[eric343]

I'm going to order a board or two for the uKGSS, because Olimex is going on vacation in 5 days. So here's version 0.94, effectively version 1.0 unless I'm as dumb as usual and forgot something:

The whole board is a half-Eurocard, so both channels will fit on a Eurocard-size PCB.

 

[tangent]

If you ask them to panelize it, your layout will be fine, but if you make them depanelize it, you'll want to scrunch things a little closer to the center, at least along the 80mm edges. Otherwise, you risk getting traces cut when they depanelize it.

It's unlikely that you've got missing components, or bad connections, or crossed traces on that board, since you're usng Eagle.

Some quibbles:

- R35 (?) seems to be underneath R23, or vice versa. (Lower right)

- SMASH components and line their part names up inside or close beside the components. Right now, you've got part names all over the place. I wouldn't be confused about R35 and R23 if the names were lined up....

- You might turn off component values. At least when generating Gerbers

- Use a Gerber viewer to verify that the files it generates are correct -- don't trust that WYSIWYG! The most common mistakes are missing/extra layers turned on, and incorrect rotation of layers w.r.t. each other so that the individual layers are correct but they don't line up.

- You should name the parts as Kevin Gilmore did for all parts. I'm sure that the TO-92 in the upper left corner wasn't called U$13 by Kevin....

- You should try rotating that same part by 180 degrees. It looks like it will route better.

- Is there any particular reason R2 and R19 don't line up with each other? Same goes for several other parts around the board

- Those circles placed at random intervals -- mounting holes? If so, it might be a good idea to try and place them on a sane grid and then work the layout around them. It looks like you've gone the other way, and dropped holes in wherever they'll fit after the layout is done.

- Rotate D5 90 degress clockwise. It'll route easier.

- Instead of the silkscreen fix ULP Olimex gives you, try the one on Eagle's web site. I find that it works much better. You _will_ need to run it -- 8 mil silk is too much to ask of inexpensive silkscreening processes.

Enough complaints...

 

[eric343]

Thanks for the 'complaints', I'll get right on them (damn Spanish and English finals are tomorrow

) and post an updated version in a bit

(it never ceases to amaze me how helpful and kind fellow DIYers are!)

 

[eric343]

- If you ask them to panelize it, your layout will be fine, but if you make them depanelize it, you'll want to scrunch things a little closer to the center, at least along the 80mm edges. Otherwise, you risk getting traces cut when they depanelize it.

-- Well, I can depanelize it myself if that's a danger- it's not that hard, and I can probably do it more carefully than they do.

-In any case
It's unlikely that you've got missing components, or bad connections, or crossed traces on that board, since you're usng Eagle.

-- That's why I love Eagle

Some quibbles:

- R35 (?) seems to be underneath R23, or vice versa. (Lower right)

-- Well, it is, partly. I'm trying to keep those HV traces as far as possible away from eachother, and if it means running a resistor lead under another resistor...

- SMASH components and line their part names up inside or close beside the components. Right now, you've got part names all over the place. I wouldn't be confused about R35 and R23 if the names were lined up....

-- Done.

- You might turn off component values. At least when generating Gerbers

-- I would, but I don't plan to change any of the values, so having the values on the PCB will reduce the risk of my getting confused and mucking something up. Which is always a danger

I'll probably take them off if/when I do a run that's not just for my own use.

- Use a Gerber viewer to verify that the files it generates are correct -- don't trust that WYSIWYG! The most common mistakes are missing/extra layers turned on, and incorrect rotation of layers w.r.t. each other so that the individual layers are correct but they don't line up.

-- I'm planning to send Olimex the .brd file, do you still think this is necessary?

- You should name the parts as Kevin Gilmore did for all parts. I'm sure that the TO-92 in the upper left corner wasn't called U$13 by Kevin....

-- Good idea, unfortunately I don't have time right now! Something for v2.0, I guess

- You should try rotating that same part by 180 degrees. It looks like it will route better.

-- You were right! Thanks!

- Is there any particular reason R2 and R19 don't line up with each other? Same goes for several other parts around the board

-- It's easier to route traces, and it might help with inductance. Who knows... and since I'm not using DIP sockets, why not?

- Those circles placed at random intervals -- mounting holes? If so, it might be a good idea to try and place them on a sane grid and then work the layout around them. It looks like you've gone the other way, and dropped holes in wherever they'll fit after the layout is done.

-- Well, I don't want to muck about with the layout TOO much if I don't have to at this point. And yeah, they are mounting holes. Again, something for v2.0, I guess. (I'm going to be marking the 'drill spots' by using the bare PCB as a template, so sane grids aren't really necessary)


- Rotate D5 90 degress clockwise. It'll route easier.

-- Well, whaddaya know, you're right, again

Thanks

- Instead of the silkscreen fix ULP Olimex gives you, try the one on Eagle's web site. I find that it works much better. You _will_ need to run it -- 8 mil silk is too much to ask of inexpensive silkscreening processes.

