Document Control questions with Variant Schematics > Forums

Unanswered

Active Topics

Forums

Forums > Silicon-package-board > PCB Design

Subject: Document Control questions with Variant Schematics

Posting to forums is available to community members only.
Login or Register

Rate this topic:

Author

Messages

IanO
Posts: 9
Online: User is Offline

5/16/2007 12:03 PM
I have a number of questions about how cadence intends to deal with document and revision control. I have searched the forums, sourcelink and the help documentation to no avail. So I hope someone on this forum has experience with document control and cadence. This post has very basic questions. I'll get to more difficult items later. The variant schematic editor looks to be a very smart tool and it allows me to store the master board along with all daughter stuffings in one project file. This is very cool, but I have questions about how to do ECOs on the daughters. We normally have a part number for each daughter schematic. This part number matches the number of the assembly. Each part number under the project can obviously be at different revision levels. How do I show a daughter part number and revision on the variant schematic? It looks to me that cadence treats the whole project as one item and does not have provisions to have sub part numbers and sub revisions. I found that I can annotate variant schematics and add text notes to them that contain the part number and revision. But if I have to make a change to the base which then has to be reloaded to the variants, all of the text added to the variant is replaced by what was on the base. Is there a way to manage custom text variables so that they can be populated with values through the variant editor? We normally have ECO information contained on each daughter schematic, but I can't see how to do that with variants in cadence. Thank you in advance for your help, Ian Overholt QSC Audio Products

pantheon
Posts: 7
Online: User is Offline

5/17/2007 5:34 AM
Hi Ian, You did not specify which of Cadence tool you are using for schematic. We are using OrCad, which can handle Variants. Most our designs are used in different assemblies and Engineer Designers here preferred to deal with ONE schematic rather different schematic for each variant. To do this we opted to add User Property to symbols in OrCad to identify which variant build any given component is used. On Documentation side they have written a customized tool that recognizes UP field out put in BOM. This customized tool can dump a separate BOM for each variant into company inventory database. We find out handling ECO/ECR are much easier this way. Regards, Pantheon

IanO
Posts: 9
Online: User is Offline

5/17/2007 9:50 AM
Whoops! I forgot cadence is composed of 10,000 tools that don't work the same way. :) We're using SPB 15.7 with concept hdl and allegro pcb. Concept has the ability to repopulate the base schematic on demand and not maintain separate variant schematics. But how will the service department service the variant models without schematics? And when a variant is revised per an ECO, where is that ECO number and date recorded on the variant? I can think of ways around this by using external (not with the cadence database) control documents, but I really hope that cadence has better document control capabilities than this. Thank you! -Ian

Richard V
Posts: 4
Online: User is Offline

5/17/2007 10:11 AM
Here is an example approach that may answer some of your questions: Given that PCB assembly part number is likely to change multiple times without requiring artwork iterations. We chose to create new Cadence Projects using the Fab part number. This choice provides an unchanging base part number on Cadence Project, along with the ability to capture multiple assembly numbers (and in your case schematics)in one project. It is also not practical to recreate a Cadence Project for each assembly number change (a variant). Keep in mind our projects contain one .brd file. If an artwork change occurs or if the design is not interchangeable (forward or backward compatible) it falls under the new number versus a revision category a new fab number is assigned and a new Cadence project is created. Or to simply, if you don't like variants or tabulation, consider a one to one relationship. One assembly to one part nuimber to one project. New numbers are cheap. Richard Van Os GE Healthcare

IanO
Posts: 9
Online: User is Offline

5/17/2007 2:05 PM
Hello Richard, We also build many variants from one board. One project had 78 variants using one board. We typically pull a part number for the board at the beginning of the project. Usually during the course of adding variants, changes have to be made to the circuit board. At those times, we pull a new part number for the circuit board and build new variants from that. Eventually, the older variants will migrate to the newer circuit board. The project with 78 variants used three different board part numbers over its development lifetime. The variant migration is a much more difficult issue with cadence, but I'm first trying to grasp the more basic concepts of cadence document control. In the case of cadence, I could put the part number of the variant as the variant name. But I do not see how to populate any ECO information (ECO number, date, approval stamp) onto the variant schematics. There are custom text variables, but they only apply to the whole project - not to just a specific variant. We used PCAD in the past and we had to have a separate schematic for each variant. We had to maintain a separate master schematic which netlisted to the board. It was very difficult to keep the daughter schematics netlistable to the board. Often during migration from one board to another, we would lose some of the original variant information. My hope is that cadence can manage this information better than PCAD did (which wasn't very well). The variant editor gives me hope, but I need to be able to pass more than component value changes to the variants. I know cadence must have been programmed to deal with ECOs, I just don't understand how it's supposed to work. Thank you, Ian Overholt

Richard V
Posts: 4
Online: User is Offline

5/17/2007 3:00 PM
Ian, We just started using the variant editor 6 months ago so I am by no means an expert. This is how we use it. We apply our different values with the variant editor at the BOM level. Which means we manually creating multiple variant.dat files for each part number. This is where you can also handle hardware and do not install instances. The variant editor has the DNI (do not install) at attribute at the BOM level . Using multiple variant.dat files and this property provides one way for us keep track of each configuration. Unfortunately this data in not tied to or driven by the schematic. Another approach could be: If you have multiple schematics you could drive different values using the schematic. To handle parts that are not installed there is a BOM_IGNORE property you can look into. DNIs parts appear in a separate area of the BOM while BOM_IGNORE will omit the parts from the BOM. I hope this helps Richard V GE Healthcare

