Can someone please help me with my Eagle Cad?

[ShadowPho]

I really like building circuits and fiddling around with microproccesors. However, I really want to move beyond a breadboard and small soldering boards. So I decided to start etching. My university has a small etching place.
So first I got Orcad 16 and tried working with that. It got to be too complicated. I started with Eagle Cad, and made my first board, but I am not sure if it's right.
Can someone please check if it is indeed correct?


This is a very simple circuit. I am attaching images of what my project looks like. I have a small microproccesor connected to a radio chip and a buzzer.

[MarkS]

I can work on this later on after I wake up. Need to sleep...

What I can say is to skip the auto router. It truly sucks.

[MarkS]

OK, I'm missing some important details. What are the manufacturers of the parts? I need a part list so I can find the data sheets so that I can verify your design. I can probably find this information just with the supplied model numbers, but I want to make sure. Pin 24 of the transmitter (I'm assuming the antenna connection?) is not connected to anything on the PCB, and is an air wire in the schematic. Not sure how to fix this without the data sheet.

Also, and please take this as constructive criticism, but your schematic is a train wreck. You really do need to take the extra time to make it clean, neat and clear, especially if you are thinking about doing this for a living.

I redid the schematic for clarity, but this is only cosmetic:

http://i18.photobucket.com/albums/b106/mspeir/Texter.jpg

[ShadowPho]

OK, I'm missing some important details. What are the manufacturers of the parts? I need a part list so I can find the data sheets so that I can verify your design. I can probably find this information just with the supplied model numbers, but I want to make sure. Pin 24 of the transmitter (I'm assuming the antenna connection?) is not connected to anything on the PCB, and is an air wire in the schematic. Not sure how to fix this without the data sheet.

Also, and please take this as constructive criticism, but your schematic is a train wreck. You really do need to take the extra time to make it clean, neat and clear, especially if you are thinking about doing this for a living.

I redid the schematic for clarity, but this is only cosmetic:


Parts list:

1x Texas Instrument MSP430F2013-16 bit proccesor Link Datasheet (http://www.ti.com/lit/gpn/msp430f2012)
1x RXD-315-KH Link Datasheet (http://www.linxtechnologies.com/Documents/RXD-xxx-KH_Data_Guide.pdf)
1x Speaker KMI-1240 Link Datasheet (http://www.smd.ru/files/upload/1237/ru/kmi-1240.pdf)
1x 3-3.3V battery - undecided on what size, how big and so on.
3x capacitors - probably 100uF just to make a cleaner voltage.
1x 32678 Crystal oscillator
5x resistors that I have not decided on values.
1x semi bright LED just to tell the circuit's hot.
1x transistor or a Mosfet.
1x three pin connector to program the proccesor.

I'd upload the pdf, but it's 2.5 mb for the microproccesor.

For pin 24, I made a 22.7 cm antenna out of a FAT wire. It has to be 22.6 cm, so I will apply it and then cut off small pieces to see the best transmission. I added that circly thingy, but it was deleted for board :(.

Thank you for your honest words, I really do take this as a complete constructive criticism. I really appreciate any criticism and comments :).

[MarkS]

I added that circly thingy, but it was deleted for board :(.


Eagle doesn't annotate traces unless they are connected to a part. The best solution would be to put a pad there. What is the diameter of the wire?

Do you need the board to be a certain size? If not, I can hand route that and shrink it by quite a bit.

Thank you for your honest words, I really do take this as a complete constructive criticism. I really appreciate any criticism and comments :).

I'm glad you took it this way. There are no schematic rules that are set in stone, so I'm not going to say that my way is best. However, it is important that the schematic be clear in case, like now, someone needs to review it. It looks to me like most of the problem is your unfamiliarity with Eagle.

I'm about to leave for work, so I'll look at the data sheets later on tonight. Also, I am a hobbyist, not an EE. I'm still learning, so I'm not going to promise you perfection. I will do my best though.

[ShadowPho]

Eagle doesn't annotate traces unless they are connected to a part. The best solution would be to put a pad there. What is the diameter of the wire?

Do you need the board to be a certain size? If not, I can hand route that and shrink it by quite a bit.

My wire is gauge 14, so 2 cm^2, so 2=pi*r^2, r=0.797884561 cm, 1.5cm diameter.
As for the board, I don't need it to be a certain size. I think it'd be better to have it as small as possible as I am going to etch it tomorrow or wednesday.

I'm glad you took it this way. There are no schematic rules that are set in stone, so I'm not going to say that my way is best. However, it is important that the schematic be clear in case, like now, someone needs to review it. It looks to me like most of the problem is your unfamiliarity with Eagle.

I'm about to leave for work, so I'll look at the data sheets later on tonight. Also, I am a hobbyist, not an EE. I'm still learning, so I'm not going to promise you perfection. I will do my best though.
:)
Right now I am trying to work Orcad and my new design does look much much cleaner. And thank you again, a helping hand is all that's needed.

[MarkS]

Looking at the data sheet for the transmitter, you really need to hand route this. Pay close attention to the PCB layout guidelines in the data sheet. You need a ground plane on the opposite side of the board, no traces running under the transmitter on the same side of the board as the transmitter and the trace to the antenna has strict guidelines. You really can't just use the autorouter, print and etch.

