Hi,it's the first i'm using allegro and i would like to know how can i convert the libraries i have from layout to allegro.Can i use them or must i design the footprints from the beginning in allegro?
Thanks for your time.
Providing that you have a sufficiently high version number, I think that at least 10.0 is required, you can use the Catalog tool. In the LSession (grey) window when Layout is started, Tools>Catalog>Create, point to the LLB file and create the catalog. This will create a MAX file, or files, of all of the library parts. (You may get multiple files since Layout has a drill limit of 40 drills per MAX file) You can then translate the MAX file with the OrCAD Layout import / conversion. Note that Layout has oversized pads for plane layers, PCB Editor won't use these so the inner layers in the conversion can be deleted, the translation will create the required "default internal" data from the regular pad for thru parts)
If you have a pre-Catalog tool version of Layout, you will need to add the footprints manually to a desgn and then convert the resulting MAX file.
1) Anything which you have on a global layer will not be translated since there is not global layer in PCB Editor.
2) Any height keepouts which are round or have a rounded section will not get translated.
In reply to KEN13:
How about Title Blocks that are parts, I can't get them into Allegro. I tried converting boards and the title block won't come in. I also converted my libraries and the parts all come in minus Title Blocks and out layer stack up that are saved as parts.
It shows a (#Refdes) where the title blocks would be but nothing more. Global visibility is on and nothing shows up.
I don't want to recreate every single title blockl and all the text associated with them.
Lonf time Pads user and worked with Orcad and now this company is finally switching over to Allegro from Orcad10.5
Any help is appreciated..
In reply to DonlAZ:
I suspect your title block is on a layer that the translator does not support. What layer in Layout are you using for Title Blocks ?
From memory mine are on the asy top layer and they translated into Allegro fine without issue.
BTW, Orcad 10.5 is very old, You might want to pull your designs and libs in to an orcad 16 x version of Layout first save them and then try export etc. I believe the last ver of Layout was 16.2
In reply to ScottCad:
Thanks Scott for your reply!!
Yes 10.5 is old but government contractors like stability and don't change much..
The Title block is on the Drill Drawling layer and we're just now upgrading to 16.3 and want to get out libraries and title block info into it.
I also sent it into suport a few days ago and they got back to me a few days later on Friday. They guy had the file first thing that day but haven't heard back yet so not sure what the fix will be. I wouldn't think it should be that hard to translate. Long time Pads user and just now learning Allegro at a new position. Well used Orcad for a few year here until it got slow and now back again and tney're finally upgrading.
Thanks again for your help..
Hi Don got to love the Gov Work : )
Since your Title Block is on the drill layer I would move that to the ASSY Top layer in layout as a first step. I had a bunch of designs done in the layout 16x package and they translated really well into Allegro. With the title block on the assy top layer in layout when you translate the design it will put it on the Board Geometry > Assembly detail layer in allegro which is a good fit.
If you have the opportunity try upgrade to Allegro 16.5 which is the latest. They made great ease of use strides with 16.5 but still no library manager yet.. Perhaps V 16.6 will get one : )
Actually thinking about allegro I still use layout to create footprints and import them into Allegro because well it is easier : )
Best of luck with the migration
Great tip on creating library parts thanks!! Oh and supposedly 16.5 is to be installed at some point.
Now onto other topics, can Allegro really not bring in a simple title block and notes conversion,,, WTF
I tried moving them to an Assy layer but nothing comes over in the translation. I can't beleive they couldn't open the file in a mid version between 10.5 and 16 and upconvert. I used Pads for 17 years so I was used to support being supportive ;-)
I can't imagine a large company telling its customers they have to breate a bunch of work because we can't figure out how to tranlate our own files.
I got this from cadence:
I could find out that the Manufacturing Notes and the lines of the Title Block are not getting translated during Orcad Layout to Allegro Translation. This is a known limitation and we have asked our R&D team in past to add this functionality. But the issue is not planned for implementation in near future with the releases under development.
Unfortunately I could not find any work around for translating the data. It will be required to add these title blocks as Format Symbol in Allegro PCB Editor.
As I am not in condition to provide any support regarding this known limitation, I am planning to close the Service Request.
Don, I was incorrect about having the TitleBlock on the assy layer in layout. It should be on the FAB layer. Moving between tools I guess I got my layers mixed up. Anyway I opened one of the .tch template files in layout which contained a title block. I saved out the file as a max file and then imported into allegro.
The import of the template worked good and came across OK as far as I can see. In Allegro it put the fab drawing on the Assembly_Detail layer.
I added some notes to the max file fab layer to see if they would import into allegro and they came across ok. Text size needs adjusting but other than that the template looks good.
Give that a go and see if it works. I was using layout 16.2 for the test.
I got it to work finally. I stipped out all the copper area's through the spreadsheet and got it to come in but the text sizes are all messed up and overlaping the successive lines. Now I've got to get the text size and import our Logo, it was the cause of the copper area's.
Thanks for your help in this Scott!!! I'm still amazed tech support couldn't figure this out over a week long user..