It took me like 24 solid hours. Does anyone see any flaws I might have overlooked? Particularly the use of the voltage supply nets? And the logic involved in triggering the alarm.

I was also wondering if anyone knows if it's possible to break the pcb into two boards, and how would I do that?
Would I have to manually insert all the jumpers/ribbon cable connectors into the schematic?

Thanks Guys!!

 

Just a couple of suggestions. Keep in mind I
don't know how familiar you are with Cadsoft Eagle.

Use the "Smash" command (in the Edit menu or on the toolbar)
to allow the Name and Value of the component to be
moved, rotated etc. This will clean-up the drawing and make
it easier to read.

28 Errors all seemed to be associated with VDD, V+, Vss, and
Ground. I know this frustration. My solution is not elegant, but
I'll usually redraw or alter the library component so it does not use
the "power pins". I think making/altering Library components must
be one of the reasons that everybody thinks Cadsoft Eagle has
such a steep learning curve.

 

IC12A pin 1 needs a current limiting resistor for the transistor base (driver for LMP1). Without it, you'll overload the output.

I didn't do an extensive check of it (don't have the time), but otherwise it looks OK.

The freeware version of Eagle will only support boards up to ~3" x ~4". I don't remember what the size of your ExpressPCB board is offhand, but I'll bet it's larger than that.

Oops, the single board version that I "tweaked" on awhile back is 4"x10".

If you're going to use Eagle to make the boards, I'll suggest that you break the display section up into 3 separate boards; one each for hours, minutes and seconds. Leave jumpers/spaces/DIP switches/whatever on the boards so that they can be quickly/easily configured for whichever function is required; and the HV supplies to other boards. Consider using dual-row headers and ribbon cables to connect the boards together.

That could save a lot of hassle if someone was building a project, and zapped one of their boards somehow.

 

Just a couple of suggestions. Keep in mind I
don't know how familiar you are with Cadsoft Eagle.

Use the "Smash" command (in the Edit menu or on the toolbar)
to allow the Name and Value of the component to be
moved, rotated etc. This will clean-up the drawing and make
it easier to read.

is there any way to un-smash a part and lock the values into the place I put them?

28 Errors all seemed to be associated with VDD, V+, Vss, and
Ground. I know this frustration. My solution is not elegant, but
I'll usually redraw or alter the library component so it does not use
the "power pins". I think making/altering Library components must
be one of the reasons that everybody thinks Cadsoft Eagle has
such a steep learning curve.

Do you happen to know how this is an error? I don't understand why it get's flagged as one, isn't that how the power and ground pins are SUPPOSED to be connected??
I can make and alter parts all right, I had to for the nixie tubes and FET's.

IC12A pin 1 needs a current limiting resistor for the transistor base (driver for LMP1). Without it, you'll overload the output.

AHH!! Thanks wookie!!

I didn't do an extensive check of it (don't have the time), but otherwise it looks OK.

The freeware version of Eagle will only support boards up to ~3" x ~4". I don't remember what the size of your ExpressPCB board is offhand, but I'll bet it's larger than that.

Oops, the single board version that I "tweaked" on awhile back is 4"x10".

If you're going to use Eagle to make the boards, I'll suggest that you break the display section up into 3 separate boards; one each for hours, minutes and seconds. Leave jumpers/spaces/DIP switches/whatever on the boards so that they can be quickly/easily configured for whichever function is required; and the HV supplies to other boards. Consider using dual-row headers and ribbon cables to connect the boards together.

That could save a lot of hassle if someone was building a project, and zapped one of their boards somehow.

I think I'll either break it up into 5 boards (3 display, 1 power, 1 logic), or export the netlist and use a different program. (then there's always uTorrent...)

Regarding the ribbon connectors, can you insert those while making the boards, or must they be inserted in the schematic?

 

is there any way to un-smash a part and lock the values into the place I put them?

Not really. You'd have to edit the symbols in the library and re-load them.
If I'm smashing a part to move the NAME or VALUE fields around, I may temporarily set the grid quite fine, like 10 mils, to get the text just where I want it - and then immediately go back to 100 mils / 0.1" in the schematic, or 50 mils in the board. If you forget to go back to 100/50 mils, you can wind up with a mess to clean up.

Do you happen to know how this is an error? I don't understand why it get's flagged as one, isn't that how the power and ground pins are SUPPOSED to be connected??

Eagle wants the exact names to match for POWER pins. That's the only way it can make certain that VDD pins are connected to VDD names, GND
pins to GND names, etc. As long as they are WARNINGs and you know it's OK, then you can approve them. If there are ERRORs, you have to fix them. You will wind up in trouble if you try doing something like putting two differently-named SUPPLY symbols on a node, as they will "fight" each other, and you can wind up with a mess on your board.

I think I'll either break it up into 5 boards (3 display, 1 power, 1 logic), or export the netlist and use a different program.

3 display and separate power/logic is what I was thinking.

(then there's always uTorrent...)

Don't do that. It's not just the legality thing; you will really shoot yourself in the foot if you do that.

If Eagle detects that anything in a file was made from an illegal copy of the software, it will refuse to open it. That is yet another reason to not use other peoples' library files.

Regarding the ribbon connectors, can you insert those while making the boards, or must they be inserted in the schematic?

You should start breaking the schematic up into three separate schematic files; One for the logic, one for the supply, and one for the reconfigurable common display board.

Then add the connectors into each of the separate schematics. You should make certain that you get all of the signal names the same in the separate schematics.

