Placement replication was introduced in Allegro PCB Editor SPB16.2. At that time, the application was limited to replication of component placement. The SPB16.3 release introduces the support of etch circuits (shapes, clines, vias) as well as ease of use improvements associated with basic move, mirror and rotate functions. Once replicated circuits are placed, physical changes such as moving components or modifying etch circuits are easily instantiated across all instances with a new update command.The methodology for creating and applying replicated circuits is similar to that of SPB16.2 however the stored file format is different due to the support of etch and the refresh capability. The file format leverages the legacy module (.mdd) database structure and replaces the circuit replicate file (.crf) format. SPB tools continue to support the front end driven re-use flow and the backend driven placement replication which is schematic neutral. Placement replication files can be leveraged across different designs containing common circuitry blocks such as decoupling schemes for high pin count devices, memory arrays, and IO channelsPlacement replication is only available within the "Placement Edit" application mode environment. The use model requires the pre-selection of symbols followed by a RMB action command.
Aligning modules and replicated circuitsThe alignment of re-use modules and place replicate circuits is now supported in Placement Edit Application mode. The use model is similar to the Align Components command that was introduced in 16.2. The three step process begins with a window selection of the module circuits; hover over a symbol within the circuit you wish all others to be aligned to and then using the right mouse button command "Align Modules" to perform the alignment.
Using the commands1. Enter the placement application mode.
2. With the seed circuit placed, window select all of the components followed by a right mouse button "Place Replicate Create." When accessing the right mouse "Place Replicate Create." menu item be sure to hover over a component element, such as a pin, in order to get the right mouse button menu. Hovering over black space will not produce the commands related to the selected elements.
All intra connected circuitry will be highlighted.
3. You will be given the opportunity to select or unselect additional etch from that which was auto-generated for the seed circuit. A typical application may be to extend the circuit to include I/O.At the Allegro command window you will be prompted "Select/unselect additional etch as needed, then click Done." Select or unselect additional etch elements using the combination of the left mouse button and the control key. In the image below the 5 clines off of U120 were selected.
4. You will be prompted to "Pick origin or use RMB for Snap to" functionality. Use the Snap to functionality to snap to a pin or via or other element.5. You will be prompted, with a GUI to save the seed circuit. It will be stored in .mdd format.6. Window select the remaining components that you want to replicate followed by a right mouse button "Place Replicate Apply". You can either continue in the right mouse button selection to select the replication module or select "Browse" to use a GUI to select the module.. Minimize the selection to relevant components to minimize any performance impact.
7. The following interface appears which lets you swap components. The first column lists the contents of the next circuit to be placed, the second column lists the swappable components in that circuit. When a component is selected in the "Swappable" column, a list of components to swap with appears in the "Swap With" column.
8. Selecting "OK" will place the replicated circuit on your cursor.
9. Place all of the circuits. Care doesn't need to be taken to place them in proper alignment.
10. Window around all of the replicated circuits, including the seed circuit, and select right mouse button "Align Modules" while hovering of a component that you wish the other circuits to be aligned to.
11. If a change needs to be made to the circuitry you can make those changes and then update those changes to the other replicated modules. IN the image below some delay has been added to etch.
12. Set the super filter (right mouse button) to "Module". Hover over the circuit that the changes were made to and select, using the right mouse button, Place replicate apply. You will be prompted to select/unselect additional elements and then select "Done".
13. A file save GUI will be presented to you where you can save the circuit. At that time the updates will be applied to the circuits in the design.
-14. While you are in the placement application mode and the super filter is set to "Module" you can move the replicated circuit as a group by hovering over the module and selecting "Move". You can also take advantage of single pick functionality by enabling the right mouse button functionality "Customize -- Enable Single Click Execution." Using this you only select the module to move rather than hovering over the module and selecting "move" from either the right mouse button or the Allegro menu.14. While you are in the placement application mode and the super filter is set to "Module" you can move the replicated circuit as a group by hovering over the module and selecting "Move". You can also take advantage of single pick functionality by enabling the right mouse button functionality "Customize -- Enable Single Click Execution." Using this you only select the module to move rather than hovering over the module and selecting "move" from either the right mouse button or the Allegro menu.
As always - I welcome your feedback and suggestions on using the new SPB16.3 features.
Jerry "GenPart" Grzenia
I'm not too sure of the exact nature of the issue you're having based on your description. It "may" be a older release problem, or a database problem, or just a use model issue. The best method to getting this resolved would be if you contact our Customer Support team at http://support.cadence.com so that an Allegro PCB Editor expert AE can work with you to resolve this specific issue.
i am using cadence16.3. my old project is orcad9 i am translate this pcb to cadence 16.3. after converting one ic(U1) is hide.that U1 manually place there.i try to place that component but that component not placed.please tell me any another way of this project translation
PCB Design L would be the lowest level product supporting these SPB16.3 features.
Is this option available in Orcad PCB Editor 16.3?
What I suspect you're trying to do, is if you move the Ref Des position(s) for footprints on the original circuitry that you made the copies (replications), you want all the Ref Des positions in the replicated circuits to also move accordingly. You need to move each of the replicated circuit Ref Des positions individually. Let me know if this answers your question.
How to "replicate update" the silcscreen drawings, e.g. Ref Des positions and orientation?
Hi Ashok -
This functionality is part of the Allegro PCB Editor SPB16.3 release - you don't need to purchase anything separately. Also, while you're replicating the modules, the part ref des/pin # values are being driven from the schematic netlist - this is why you see the values automatically being updated as you replicate a circuit. So, the synchronization is maintained.
while using this repeat placement how to sync the repeated placement with the schematics. also please let me know is this function a model which needs to be purchased seperately?
The Allegro Free viewer for the SPB16.3 release is now available!
You can flip & rotate, but the stack needs to be the same. If you try to place it on a board with a different stackup the application will issue a message that the stackup are not the same and not place it.
Good write up Jerry.
You mentioned a mirror function - will this support flipping the circuit to the other side of the board? So, in a 4 layer board, layer 1 is mapped to layer 4, layer 2 to 3 and so on?
Also, if I wanted to use a circuit from one design in another, do the layer stackups have to be the same?
The SPB16.3 free viewer is not available for download just yet. When it is, you can use the Cadence Online Support Solution# 11250908 to locate it (www.cadence.com/.../Downloads.aspx)
If you have installed Allegro you can use the executable in Cadence_installation_directory/tools/pcb/bin/allegro_free_viewer.exe
When will 16.3 viewer be available?