Platform forum

Allegro .brd PCB to Altium .PCBDoc

Taner , 05-10-2019, 06:27 AM

Hi Robert how are you? I try to convert Allegro *.brd file to Altium Designer 19 *.PcbDoc, but i can't. I find a few solution on web but the are not solve my problem. Like the shows below. https://nilsminor.de/index.php/2018/...m-pcbdoc-file/ https://www.altium.com/documentation...ro+Import))_AD Would you please give same idea how to solve this. Best Regard, Taner
robertferanec , 05-12-2019, 09:21 AM
And where exactly is the problem? What step doesn't work? Install OrCAD Lite (it's free), then go to Altium and use import (I do not have access to Altium right now to describe the steps exactly, but you should be able to find the import in main menu).
Taner , 05-13-2019, 01:05 AM
When i try to import *.brd file a accpet thos message.
robertferanec , 05-13-2019, 03:51 AM
Did you install OrCAD Lite? Altium needs one special file from Allegro to be able to import the board.
Taner , 05-13-2019, 04:15 AM
Yes, Cadence Orcad Lite 17.2 is installed. I try to convert BeagleBone_Black_RevB6_nologo.brd​ file to Altium PcbDoc file.
​I follow steps for import *.brd file: File > Import Winzard > Allegro Design File
robertferanec , 05-13-2019, 06:17 AM
You need to find where the exctracta.exe file is located and you need to add the PATH into you environment.

For example in my case it is located in "D:\Cadence\SPB_17.2\ools\bin" so I had to add it into START -> right click on My Computer -> System properties -> Advanced -> Environmental Variables. Then, in System Variables, select Path, Edit and add ";D:\Cadence\SPB_17.2\ools\bin" at the end. After the change, you will need to switch off and switch on Altium.
Taner , 05-13-2019, 08:04 AM
Would you please explain exactly?
robertferanec , 05-13-2019, 08:57 AM
My Windows are not in english - but I hope this picture will help at least a little bit (you can always google for "how to add environmental variable to windows path"):

Taner , 05-13-2019, 09:16 AM
Problem is SOLVED. Look link: https://www.youtube.com/watch?v=LhSN76oEucg
robertferanec , 05-13-2019, 11:11 AM
That's great, that you were able to solve it!
M. Namvar , 05-14-2021, 01:24 PM
@@Taner and @@robertferanec
I used the method above, but the imported PCB does not have any track and plane (No cupper ) in all layers.
can you help me?

Taner , 05-17-2021, 02:30 AM
Hi Namvar,
you can try with attached files.

Best Regards,
robertferanec , 05-17-2021, 03:57 AM
I used the method above, but the imported PCB does not have any track and plane (No cupper ) in all layers.
It should work. When going through the wizard, I think you should see how the Allegro layers are going to be imported on what specific Altium layers? Could you attach a screenshot from that step here?
M. Namvar , 05-19-2021, 03:38 AM
I used these settings and it resolved (after setting the place boundary height to zero) and resolving DRC errors.
but look at the 3D View!
robertferanec , 05-24-2021, 01:51 AM
Yeah, I am not sure if 3D models are imported.
Wyku , 11-23-2021, 07:20 AM
Originally posted by M. Namvar
I used these settings and it resolved (after setting the place boundary height to zero) and resolving DRC errors.
but look at the 3D View!
@@M. Namvar Can you explain further what steps you took to get your missing copper/internal layer information to show up properly? I'm having the exact same issue you described in your first post and haven't been able to resolve it (Altium Support hasn't either).
Lakshamana Balakrishnan , 11-24-2021, 10:37 PM
@Wyku , IF copper only be the problem You can extract dxf from allegro as copper layers (including tracks,polygons only) and import into altium to get the desired tracks.
Wyku , 11-25-2021, 07:12 AM
@Lakshamana Balakrishnan I did try out various things like that, but it's a large board that would be extremely time consuming to reconvert everything that way. It also removed all vias and net information of course, so it's not a very useful import.
Lakshamana Balakrishnan , 11-25-2021, 08:59 PM
@Wyku You better try once a fresh start with below video. It may help you.

