- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
As someone who is familiar with importing Orcad Schematic and Allegro PCB into Altium, I have to ask the question why doesn't Cypress save the .brd file in ASCII format. This way, almost every EDA tool can import Allegro PCB files with minimal issues. Instead, Cypress saves the .brd files in BIN format which requires that you have a "compatible or latest version" of Allegro installed on you system to convert the BIN file to ASCII so that you can import that PCB. I would ask that anyone at Cypress who has Allegro installed, please read in the .brd file and save it as ASCII format. This way, we get the PCB footprints and synchronizing the Schematic to the PCB is pretty easy.
Here are the PSOC KITS I'm working on:
CY8CKIT-062-WiFi-BT
CY8CKIT-149
The only other way to achieve this is to Import the Gerber file and convert to PCB
1) import the Gerber files into CAMtastic (%FSLAX25Y25*MOIN*% - English not Metric, Leading Zero Suppression, 2 Digit Integer, 5 Digit Decimal)
2) import NC Drill file (INCH - English not Metric, No Zero Suppression, 3 Digit Integer, 6 Digit Decimal)
3) generate Netlist
4) export to PCB
5) Setup PCB Stackup
5) Add footprints to each Schematic symbol
6) Synchronize Schematic with PCB
7) Place all components on Board and delete original pads imported from Gerber file
😎 Delete almost 2,000 polygons and create all necessary polygons
As you can see, this is a crazy amount of work and all this can be avoided if the Cypress Engineer or PCB Contractor would take 5 min to export their PCB in Allegro ASCII format. If Cypress is interested, I am prepared to convert any of your PSOC Kits to Altium format and post them for the Community. The process I use to import the files into Altium does find Schematic/PCB inconsistencies that are common for developers using Orcad/Allegro. While I do generate a gerber output and compare it to the original gerber file, the standard proviso will apply: "Use at your won risk".
Regards,
John
Solved! Go to Solution.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
I followed that articles suggestion and downloaded a trial version of Orcad.
The conversion from Allegro to Altium worked fine. This would only take a few minutes for each Eval Kit and would make our lives a lot easier.
Here is what I did:
I added the C:\Cadence\SPB_17.2\tools\bin into my path.
I copied the Allegro2Altium.bat file plus all the config file from C:\Program Files\Altium\AD19\System to the folder containing the Cypress Allegro brd file.
Then I ran the following command:
Allegro2Altium.bat CY8CKIT-062-WiFi-BT Layout.brd
This produced a file called CY8CKIT-062-WiFi-BT Layout.brd.alg, which I was able to import into Altium using the Import Wizard.
Regards,
John
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
Hi John,
I suppose you are trying to convert Allegro PCB files to Altium format. This needs Allegro and Altium to be installed in same machine and Altium conversion wizard will directly connected to Cadence Allegro PCB installation .
I am sorry but presently we don't have both Allegro and Altium installed in the same machine.
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
Thank you for your reply, but that wasn't what I was asking for. I don't want anyone else to convert the PCB from Allegro format to Altium as you stated. I am willing to do that as long as Cypress provides the Allegro PCB in ASCII format. Anyone who has Allegro installed on their machine can open the Allegro PCB and save it in ASCII format. Should take a few minute to complete.
Regards,
John
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
Hi John,
You can try the solution which have been given in below links, it may be helpful:
https://www.altium.com/documentation/18.0/display/ADES/((Allegro+Import))_AD
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
Thank you again for all your help. The links you provided confirm what I have been saying. If you want to import Allegro bin format into Altium, you have to have a licensed copy of Allegro installed on your system. I'm not sure why you say there is no option to save the brd file in ASCII format. I have converted many Allegro files into Altium format for the BeagleBoard community and they just send me the Allegro file in ASCII format.
Regards,
John
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
Doing a little more research, apparently there is a program called extracta.exe which is use to convert the BIN file to ASCII format. This file is part of the Allegro installation.
Regards,
John
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
I found this article that may help:
https://nilsminor.de/index.php/2018/05/15/how-to-convert-an-allegro-brd-pcb-to-altium-pcbdoc-file/
Regards,
John
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
From that article, you run the Allegro2Altium batch file (attached), which runs the extracta.exe file from Allegro. The batch file requires several configuration files which I have attached.
So my guess is you would just run Allegro2Altium.bat <Allegro.brd>
Regards,
John
- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report Inappropriate Content
I followed that articles suggestion and downloaded a trial version of Orcad.
The conversion from Allegro to Altium worked fine. This would only take a few minutes for each Eval Kit and would make our lives a lot easier.
Here is what I did:
I added the C:\Cadence\SPB_17.2\tools\bin into my path.
I copied the Allegro2Altium.bat file plus all the config file from C:\Program Files\Altium\AD19\System to the folder containing the Cypress Allegro brd file.
Then I ran the following command:
Allegro2Altium.bat CY8CKIT-062-WiFi-BT Layout.brd
This produced a file called CY8CKIT-062-WiFi-BT Layout.brd.alg, which I was able to import into Altium using the Import Wizard.
Regards,
John