下载

    看看哪些下载,最适合您的需求

      如何购买

      请联系当地销售网点,提升您的设计环境

                        • Altium Designer

                          专业统一的设计系统,高效轻松的环境和原生态3D PCB编辑器

                        • Altium数据保险库

                          ECAD设计数据、库、工作流程和团队管理的一体化平台

                        • Altium年度客户服务计划

                          Altium产品不断更新,为您提供最新技术

                        • TASKING

                          世界知名的 卓越编译技术,TASKING工具已有超过25年的历史。

                        • 产品扩展

                          衍生工具,系统分析,新设备以及Altium产品设计流程的扩展支持

                        • Altium DXP开发平台

                          创建并设置自定义扩展,为Altium产品集成业务系统

                        • Octopart

                          快速、精准和简单地使用元器件搜索,连接您与元器件数据和供应链的纽带。

                        Altium Designer 16

                        轻松的原生3D PCB设计

                        年度客户服务计划

                        始终使用最新科技保持高效率设计

                        • 论坛

                          Altium用户与发烧友的互动平台

                        • 博客

                          我们的博客展示我们关注的领域,希望同样也能激起您的兴趣

                        • 创意

                          为Altium工具新功能开发提交您的创意并参与投票

                        • Bug 提交

                          通过提交Bug,对重要事项进行投票,帮助提升软件性能

                        • 微博墙

                          您订阅的AltiumLive,邀您一起参与关注

                        • 测试项目

                          参与我们的测试项目,更早获取Altium最新版

                        下载

                        看看哪些下载,最适合您的需求

                        客户成功案例

                        我们的用户正在改变着各行各业,了解详情

                        如何购买

                        请联系当地销售网点,提高您的设计环境

                        • 文档

                          您在TechDocs上,可以找到大量在线的免费文档

                        • 培训与活动

                          查看时间表,注册遍布全球的线上及线下的培训和活动

                        • 设计内容

                          浏览我们免费的大容量设计内容库,其中包括元器件,模板和参考设计

                        • 网络研讨会

                          在线参加网络研讨会或观看我们以往的研讨会视频。

                        • 技术支持

                          使用多元化的技术支持模式及自助服务选项来解决您的问题。

                        • 视频库

                          简洁明了的指导视频教程,帮助您启程Altium Designer

                        如何使用CAD原理图绘制电缆装配:第2部分

                        By Sainesh Solanki, Dec 31, 1969

                        Creating the library components

                        The first step is to collect the necessary information needed to create a cable head assembly:

                        • Connector Head data sheets.
                        • Crimp information and drawings.
                        • Cable data.
                        • Heatshrink data.

                        Additional tools may be required to assemble the cable, but that will be saved for a later discussion. For now, we have taken note on what is required to create the library parts for drawing the cable assembly. We will start by creating a multi-part component for each connector head. The first part in this multi-part schematic component will be the graphical diagram of the connector head, which provides the visual representation for the assembly drawing. Figure 1 shows an example of how this will be styled, and will be scaled 1:1 with the real physical part.

                        Figure 1.  1:1 drawing of the connector head

                        The second part in the multi-part schematic component, will be the traditional IEEE-315 style electrical schematic symbol for the multi-position connector (see Figure 2). This second part provides the electrical pins and diagram for generating a netlist of connections, so later on we can generate the necessary post-assembly test jigs and programs.

                        Figure 2.  Schematic Symbol of Connector

                        The final part is what I call the line item bubble (refer to Figure 3). This bubble will be used to make notes on the drawing linking what the part is to its reference to the bill of materials (BoM).

                        Figure 3.  Schematic Symbol of Line Item

                        These are coordinated into separate gates (or subparts) within a library component of the library editor. Each part has important information with regards to the cable assembly. That importance will be explained later on, but for now I will discuss how to create the connector head component and cable component.