Wyku , 11-26-2021, 09:33 AM
@Lakshamana Balakrishnan thanks for the link to the video. It was the same process as some of the other attempts I've made, but with a few slight tweaks including the .bat file having slight differences compared to the latest one in Altium 21 so I gave it another try--unfortunately the result was the same.

Top Layer Example (OrCAD vs. Altium Import):

Inner Layer Example (OrCAD vs. Altium Import):
robertferanec , 11-29-2021, 08:01 AM
@Wyku maybe, could you attach the window from the import wizard where you are assigning allegro layers to the altium layers? PS: Some time ago, when I was trying to import a very complicated PCB from allegro to altium, I was not able to do that, but in that case altium froze or crashed. It looks like, in your case it went through the process, so maybe there is something in settings (?)
Wyku , 11-29-2021, 08:25 AM

These are the import settings I'm using (default):

These are the layer selections. There's a bunch more, but I've tried importing with everything selected (there are A LOT of Allegro layers...) and stripping it down to just the basics, but the result is the same unfortunately.

robertferanec , 11-29-2021, 08:45 AM
This looks correct. Did you try to export only one layer, just to see if ti will be exported correctly?
Wyku , 11-29-2021, 08:52 AM
@robertferanec I've tried importing single layers, but it doesn't help either. I haven't tried exporting a single layer though--any tips on how to do that? I've just been using the Allegro2Altium script to generate the .alg file.
robertferanec , 11-30-2021, 01:26 AM
I meant importing. Hmm, I am not sure what the problem could be. I would expect this to work ....
Wyku , 11-30-2021, 07:40 AM
@robertferanec Yeah, it seems to be stumping everyone at the moment, unfortunately. That's why I was interested to hear from @M. Namvar since it looked like he had the exact same issue (albeit on a smaller looking board), but was able to resolve the issue somehow.
Lakshamana Balakrishnan , 11-30-2021, 09:28 PM
@Wyku Please give a try with Reverse engineering from Allegro Gerber into Altium Camtastic file and then convert to Altium Pcb. I suggest this method to utilise the copper from that (Gerber converted Altium PCB board) into your (Previously Converted Board by Import Wizard).

Please find the process of converting any gerber into Altium PCB from the below link.
Reverse Engineering from Gerber to PCB | Altium Designer | Knowledge Base
Wyku , 12-02-2021, 03:09 PM
@Lakshamana Balakrishnan I had tried that method probably a dozen times or more and it kept giving me an error about layers not being assigned properly, which they were and I would continually reset properly after 2 of them would get changed during the failed export to PCB, but somehow on the second attempt after trying it again after your suggestion (mainly to capture the error screens) it actually worked!

I haven't had any luck getting a netlist to import that would allow me to rename all the nets like they're supposed to be named, like the walkthrough's state can happen. I have an IPC-D-356 netlist that seems to have everything in it, but then Altium complains that it doesn't contain net names... I just can't win. 🤦‍♂️😂 If I just import the Gerbers first it won't let me import the netlist at all, but if I do the Quick Load and do everything at once it imports, but it still doesn't seem to like having it there. Any other tips you could provide would be much appreciated!

Also, is there anyway to get the actual drill/hole sizes to import properly rather than just their locations marked by an aperture? I think I read that it was a limitation based on it being an Allegro export or version issue, but I'm not 100% sure on that.
Lakshamana Balakrishnan , 12-09-2021, 03:32 AM
@Wyku Cheers!

For Netlist sync, You try to sync it with schdoc again if you have or else try the method of Importing netlist into Pcbdoc directly with help of exporting Protel netlist from orcad.

For actual drill/Hole, You should be care of gerber settings format of both allegro and altium like 4:4, Leading Zeros whatever needed. If you set this correctly, It will import.

Hope it helps!!
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?