IanO
Posts: 9
Online: User is Offline

5/17/2007 4:23 PM
Richard, I can understand how the variant editor changes the values on variants. And I have seen how the variant information can be backannotated to a variant schematic. But I still don't understand how to show any revision information on that variant. The only handle I currently see available to identify variant part numbers and revisions is in the name of the variant file itself. If the variant is backannotated to schematic named version. But this still doesn't allow me to say anywhere on the variant that ECO 8923 changed it from Rev A to Rev B and it happened last week. Using the file name to identify the part number and revision is a fairly low-tech document control situation - one we had to use with PCAD. I had higher hopes for cadence because it is a much more powerful tool. Thank you! -Ian

pantheon
Posts: 7
Online: User is Offline

5/18/2007 4:58 AM
"Whoops! I forgot cadence is composed of 10,000 tools that don't work the same way. :)" No you did not forget, I guess it went missing on me that CIS OrCAD and HDL are identical tools with differnt names!!!!! Thank You, P.

dallas
Posts: 0
Online: User is Offline

5/18/2007 5:38 AM
It sounds like we need to have a "custom text" definition section in the variant.dat files. Then you can edit the variant.dat to capture the ECO rev for each variant individually.

IanO
Posts: 9
Online: User is Offline

5/21/2007 9:47 AM
Hello Dallas, Custom text in the variant.dat file could work. I would imagine the difficulty in implementing this would come from trying to place it somewhere on the schematic drawing. The custom text would have to be setup in such a way that you place the field on the base and update that field on the variant. Right now if you create a custom text variable, that variable applies to the whole project. So you can't have 2 values for the same variable in two separate schematics. I can't shake the feeling that there is a solution already built into concept hdl and I just haven't found it. It seems like this is a basic documentation need and therefore it is probably addressed already. But I'm a new cadence user, so maybe I'm giving too much credit. :) -Ian

jcteyssier
Posts: 0
Online: User is Offline

5/21/2007 11:42 AM
Why do you not use one .cpm file per variant? Custom texts are store in cpm file, so: - One "master" cpm file to creta the "full board" - Several cpm's just to manage custom variables. It cans be used just for the "outputs": plots, pdf,.... I have never use variant module (maybe in future?) Jean-Charles

IanO
Posts: 9
Online: User is Offline

5/21/2007 12:12 PM
If I use a separate .cpm file for each variant, it seems like when I need to change the base then I will have to make the change separately on each variant. This is essentially how we had to use PCAD in the past. Variants were separated from the base and usually could not netlist to the board (because you can easily misconnect most resistors and capacitors from a netlist perspective). As a separate penalty, it doesn't look particularly easy to take a schematic from one .cpm to another. I read about how to do it on sourcelink, but when I tried it I lost my original schematic and didn't appear to have the one I copied either. Thank goodness we use a software vault so I could delete the project I corrupted and I download my working project again! We have adopted the policy of simply copying whole project when we want to reuse a significant portion of an existing schematic. So I could copy the project and then delete the board. This method could work, I'm just a little wary of it because it requires more manual maintenance of the project(s). That can be a recipe for trouble down the line when someone with no background on this project has to do some maintenance. Thank you for the suggestions -Ian

jcteyssier
Posts: 0
Online: User is Offline

5/21/2007 9:01 PM
I beleive you try to create new cpms with project manager. Dont't! Just copy with operating system utiliti (ctrl-cctrl-v on windows) the original file and rename it (like: my_old_file_version2.cpm). So all works with this new one. Then just edit custom variables (text editor in right cpm section or with projmgr setup). Be care to mofiy only that. All of that can be automated with a perl (or watever you are familiar) script. Hope this help.... Jean-Charles (well, coffe time for me!)

IanO
Posts: 9
Online: User is Offline

5/22/2007 1:50 PM
OK, now I see what you are saying. This would work, however to me it looks like a workaround that defeats the "intelligence" that cadence tried to build into the suite. We essentially had to do this with our PCAD suite, but we would like to take advantage of the more powerful database management tools that cadence appears to be built with. Performing significant workarounds will be our fallback position if we can't get cadence to better manage the database. Thank you for your input! -Ian

IanO
Posts: 9
Online: User is Offline

6/13/2007 10:49 AM
I'm still working with Cadence support on this issue. I will publish the solution here when we resolve the issue. -Ian

cdavies
Moderator
Posts: 55
Online: User is Offline

6/13/2007 11:15 AM
We have chosen to implement separate cpm files for each variant. We have a tool that will generate a new cpm file from the base when a new variant is generated. The variant file is examined and based on the identity of the variants, a one-to-one relationship is created between the the variant name and the varinat cpm that is created. Example: Variant name = pwra - CPM name = .pwra_variant.cpm - Note the period in the front, it make the file hidden, at least in unix. We have also implemented an editor to faciltate changing the custom text variables for each of the variant cpm files. When we plot, generate a BOM or any other aspect of a variant, we use the variant cpm file. This insures that the documents we generate have the correct identifications. For the Assembly drawings, we use color files. The color file carries the part number of the variant assembly, as well as the sheet number. Example: variant1-1.color variant1-2.color variant2-1.color variant2-2.color variant1 and variant2 above would translate to the actual assembly number. The -1 and -2 indicate sheet 1 of 2 of the drawing. We save a version of the .brd file in our PLM system with each variant including the base. This allows us to rev each variant independently. Hope the helps.

Charlie Davies

Posting to forums is available to community members only.
Login or Register

Forums > Silicon-package-board > PCB Design > Document Control questions with Variant Schematics

ActiveForums 3.6