• Welcome to our site! Electro Tech is an online community (with over 170,000 members) who enjoy talking about and building electronic circuits, projects and gadgets. To participate you need to register. Registration is free. Click here to register now.

First PCB??

Status
Not open for further replies.

Mark68

New Member
I was just curious if you could take a look at this and tell me if it looks like I will be able to do toner transfer on this board? There are several circuits that still need to be added to the board so don't worry about the uncompleted circuit. I have to make a few jumpers too. I am stretching the size of the board as it is so I can't make it any bigger than it is.
 
Last edited:

mneary

New Member
Using inches will make it easier for most of us to review. A schematic to compare is vital.

The lettering that crosses circuits will cause shorts.

The IC pads are too small. that's not enough for amateur soldering. Actually, 0.80 (0.030", or about #69) is a tiny hole and a pretty delicate drill for a first board! Or, set restring to at least 0.20 (0.010" to 0.012").

The oblique interior angles will etch poorly. 45 degree angles will look better. The circuit will still work, but it's ugly.

Try to connect traces to the center of the pads (do you have "grid" turned on?) and you will have more space to maneuver.

You might use a ground pour to make the final etching faster.
 
Last edited:

Boncuk

New Member
.. and not to forget, there is a dual trace (overlapping) between R1 and R2. Nobody knows where it should be connected.

Try to make traces out of the center of a solder pad. (most of them are connected radially to the outer ring of the pad, which spoils the overall ugly view even more.)

Boncuk
 
Last edited:

Mark68

New Member
Wow! I just want to say Thank You for great constructive criticism, everyone's imput is well appreciated.

I tryed making the pads larger but they made the traces ( I thought ) to close.

I noticed the double trace, it didn't look like it needed to be there, but I wasn't sure. It was done by the Autorouter. It will be removed.

I have alot of expensive programs each with their good points and bad points. One of the main problem I was having making up a schematic is finding the right IC's and connectors (not to mention the right size footprints for the pcb side of it. Also when setting up a dual op amp in the schematic, in every program they transfer to the pcb board as two seperate IC chips. I asked in another post about how to fix this with no luck so I opted to just start over using Sprint and making just the PCB layout. Also there are alot of add on's that are going to be soldered to the edges of the board using wires. Linear switch, 3mm and 2mm phone jacks, some led's, etc.... (I just used LED leads to put in their place becuase they were small and I could use them as connecting points)This made it difficult for the expensive programs (with my knowledge of how they work ) almost impossible to to test for inconsistancy's in the circuit to be able to transfer over to the pcb layout with the right nets, rubberbands, ground, etc...

I used the autorouter on the traces except for a few that I didn't like where it put them. Is there a way to set the autorouter so that the traces go to the center of the pads and also a setting to make 45* corners. I know that when I did the manual traces it automatically made the 45* angle? ( as mentioned up above I'm using Sprint)

Thanks for letting me know about the lettering...I used it so that I could take a picture and save it for later uses, I will delete the lettering before I print out the circuit. Not sure what 'restring' is ,and yes I had the grid on. The autorouter put 99% of all the traces even the double trace. I will move all the traces to the center of the pads, np.

I will use inches if available....I thought it best to use mm since most of the datasheets and programs use that measurment.

Thanks Again!
Mark
 
Last edited:

colin mac

New Member
As a rule of thumb, component holes should have an annular ring of at least 0.2mm. So if the holes are 0.8mm, the pad should be 1.2mm. The pad of C1 is very near the trace. Try keep a space of 0.2mm between any copper that shouldn't be shorting.
 

Mark68

New Member
Ok this is what I have so far?

My traces are .8
They are set apart by .03 min.
Pads are at 2.0
and drill holes set at .8

I fixed the close trace on the C1. Thanks You!
I set the traces to the center of the pads
I tryed to angle some traces better
Made IC pads 2.0 Thank You!

Should the drill holes be bigger? and if so, should the pads be bigger to compensate or stay the same?

If you approve let me know. If you got any more good imput, bring it on.

Thanks for all the Help, soooooooooo appreciated, you guys rock!
 
