Altium NEXUS Documentation

ExportToPCB

Modified by Jason Howie on Apr 11, 2017

Parent page: CAMtastic Commands

The following pre-packaged resource, derived from this base command, is available:


Applied Parameters: None

Summary

This command is used to export data from the CAMtastic Editor directly to a new PCB document. This enables you to recover old designs that were generated using PCB tools that are perhaps no longer supported, working backwards from the Gerber files.

Access

This command is accessed from the CAMtastic Editor by choosing the File » Export » Export to PCB command from the main menus.

The command will not become available until the netlist has been extracted (Tools » Netlist » Extract).

Use

First, ensure that the necessary layers have been loaded into the current CAM document, with respect to the design you wish to export. The Exporter can transfer entire boards into the PCB document, not just Gerber files. For example, if you are exporting a thru-hole board, make sure that the current CAM document contains at least the Top, Bottom and NC Drill layers. Mask, Overlay and other layers are beneficial, but not essential to the export. Also ensure that the netlist for the current document has been extracted.

After launching the command, a new PCB document will be generated (<CAMDocumentName>.PcbDoc) and opened as the active document in the main design window. The actual sequence of events in the transfer of information between the CAM document and the PCB document is as follows:

  1. The PCB document is created with a board outline based on the current size of the board in the CAM document.
  2. Net objects are created in the PCB document, using the net information extracted from the CAM document.
  3. The layer stack-up is generated, based on the physical layers order defined in the CAM document (Create/Update Layers Order dialog, accessed through Tables »  Layers Order).
  4. Nets are assigned to any internal planes.
  5. Nets are assigned for any split planes that exist.
  6. Clearance, Width and Power Plane Connect Style design rules are created. Relief connects are created for each plane net.
  7. Padstacks are built from the CAM data (using pads on the signal/plane layers in the physical order, followed by drill, mask, paste, etc). The padstacks are loaded into the PCB and the required style is defined (simple or full padstack).
  8. The PCB tracks are created.
  9. A DRC check is performed for the whole board.

Tips

  1. This command transfers data from the CAM document to the PCB document using the PCB API. In this way, no exported data files (in Gerber or other format) are generated, and so the need to use the PCB Editor's Gerber Importer is bypassed.
  2. Before extracting the netlist in the CAM document, make sure that the drill layer sets have been defined as required (Create/Update Layers Sets dialog, accessed through Tables »  Layers Sets). This is compulsory if you are using blind/buried vias, in order to extract the correct netlist. For blind/buried vias, you must select all layers that are drilled, not just the start and end layers. For thru-holes, start and end layers will suffice.
  3. If the Gerber files were originally generated from Altium NEXUS's PCB Editor, the Physical Layers order will be defined automatically. For other source PCB tools, you will need to assign this ordering manually.
  4. If you have the IPC-D-356 netlist for the design, you can load it into the current CAM document and use it to rename the nets to the original (and meaningful) net names that were assigned in the design.
  5. Although the IPC-D-356 netlist information is not essential to the export, it is desirable. Its presence will aid the CAMtastic Editor in separating the pads from the vias, and hence lead to the correct creation of vias instead of pads, for any blind or buried vias in the design.
  6. The generated PCB document will be added to the Projects panel as a Free Document, under the PCBs sub-folder. It is generated, but initially unsaved.

 

Found an issue with this document? Highlight the area, then use Ctrl+Enter to report it.

联系我们

联系原厂或当地办公室

We're sorry to hear the article wasn't helpful to you.
Could you take a moment to tell us why?
You are reporting an issue with the following selected text
and/or image within the active document:
Altium Designer 免费试用
Altium Designer Free Trial
我们开始吧!首先,您或者您的公司已经在使用Altium Designer了吗?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

既然您在使用Altium Designer,为何仍需要试用?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,实际上您无需下载一个试用版本。

点击下方按钮下载最新版本的Altium Designer安装包

下载Altium Designer 安装包

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

填写下方表格,获取Altium Designer最新报价。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

如果您是Altium维保期内客户,您不需要下载试用版本。

如果您不是Altium维保客户,请填写下方表格免费试用。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

您为何想要试用Altium Designer?

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

那您来对地方了!请填写下方表格申请试用吧。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

Great News!

Valid students can get their very own 6-month Altium Designer Student License for FREE! Just fill out the form below to request your Student License today.

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。

好棒!创作是一件超酷的事情,我们可以为您提供完美的设计软件。

Upverter是一个社区导向的交流平台,专为您这样的创客量身定做。

点击这里看看吧!

如果您有任何需求,请点击这里联系获取当地办公室销售代表联系方式。.
Copyright © 2019 Altium Limited

好的,您可以下载免费的Altium Designer Viewer查看文档,有效期6个月。

请填写下方表格申请。

点击[获取免费试用],并同意我们的隐私政策。您会接收到来自Altium的资讯,并允许其改变您的通知首选项。