I am a new user of Allegro PCB editor of OrCAD 16.2. I want to modify an existed PCB design (*.brd) without schematic.My question is how can I utilize netlist & device files to place a self-created PCB package symbol.
I think I need to add my package symbol to Allegro's library. To make Allegro recognize it's name. Then when I modify netlist file with the name, Allegro will link to the *.dra file which I created.
If my thinking is correct, how can I let Allegro to recognize a new symble.
I'm not sure that I understand exactly what you want
Do you want to change the footprint (package symbol) of an existing component on the brd file?
Do you want to insert a brand new component on the brd without adding it to the schematic? If so, what type of component are we talking about since you don't want to place it on the schematic first for documentation purposes?
Please let me know and it will be easier to help you.
You would first export a netlist with properties using the menu selectionFile >Export >Netlist w/PropertiesOpen the netlist in a text editor such as Textpad. Make sure the text editor you are using doesn't inset white spaces as characters.Modify the netlist to include the new package in the "$PACKAGES" section. The format you need to follow is:ALLEGRO_SYMBOL_NAME ! DEVICE_FILE_NAME ; REFDES1 REFDES2 ... REFDESnIf there are special characters, such as a hyphen, you need to surround the name with single quotes.Sample:$PACKAGESCAP300 ! 'FCAP-1' ; C1 C2 C3 DIP14_3 ! '74LS00-2' ; U96 DIP14_3 ! '74LS74-2' ; U69 If you want to add nets to the design add them to the "$NETS" section with the following syntax (Again, if special characters are used surround the net name with single quotes)netname ; refdes.pin refdes.pin ...refdes.pinsample:$NETS'-MTCAS' ; R1.3 '-PRE' ; K1.6 R1.8 U69.4 U69.10 '-S0' ; U69.1 U69.13 A ; R1.7 U1.13 U69.12 Save the netlist as a new name.If you don't have the device file for the symbol you can create that using "File >Create Device" when in the symbol Editor.Open the design you want to modify and import the new netlist using the menu selectionFile >Import >LogicSelect the "Other" tabBrowse to the netlist file using the epsilon (...)Enable (Check) the "Supersede all logical data" checkbox.Select "Import Other"You should see the component available in the Place >Manually dialog. If you do not ensure that all of the pads, .psm and device file are in the correct paths; padpath, psmpath and devpath respectively.Place and route the component. You will need to update a schematic if you want this addition documented for the future.
Hope this helps,
In reply to Ejlersen:
I want to insert a new package on the brd without adding it to the schematic. The reason is that this design was releasing from a company. Their schematic was designed by Viewdraw software and I don't own the software. Accordingly, I decide to modify the PCB by netlist.txt & device file.
Now I have a problem to add a self-created package symble. I don't know how to add my own symble to the brd after I created it. Is there a specific folder to save the *.dra, and device file, then Allegro can recognize my symble?
thank you for your kindly response
In reply to Rik Lee:
This is really a detailed response. I followed your indication and success to add an existed symbol. But I do'nt know other ALLEGRO_SYMBOL_NAMEs which not exist on the exported netlist.txt. And I don't know how to sign a self-created symbol to be an ALLEGRO_SYMBOL_NAME.
Do you know where can I get an ALLEGRO_SYMBOL_NAME list and how to sign my own symbol be a ALLEGRO_SYMBOL_NAME?
You have mentioned "padpath, psmpath and devpath", so I tried to type each of them to the command line and got error "E- Command not found: padpath". I am not understanding this part, can you explain to me again?
I know it spend time to answer questions, but it would be very helpful to me. Thank you very much!
In reply to Kennn:
The ALLEGRO_SYMBOL_NAME is the name of the symbol that you created or have access to in your library such as a DIP14 or CAP300 which you want to add to your design.The psmpath, padpath, and devpath are the paths to your library parts.
"padpath, psmpath and devpath" are not run through command line. These are settings follow the process SETUP>USER PREFERANCES> in categories select PATH>LIBRARY and set the paths.