Also, the speaker that you have in the schematic is not the same as the one in the data sheet. The speaker in the schematic is a through hole PCB mount and the one in the data sheet is a surface mount.

I'd also recommend a smaller (physical size) crystal. The one you use here is positively massive compared to the 32K crystals I've seen.

The transmitter should be routed similar to this:
http://i18.photobucket.com/albums/b106/mspeir/HandRoute.jpg

[ShadowPho]

Wow, thank you so much. I am still looking at this thinking about how to route the rest of this. I will give take a shot at it tomorrow and see how it turns out.

[MarkS]

Oops... Nevermind...

[MarkS]

Wow, thank you so much. I am still looking at this thinking about how to route the rest of this. I will give take a shot at it tomorrow and see how it turns out.

There are many ways to do this. If you aren't scared of soldering surface mount components, almost everything on the board can be changed and the routing will actually be easier.

However, sticking with the through-hole components, I came up with two variations.

Spread out:
http://i18.photobucket.com/albums/b106/mspeir/SpreadOut.jpg

Compact:
http://i18.photobucket.com/albums/b106/mspeir/Compact.jpg

I'm sure an EE can come up with a nicer solution, but I'm happy with either one. I like the first design best. It is a little bigger, but less messy.

BTW, what is the purpose of C4?

[ShadowPho]

Wow, thank you, that looks wonderful. As for surface mount, I tried it out, and I really like it, but I don't (currently) have many parts with are SM. Most of my cave contains through-hole stuff.
As for C4, I was thinking of putting a big capacitor on C4 in order to regulate the power supply the most and then C5 and C1 with smaller values but closer to actual components.

And wow the more I look at this the more I like it. How did you make the board really pretty and stuff? Is it still the same mode but just with a different background?
Is OrCad any better at routing?

Edit:

Thank you again! I will give this same circuit a try after my final tomorrow and then will see if I can etch it and play some with radios :D.

[MarkS]

The blue background is the ground plane. This is necessary in your design. To do this in Eagle, change the name of the ground signals in the schematic from "n$xx" to "GND". Then, in the board file, create a polygon in the layer you want it in and name it "GND" and press the ratsnest button (the green x with five dots).

You really do not need to clean up the power supply in this case. Batteries (usually) give a perfectly flat voltage. If you were using a regulator, then decoupling caps would be a must. I'd still keep the two near the IC's just as standard practice, but C4 can go without any harm.

Here is the updated Eagle files. Look them over. If you can get Orcad, by all means do so! Eagle is good, but really at the low end of the scale. Orcad is at the high end.

[ShadowPho]

The blue background is the ground plane. This is necessary in your design. To do this in Eagle, change the name of the ground signals in the schematic from "n$xx" to "GND". Then, in the board file, create a polygon in the layer you want it in and name it "GND" and press the ratsnest button (the green x with five dots).

You really do not need to clean up the power supply in this case. Batteries (usually) give a perfectly flat voltage. If you were using a regulator, then decoupling caps would be a must. I'd still keep the two near the IC's just as standard practice, but C4 can go without any harm.

Here is the updated Eagle files. Look them over. If you can get Orcad, by all means do so! Eagle is good, but really at the low end of the scale. Orcad is at the high end.

Thank you again! I don't think I can repeat how many times I am grateful for your help :D.
I am looking at it over right now. It looks very good and tasty.

As for Orcad, I already have it (v16), but it's really complicated and I haven't opened the manual just yet.

[Super Nade]

Get rid of the T's if and increase the miter on the power trace if possible. Also, where is your switch? :)

Other than that, the trace layout looks good. These guys are cheap-->https://www.barebonespcb.com/!BB1.asp

[ShadowPho]

Get rid of the T's if and increase the miter on the power trace if possible. Also, where is your switch? :)

Other than that, the trace layout looks good. These guys are cheap-->https://www.barebonespcb.com/!BB1.asp

Thank you! What is miter?
As for the switch, there's a batter to take out :).
A switch would be a good idea, though, I'll put it in.

And those guy do look pretty good. 10 boards of 5x5inches at @$15 = $150

edit: psst, thanks for moving and not deleting this thread =P

[Super Nade]

A mitre is an angle added to the trace. You don't want 90 degree elbows as it introduces stray capacitance and cross-talk.

Check out some stuff I did (really simple though). (The tread below has the older version of the project)
http://www.ocforums.com/showthread.php?t=557533

[ShadowPho]

A mitre is an angle added to the trace. You don't want 90 degree elbows as it introduces stray capacitance and cross-talk.

Check out some stuff I did (really simple though). (The tread below has the older version of the project)
http://www.ocforums.com/showthread.php?t=557533

AWWW MAN. Screw my final, I am rendering my curcuit in 3D.

Thanks for showing that. Really cool. :D

I will definitely remove the right angles, C4 capacitor, add a switch, render in 3D, etch and then program it lol.

[Super Nade]

Study for your final and we can discuss this after you are done with exams. Work before play. ;)