Polygon Pours and Copper Regions. Fills and Solid Regions. Modified by Admin on Nov 18, 2013
|
|
- Jennifer Clarke
- 5 years ago
- Views:
Transcription
1 Polygon Pours and Copper Regions Old Content - visit altium.com/documentation Modified by Admin on Nov 18, 2013 A common requirement on a printed circuit board is large areas of copper. It could be a hatched region of grounding copper on an analog design; a large, solid region of copper for carrying heavy power supply currents; or a solid ground area for EMC shielding. In Altium Designer areas of copper can be defined using three different design objects: Fills, Solid Regions and Polygon Pours. The advantage of a Polygon Pour is that it automatically pour around copper objects that belong to another net, in accordance with the applicable Electrical Clearance and Polygon Connect Style Design Rules. This article briefly discusses Fills and Solid Regions, and then explains how Polygon Pours (also called copper pours) are used to create regions of copper on a PCB. It covers such topics as placing and modifying Polygon Pours, setting properties, controlling the clearance using design rules and repouring. Fills and Solid Regions A example of a Solid Region, that is selected. A Fill (Place» Fill) is a rectangular shaped design object that can be placed on any layer, including copper (signal) layers. Fills are limited to a rectangular shape and will not avoid around other objects, such as Pads, Vias, Tracks, Regions, other Fills or Text. If a Fill is placed on a signal layer it can be connected to a Net. A Region (Place» Solid Region) is a design object used for defining polygonal shapes. A Solid Region (commonly just called Region) can be placed on any layer, including signal (copper) layers. Like a Fill, a Region does not avoid around other objects, such as Pads, Vias, Tracks, Fills, other Regions or Text. If a Region is placed on a signal layer it can be connected to a Net. The Region object also has a number of special properties that allow it to be used for:
2 Polygon cutouts - where it is essentially a negative (empty) object that the surrounding Polygon pours around. Board Shape cutouts - where it also acts as a a negative (empty) object to define an irregular cutout or hole in the board. Custom Pad shapes - where it defines the copper area of an unusual pad, giving the ability to define automatically matched-shape solder and paste mask contractions/expansions. Polygon Pours A Polygon shown as solid and hatched, demonstrating varying clearances and controlled connection style and air gap. A Polygon Pour (Place» Polygon Pour) placed on a signal layer creates a polygonal (multi-sided) area of copper, which can either be solid or hatched. As they are poured, Polygons automatically allow for clearances around electrical objects belonging to a different net, connect to objects of the same net, and fill irregularly shaped areas. Clearances and connection properties are controlled by the applicable Electrical Clearance and Polygon Connection Style design rules. Placing a Polygon Pour Select the Place» Polygon Pour command to place a Polygon on the current layer in the PCB Editor. When the command is run the Polygon Pour dialog displays, where you set the fill and net connection options and pour-around properties. Click OK and the cursor changes to a crosshair, ready to draw the Polygon outline.
3 The Polygon Pour dialog, where you configure the properties of the polygon before placing it. When you place a Polygon, you are defining the outline of the Polygon object. Once the outline is complete, the polygon will automatically fill, in accordance with the Fill Mode and other options selected in the dialog. Polygon Fill Mode There are 3 supported Fill Modes, Solid, Hatched or None. Solid (Copper Regions) - If this mode is selected the Polygon is internally constructed from Solid Region objects, with a separate Region for each contiguous area of copper in the completed polygon. This type of polygon is output to Gerber using Gerber region definitions. Note that circular cutouts are not supported in the Gerber region definition, so the arcs (holes) for circular cutouts are actually approximated by straight chord sections. The accuracy of these is defined by the Arc Approximation setting in the Polygon Pour dialog. Polygons of this type are generally faster to pour and result in smaller PCB and Gerber file sizes. Hatched (Tracks/Arcs) - If this mode is selected the polygon is created from Track and Arc objects. By adjusting the Width and Grid settings of the Track/Arc objects, the completed polygon can either be hatched or solid in appearance. Polygons of this type are generally slower to pour and result in larger PCB and Gerber file sizes. Hatched polygons are often used in analog designs. Note that the outline of a Hatched polygon is created from Tracks and Arcs, with the user-defined edge of the Polygon at the center-line of the outline Tracks and Arcs.
4 None (Outlines Only) - this mode is essentially the same as the Hatched mode. It also uses Tracks and Arcs to define the boundaries, but the fill-in Tracks and Arcs are not added. This mode can be useful if you are analyzing the structure and design of various polygons and attempting to understand the interaction of overlapping polygons. This mode is also useful when design changes are being made and the polygon is interfering in this process. An alternate approach to using outlines during design changes is to Shelve the polygons, where they are retained in the PCB file, but removed from view. The Placement Process In Altium Designer's PCB Editor the process of how you define any multi-sided polygonal object, such as a Solid Region, the Board Shape or a Polygon, is the same. Solid objects are closed objects, so regardless of how far you are through the placement process, the software will show a line from the cursor back to the object's starting location. This line will become the solid object's last edge if you press Escape (or right-mouse click) to terminate the placement process. The placement process is a process of defining the corner locations, with various corner modes being available. Corner Modes There are 5 different corner modes available during polygon placement: 45º, 45º arc, 90º, 90º arc and Any Angle, as shown in the images below (click to enlarge). The different corner modes available during polygon placement, press Shift+Spacebar to cycle through the modes. Tips on Placing a Polygon: Press Shift+Spacebar to cycle through the corner modes Press Spacebar within each corner mode to toggle the corner direction (except for the Any Angle mode). Press Backspace to remove the last corner. Press Esc or Right-Mouse click to terminate the placement process, the software will close and complete the Polygon. For the Arc corner modes, the arc can be re-sized using the and keys. Hold Shift to accelerate the re-sizing process. Understanding the Look-Ahead Feature There are many situations during PCB design where the designer needs to be able to predict where a future track segment or object edge must go, without committing to place that object. To support this requirement Altium Designer includes a feature called Look-Ahead. When Look-Ahead is enabled the
5 track/object edge currently attached to the cursor is not placed when the designer clicks, only the previous segment is placed. To say that another way, the last segment allows the designer to lookahead to where they will place the future segment. Press the 1 shortcut during object placement to toggle Look-Ahead on or off, note how the display changes to display each mode. In track placement, the segments to be placed by the next mouse click are shown as hatched, and the Look-Ahead segment is shown as hollow or empty. In solid-object placement, the edges to be placed by the next mouse click are shown as solid white lines and the Look-Ahead edge is shown as a dashed white line. The following images shows how the display of track segment changes when the Look-Ahead feature is on and off. Track placement with Look-Ahead on (left image) and off (right image). The next mouse click will place the hatched track segments. The Look-Ahead feature also works during Polygon Pour placement, press the 1 shortcut (during object placement) to toggle it on and off. The following images show the first corner placement of a Polygon Pour, first with Look-Ahead on, then with Look-Ahead off.
