Altium Designer NB2DSK01

nb2dsk01

Need your help for compelete schematic and other documentation of Altium NB2DSK01 board, and it's P03 memory card add-on board, it is urgent!

Thanks in advance.

Comment: The project files on Altium Designer 6.9 example folder is not compelete, many design sheets are missing!

altium flex board

The complete schematic is included as a PDF in the Help folder. The 72 page document name is "NB2DSK01 Desktop NanoBoard Schematics.pdf".

What sheets do you think are missing from the schematic in the examples folder?

altium designer analyse net

Thank you for PDF file address, I got it.

Comparing this file with schematic on examples folder, most sheets are missing! Schematic project contains less than 10 pages but PCB is full! Would you try to open it once.

nb2dsk01.

You are correct, the release version appears to have only a few sheets as examples. They must have decided to try and trim a little off the size of the distribution disk by moving the full schematic to the PDF document. The were criticized when AD6 came out for including WMV files in the examples, and thereby needlessly increasing the size of the product installation.

I had a complete schematic from other sources, and I see that the folder name is different from the one on the distribution disk.

altium turn off loop removal

The release on AS 08 is complete!

A gray designator appears around the main designators, what is that gray one? Is it indicating a design variant?

altium cutout

If you look at the bottom of the Schematic Editor window, you'll see two or more tabs after you compile a schematic. One of the tabs is labled "Editor" and the other tabs will have the expanded names of multi-channels (sheets where the "repeat" directive was used").

On the expanded tabs, the gray designators are the physical designators that were expanded from the logical designators on the schematic. If there was no expansion, there will be no extra gray designators. The expanded physical designators are the ones that will be passed to the PCB.

@ltium Designer NB2DSK01

On this board, component R137 and other similar big componenets has two via connected to each pad. AD usually remove the second via, how we can instruct AD to keep the second via connected to pad.

You turn off loop removal. Global loop removal is set with a check in Preferences>>PCB Editor>>Interactive Routing>>Automatically Remove Loops.

You can also turn it off one net at a time by setting the PCB Panel to "Nets", and double clicking on the netname you want to turn off or on.

You can get to the same dialog by right clicking over a track, and selecting Net Actions>>Properties.

@ltium Designer NB2DSK01

- What is your opinion about overall quality of rouing in this board? Is it manual routed or auto-routed? In the case of manual, how long it might take to route it?

- Is AD or ADS08 able to do team based PCB design?

Added after 33 minutes:

-What is the use of Analyze Net command?

The board is most likely manually routed. Manual routing will always give you the best results. Autorouters just find the shortest route between two points, and can't anticipate things like underlying plane splits, or analog and digital return paths - unless you set up such things in routing constraints. By the time you've done that, you might as well have laid the track by hand.

I think the designer did a pretty good job, but I would have used fewer polygon pours. It's possible he or she used so much copper because there's no shielded enclosure. There could have been a problem meeting the EMC requirements.

My guess would be about 3 weeks to route a board like this. It depends on how many footprints had to be custom made, and how many were already available in existing libraries. A lot of time in laying out a board is spent doing component data research.

Any design software can do "team based design". I personally don't believe in it. It's like the old saying, "an elephant is a camel designed by a team". There are several companies who keep their designs on a server, and each member of the "team" takes turns working on the board. AD lets you lock out a file so others can view it, but only the first person to open it can actively edit. In that way, conflicting edits are prevented.

Analyze net is just what is sounds like - it does a signal integrity analysis of the selected net or nets.

@ltium Designer NB2DSK01

Analyze net doe not work for me as we want it to do!

For board cut out what rules we should consider? Is it possible to do any cut out with any shape? I am interested to know what machinery or may be drilling method is used to make them.

About flex board, do we have to obey specific rule to design them or "flex" is just a matter of manufacturing?

Regarding power boards, 220/110-3.3/5.0, you may see a cut out under the main ferrite transformer. We know that high side and low side is electrically isolated and jut coupled optically. Why we have to put such cut out on PCBs?

You should read "TU0113 Performing Signal Integrity Analyses.pdf". Beginning on page 7, it explains reasons why certain things may cause a net analysis to fail.

You need to talk to your board fab about their ability to do cutouts. Cutouts are routed out of the board, and the fab will tell you what limits they have for routing tool size, corner radii, board thickness, etc.

Every large fab has a design guide for laying out flex circuits. All you need to do is go to their website to download them. Try typing "flex circuit guide" in Google, and you'll get a bunch of listings to choose from. There also is a brief discussion of some considerations in a magazine article at https://pcdandf.com/cms/cms/content/view/2948/95/.

Cutouts under a transformer can be for a number of reasons. One is to provide more room by allowing the core to extend below the surface level of the board. Another is to provide ventillation in an area where the board could warp from transformer heat. Another, is to provide more isolation between the primary and secondary terminals. In other words, there's no one reason to make a cutout. It depends on the component, the board, and what problem you are trying to solve.