                        The Connector Head Component:

                        2D Connector Head Drawings - Part A and C

                        The connector head part is an accurate scaled plan-view of the real connector. While you could draw this directly in the schematic library editor, most connector manufacturers provide drawings in DXF or DWG format for MCAD tools. So it will be faster to obtain such a drawing as seen in Figure 1, by first importing the DWG or DXF drawing of the connector head into the Schematic Editor. When performing this step, ensure that the scale is 1:1. You can also generate 2D front/top plan drawing in DXF from 3D mechanical models and then import those to Altium Designer. Once imported into the Schematic Editor, make sure you select the entire connector head and unionize the entire selection by going to Tools » Convert » Create Union from Selected Objects. Once that is done, you can then copy and paste the entire primitive drawing into the library editor as seen in this figure below in Figure 4:

                        Figure 4.  Profile view of a DSUB connector within Altium’s Library Editor

                        In the sample library (link here)[a], you will see that part A is the face (front) view and part C is the profile (top) view. I created the library in this particular manner based on my previous work experience in creating cable components. However, it is ultimately up to the user or design group to decide which part of the component will be designated by face and profile. Whatever you choose, make it consistent across all your connector library parts.

                        The Line Item Bubble - Part B

                        The following parts within the component are designated as a schematic symbol and line item bubble. The line item bubble has a specific purpose. Its function is to designate the graphical representation and reference it to the BoM. To create the line item bubble, a simple Full Circle is placed in the center of the Schematic Library Editor, and within the component properties you add a parameter Line Item. The value of the parameter is then placed in the centre of the Full Circle. The result of the component drawing is shown in figure 5 below:

                        Figure 5.  Line Item Bubble with parameter embedded

                        Figure 6.  If you notice within the Component Properties, the Line Item is added and made visible

                        Line Item Parameter

                        Although the Line Item Parameter is shown in Figure 5, it is set to invisible once you’ve placed it in the Line Item Bubble. This done so that when you place the connector parts within the Schematic Editor for your cable drawing, this parameter’s text will not show up until you reached the last part of the component, which should be the Line Item Bubble. More information on this will be explained later when we discuss on how to actually begin drawing cable assemblies.

                        Now that we have covered the connector head component, the next component to create is the cable itself, which is much simpler to than the connector head.

                        Cable Component:

                        Why create a cable component?

                        First - maybe to state the obvious but it should be asked - why create a cable component? Doesn’t Altium Designer already have wire, bus and harness objects? Good question. Bare in mind though that these objects are for establishing connectivity (i.e. building a net list), and do not represent the physical cable you would have to purchase or manufacture. For cable assembly of course we need this information represented in the BoM for supply chain resolution.

                        The cable component will only encompass two sub-parts in it: One being the schematic symbol, and the other being the Line Item. Most cable drawings I’ve studied use the oval shape shown above. This provides an aesthetically pleasing look. The top and bottom are just arcs connected by dotted line objects. So, as followed, Figure 7 shows a diagram of the cable in schematic format:

                        Figure 7.  Schematic Symbol of Cable Drawing

                        Pins in a cable?

                        Referring again to Figure 7, the dots that are distributed evenly in the middle of the drawing are pins with a unit length of 0 mil. These ‘pins’ represent the electrical connectivity of the cable itself, and will ultimately be linked in the netlist with connections to the connector heads. When you are wiring up the design, it then becomes a simple and quick process. However, this will be further elaborated a future installment.

                        Line Item for the Cable Component

                        The second module for the cable component is the line item bubble, much the same as the one used in the connector head component. After that, you have completed making the cable library component. The reason we have this component setup is that many users will draw out their cable assemblies in different sheet sizes (A, B, C, etc.), and the cable itself can be drawn by the designer different lengths or in more complex shapes (e.g. in a serpentine fashion). Therefore the line item sub-part offers the guarantee that you always have the right parameter text to represent the cable used, and it can be placed on the schematic sheet wherever needed.

                        In the next Cable Design blog, I will show how to create crimp and heatshrink components and demonstrate how all the components assemble together to generate an elementary cable drawing. Keep reading!

                        [a]Need to add HTML link to zip file for download