So I was trying to update the title block of a schematic that I have. The title block that was on there was out of date . I clicked on place --> title block and was able to find the title block that I need. I also have a .OLB file that contains that title block. Then I created a Netlist with the old BRD file as the input file (To keep it as is but modify changes) but when I do that I still do not see / cannot place the title block that I need. Under Place --> format symbols in Allegro , I do see a title block that is coming from the database (But it's the old one). I don't know what to do at this point and would appreciate any tips. I did make sure that the path to where the library is , is defined in the user preferences. I also tried copying the title block under the library folder in capture before creating my Netlist and that did not work either.
Thank you all.
Title blocks in OrCAD Capture and PCB Editor are not the same or linked, they are just a drawing template. You would need to create your own Format Symbol for PCB Editor which could be an imported DXF or manually drawn titleblock. Open one of the supplied defaults from C:\Cadence\SPB_17.4\share\pcb\pcb_lib\symbols like asize or bsize to get an idea what you need to define. Once saved you can place this manually in a design using the Place - Manually command, change the drop down from components by refdes to Format symbols. Also make sure you enable Library under the Advanced settings tab.
I do have a BRD file with the correct title block template. If I understood correctly, I can open a BRD file that has the correct title block template and then deactivate all the layers except for the title block then export DXF, then create a new format symbol drawing with allegro , import the DXF , then save the format symbol under one of the paths that I have defined for psmpath and padpath? After that I should be able to place component manually under format symbols? Thanks a lot Steve!
Update: I have tried that and my title block now is showing under format symbols. However, there is no preview available and when I tick that option I do not see anything to be placed. Any tips?After selecting the format symbol, clicking on the canvas to place it removes my selection (The tick)
Thank you Steve
Maybe this info will help you out. As Steve pointed out Cadence offers a number of templates to use & these can be modified to your liking fairly easily. They are located at C:\Cadence\SPB_17.4\share\pcb\pcb_lib\symbols. Look for Asize,B,C,D .dra etc in there as a starting point.
A good way to approach using templates is to create a folder on your drive, maybe call it Allegro_Templates & copy the above A,B,C,D .dra's there as a starting point.
Next add that folder into your Library PSM path in the user preferences.
Open one of the templates .dra in the pcb editor. If it does not show up enable the "Drawing Format" options under Display Color/Visibility. At this point you can change things to your liking from the base template, for example the colors or the template border. Pretty much anything you like. Here is a pic.
You can even add in manufacturing notes etc so when you create a board you wont have to keep repeating that process. Sky's the limit.
When you get everything the way you want it go to Setup > Design Parameters > Design Tab and verify the drawing type is of type "Format". Lastly do a save as to save out the DRA. When you do the save as another file will be created called a .osm and it is this .osm file that will be used when you create a new board that needs that template. Since the folder is in your path when you go to place and select "Format Symbols" you should see it in the list.
At this point if you created a new board and placed that .osm template you could save the design out as something like B-Size_Template.brd. The advantage here is when you do a new schematic for say a new design you can use that saved in essence blank pcb that has the template all ready to go so you don't have to fiddle placing osm template symbols. Having a good starting blank board with a good template can save you a hell of alot of time doing new designs.
Thank you very much for your reply. Do you think I could achieve the same thing by exporting a DXF of another board (and turning all colors off except for the title block) and then importing it onto my board? Even thought I could see the symbol that I saved I wasn't able to place it/I might have saved the symbol as .osm and maybe that's why I couldn't. Thank you and Steve for your feedbacks.We do have some logos as well so I was trying to avoid having to embed these in one of the titleblock templates that come with Cadence.