Altium PCB files for i.MX6UltraLite Evaluation Kit

[durmus]

Hi all,

This topic Altium Files for i.MX6ULtraLite Evaluation Kit has the schematic files for Altium and directs to design files i.MX6ULtraLite Evaluation Kit|Freescale from where we can get Allegro .brd file for PCB layout.

When I convert ".brd" file in Altium, everything seems to be out of bound in Altium PCB editor. However, for the previous design files (for instance LAY-27392_C.brd in SABRE for Smart Devices Reference Design|Freescale ) I did not have this problem. Maybe related to ".brd" file version?

Can someone please upload i.MX6UltraLite Evaluation Kit .brd files in previous versions of Allegro (16.2)? Or maybe .alg files that are compatible with the curent .brd files?

Thanks.

[buka_2004]

Hi all,

I don't have an Allegro license to translate the file .brd to Altium. I only have Allegro Free Physical Viewer.

Are there Someone can translate "LAY-28617_C2.brd" to Altium PCB Editor format .PcbDoc?

[Yuri]

@buka_2004 
Hello,

  Please, create separate request.

https://www.nxp.com/support/support:SUPPORTHOME?tid=sbmenu

Regards,
Yuri.

[Yuri · Accepted solution]

Hello,

  Please try the enclosed PCB files.

Regards,

Yuri.

[durmus]

Hi Yuri,

Thank you for your reply.

I've converted these files, but the result is still the same.

Assuming "163" in file names corresponds to version 16.3, if it is not too much trouble can you please post them in version 16.2? I hear that there is a big change between those versions. Maybe my Altium does not convert quite correctly for versions greater than 16.2. But I know it does convert 16.2 files.

Thanks.

[durmus]

Hi Yuri,

With a little bit tweaking, I was able to recover the PCB data in Altium PCB Editor. Everything is fine now.

Thanks.

[EgleTeam]

Hi Dusmus,

What did you do? I have the same problem you had before.

Thanks in advance.

Regards,

Manuel.

[durmus]

Hi Manuel,

When I do the conversion, everything appears outside the working area of Altium Designer (you don't directly see them, but you can see the positions of every object in through the PCB List). I've noticed I could still move any object outside working boundary. Therefore, I've selected everything and moved them a suitable amount along x and y axes so that they are in the working area.

Hope this helps.

[EgleTeam]

Thank you Durmus,

unfortunately I can't do it.: I move all to the working area but I still see nothing. Which position do you move the selection (how large is the selection of all the componentes)?. Would you be so kind as to reproduce the procedure step by step?

Regards,

Manuel.

[durmus]

Hi Manuel,

Here is what I did:

Conversion:

- I have not converted all the layers. There are a ton of mechanical layers I do not need. Also I did not include paste, solder mask layers either. Here are what I've converted: TOP, GND, POWER, BOTTOM, DRILL, OUTLINE and SILKSCREEN layers. If you need anything else, make sure you include just what you need. Because they add to the complexity.

Altium PCB Editor Rework:

1. First things first, make sure you have the correct layout. You can't see it in 2D mode though. However, in 3D mode with a little bit zooming/unzooming/moving around you should be able to see the board, copper, silkscreen, etc.

2. Back in 2D mode, go to PCB List panel and list all objects. I have about 18.6k objects for BB board and 17.2k objects for CM board. Depending on what you converted those values will vary. Order them by X and Y coordinates respectively and note minimum values. Some objects (net, poly, region, etc.) do not have coordinate information, but it is not important.

3. With everything selected, Shortcut 'M' -> Move Selection by X, Y... and move them accordingly to your working area. For example, minimum X value for me was around 3100mm and min Y value was around 2600mm. I moved everything by -3000mm in X and -2500mm in Y.

Important Note: Untick "Lock Primitives" property for objects that have it (e.g. components). Otherwise some objects will move twice.

These steps worked for me. I hope it will for you too.

[EgleTeam]

Hi Durmus,

I have managed to move the components on top layer  and all the polygons, not the bottom components, neither all the nets.

Could you share your converted files?

Thank you even if you can't.

Manuel.

[durmus]

Hi Manuel,

Of course I can share them. But keep in mind that I have only converted aforementioned layers.

Kind regards,

Durmus

[EgleTeam]

Hi Durmus,

thank you soooo much! :-). Is more than enough with these layers: we only want to have a look in the layout. I always use my own footprint libraries. Please, have a look in our website and email me if we can help you in something (I owe you one ;-) ).

BTW: Great work and congratulations to the Freescale engineers that have designed the die of the processor. In comparisson with i.MX28 the ball assignament is much better: is amazing to be able to fan-out all the signals with only 2 layers!!!.

Best regards,

Manuel.