6 Look_ahead is on, on the next mouse click the solid line becomes a polygon edge, but not the dotted line. Note the solid return line, it shows how the polygon will be closed if the designer terminates polygon placement.
7 Look_ahead is off, on the next mouse click both of the solid lines becomes polygon edges. Note the solid return line, it shows how the polygon will be closed if the designer terminates polygon placement. Press the 1 shortcut to toggle the Look-Ahead on or off. Note that this shortcut only works during object placement. Press the ~ (Tilda) key (or Shift+F1) during placement for a complete list of in-command shortcut keys. Connecting the Polygon to a Net A Polygon can be attached to a net. Select the required net in the Connect to Net drop-down in the Polygon Pour dialog. The Polygon pour will connect to each pad on this net that is found within the outline of the Polygon. How the polygon connects to the pads is determined by the applicable Polygon Connect Style design rule. The clearance between the polygon and objects belonging to other nets is determined by the applicable Electrical Clearance design rule. How the polygon treats objects on the same net, such as routing tracks, is determined by the option selected in the Pour Over drop-down: Pour Over All Same Net Objects - choose this option if you want the Polygon to automatically connect to all objects on the same net as the pour. Pour Over Same Net Polygons Only - choose this option (default) if you want the Polygon to automatically connect to only Polygon objects inside its boundary, which are attached to the same net. Don't Pour Over Same Net Objects - choose this option if you specifically do not wish the Polygon pour to connect to any other, non-pad objects on this (or any other) net. Remove Dead Copper When a polygon is poured there can be regions (islands) of the polygon that are completely isolated from the connected net, due to the presence of other tracks, pads and so on. To have the software detect and remove these isolated islands of copper, enable the Remove Dead Copper option. If a Polygon pour is placed on a non-signal layer it will not be poured around existing objects, as these objects are not assigned to a net and therefore do not belong to anything. Controlling the Polygon Connection Style Main article: Polygon Connect Style Design Rule How the polygon connects to pads on the net that it is attached to, is controlled by the applicable Plane - Polygon Connect Style design rule (Design» Rules).
8 How the polygon connects to pads on the net is determined by the Polygon Connect Style design rule. Three connection options are available: Direct Connect - the polygon effectively pours over the pad, creating solid copper to the pin. Relief Connect - A spoke-style connection is created: define the Number of conductors, the Angle of these conductors (90º or 45º), Conductor Width,and the Air Gap Width ** (the clearance between the edge of the pad and the edge of the polygon surrounding the pad). No Connect - the pads on the net will be isolated from the polygon. The Air Gap Width setting (the clearance between the edge of the pad and the edge of the polygon surrounding the pad) was added to Altium Designer in Update 19. This setting now controls the clearance between the edge of the pad and the surrounding polygon, whereas the Electrical Clearance design rules did this in earlier versions of Altium Designer. When a board designed in an early version of Altium Designer is opened in Altium Designer Update 19 (or later) a warning will appear, it is important that you review and set the Air Gap settings in the Polygon Connect Style Design Rules in this situation. Controlling the Polygon Clearance Like any object placed on a signal (copper) layer, the clearance of a polygon from objects that it is poured around is controlled by the applicable Electrical Clearance design rule.
