Orcad X - organizing footprints and padstacks - Page 1
Forum section: electronics / general

author: geomer
author_rank: Newbie
timestamp: April 06, 2025, 08:01:09 pm
content: Hi Guys,I am starting to learn Orcad X. I've gone through a few tutorials on how to create footprints and I have a question which none of them seems to answer. Coming from Altium, I know footprint libraries get quite large; many library files with many footprints in them. In Orcad X, each footprint gets it's own file (which is also what KiCAD is doing) so that means many footprint files. But, what makes footprint organization worse are the padstacks. Each footprint can have a number of different pads and each pad type/size/shape gets it's own file. I get that padstacks get reused in footprints, but, when starting drawing a new footprint, how to you know oiff a particular padstack already exists? You could search by filename, but a padstacks has many parameters and it's not possible to capture all of them in the filename. When you have 10 footprints and 20 padstacks, it easy. But when you get to hunderds of footprints, it could become caotic. So, how do you guys who have worked with Orcad in small teams organize libraries (by folder structure and otherwise)?George

author: temperance
author_rank: Super Contributor
timestamp: April 06, 2025, 08:56:49 pm
content: I use one large directory for all those pad stacks. Most pad stacks are unique anyhow. But If you have a SOT23 and you need a SOT23-5, you can start from the SOT23.

author: nctnico
author_rank: Super Contributor
timestamp: April 06, 2025, 10:26:58 pm
content: I have the padstacks in a different directory as well. Typically I name these like footprint.pad footprint-mech.pad. So I can at least figure out which padstack goes with which footprint. And ofcourse, if a certain type of footprint has different number of pins (like a range of connectors), you obviously can re-use the same padstacks. The same for SOIC, QFN and LQFP chip footprints. I don't work in a team but I do have all my libraries in a git repository (accessible over the network) so I can transport between different computers and keep track of changes.If you come from Altium: make sure to create footprints for mounting holes. Mechanical footprints for holes with no electrical connection, regular footprints for holes with an electrical connection. This allows for a better control of what is on your board and keep the holes consistent. I have a design made by somebody else in Altium and it has 3 different styles of mounting holes (all wrong BTW) because the designer just put pads on the board. The same with vias. Some are tented, some are not. This just doesn't happen with Orcad (Allegro). The whole process is more rigid leading to less chances of errors and a more consistent design.

author: Uky
author_rank: Regular Contributor
timestamp: April 07, 2025, 07:50:49 pm
content: Since a task can be accomplished in many ways, there are not really thatmany "best practices". One has to evaluate whats suits best.I am working from home and have organized my Cadence installationso that the software is installed on my workstation and the librariesand customer projects resides on my own server.On one of the servers mapped disks top level is "\LIB" which resides directly under the root.Then Sub-levels\PAD\ (pads goes here)\SHP (shapes goes here)\FP (footprints, both .DRA and .PSM goes here)(And more sub directories for .DXF's, board templates, etc.)Since Cadence alows for multiple libraries in the user preferences"search" structure, you will want to keep the folder names shortand make sure that not two footprints with the same name existsin different libraries.I have chosen not to include any of the Cadence supplied footprints in thesearch string definitions since they do not adhere to the standards that my customers are using.Many free footprint providers uses long and IMO cumbersome naming conventionsmaking manual searching for already created pads time consuming when creating new footprint.Besides, many of them creates the fp's in a way that eg. silk screen appears over padsor uses way to thick appertures.I create pads (using metric dimensions) according to the following(all with file name extension .pad):smd0_80x0_30 = Surface mount pad. 0.8 x 0.3 mm (X,Y)np3_55 = non plated hole, 3.55 mm diameter.2_20rd1_00 = thru hole, 2.2 mm diameter, 1.0 mm plated hole.2_20sq1_00 = same but square pad.Via holes without solder mask opening are named eg. via1_00x0_20 (Diameter x hole)etc.These namnes turns up nice and sorted in the file explorer. it is easyto see if a particular pad has been created earlier.

author: passedpawn
author_rank: Contributor
timestamp: April 09, 2025, 03:59:50 am
content: I never search for a pad. I create new ones for everynewpart. However, of course, I have standard libraries that I have created.I have a set of folders for standard library parts (0603 passives, SOT23, SMA diode). These are all defined in the pad and footprint library paths. These paths are absolute paths. These standard libraries are in a set of folders I created and added to the schematic and pcb layout paths. See folder structure below.For each new design, new parts that are unique to that design (ICs, odd inductors, etc) get a local path in the project. That path looks like "../../symbols". This path is relative to the project.

author: geomer
author_rank: Newbie
timestamp: April 16, 2025, 07:30:10 pm
content: Thanks guys, appreciate the input.While on the subject of libraries, I do have another question. Do you use the cloud workspace for storing and using libraries? I'm not a fan of having data on the server of someone else, but, having cloud libraries does bring some benefits. I've used Altium's A365 in the past and the biggest advantage to using A365 library system compared to file based libraries is the introduction of components. When using file based local libraries, you essentially create a symbol in a schematic library, which has a footprint and manufacturer data attached. When you create a resistor or a capacitor library, you essentially have to copy the symbol for each entry, changing only the parameters. With could based libraries, you use components, which are basically just entries into a database, which have links to symbols, footprints and manufacturer data. I find approach much better, as you can reuse the same symbol over and over again (like with a resistor and capacitor for example).So, what kind of a system do you guys use with Orcad X? File based, cloud based or something else?George

author: nctnico
author_rank: Super Contributor
timestamp: April 16, 2025, 07:49:50 pm
content: What you need is the Orcad-CIS option. This uses a database to link symbols, footprints, part numbers, order numbers, datasheets, etc, etc together into a part definition. I have been using Orcad-CIS for 25+ years and am I strong proponent of a database driven workflow. Actually, I think Orcad-CIS works better compared to Altium's component database as far as my limited experience with using Altium goes. If you update the database driven part properties in Orcad, the part properties ARE actually updated. Altium is hit &miss.But none of this has to do with cloud. My database runs local (I use an MS-Access database located on a network share). I have the libraries and so on in a GIT repository which can be distributed to other computers over the local network. But git can also be used online using services like Github, Bitbucket, etc.

author: Uky
author_rank: Regular Contributor
timestamp: April 20, 2025, 08:33:49 am
content: +1(I use the same configuration - Access database, No cloud connection.)Using CIS BOM generation is also a powerful feature.IMO - Cadence should have included CIS in all OrCAD products.