A panel design contains a set of PCBs representing instances of finished Pulsonix PCB designs. Use it to design your own panel layout to best accommodate multiple PCB designs, and optionally include profile shapes with breakout tabs or panel scoring lines to enable separating the PCB boards from the manufactured panel. These Tab-Rout shapes can be included in the drill output to either mill around the edges of the board outlines, or you can create V-score lines along the edge of each PCB board used to break the board out of the finished panel.

A Panel Outline can be added to a Panel design, this will contains design items; Copper on electrical layers can be added where needed, Mounting Holes can be added for tooling holes, Free Pads or Documentation Symbols added for fiducial alignment markers and text added for documentation purposes. A combination of these items can be used to create test coupons within the panel.

The Panel Wizard can be used to create an initial panel design containing multiple instances of a PCB design. If you do not use a technology file, the Layers, CAM Plots and Variants will be copied directly from the PCB design.

Alternatively, an empty panel design can be created by using New from the File menu and selecting Panel Design from the Designs tab. Once you have a new panel, the interactive options, such as Insert PCB Design can be used to add panel detail.

Locating this option

Available from: File menu > New > Designs tab > Panel Design option

The Panel Editor

Panels can be constructed to fit rows and columns in arrays of ‘like’ designs to maximise the use of the panel. If quantities of finished boards are required, this is the most efficient use of a panel. You can also add different PCBs to a panel and arrange them to get the ‘best fit’. Again, this maximises the use of the panel.

The illustration below shows a Panel with an array of ‘same’ PCBs set out as a 4x2. It also shows added detail within it used for final manufacturing; tab-rout paths and fiducial holes.

The Panel Editor process flow

There are two different methods of working:

  • Use the Panel Wizard and let it add the panel outline and PCB design. You will then add the panel detail such as Tab-Routing and Doc Symbols etc. The wizard is designed to make the process of starting a new panel easy for you.
  • Create a new panel using the New Panel option on the File menu. This will create you a blank panel design. From here, you can add your Panel Outline, PCB Designs and additional detail such as Tab-Routing and Doc Symbols etc.

Design entities within the Panel Editor

A panel is made up of a number of facets, each one is described briefly below with more detail available by clicking on their links:

Panel Outline

This is used to define the ‘size’ of the overall panel. It is added using the Insert Panel Outline option. The PCB designs are then placed inside the panel outline. It is usually a rectangle of a standard panel size, but sometimes is added as a shape with chamfered corners to assist with alignment through the assembly equipment. You can define a size for a panel border using Design Rules for the panel furniture.

PCB Designs

A PCB design or multiple PCB designs are inserted into the panel using the Insert PCB Design option or through the Panel Wizard. A PCB Design must have the same number of electrical layers and the same layer spans as defined in the panel design technology.

The PCB instance shown in the panel is just a representation of the actual PCB design, it does not contain the complete PCB contents. Each instance will display it’s board outline and mounting holes, along with any documentation shapes that are on layers that use a layer class with the Draw Shapes In Panel Design switch enabled. For example this could be used to display all silkscreen shapes. It will also contain any shapes, text, copper etc that are outside of the board outline and either on an electrical layer or on a layer using a layer class with the Check Items Outside Board switch enabled. Both layer class switches will be taken from the panel design layer classes. If you change these switches, reload all PCB instances to see the effect of the changes.

Tab-Rout Paths

Once the finished panel has been manufactured, each board must be removed. You can choose between using Tab-Routing or V-Scoring to separate the boards, or use a combination of both. This choice should be a decision made with your manufacturer. If milling the boards out using tab-routing is your choice, you can create tab-rout shapes around the outside of each board as a path for the profile router. These can be created free hand using one of the Insert Tab-Rout options, or can be automatically created around a selected PCB design using Create Tab-Rout Around PCB from the context menu.

These shapes will display their direction using arrows to help you align the cleaner cut side of the milling tool along the board edge.