9 The clearance from the Polygon to objects on other nets is controlled by the Electrical Clearance design rule. It is common practice to have a larger clearance between a polygon and other net objects, to achieve this a polygon-specific Electrical Clearance design rules can be defined. An example of this is shown in the image above (click to enlarge), where the rule states that: Objects that are InPolygon, and belong to a Net Class called Power and All other copper objects Must be at least 0.3 mm apart. In this example the designer is targeting only the Polygons attached to power nets, which require a greater clearance than other non-power net Polygons. Remember that the Polygon Clearance rule must also have a higher Priority than any general clearance rule to have any effect. When defining an Electrical Clearance rule for Polygons, you must use the InPolygon (or InPoly) Query keyword, rather than IsPolygon (or IsPoly). This is because the clearance rules operate on the primitives (regions, tracks and arcs) that make up, or are in the Polygon, rather than the Polygon as a whole object. A valid clearance rule for Polygon pours would be between InPolygon objects and All other objects. Re-pouring a Polygon There are a number of ways a Polygon can be re-poured. To repour a Polygon:
10 Double click anywhere on the Polygon to open the Polygon Pour dialog, change settings as required and click OK. Right-click on the Polygon, then in the floating Context menu select Polygon Actions» Repour. In the Polygon Manager (Tools» Polygon Pours» Polygon Manager), select the required Polygon, then click the Repour button. Use the appropriate Repour command in the Tools» Polygon Pours sub-menu. Confirm the repour by clicking Yes in the Confirm dialog. To edit a Polygon the layer that the Polygon is on must be the current, or active editing layer. Polygon Cutouts A Polygon Pour Cutout is essentially a negative copper region, that is the designer is defining a void or hole in the Polygon. To define a cutout in a Polygon select the Place» Polygon Pour Cutout command, then click to define the cutout shape. Once the cutout has been defined the Polygon must be re-poured, it will then pour around the cutout definition. Remember that the cutout is actually a Solid Region object, it can be re-sized by clicking once to select it, then clicking and holding to drag an edge or a vertex. After re-sizing the cutout the polygon must be re-poured. The cutout has been placed (left image), and the Polygon has been re-poured (right image). Creating a Polygon Pour From a Set of Tracks As well as defining areas of electrical copper on a board, Polygons and Solid Regions are also used to define other polygonal-shaped design objects, such as a special symbol or a company logo. If an outline of the required shape has been defined in another design tool, such as AutoCAD, it can be exported as DXF and then imported into Altium Designer. That outline can then be converted into a Polygon or a Solid Region. To convert a set of tracks to a polygon, select the track segments and then select Tools» Convert» Create Polygon from Selected Primitives from the menus. Note that:
11 The Polygon will be created on the current (or active) layer, not the layer that the selected tracks are on. This means you can define the shape on a Mechanical Layer, then create the polygon on a signal layer. The selected tracks will still exist after polygon has been created, and will remain selected. If the polygon is created on the same layer as the selected tracks it will pour within the tracks, in accordance with the applicable Electrical Clearance Design Rule. The Polygon will be created with its Fill Mode set to None (Outline Only), double click on it to re-pour it with the required Fill Mode. For Altium Designer to be a able to perform a track to polygon conversion, the outline must be correctly define. That means the outline must form a closed shape, with the ends of touching track segments correctly meeting (starting/ending in the same X, Y location). Moving a Polygon Pour Click and drag to move a Polygon pour. Hold down the SHIFT key to select multiple Polygon pours to move. The rebuild Confirm dialog appears when you release the mouse button. Click Yes to repour the Polygon pour(s) in their new location. Reshaping a Polygon Pour A Polygon, with 90º arc corners, being re-sized. An existing Polygon pour can be reshaped. To do this, first right-click on the polygon and select Polygon Actions» Move Vertices (or Edit» Move» Polygon Vertices). The following actions can then be performed: Position the mouse cursor over an edge, click to select the edge, slide that edge to a new location, then click to place it. Click to select a vertex, move that vertex to a new location, then click to place it. If you select a vertex at the center of a straight edge this will in effect break that single edge into 2 new edges.
12 To remove a vertex, click to select and move it, then press the Delete key on the keyboard. The software will remove that vertex, then automatically move the next vertex in an anticlockwise direction to the cursor. The visual effect is that it appears to remove not the current vertex, but the next one in an anti-clockwise direction. Right-click to terminate reshaping, then click Yes in the Confirm dialog to re-pour the Polygon in the new shape. Slicing a Polygon Pour The Place» Slice Polygon Pour command is used to slice a single Polygon pour into two or more separate Polygon pours. When you select the command you are in slice mode (similar to track placement mode), click (or press ENTER ) to anchor a series of vertex points that define the slice line. When defining the slice, press Shift+Spacebar to cycle through the corner modes, press the Spacebar to toggle between the Start and End corner modes and use the Backspace key to remove the last placed corner. Place the end of the slice beyond the edge of the Polygon. When you have finished defining the slice, right-click (or press ESC). A confirmation dialog appears stating how many new Polygons will be created. Click Yes and confirm that you wish to rebuild the Polygons. Shelving a Polygon Pour During the design process it is normal for changes to occur - components might be added or change, routing may need to be updated. To simplify the management of existing Polygons during this process, they can be Shelved. This temporarily hides them from the editor, but retains them in the PCB database. To shelve all Polygon pours in the current design, select the Tools» Polygon Pours» Shelve n Polygon(s) command (where n is the number of Polygon pours that have been detected in the design). To restore all shelved Polygon pours, select the Tools» Polygon Pours» Restore n Shelved Polygon(s) command (where n is the number of Polygon pours that are currently shelved). You can also selectively shelve via the right-click menus command, or the Polygon Manager. Using Polygon Pours on Non-copper Layers Polygon pours can be used on non-copper layers. If a Polygon pour is placed on a non-signal layer, it will not pour around existing objects because they are not assigned to a net. The Polygon Pour Manager Main article: Polygon Pour Manager The Polygon Pour Manager dialog provides a high-level view of all Polygons that currently exist in the PCB workspace. This manager also allows you to name and rename each Polygon, set the pour order of Polygons, perform re-pouring or shelving actions on selected Polygons and add/scope design rules for selected Polygons as well.
13 The Polygon Manager gives full control over all the Polygons in the design. Notes about the Polygon Pour Manager: The Polygon Pour Manager dialog is launched from the Tools» Polygon Pours submenu. A Polygon is automatically named during placement, you are free to rename it to suit your design. Note that the Name can be used to scope design Rules targeting a Polygon Polygon. The Pour Order section at the bottom of this dialog allows you to re-arrange the pour order of Polygons with the Move Up, Move Down, and Auto Generate buttons. You can also change order using mouse drag-and-drop functionality, which is far more expedient in designs featuring many polygon pours. Pour order can be important when there is a Polygon completely enclosed within another Polygon, typically you would order from the smallest Polygon down to the largest Polygon. The Auto Generate button will order the Polygons from smallest area to largest area, on a layer-by-layer basis. Since the Polygon manager can perform actions that change the design, such as repouring selected Polygons, it must execute pending actions before accepting a new request that can change the design. A message alerting you about this will appear (shown below). If you click the Repour button you have the choice of re-pouring all Polygons, selected Polygons or Polygons that have violations. Update progress can be monitored on Altium Designer's status bar. If you perform a Shelve, Lock, or Ignore from DRC action for selected Polygons the action is not performed immediately. In these cases the actions are performed when you click the Apply or OK buttons.
