Whether you are just learning PCB design or have become a PCB Layout engineer, Allegro software is a tool that everyone must master. Next, 2PCB will share some tips on using Allegro software with you, hoping to help you.
Unit conversion
1mil = 0.0254 mm
1mm = 39.3701 mil
By default, we prefer to use mil units to draw PCB boards.
Allegro establishes the board frame of the circuit board
1) Set the drawing area parameters, including units and size.
2) Define outline area
3) Define route keepin area (Z-copy operation can be used)
4) Define package keepin area
5) Add positioning holes
Create bus
1) Open constraint manager (electronic constraint spreadsheet)
2) Display the specified network flying line: Display –> show rats –> net Then select the network to be displayed in the constraint manager
3) If you want to set equal length lines, but there are termination resistors on the line, you need to set it (x net) so that the termination resistors are crossed during calculation. This requires setting a simulation model library for each termination resistor. After the setting is completed, you can see that the network has become x net in the constraint manager
4) Add signal simulation model library: Analyze –> SI/EMI Sim –> Library Add model library –> Add existing library –> local library path
5) For each newly added model: Analyze –> SI/EMI Sim –> Model The devices in the project will be displayed, and then simulation models will be added for each device. For components in the system library that have their own model library, Auto Setup can be used to automatically complete it. For models that are not in the system library, select find model
6) In the constraint manager, click object -> right click, and you can use the filter to select the network you want to select. You can choose differential pairs, x net, etc.
7) Create a bus: In the constraint manager, select net -> routing -> wiring and then select the network you want to create as a bus -> right click, create -> bus
Set topology constraints
Wire length constraint rule settings
1) The requirement for wire length is actually to set the delay, which can be set according to length or delay
2) Open the constraint manager -> Electronic constraint set -> All constraint -> User – defined Select the network set when setting the topology -> right click and select SigXplore -> select in pro delay. In other words, if you want to set the wire length constraint, you need to define a topology first, and then specify the network constraints of this topology.
Relative delay constraint rule setting (i.e. equal length setting)
1) Before setting the relative delay constraint, you also need to establish the topology constraint first
2) In the topology constraint dialog box –> set constraint –> Rel Prop Delay set a new rule name –> specify the network start and end point –> select local (select this option for the two branches of the T-type network) and global (for bus-type signals)
Rename component serial number
1) Logic–>Auto Rename Refdes–>Rename–>Pop-up dialog box, select Use default grid and Rename all
2) components–>Click more, OK–>Click rename to rename
Allegro package origin modification
1) After opening the dra file, in the menu bar setup – change drawing origin
2) Enter the new reference point position in the command bar, if you want to change the new coordinate position to 1,2. Enter x 1 2
Add vias during Allegro routing
1) Perform simple settings before placing vias.
In the menu bar Setup->Constraints->physical
Find vias in the list and click it. A dialog box will appear and select the required vias in the dialog box. (If there are many types, you can enter v* in the filter below)
After selecting the vias, just close it.
Of course, there are many constraints to set here, such as how large the line width corresponds to how large the via is.
2) Use vias:
During routing, double-click the left button to add vias, or right-click.
Differential routing
1) Differential line routing: route –> connect and then select a pin in the differential pair. If the differential pair has been defined, the differential pair routing will be automatically performed.
2) If you want to change to single-ended routing when routing differentially, you can right-click: single trace mode
Change text size
1) Setup–>design parameter–>Click Setup text sizes in the text tab and change the line width [common values 20, 25, 30, 6, 3]
2) Edit–>change, select only Text on the find page of the control panel; set class to Ref Des and New subclass to Assembly_Top on the options page, check the Text block column and select the font size à select the entire PCB board, all fonts are highlighted–>right-click done