Last edited:

3v0

Coop Build Coordinator
Forum Supporter
A few observations.

R6 and the trace above it are too close. Move one or the other. I would move R6 down so the trace to the left is horizontal to get the clearance.

C1 should be rotated 90 degrees clockwise. It will unwind the traces around it.

Move R2 left so that it is just below the LM358. That will take the curve out of the trace from pin 7 of the IC.

I would move R1 down a bit to allow straighten the trace from R4.

The trace from LM358 could go directly to R4 then continue on. No need for the branch.

Where possible make traces that T instead of Y.

Eagle has a tool the fills in the center of pads leaving small spot to start the drill in. You could duplicate that by using very small holes and large pads.

3v0
 

colin mac

New Member
R6 does look a little close but the rest doesn't look so bad. If you attach the gerber and drill files here, I can check the pcb properly. Or just give me the eagle file and I'll extract them and check it.
 
Last edited:

mneary

New Member
Major improvement. With improvement(s) noted should make a nice toner transfer.

Often I forget some of the I/O pins, power connections, and especially mounting holes. Do you have this accounted for?
 

Mark68

New Member
K....here's the changes, what do you think?

I didnt realize people posted again so I add this:

If you attach the gerber and drill files here, I can check the pcb properly. Or just give me the eagle file and I'll extract them and check it.
All foreign language to me?? LOL. Care to elaborate?

Often I forget some of the I/O pins, power connections, and especially mounting holes. Do you have this accounted for?
I believe so....I have made one allready, but the PCB was made for me. I am pretty sure about all the connections since I have put it together. I saw that someone on another post had mentioned buying the small drill press at Harborfreight. I saw it last week for 51% off so I bought it for $35 US. Hopefully this will help out with the drilling. Still not sure if I should make the drill holes bigger and if I do, if I will have to change the pad size.

You guys are totally awsome. I cannot believe this forum. I have never ever been in a forum where people don't flame noobs and make them feel like crap. Thanks so Much!

Anything else you want to add I encourage. I can tell by looking at this latest one ( 3vO ) It is looking alot better.
 
Last edited:

colin mac

New Member
Gerber files are the standard text files that represent the PCB data.
Extracting the gerbers from Sprint is easy. It's just File > Export.
The Excellon option will extract the drill file. Choosing gerber will extract the copper layer.
 

3v0

Coop Build Coordinator
Forum Supporter
It look much better to me too. You can work on PCB layout till you are old or dead. At some point you have say good enough. I like to stop layout and come back to it in a day or two. That lets me see things I can not when I am working on it. When I populate the board I have the layout open and make changes too. The world can disagree with what looked good on paper. You may even find things you do not like or would like to have during use.

I am glad you snagged the HF drill press on sale. It was on sale when I got mine too and it has turned out to be a good investment.
 

mneary

New Member
I have the HF drill press too, great deal with the discount!

I would build one and see what happens. The only interesting places are on the LM358 pin 1&2, 2&3. You'll just have to inspect it before etching.
 

Mark68

New Member
Couple Questions:

Can I cutout the 4 corners of the PCB Board? Or can you only make square boards?

How can I get rid of those 3 connection strings? When I click on 'remove connection bands' It does not get rid of them. It says " 0 removed, 3 remain "?

Does the ground plain (which I wont use for ground ) distance look ok? It's set at .7?
 
Last edited:

mneary

New Member
This is a toner transfer board, correct? You can make it any shape you can handle. If you send it out, your fabricator may have restrictions.

The connection bands are probably on their own "layer" and you probably can turn that layer "off". If there's no other way, you can trick the software by renaming the segments differently so the software doesn't think they need to be connected.

At very low frequencies the plane is usually harmless and is a good way to extend the life of your chemicals. But I don't recommend a floating plane area for designs that contain signals above a few Hertz. I like to connect them to GND or something like it. 0.7 is a conservative clearance. I would make it 0.5 or even 0.4 and have fewer isolated patches. If this is your first toner board, might stick with 0.5 (you're keeping my calculator warm ;-).
 
Status
Not open for further replies.

Latest threads

EE World Online Articles

Loading
Top