14 Any pending edits must be applied before a new edit can be performed. Reporting on Polygons For more information about the Polygon pours in your PCB, you can use the Board Information Report or list the properties of a Polygon pour and its children. Select Reports» Board Information. The number of Polygons detected on the PCB is shown in the PCB Information dialog. Keep in mind that this total reflects not only Polygon pours, but also internal planes and split planes. For a detailed listing of Polygon properties, use the PCB List panel. Using the List Panel to View and Edit Polygon Properties Main article: PCB List The PCB List panel provides an alternate approach to view and edit all design objects that currently exist in the workspace. To display the PCB List panel click the PCB button down the bottom right of the workspace, then select PCB List from the menu. The PCB List panel presents data in a tabular, or spreadsheet-like format. By default it will display all objects in the workspace. Use the controls across the top of the panel to filter down the list, in the image below you can see that the PCB List panel is set to Edit, All Objects, only of kind Polygon (click to enlarge). The properties of one or more polygons can be edited in the PCB List panel. The PCB List panel can be used to review and edit Polygon pours. Source URL:
Polygon Pour. Summary. Availability. Modified by on 19-Nov Parent page: Objects
Polygon Pour Old Content - visit altium.com/documentation Modified by on 19-Nov-2013 Parent page: Objects A Polygon Pour (brighter red) being used to create a large GND area on a board. Summary A polygon
More informationPolygon Pour. Modified by Susan Riege on Aug 13, Parent page: PCB Dialogs. Other Related Resources Polygon Pour (Object)
Polygon Pour Modified by Susan Riege on Aug 13, 2018 Other Related Resources Polygon Pour (Object) Parent page: PCB Dialogs The Polygon Pour dialog in Solid mode, Hatched mode and None mode. Summary This
More informationPublished on Online Documentation for Altium Products (
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) Home > Coverlay Polygon Using Altium Documentation Modified by Phil Loughhead on Oct 24, 2018 Parent Page: PCB
More informationEnhanced Polygon Editing and Management. Poured or Unpoured Polygons. Modified by Jason Howie on Nov 13, 2014
Enhanced Polygon Editing and Management Old Content - visit altium.com/documentation Modified by Jason Howie on Nov 13, 2014 Most board designs today incorporate areas of copper, which are easily created
More information3D Body. Summary. Modified by Admin on Sep 13, Parent page: Objects
3D Body Old Content - visit altium.com/documentation Modified by Admin on Sep 13, 2017 Parent page: Objects A sphere, a cylinder and 4 extruded rectangles have been used to create the 3D body for an LED.
More informationSchematic Editing Essentials
Summary Application Note AP0109 (v2.0) March 24, 2005 This application note looks at the placement and editing of schematic objects in Altium Designer. This application note provides a general overview
More informationPreparing the Board for Design Transfer. Creating and Modifying the Board Shape. Modified by Phil Loughhead on 15-Aug-2016
Preparing the Board for Design Transfer Old Content - visit altium.com/documentation Modified by Phil Loughhead on 15-Aug-2016 This article describes how to prepare the new PCB file so that it is ready to
More informationCycle through three routing modes (ignore, avoid or push obstacle) Toggle electrical grid on/off
PCB Editor Shortcuts Old Content - visit altium.com/documentation Modified by on 13-Sep-2017 Parent article: Shortcut Keys PCB Editor Shortcuts + E + B + PAGE UP + PAGE DOWN Cycle through three routing
More informationOutline Vertices Editor for Polygonal Pours and Regions
Outline Vertices Editor for Polygonal Pours and Regions Old Content - visit altium.com/documentation Modified by on 13-Sep-2017 Related Videos Outline Vertices Editor for Polygon Pours and Regions Offering
More informationTUTORIAL SESSION Technical Group Hoda Najafi & Sunita Bhide
TUTORIAL SESSION 2014 Technical Group Hoda Najafi & Sunita Bhide SETUP PROCEDURE Start the Altium Designer Software. (Figure 1) Ensure that the Files and Projects tabs are located somewhere on the screen.
More informationMoving to Altium Designer from Protel 99 SE. Contents
Moving to Altium Designer from Protel 99 SE Contents Design Database Become a Design Workspace & Projects Importing a 99 SE Design Database Creating the Altium Designer Project(s) Manually Adding and Removing
More informationInteractively Routing a Net
Interactively Routing a Net Old Content - visit altium.com/documentation Modified by on 18-Nov-2013 Interactive Routing is more than placing down track objects to join the dots (pads). Altium Designer
More informationBoot Camp-Special Ops Challenge Quiz
1. What s the key difference between a panel and dialog window? a. There is none b. Panels must be closed in order to continue editing, whereas dialogs can be left open c. Dialogs must be closed in order
More informationBaseline dimension objects are available for placement in the PCB Editor only. Use one of the following methods to access a placement command:
Baseline Dimension Old Content - visit altium.com/documentation Modified by on 19-Nov-2013 Parent page: Objects A placed Baseline Dimension. Summary A baseline dimension is a group design object. It allows
More informationDefining Board Regions and Bending Lines
Defining Board Regions and Bending Lines Old Content - visit altium.com/documentation Modified by on 29-Nov-2016 Related Videos Bending Lines Layer Stack Regions A Board Region is the term used to describe
More informationA Bus is a polyline object that is used, in conjunction with other objects, to define the connection of multiple nets.
