Some help with Cadence Capture And Cadence Orcad - Page 1
Forum section: electronics / general

author: coldfiremc
author_rank: Regular Contributor
timestamp: May 25, 2019, 11:46:46 pm
content: Hi, I'm designing a little circuit with Orcad. In the schematic flow, I used some external spice models provided by manufacturers. One of the models was a complete .OLB capture Library. However, when i'm going to make the netlist, the utility fails, complaining there is no PCB layout for the part. The part package has inside it some .dra, .step and .PSM models and pcb layouts, but i don't know how to Setup capture to use this information, but I don't know how to provide this information to CaptureSpecifically, the parts are a couple of Wurth Inductors. Wurth provides pspice and pcb files in the website, but I don't know how or where to load the PCB files.Hope you can help me a little :-thanks

author: nctnico
author_rank: Super Contributor
timestamp: May 25, 2019, 11:55:09 pm
content: It seems to me that the parts don't even have a PCB Footprint property. Which is kind of to be expected from a schematic used for simulation. What kind of netlist are you generating?

author: coldfiremc
author_rank: Regular Contributor
timestamp: May 26, 2019, 12:15:09 am
content: PCB netlist.The problem is: I have the DRA and PSM files, but I don't know how to load them

author: nctnico
author_rank: Super Contributor
timestamp: May 26, 2019, 02:04:35 pm
content: What do you want to achieve? A PCB layout or a simulation? For simulation you use the Spice models but these won't have footprints assigned to them. Generally you don't use a simulation library for a PCB layout.

author: sorenjul
author_rank: Newbie
timestamp: May 29, 2019, 12:36:53 pm
content: HiTo add footprint information to parts in Capture just double click on the parts and add the file name of the footprint to the property named PCB Footprint.Schematics used for simulation can easily be used for PCB Layout PSpice components typically have a PSpice_only property set which leaves them out of the netlist - just make sure you haven't added series components because that will give you open connections. Some manufacturer doesn't create schematic symbols that match the physical package of the component for PSpice simulation so check them and verify that they have the same pin numbers.Another option is to have schematic folders in your project for simulation and others for PCB layout - this way you store all your design information in a single project.After netlisting place your padstacks (.pad) and footprints (.dra & .psm) in the correct folders - typically your system will be configured to look into the same folder as your pcb layout file (.brd) or in a subfolder named symbols.This should get you going :-)

author: nctnico
author_rank: Super Contributor
timestamp: May 29, 2019, 07:09:02 pm
content: I'd be careful with using simulation symbols for PCB layouts because the pin numbers are often different and/or incomplete. It is better to have seperate libraries for simulation and PCB design. I'm not saying it can't be done but most of the symbols which come with simulation models I've seen from manufacturers aren't suitable for PCB design.

author: coldfiremc
author_rank: Regular Contributor
timestamp: June 02, 2019, 06:54:01 am
content: That did it :- . Adding the footprints to folders and everything worked.That inductor was the main problem. Now Footprint loads correctly (and also the part is simulation capable)Kind of related...An easy way to put heatsink layouts?