You don't want to add things like headers, connectors, etc. into the board alone.

 

Not really. You'd have to edit the symbols in the library and re-load them.
If I'm smashing a part to move the NAME or VALUE fields around, I may temporarily set the grid quite fine, like 10 mils, to get the text just where I want it - and then immediately go back to 100 mils / 0.1" in the schematic, or 50 mils in the board. If you forget to go back to 100/50 mils, you can wind up with a mess to clean up.


Eagle wants the exact names to match for POWER pins. That's the only way it can make certain that VDD pins are connected to VDD names, GND
pins to GND names, etc. As long as they are WARNINGs and you know it's OK, then you can approve them. If there are ERRORs, you have to fix them. You will wind up in trouble if you try doing something like putting two differently-named SUPPLY symbols on a node, as they will "fight" each other, and you can wind up with a mess on your board.

K, thanks.
W as actually kinda proud of myself, I managed to do it all without any ERRORs

Don't do that. It's not just the legality thing; you will really shoot yourself in the foot if you do that.

If Eagle detects that anything in a file was made from an illegal copy of the software, it will refuse to open it. That is yet another reason to not use other peoples' library files.

Darn. Why must software be so overpriced.

You should start breaking the schematic up into three separate schematic files; One for the logic, one for the supply, and one for the reconfigurable common display board.

Then add the connectors into each of the separate schematics. You should make certain that you get all of the signal names the same in the separate schematics.

You don't want to add things like headers, connectors, etc. into the board alone.

Kk
Am I going to need dampening resistors on the ribbon cable lines to prevent ringing or will the induction be low enough that it won't be a problem?

 

K, thanks.
W as actually kinda proud of myself, I managed to do it all without any ERRORs

That's good.

Darn. Why must software be so overpriced.

You think that's expensive?
Try Altium Designer. I think the professional version was running about $20k a seat last time I checked, and that was several years ago.

If you want free, you can either deal with Eagle's freeware limit of 2 layers,
3"x 4" boards and single-page schematics, or perhaps try something like TinyCad.

I tried using the demo version of DipTrace, but didn't care for it much. It seems to me that Eagle has a better interface; but it's hard for me to be objective as I've been using Eagle for awhile.

Am I going to need dampening resistors on the ribbon cable lines to prevent ringing or will the induction be low enough that it won't be a problem?

Not a bad question. It wouldn't hurt to put some in there. You can get resistors in DIP packages, which will save you assembly time.

 

You think that's expensive?
Try Altium Designer. I think the professional version was running about $20k a seat last time I checked, and that was several years ago.

If you want free, you can either deal with Eagle's freeware limit of 2 layers,
3"x 4" boards and single-page schematics, or perhaps try something like TinyCad.

I tried using the demo version of DipTrace, but didn't care for it much. It seems to me that Eagle has a better interface; but it's hard for me to be objective as I've been using Eagle for awhile.

Eh, I'll manage with the multiple boards... I kinda like the idea anyway

Not a bad question. It wouldn't hurt to put some in there. You can get resistors in DIP packages, which will save you assembly time.

What sounds like a good ohmage?
A couple hundred?

[EDIT]
Nevermind, found that wookie said 220 in another thread.

 

GRR...
Does anyone know what the name for the thing that the female socket attached to the cable itself plugs into is?
The part that actually mounts to the board with all the little pins sticking up?
I can't seem to get the store sites to turn any up in the searches.

 

GRR...
Does anyone know what the name for the thing that the female socket attached to the cable itself plugs into is?
The part that actually mounts to the board with all the little pins sticking up?
I can't seem to get the store sites to turn any up in the searches.

They are known as pin headers - there is a standard Eagle library for these called pin-head.lbr or something similar - it contains a whole set of different combinations & spacings. The enclosed headers with keyways etc. are in the con-xxxx.lbr libraries - I would give you the exact one but I'm not on a computer with Eagle at the moment.

You were complaining about the cost of professional CAD packages - Eagle has a "non-profit" usage license for a full version of Eagle for USD 125 or thereabouts. This is a complete bargain (if you can afford it!) but they tend to keep pretty quiet about this version.

I would second the comment above about never using a "torrent" version of Eagle, i.e. cracked s/w. Eagle has a lot of internal defence mechanisms against this and will not open files it thinks have been created by cracked versions or warez.

 

is there any way to un-smash a part and lock the values into the place I put them?

Yes,in layout editor we have this option.From Edit menu or Command toolbar,select Lock or Smash command and then click over the component to apply the command.
Another way,right click over any component and from the context menu you will find these options,if the component is already smashed or locked then the options will be unsmash and unlock.

Does anyone know what the name for the thing that the female socket attached to the cable itself plugs into is?

A picture will be good but I think you are talking about PCB connectors/bars/headers.
Anyway I use these, here is a photo

If these you are talking about,then you can make your own package as these comes in 40 or in more pins package and we cut it as per our needs...or as said earlier use "pinhead.lbr" package.

Good Luck

 

Headers!
Thanks guys!

Anywho, I done and done the broken up schematic- it's (they're?) in the zip for whoever's curious.

Question-should I worry about switch de-bounce for the switches used for setting/reset?

I used 5 ribbon cables, 3 10 pin and 2 16 pin. I put resistors on all the signal lines, checked to make sure it wouldn't mess any "setting" signals up impedance wise, doesn't look like it should.
I didn't smash and move everything yet, I might in the future, right now I'm going to bed.