Bus Old Content - visit altium.com/documentation Modified by Admin on Sep 13, 2017 Parent page: Objects A Bus is a polyline object that is used, in conjunction with other objects, to define the connection
More informationEditing Multiple Objects. Contents
Editing Multiple Objects Contents Selecting Multiple Objects Inspecting the Objects Editing the Objects Editing Group Objects Step 1. Selecting the Capacitors Step 2. Changing the Comment String Step 3.
More informationPublished on Online Documentation for Altium Products (https://www.altium.com/documentation)
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) Home > PCBLIB List A New Era for Documentation Modified by Susan Riege on Jan 24, 2018 Parent Page PCB Panels
More informationCreating a Custom Pad Shape. Standard Pad Attributes. Creating a Custom Pad Shape. Modified by on 13-Sep-2017
Creating a Custom Pad Shape Old Content - visit altium.com/documentation Modified by on 13-Sep-2017 Standard Pad Attributes Altium Designer's standard pad object can: Be set to a number of different shapes,
More informationProtel 99 SE. Designer s Handbook Supplement. Runs on Windows NT/95/98. Making Electronic Design Easy
Making Electronic Design Easy Protel 99 SE Designer s Handbook Supplement Runs on Windows NT/95/98 Increase your PCB Design Productivity with Protel 99 SE Welcome to the Protel 99 SE Designer's Handbook
More informationProtel 99 Installation Notes
Protel 99 Installation Notes Frozen Content Modified by Admin on Nov 21, 2013 Protel 99 SE Service Pack 6 Information Installation Notes To install the Service Pack run the downloaded file and follow the
More informationMoving to Altium Designer from Pads Logic and PADS Layout
Moving to Altium Designer from Pads Logic and PADS Layout Old Content - visit altium.com/documentation Modified by on 13-Sep-2017 Translating complete PADS Logic and PADS Layout designs, including PCB,
More informationBaseline dimension objects are available for placement in the PCB Editor only, by clicking Home
Baseline Dimension Modified by Jason Howie on 24-Oct-2014 Parent page: Dimension A placed Baseline Dimension. Summary A baseline dimension is a group design object. It allows for the dimensioning of a
More informationImporting the Source Models. Placing a 3D Model in the Workspace. Modified by on 25-Jul-2014
Importing the Source Models Old Content - visit altium.com/documentation Modified by on 25-Jul-2014 Placing a 3D Model in the Workspace A 3D model can be placed into a PCB document at any time. Note that
More informationPart. Summary. Modified by Susan Riege on Aug 5, Parent page: Objects
Part Old Content - visit altium.com/documentation Modified by Susan Riege on Aug 5, 2016 Parent page: Objects Related Resources Net Ties and How to Use Them (PDF) The Part represents the actual physical
More informationPads are used to provide both mechanical mounting and electrical connections to the component pins.
Pad Old Content - visit altium.com/documentation Modified by Jason Howie on 19-Aug-2015 Parent page: Objects Pads are used to provide both mechanical mounting and electrical connections to the component
More informationLesson 5: Board Design Files
5 Lesson 5: Board Design Files Learning Objectives In this lesson you will: Use the Mechanical Symbol Editor to create a mechanical board symbol Use the PCB Design Editor to create a master board design
More informationCreating a Custom Pad Shape. Contents
Creating a Custom Pad Shape Contents Standard Pad Attributes Creating a Custom Pad Shape Strategies for Creating Custom Shapes Using Guides to Place a Region Converting an Outline to a Region Defining
More informationPublished on Online Documentation for Altium Products (https://www.altium.com/documentation)
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) Home > Sheet Symbol Using Altium Documentation Modified by Susan Riege on Apr 11, 2017 Parent page: Schematic
More informationPCB Rules and Violations
PCB Rules and Violations Old Content - visit altium.com/documentation Modified by on 6-Nov-2013 Parent page: Panels Browse, edit and interactively view design rules and their associated violations. Summary
More informationOrcad Layout Plus Tutorial
Orcad Layout Plus Tutorial Layout Plus is a circuit board layout tool that accepts a layout-compatible circuit netlist (ex. from Capture CIS) and generates an output layout files that suitable for PCB
More informationProbes are available for placement in the Schematic Editor only, by choosing Place» Directives» Instrument Probe [P, V, I] from the main menus.