-- Thanks for the tip! You're right... doesn't it look cool while it's running?

 

[tangent]

Quote:

I'm planning to send Olimex the .brd file, do you still think this is necessary?

Yes, because they just do the default Gerber generation sequence -- they don't "think" at all. I sent them a BRD once, they complained that some of the text ran off the edge of the board. So, I learned to make my own Gerbers, and found out that indeed, the text ran off the edge because one layer was rotated with respect to the rest if you used Eagle's default settings. With a few changes, it made the board come out correctly.

If you make your own Gerbers and you check them in a Gerber viewer you trust, there's no finger-pointing later if it comes out wrong. It's always your fault if it's broken, which is the way it should be.

Quote:

since I'm not using DIP sockets, why not?

It's prettier when things are lined up and spaced evenly. Same comment applies to running resistors underneath each other.

New problems:

- D5 appears to have one of its holes smaller than the others. Is this a via? Have you run DRC?

- R27 and R29 -- DRC will bitch about this, too, I suspect

 

[eric343]

Quote:

Originally posted by tangent Yes, because they just do the default Gerber generation sequence -- they don't "think" at all. I sent them a BRD once, they complained that some of the text ran off the edge of the board. So, I learned to make my own Gerbers, and found out that indeed, the text ran off the edge because one layer was rotated with respect to the rest if you used Eagle's default settings. With a few changes, it made the board come out correctly. If you make your own Gerbers and you check them in a Gerber viewer you trust, there's no finger-pointing later if it comes out wrong. It's always your fault if it's broken, which is the way it should be.

Good point

Quote:

It's prettier when things are lined up and spaced evenly. Same comment applies to running resistors underneath each other.

Yes, I know, but with finals coming up and a very tight deadline (they go on vacation on the 20th, after all), prettiness is really the last of my concerns

Quote:

New problems: - D5 appears to have one of its holes smaller than the others. Is this a via? Have you run DRC? - R27 and R29 -- DRC will bitch about this, too, I suspect

1 - WEIRD. DRC has always given a "drill distance" error for D5, but I could never figure out what it was talking about. So I tried clicking 'delete' over that hole, and the hole enlarged! There was a hidden via there that I didn't know about...

THANKS!

2. Nope, DRC OKs it.

 

[eric343]

Regarding the Gerber thing... can you recommend any good Win2k-compatible viewers? I grabbed ViewMate by Pentalogix and it's giving me images like this:

 

[tangent]

Looks like it's showing only the top silk layer. The thing you must understand about Gerbers is that there's one file per layer, and you can turn them on and off independently in the viewer, just like you can turn them on and off in Eagle with the DISPLAY command.

When running the CAM files you have to make sure that all of the layers you want Olimex to have are being generated -- this is done in the CAM parameters dialog. Then you have to make sure you're giving all of these files to the Gerber viewer; don't forget the drill file! And finally, you may not be telling the Gerber viewer to show them all. It's very convenient to turn these on and off in various combinations so that you can see how they all interact.

Personally, I use GC Prevue, from Graphicode.

 

[eric343]

Hmm, I think it's time for me to RTFM. Unfortunately, I'm going to have to do it tomorrow...

How do you use Prevue? It doesn't seem to want to take the Gerber files...

 

[tangent]

Quote:

How do you use Prevue? It doesn't seem to want to take the Gerber files...

You "import" the Gerbers. Its native format is a single file for all layers, which is what Open is for.

To be honest, I don't use GC Prevue much. I use Eagle on Linux, and so I use a Linux-based Gerber viewer most of the time.

 

[eric343]

Ah. Thanks

Incidentally, for anyone that's interested, all the files (BRD, etc) are stored here: http://www.drsue.net/files/gilmore2pcb/r5

 

[eric343]

Hrm...

Why don't the layers line up properly?

And how the heck do you move the stuff that the silk-correction script generated onto layer tplace? If I can't get the gerber ouput to work I may have to send Olimex the .brd and a PNG of what the whole thing should look like.

 

[eric343]

(yes, that image is from GC preview)

 

[tangent]

I'll bet you're glad you did your own Gerbers, because guess what, you've got the rotation problem I talked about!

In the CAM processor dialog, click through the layers, and I'll bet that you find that Mirror or Rotate is checked on the incorrect layers. Uncheck these, and save the new CAM job out to your project directory -- you don't want to keep changing these parameters every time you re-gen the Gerbers.

As for getting the larger silk lines to show up, you do that by turning on the new 100+ numbered layers instead of the original silkscreen layers in those tabs on the CAM job. Another good reason to save out a custom CAM processor.

 

[eric343]

Thanks

By the way, how would one copy the contents of one layer to another? I.e. if I wanted to copy the _tplace to tplace...