waive命令,点击DRC删除即可。   12 约束设置,Setup --> Constraints -->Constraints Manager...   --> [Physical]       --> [Physical Constraint Set]           --> [All Layers]               线宽设置为>=6mil,添加过孔(小于6的非0值都设为6或更大)       --> [Net]           --> [All Layers]               电源与地网络设置至少30mil,大功率大电流网络也设置大些   --> [Spacing]       ... 设置线间距、VIA间距等,都至少设为6mil,6mil是根据PCB厂家定的   13 布局布线   接插件(如DB9、JTAG接口、电源接口等)放在PCB板周边;   。。。     布线时双击添加过孔,Options中Act可改变当前PCB面,Linewidth设置线宽;   [Route] --> [PCB Router] --> [Route Automatic…]可自动布线;   。。。   14 添加丝印   (1)自动添加丝印       Manufacture --> Silkscreen         --> [Layer] Both         --> [Elements] Both         --> [Classes and subclasses]         --> [Package geometry] Silk         --> [Refrence designator] Silk         ... 其它选择None   点击Silkscreen完成丝印添加     (2)手动添加丝印信息       --> Add --> Text       Class:Subclass=Manufacture:AutoSilk_Top       设置字号及线宽后输入文字信息     注:丝印字号修改,Edit--> Change,Find中选只Text,       Class:subclass=Manufacture:空       设置字号线宽,全选后Done即可   15 添加覆铜,Shape --> Polygon   Class:Subclass=Etch:Top   Option中勾选上CreateDinamic Shape,选择Assign netname为Gnd网络     添加底层覆铜,Class:Subclass=Etch:Bottom     删除顶层和底层死铜,Shape--> Delete Islands,Delete allon layer   16 查看报告,Tools --> Quick Reports   至少检查如下4项:   Unconnected Pins Report   Shape Dynamic State   Shape Islands   Design Rules Check Report   17 数据库检查,Tools --> Database Check   勾选全3项,点击Check检查,Viewlog查看错误日志   18 钻孔文件生成   (1) 钻孔参数文件生成,Manufacture--> NC --> NC Parameters   按默认设置,点close后生成nc_param.txt     (2) 钻孔文件生成,Manufacture--> NC --> NC Drill   如果有盲孔或埋孔,则Drilling中选择By Layer,否则默认,   点Drill生成*.drl文件,点击Viewlog查看钻孔文件信息     (3) 不规则孔的钻孔文件生成,Manufacture--> NC --> NC Route   默认设置,点击Route生成*.rou文件     (4) 钻孔表及钻孔图的生成,Manufacture--> NC --> Drill  Legend   如果有盲孔或埋孔,则Drilling中选择By Layer,否则默认(单位为mil),   点击OK生成*.dlt文件   19 生成光绘(Gerber)文件   (1) 设置光绘文件参数,Manufacture--> Artwork       --> [General Parameters]           --> [Device type] Gerber RS274X           --> [OUtput units] Inches           --> [Format]               --> [Integer places] 3               --> [Decimal places] 5       --> [Film Control] 设置层叠结构(10层)           -->[Available films]               --> [Bottom]                   --> ETCH/Bottom                   --> PIN/Bottom                   --> VIA Class/Bottom               --> [Top]                   --> ETCH/Top                   --> PIN/Top                   --> VIA Class/Top               --> [Pastemask_Bottom]                   --> PackageGeometry/Pastemask_Bottom                   -->Stack-Up/Pin/Pastemask_Bottom                   -->Stack-Up/Via/Pastemask_Bottom               --> [Pastemask_Top]                   --> PackageGeometry/Pastemask_Top                   -->Stack-Up/Pin/Pastemask_Top                   -->Stack-Up/Via/Pastemask_Top               --> [Soldermask_Bottom]                   --> Board Geometry/Soldermask_Bottom                   --> PackageGeometry/Soldermask_Bottom                   -->Stack-Up/Pin/Soldermask_Bottom               --> [Soldermask_Top]                   --> BoardGeometry/Soldermask_Top                   --> Package Geometry/Soldermask_Top                   -->Stack-Up/Pin/Soldermask_Top               --> [Silkscreen_Bottom]                   --> BoardGeometry/Silkscreen_Bottom                   --> PackageGeometry/Silkscreen_Bottom                   -->Manufacture/Autosilk_Bottom               --> [Silkscreen_Top]                   --> BoardGeometry/Silkscreen_Top                   --> PackageGeometry/Silkscreen_Top                   -->Manufacture/Autosilk_Top               --> [Outline]                   --> Board Geometry/Outline               --> [Drill]                   --> Board Geometry/Outline                   -->Manufacture/Nclegend-1-2           选中Checkdatabase before artwork复选框!           --> [Film options]               --> [Undefined line width]                   选中层叠结构中的每一层,都设置为6mil               --> [Shape bounding box]                   选中层叠结构中的每一层,都设置为100               --> [plot mode]                   选中层叠结构中的每一层,无特殊情况都选择Positive               --> [Vector based pad behavior] 选中每一层都勾选上   点击OK完成参数设置                                 (2) 生成光绘文件,Manufacture--> Artwork   仔细检查层叠结构的设置,很重要,不能出错!   Select all选择所有层,确认选中Check database before artwork,   执行CreateArtwork生成光绘文件,点击Viewlog查看生成光绘信息,确保没有任何error!   20 打包Gerber文件给PCB厂商   共14个文件:10{*.art}+ 1{*.drl} + 1{*.rou} + 2{*.txt}   TOP.art   Bottom.art   Pastemask_Top.art   Pastemask_Bottom.art   Soldermask_Top.art   Soldermask_Bottom.art   Silkscreen_Top.art   silkscreen_Bottom.art   Outline.art   Drill.art   art_param.txt   nc_param.txt   *.rou   *-1-2.drl     打包成*.rar等压缩包发给厂商