Instrument Probe Old Content - visit altium.com/documentation Modified by Admin on Nov 18, 2013 Parent Page: Objects An Instrument Probe. Summary An instrument probe is a design directive. It instructs
More informationDrill Table. Summary. Availability. Modified by on 19-Nov Parent page: Objects
Drill Table Old Content - visit altium.com/documentation Modified by on 19-Nov-2013 Parent page: Objects The Drill Table presents a live summary of all drill holes present in the board. Summary A standard
More information- create new schematic to the new project, PCB design begins with a schematic diagram, which present how components are connected
Eagle 8.x tutorial - create a new project, Eagle designs are organized as projects - create new schematic to the new project, PCB design begins with a schematic diagram, which present how components are
More informationPADS-PowerPCB 4 Tutorial (with Blazeroute)
PADS-PowerPCB 4 Tutorial (with Blazeroute) PADS-PowerPCB is the ultimate design environment for complex, high-speed printed circuit boards. PROCEDURE FOR SIMULATION IN SCHEMATICS 1. Importing Design Data
More informationGetting Started with PCB Design
Getting Started with PCB Design Summary Tutorial TU0117 (v1.2) April 13, 2005 This introductory tutorial is designed to give you an overview of how to create a schematic, update the design information
More informationPCB. Parent page: Panels. Mod. ifi. 6Jan -20. Old Content - visit altium.com/documentation
PCB Old Content - visit altium.com/documentation Mod ifi ed by on 6Jan -20 15 Parent page: Panels The PCB panel gives you full access to board objects, items and classes via a filtered browser. Summary
More informationMoving to Altium Designer from Protel 99 SE
Moving to Altium Designer from Protel 99 SE Summary This article outlines the process you go through to transfer a Protel 99 SE design into the Altium Designer environment. Protel 99 SE uses the design
More informationPCB Design Training Module
PCB Design Training Module Document Version 1.01, December 4, 2006 Software, documentation and related materials: Copyright 2006 Altium Limited. All rights reserved. You are permitted to print this document
More informationTutorial - Getting Started with PCB Design
Tutorial - Getting Started with PCB Design Old Content - visit altium.com/documentation Modified by Phil Loughhead on 3-Aug-2016 Welcome to the world of electronic product development environment in Altium
More informationWorking with the Board Insight System
Working with the Board Insight System Old Content - visit altium.com/documentation Modified by on 29-Jul-2014 Board Insight is a configurable system of features that give you complete control over viewing
More information13 Vectorizing. Overview
13 Vectorizing Vectorizing tools are used to create vector data from scanned drawings or images. Combined with the display speed of Image Manager, these tools provide an efficient environment for data
More informationRelease Highlights for BluePrint-PCB Product Version 3.0
Release Highlights for BluePrint-PCB Product Version 3.0 Introduction BluePrint V3.0 Build 568 is a rolling release, containing defect fixes for 3.0 functionality. Defect fixes for BluePrint V3.0 Build
More informationPhotoshop / Editing paths
Photoshop / Editing paths Path segments, components, and points Select a path Adjust path segments Add or delete anchor points Convert between smooth points and corner points Adjust path components Path
More informationPCB. Modified by Rob Evans on 28-May Parent page: PCB Panels
PCB Modified by Rob Evans on 28-May-2015 Parent page: PCB Panels The PCB panel gives you full acces to board objects, items and classes via a filtered browser. Summary The PCB panel allows you to browse
More informationComplete Tutorial (Includes Schematic & Layout)
Complete Tutorial (Includes Schematic & Layout) Download 1. Go to the "Download Free PCB123 Software" button or click here. 2. Enter your e-mail address and for your primary interest in the product. (Your
More informationRadial Diameter Dimension. Contents
Radial Diameter Dimension Contents Description Availability Placement Editing via an Associated Properties Dialog Editing via the PCB Inspector Panel Editing via the PCB List Panel Graphical Editing Notes
More informationThese notes list the main functional changes and problem fixes in each release of the software. They are listed in order, latest first.
Pulsonix Change Notes These notes list the main functional changes and problem fixes in each release of the software. They are listed in order, latest first. Version 3.1 Build 2273 : 18 Jul 2005 None.
More informationPCB List Panel. Contents
PCB List Panel Contents Function Content and Use Defining Panel Display Scope Working with Filtered Objects Displaying Workspace Selection Displaying Filtering Results Using the Panel to Select Objects
More informationPCB Design View. Contents
PCB Design View Contents Placing a Design View Defining the View Area Setting the Location and Scale of the Design View Defining the Title Interactively adjusting the Scale, Size and Focus of the Design
More informationAltium Encoder Demo. Step 1 - Create a Polar Grid
Altium Encoder Demo Note: In this tutorial I have used metric units. Altium defaults to Imperial units, you can change to metric once you have started a new PCB by selecting DESIGN>BOARD OPTIONS and then
More informationCreating a Multi-board Assembly
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) 主页 > Creating the Physical Multi-board Assembly Using Altium Documentation Modified by Susan Riege on Mar 23,
More informationChapter 4 Determining Cell Size
Chapter 4 Determining Cell Size Chapter 4 Determining Cell Size The third tutorial is designed to give you a demonstration in using the Cell Size Calculator to obtain the optimal cell size for your circuit
More informationCreating a PCB Design with OrCAD PCB Editor
Creating a PCB Design with OrCAD PCB Editor This guide is focused on learning how to create a PCB (Printed Circuit board) design. The guide will make use of the PCB Flow menu that is part of this workshop
More informationFrom Idea to Manufacture - Driving a PCB Design through SOLIDWORKS PCB
From Idea to Manufacture - Driving a PCB Design through SOLIDWORKS PCB Modified by Jason Howie on 24-Oct-2017 Welcome to the world of electronic product development in Altium's world-class electronic design
More informationTutorial : First board in CircuitMaker.
Tutorial : First board in CircuitMaker. Objectives 1. Create a new project in CircuitMaker. 2. Design electronic circuit in CircuitMaker schematic editor. 3. Design a pcb board for your circuit in CircuitMaker
More informationRelease Highlights for CAM350 Product Version 10.7
Release Highlights for CAM350 Product Version 10.7 Introduction CAM350 Version 10.7 is a support release that introduces new functionality, including encryption of CAM350 macros. New Functionality The
More informationDesign capture, simulation and layout - an introduction Tutorial
Design capture, simulation and layout - an introduction Tutorial A step-by-step introduction to Altium s complete board-level design system 1 Software, documentation and related materials: Copyright 2002
More informationIntroduction to Microsoft Office PowerPoint 2010
Introduction to Microsoft Office PowerPoint 2010 TABLE OF CONTENTS Open PowerPoint 2010... 1 About the Editing Screen... 1 Create a Title Slide... 6 Save Your Presentation... 6 Create a New Slide... 7
More informationA board is split into distinct regions by placing Split Lines (blue in color), which run from one edge of the board shape to another edge.
