Allegro - OrCAD Reuse module Procedure Problems > Forums

Unanswered

Active Topics

Forums

Forums > Silicon-package-board > PCB Design

Subject: Allegro - OrCAD Reuse module Procedure Problems

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

Rate this topic:

Author

Messages

robyd
Posts: 17
Online: User is Offline

6/07/2006 10:24 AM
Hi all I am currently in the early stages of layout involving reuse modules. me and my customer had one success building a reuse module ( MDD ) and re loading it to other BRD 4 times. i checked that routing passes silk and assy Ref Des changes and even moving and changing components rotation. then asked the customer in order to check the entire procedure to delete and add a component to the base module and to see if the changes propagate to the main BRD. but then all kinds of problems begun. as i think they are related to the OrCAD anotation procedure. I get duplicate RefDes in the main BRD ( each module contains R20 ) we tried updating the REUSE_ID in the schematic of the module. and i also noticed that only CS traces are copied to the modules ( other layer traces are deleted ) has any of you passed thru this procedure with success ? any recommendations ? am i doing something wrong ? any help will be appreciated thank's

cmusetti@silverstorm.com
Posts: 0
Online: User is Offline

6/07/2006 11:25 AM
From what you have said iyou have left out a lot of steps here. 1st if you make a change to the base module you need to do a tools->annotatate-> Allegro Reuse tab and generate the reuse module symobal. 2nd) need to replace the cache for that reuse module symbol by doing a replace on that symbol 3rd) If you have made a change that effect the physical symbol .mdd which adding a component would you need to update the .mdd by reading the netlist created from the reuse module schematic into and then place the component and route if thats what you want. then recreate the .mdd file 4th) you need to take theschematic with reuse symbols in it and tools->annotatate-> Allegro Reuse tab and reunumber the design for using reuse modules since you have all ready associated the schematic to a board you will want the action to be set to incremental. 5th) netlist and read into board It sounds like the renumber action step was missed or set to absolute. There is a paper out there on this procedure check it out http://www.cdnusers.org/Articles/Download/tabid/163/Default.aspx?title=Capture/CIS/Allegro%20Design%20Reuse%20Flow%20with%20Electrical%20Constraints Hope this helps Carl

robyd
Posts: 17
Online: User is Offline

6/08/2006 11:01 AM
Hi Carl thank you for the info in your reply you say [quoteΤnd) need to replace the cache for that reuse module symbol by doing a replace on that symbol[/quote] i don't understand your terminology can you explain replace the cahche . there are detailed instruction in the Orcad HELP >learning Capture > Capture Allegro Design Reuse which i followed both in orcad and allegro. the first try worked very smooth. (including changes to Comp placement route ans save new MDD and update to the root PCB) then i asked the EE as an Experiment to add and remove a component and do connectivity change in the reuse design in order to check the procedure before the real work ( which will invovle 8 big modules - each about 150 comps - which may change during the work) but then the problems started : we had few cases components with out RefDes ... "R?" componets without REUSE_ID assigned. comps with duplicate Part Refernce in the OrCAD which resulted in 4 R20 in the Base PCB. we noticed that it happens when both reuse design and base design are open in capture and that before annotating the reuse design we have to uncheck and recheck the Generate Reuse Module before selecting the OK on the Annotate > Allegro Reuse TAB. the EE Duplicated one of the existing Res in the reuse design for our experiment . and then the duplicated Res's have same Part Reference as the copied Res. when got the base design ( at our PCB layout office) same parts in different reuse block had same Part Reference. we found that it is related to the fact that the implementation path of the blocks at the customer were different path then mine (which i updated manually) then he changed the implementation path to be only the reuse design name and saved it in same directory as the base design which i also did. we had about 8 netlist to try and solve the problem but we haven't solved it yet. i am almost sure that the problem is related to the OrCAD side and not to the Allegto. i hope that the answer is around the corner. can you direct me to it ? i started reading your methodical technical article . and me and the EE will have to work with it as a checklist. thanks for your help

robyd
Posts: 17
Online: User is Offline

6/08/2006 12:24 PM
Hi Carl 2 more questions 1. do the REUSE_ID , REUSE_PID , REUSE_NAME , REUSE_INSTANCE properties must be present in the allegro.cfg ( configuration file ) ? 2.is it mandatory to lunch the allegro from within the OrCAD Capture or my customer can mail me the net file ( 3 DAT files) and i use import logic. thanks