Create Breakout Tabs

Gaps in the routing can be created using the Create Breakout Tabs function to form the breakout tabs to keep the PCB boards attached until the panel is ready to be broken apart. This function allows you add small drill holes in the tab, often called mouse bites, to aid the breaking out of the boards. If you have made a mistake and placed them in the wrong place, the breakout tabs can be removed from the tab-routs using the Remove Breakout Tabs tool.

Default settings for mouse bites can be found of the Panel Defaults page.

Applying Tab-Routs to All Board Outlines

When you have a PCB instance selected in the Panel Editor, use the Apply Tab-Rout to All Instances option available on context menu. This will take the existing tab-rout pattern and copy it to all similar PCB instances in the panel.

V-Score Lines

Adding V-Score lines to your design enables your manufacturer to score the panel using a V shaped cutter ready for the boards to be separated by breaking the panel along these grooves. These lines are always added as single lines parallel to the x-axis or y-axis. Usually they will be added across the entire width or height of the panel, but can also be created inside the panel if jump-scoring is required.

These lines will display their direction using arrows to help you create alternate direction score lines if required.

Copper

Panels often have cross hatched copper shapes added between odd shaped boards or in the panel border to strengthen the panel. If creating a multi-layer panel these shapes can have their cross hatching offset slightly on each layer to balance the copper coverage without adding too much weight. Copper can also be used to simulate tracks in a test coupon.

Mounting Holes

Use Insert Mounting Hole to add tooling holes in the panel border.

Documentation Symbols

Within a panel, Doc Symbols can be used to add additional information, such as Test Coupons, Fiducial Markers and V-Score notation for example.

Text and additional detail

You can add Text to a panel. This can be used to add additional information that is not already covered within the PCB design or on documentation layers. You can also add items such as Text Callouts, Drill Tables, User Reports and Attributes to a panel.

Variants

If the PCB designs in the panel contain Variants, the same variants must be added to the panel design if you want CAM Plots and Reports to take into account component and attribute variant differences.

Note: When creating a panel using the Panel Wizard with no technology file, the Variants will be automatically copied to the panel from the PCB design.

Checking The Panel

You can define Design Rules for Panel items that will be used by Design Rule Check. This includes checking that PCB boards are not within the panel border and are a specified minimum distance apart. It also allows you check that parallel V-Score lines are far enough apart and specify if jump scoring is allowed, or if the V-Scores need to cross the entire panel.

Manufacturing The Panel

The panel design can have manufacture outputs created just like you can for a PCB design. As well as the creating Plot outputs, you can also create DXF, ODB++, IPC-2581 and LPKF format output files.

You can create documentation plots that just contain what you can see in the panel design for each PCB board. When satisfied with the PCB board placement, manufacturing outputs can be created for each layer in the panel containing the full content of each PCB board.

The Panel Outlines, Tab-Routs and V-Score shapes can be included in a Gerber plot as instructions for your manufacturer, or can be output using NC Drill format to drive a V-scoring machine. This is done by creating separate plots using process “Panel” in which you can choose which shapes to output. Note: Horizontal and vertical V-scores can be separated into different plots.

Note: When creating a panel using the Panel Wizard with no technology file, the CAM/Plots will be automatically copied to the panel from the PCB design.

Generating Panel Reports

The Design Status Report can be used to report the size of the panel and list the paths of the PCB designs that are used in the panel.

The Report Maker can be used to generate a parts list or drill file for the whole panel using the standard PCB design user reports. This is done by adding the Include PCB Design Contents command at the top of the report script, and checking the Available for Panel box for the script. The Is Panel Design command can be used to differentiate between generating the report for a PCB design or panel design, for example to output the PCB Instance name before the component name for a panel design to uniquely identify each component.

The Report Maker can also be used to report items used in the panel design itself. This includes PCB Instances, Panel Shapes (Outlines, Tab-Routs and V-Scores) and Mounting Holes.

Panel Wizard | Insert PCB Design | Insert Panel Outline | Insert Panel Tab-Rout | Create Breakout Tabs | Remove Breakout Tabs | Insert Panel V-Score | Insert Doc Symbol | Plots | DXF | ODB++ Output | IPC-2581 Output | LPKF Output | Report Maker | Variants