Board Region Old Content - visit altium.com/documentation Modified by Admin on Nov 6, 2013 Parent page: Objects A board is split into distinct regions by placing Split Lines (blue in color), which run
More informationCollaborate, Compare and Merge Panel. Contents
Collaborate, Compare and Merge Panel Contents Panel Access Terminology and Status Messages Actions section Work in Progress Regions Version Control Status Difference Map section Cell Differences See Also
More informationAltium Designer Viewer - Viewing PCB Documents
Altium Designer Viewer - Viewing PCB Documents Old Content - visit altium.com/documentation Modified by on 6-Nov-2013 In Altium Designer Viewer PCB documents are opened in the PCB Editor. The tools and
More informationAllegro PCB Editor with Performance Option or higher. The Reuse function can be used to create panels in PCB Editor
Title: Product: Summary: Panelization with Reuse Allegro PCB Editor with Performance Option or higher The Reuse function can be used to create panels in PCB Editor Author/Date: Beate Wilke / 07.02.2011
More informationSchematic Libraries, Models and Integrated Libraries
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) Главная > A Look at Creating Library Components Using Altium Documentation Modified by Jason Howie on Apr 11,
More informationAn Insider's Guide to the Query Language
An Insider's Guide to the Query Language Summary This article attempts to de-mystify what queries are, how and why they are used, and to provide insights into how these queries can be executed. An appendix
More informationCopyright 2015 Integrated Environmental Solutions Limited. All rights reserved.
Tabular Room Data User Guide IES Virtual Environment Copyright 2015 Integrated Environmental Solutions Limited. All rights reserved. No part of the manual is to be copied or reproduced in any form without
More informationVersion 16 Software Update Details. Problem Fixes in Version (18-Sep-2013) Problem Fixes in Version (17-Apr-2013)
Version 16 Software Update Details Problem Fixes in Version 16.0.9 (18-Sep-2013) o Editing a package in a library containing a user-defined package that uses a Prism would cause that Prism element to become
More informationString. Summary. Availability. PCB Editor. PCB Library Editor. Modified by on 20-Nov Parent page: Objects
String Old Content - visit altium.com/documentation Modified by on 20-Nov-2013 Parent page: Objects Placed String objects. Summary A string is a primitive design object. It places text on the selected
More informationPLAY VIDEO. Fences can be any shape from a simple rectangle to a multisided polygon, even a circle.
Chapter Eight Groups PLAY VIDEO INTRODUCTION There will be times when you need to perform the same operation on several elements. Although this can be done by repeating the operation for each individual
More informationAn Insiders Guide to the Query Language. Understanding Queries. Data Filtering - facilitating editing tasks. Modified by on 6-Nov-2013
An Insiders Guide to the Query Language Old Content - visit altium.com/documentation Modified by on 6-Nov-2013 This document attempts to de-mystify what queries are, how and why they are used, and to provide
More informationIntroduction Creating a Project Footprint Design
EEC 134 Application Note Introduction to PCB Design Cameron Vossoughi Introduction Being fluent in PCB design is essential for electrical engineers regardless of their discipline focus. This application
More informationDrill Table. Summary. Modified by Phil Loughhead on 16-Jun Parent page: PCB Dialogs
Drill Table Old Content - visit altium.com/documentation Modified by Phil Loughhead on 16-Jun-2015 Parent page: PCB Dialogs The Drill Table Dialog. Summary A standard element required for manufacture of
More information2008 년안산일대디지털정보통신학과 CAD 강의용자료 PADS 2007
2008 년안산일대디지털정보통신학과 CAD 강의용자료 PADS 2007 1 Learning the PADS User Interface What you will learn: Modeless Commands Panning & Zooming Object Selection Methods Note: This tutorial will use PADS Layout to
More informationUsing the Import Wizard
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) 主页 > Import Wizard Using Altium Documentation Modified by Phil Loughhead on Jun 18, 2017 The Import Wizard will
More informationArcView QuickStart Guide. Contents. The ArcView Screen. Elements of an ArcView Project. Creating an ArcView Project. Adding Themes to Views
ArcView QuickStart Guide Page 1 ArcView QuickStart Guide Contents The ArcView Screen Elements of an ArcView Project Creating an ArcView Project Adding Themes to Views Zoom and Pan Tools Querying Themes
More informationControlling the Drawing Display
Controlling the Drawing Display In This Chapter 8 AutoCAD provides many ways to display views of your drawing. As you edit your drawing, you can control the drawing display and move quickly to different
More informationAdding Objects Creating Shapes Adding. Text Printing and Exporting Getting Started Creating a. Creating Shapes Adding Text Printing and Exporting
Getting Started Creating a Workspace Pages, Masters and Guides Adding Objects Creating Shapes Adding Text Printing and Exporting Getting Started Creating a Workspace Pages, Masters and Guides Adding Objects
More informationPublished on Online Documentation for Altium Products (
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) Home > Creating the PCB Footprint Using Altium Documentation Modified by Annika Krilov on Apr 11, 2017 Concept
More informationAfter completing this lesson, you will be able to:
LEARNING OBJECTIVES After completing this lesson, you will be able to: 1. Create a template. 2. Understand the AutoCAD Window. 3. Understand the use of the function keys. 4. Select commands using the Pull-down
More information4 TRANSFORMING OBJECTS