CTMusetti
Moderator
Posts: 27
Online: User is Offline

6/08/2006 2:02 PM
By replace Cache I mean bringing the current up to date library symbol into the top level design. In the project wiindow expand the Design Cache folder find the symbol which is the design reuse symbol left click on it the right click and select replace cache. The only way ref des came out like R? is if the design was not annotated for allegro reuse before netlisting You can not change the implementation path easily for the schematic reuse symbol there fore should always be left alone this is a known limitation tat is documented. This sounds like the classic problem of nothing behind the scenes in the ORCAD Allegro flow doing any type of management. With concept you had tools like Heirarchy manager and Design Sync to keep the data inline, with ORCAD there is nothing and you must mange these processes yourself. And you must be methodical in your approach or else all hell can break out just like this. So what I am telling you is change must be made wit in the procedure that I have outlined for you and backannotation should be used, when you are doing this whoever is edditting the board and is affecting logic must communicate with the person editting the schematic that they can't be editting and making changes while this is going and vice versa. The REUSE propeties do not need to be present in the allegro.cfg It is not mandatory to launch allegro from with in ORCAD Hope this helps

robyd
Posts: 17
Online: User is Offline

6/11/2006 9:24 AM
Hi Carl thank you very much for your detailed answers. we finally found other problem with the occurances and instances defenition in the reuse design. regarding your replace cache explanation : our reuse design is not saved as a symbol but referenced as an external design ( which is best ?) i now check the reuse and base design netlists to see whether : 1. the reuse net (*prt.dat) contain the REUSE_ID propertiy for the components. 2. the base net contain the REUSE_NAME , REUSE_INSTANCE, REUSE_PID which is on of the indicators for the health of the reuse procedure in the OrCAD. what we have seen is that after chnages made to the reuse design (adding deleting comps) re annotating and netlisting (both designs) not always the attributes mentioned appear correctly. sometimes they appear only after few times annotating or exiting or rechecking the check box in the Allegro reuse TAB and then annotating. so still something is happening behind the scene in OrCAD. now that i have the PCB loaded with my four modules (in my PCB test case )i have few more questions. we placed the modules randomly on the PCB for future fine placement. module movement and rotation and changes to route is possible within the placed moudules. but for example if the reuse module should be updated during the layout then a new net and .MDD should be done and then new net import for the base PCB and then do an Update Symbols ... on the PLACE menu. and here is my question the update moves the modules to the first randomly placed origin and same initial rotation. so i tried deleting the moudule and replacing it but it doe's not apear as not placed moudule instace . so i tried loading the net list again and then to place it but it doesn't appear in the moudule instances list. when doing a Update Symbols ... on the PLACE menu the moudule appears again at it's original placed location and rotation. as if the initial placement is recorded in the BRD file and can not be overridden. so it means that the moudule should be placed at the first time exactly on it's final position without having the option to fine tune it's location ? it can't be this way !! am i missing something. is there a way to change the moudule placement location and rotation ? or is it something not being addressed yet ? thank's again for your help roby

robyd
Posts: 17
Online: User is Offline

6/11/2006 10:17 AM
Hi Carl sorry for being so jumpy. I found the answer for the module movement and rotation by exploring the HELP. It is done using the Groups Find Filter. the explanation found at Para 8 : Working With Groups and Modules of the algroplaceTOC.html in the documantation. i should have read the HELP before jumping ;-) but if you have a clue for the fist described phenomena with the REUSE properties i will be very thankful roby

CTMusetti
Moderator
Posts: 27
Online: User is Offline

6/13/2006 6:24 AM
Roby, I am having a difficult time understanding exactly what the problem is. I'm not sure if it can map the properties correctly if there is no reuse symbol though. I have always created library symbols and reference the schematic logis from that symbol I create. If you notice in the allegro reuse tab of the annotation menu there is a function to generate the reuse module. When you make a change to that reuse module you will need to do this. Then netlist and read into the allegro reuse .mdd and create an updated allegro .mdd This is what keeps the reuse properties in sync with the top level after doing an anotate at the top level. When I was last using the reuse modules in 14.2 there was no update module available and was deleting and rea adding the symbols to get updates, and boy do I understnd you pain here. Very time consuming and error prone. I am now on 15.5.1 and now see the update modules and am going to play with that to understand how that works. Thanks for the documenttion hints. If you want you can call me and we can go through your design over the phone so I can get a better appreciation for what the problem is. I have not been able to reprouce those type of results by following the change procedure outline earlier. I can disrupt the reuse properties by doing a step out of order or by skipping a step. Hope this helps Carl 610 233 4828

lemery
Posts: 1
Online: User is Offline

11/29/2007 11:00 AM
I had the same problem with the layers. Check all the layer names to be sure that the module layers match up with the top level Allegro file.

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

Forums > Silicon-package-board > PCB Design > Allegro - OrCAD Reuse module Procedure Problems

ActiveForums 3.6