联系我们
联系原厂或当地办公室
Parent page: Finalizing the Board Design
Via stitching is a technique used to tie together larger copper areas on different layers, in effect creating a strong vertical connection through the board structure, helping maintain a low impedance and short return loops. Via stitching can also be used to tie areas of copper that might otherwise be isolated from their net, to that net.
Via shielding has a different function, in RF designs it is used to help reduce crosstalk and electromagnetic interference in a route that is carrying an RF signal. A via shield, also known as a via fence or a picket fence, is created by placing one or more rows of vias alongside the signal's route path. In Altium Designer, this is referred to as via shielding.
Altium Designer supports both via stitching and via shielding. In the image below, shielding vias are highlighted, move the cursor over the image to highlight the stitching vias that have been added to this board.
Use the Via Stitching and Via Shielding commands to stitch copper on different layers, and to add a wall of shielding vias adjacent to a route path (hover to highlight shielding vias).
Let's look at stitching vias first, and then shielding vias.
Via stitching is run as a post-process, filling free areas of copper with stitching vias. For via stitching to be possible, there must be overlapping regions of copper that are attached to the specified net, on different layers. Supported regions of copper include Fills, Polygons and Power Planes.
Select the Tools » Via Stitching/Shielding » Add Stitching to Net command from the menus to add stitching vias to a specific net. The Add Stitching to Net dialog will open, where the Stitching Parameters and Via Style are specified. Using the selected net, the stitching algorithm identifies all Fills, Polygons and Power Planes attached to that net and attempts to connect them through the board, using the specified via and stitching pattern.
The via stitching algorithm treats Polygons, Fills and Planes in the following way:
Notes about the Add Stitching to Net dialog settings:
As well as covering the entire board, stitching vias can be constrained to a user-defined area. When the stitching is within a user-defined area, that area of vias can be interactively moved and resized, if required.
Enable the Constrain Area option to restrict stitching vias to a user-defined area.
To constrain via stitching to a specific area, enable the Constrain Area checkbox in the Add Stitching to Net dialog, as shown above. As soon as you enable this option the dialog will close and the cursor will change to a crosshair, ready to define the area - note the Status bar, it will prompt Select the first point of the area.
The process of defining a via stitching area is the same as defining a solid region or a polygon, you:
During placement there are a number of different corner modes available:
Press Shift+Spacebar to cycle corner modes, Spacebar to toggle the corner direction, 1 to toggle between placing 1 edge or 2 with each click.
Once the area is defined you will return to the Add Stitching to Net dialog, so you can configure the rest of the settings. Click OK when this is complete, Altium Designer will then analyze the area, identify potential via sites, and place the stitching vias.
The set of vias in each unique area of via stitching are clustered into a Union (a set of objects that the PCB editor recognizes as a single group). The entire union can be moved, and the area can also be resized.
To modify via stitching that is constrained to an area:
Drag a selection window to select a stitching area, then move or resize by positioning the mouse to get the correct cursor.
To place a via shield around a routed net, select the Tools » Via Stitching/Shielding » Add Shielding to Net command from the menus. The Add Shielding to Net dialog will appear, configure the Shielding Parameters and Via Style as required. The vias will be placed along both sides of the chosen net, wherever it is possible to place a via that complies with the applicable design rules.
Notes about the Add Shielding to Net dialog, and using shielding vias:
As well as adding shielding vias along each side of the routing, you can also include shielding copper, as shown in the image below. To do this, enable the Add shielding copper option. This copper is created as a polygon, so it obeys the applicable Clearance and Polygon Connect Style design rules.
The Add shielding copper option will add a polygon that encloses the shielding vias. The polygon edge that is away from the shielded net will touch the edge of the vias. The polygon edge that is adjacent to the shielded net will be set back from the net by the applicable Clearance design rule. If the Add clearance cutout option is also enabled, the polygon will instead be set back from the shielded net by the Distance setting in the Add Shielding to Net dialog. Hover the cursor over the image below to see the difference.
Shielding vias around a net with the clearance cutout option enabled, move the cursor over the image to disable the clearance cutout option.
Each via in a stitching or shielding array is identified by the addition of of a string to the net name, such as [VS1], as shown in the image below, where:
Vias that belong to an array have an additional string, such as [VS1] for [Via Shielding group 1],
and [VSH4] for [Via SHielding group 4], appended to their net name.
To simplify the process of working with an array of stitching/shielding vias, both kinds are automatically clustered into a union.
To select the array, switch the PCB panel to Unions mode and select the required Via Stitching or Via Shielding union. All vias that are part of that array will select, if the Select checkbox is enabled in the panel (as shown in the image below). Alternatively, double click on any via in the array to open the Add Stitching to Net dialog or the Add Shielding to Net dialog and edit the array.
Use the PCB panel in Unions mode to select all vias in a stitching or shielding array. In this image all 4 via shielding unions are selected.
Selection behavior:
The properties of a stitching or shielding via set can be edited once it has been selected, in the Via Stitching or the Via Shielding mode of the Properties panel.
An example of an edit being performed to a via shielding.
As soon as any property has been edited in the panel, the Changes pending message and buttons appears at the bottom of the panel - use the appropriate button to complete your editing action.
Once stitching is complete, you will need to re-pour the polygons if the applicable Polygon Connect Style design rule specifies a relief connection style. This can be done using the commands in the Tools » Polygon Pours sub-menu.
联系原厂或当地办公室
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
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
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。
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。
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。