4 TRANSFORMING OBJECTS Lesson overview In this lesson, you ll learn how to do the following: Add, edit, rename, and reorder artboards in an existing document. Navigate artboards. Select individual objects,
More informationExercise 1. Section 2. Working in Capture
Exercise 1 Section 1. Introduction In this exercise, a simple circuit will be drawn in OrCAD Capture and a netlist file will be generated. Then the netlist file will be read into OrCAD Layout. In Layout,
More information3D Body. Modified by Jason Howie on 8-Oct Parent page: PCB Dialogs. Other Related Resources 3D Body (Object)
3D Body Modified by Jason Howie on 8-Oct-2016 Other Related Resources 3D Body (Object) Parent page: PCB Dialogs The 3D Body Dialog. Summary The 3D Body dialog allows you to modify the attributes of an
More informationUTEXAS Embankment on Soft Clay
GMS TUTORIALS Figure 1. Sample slope stability problem from the Utexam1.dat file provided with the UTEXAS4 software. 1 Introduction UTEXAS4 is a slope stability software package created by Dr. Stephen
More informationSNOWFLAKES PHOTO BORDER - PHOTOSHOP CS6 / CC
Photo Effects: Snowflakes Photo Border (Photoshop CS6 / CC) SNOWFLAKES PHOTO BORDER - PHOTOSHOP CS6 / CC In this Photoshop tutorial, we ll learn how to create a simple and fun snowflakes photo border,
More informationOsmond Tutorial. First Page / J C Chavez / / Osmond Tutorial
Osmond Tutorial Draft Version corresponding to Osmond PCB Design Version 1.0b2 November 30, 2002 J C Chavez http://www.swcp.com/~jchavez/osmond.html jchavez@swcp.com First Page / J C Chavez / jchavez@swcp.com
More informationOrcad Layout Quick Reference
Orcad Layout Quick Reference Shortcut keys Toolbar Command mapping from Layout v7.10 to Layout Release 9 Cadence PCB Systems Division (PSD) offices PSD main office (Portland) (503) 671-9500 PSD Irvine
More informationUnified Cursor-Snap System (PCB)
Unified Cursor-Snap System (PCB) Old Content - visit altium.com/documentation Modified by on 21-Nov-2013 Related Videos Advanced Snap Management Cursor snap is the process whereby the physical mouse cursor's
More informationFrom Idea to Manufacture - Driving a PCB Design through CircuitStudio
From Idea to Manufacture - Driving a PCB Design through CircuitStudio Modified by Susan Riege on 13-Sep-2018 Welcome to the world of electronic product development in Altium's world-class electronic design
More informationSummary. Access. The dialog is accessed from the PCB Editor, by selecting Design» Rules from the toolbar.
Published on Online Documentation for Altium Products (http://www.altium.com/documentation) 主页 > PCB Rules and Constraints Editor Altium 技术文档新纪元 Modified by Phil Loughhead on Jun 19, 2017 The PCB Rules
More informationPCB Layer Stack Management
PCB Layer Stack Management Old Content - visit altium.com/documentation Modified by on 29-Nov-2016 Related Videos Define New Layer Stacks Layer Stack Regions A printed circuit board, or PCB, is used to mechanically
More informationComments. Summary. Modified by Rob Evans on Jun 10, Parent page: Workspace Manager Panels
Comments Modified by Rob Evans on Jun 10, 2015 Parent page: Workspace Manager Panels The Comments panel showing a collection of user comments for the currently active project. Summary The Comments panel
More informationPCB Filter. Summary. Panel Access. Modified by Admin on Dec 12, PCB Inspector. Parent page: Panels
PCB Filter Old Content - visit altium.com/documentation Modified by Admin on Dec 12, 2013 Related panels PCB Inspector Parent page: Panels Quickly locate and highlight objects using logical queries in
More informationPublished on Online Documentation for Altium Products (
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) Home > SnapSTEPModel Using Altium Documentation Modified by Jason Howie on Apr 11, 2017 Parent page: PCB Commands
More informationCADSOFT EAGLE TUTORIAL
CADSOFT EAGLE TUTORIAL IEEE OPS 2013-2014 By Shubham Gandhi, Kamal Kajouke 1 Table of Contents 1. Introduction 1.1 Getting Started 1.2 Eagle Schematic Editor 1.3 The Toolbar and Command Bar 1.4 Importing
More information3ds Max Cottage Step 1. Always start out by setting up units: We re going with this setup as we will round everything off to one inch.
3ds Max Cottage Step 1 Always start out by setting up units: We re going with this setup as we will round everything off to one inch. File/Import the CAD drawing Be sure Files of Type is set to all formats
More informationParent page: PCB Panel
Published on Online Documentation for Altium Products (https://www.altium.com/documentation) 主页 > PCB Library Using Altium Documentation Modified by Annika Krilov on Apr 11, 2017 Parent page: PCB Panel
More informationAfter completing this lesson, you will be able to:
LEARNING OBJECTIVES After completing this lesson, you will be able to: 1. Create a template. 2. Understand the AutoCAD Window. 3. Understand the use of the function keys. 4. Select commands using the Pull-down
More informationTutorial 1 Engraved Brass Plate R
Getting Started With Tutorial 1 Engraved Brass Plate R4-090123 Table of Contents What is V-Carving?... 2 What the software allows you to do... 3 What file formats can be used?... 3 Getting Help... 3 Overview
More informationBasic Concepts. Launching MultiAd Creator. To Create an Alias. file://c:\documents and Settings\Gary Horrie\Local Settings\Temp\~hh81F9.
Page 1 of 71 This section describes several common tasks that you'll need to know in order to use Creator successfully. Examples include launching Creator and opening, saving and closing Creator documents.
More informationThe Mathcad Workspace 7
For information on system requirements and how to install Mathcad on your computer, refer to Chapter 1, Welcome to Mathcad. When you start Mathcad, you ll see a window like that shown in Figure 2-1. By
More information