Creating a replacement pcb

[Western]

Hi Guys, I’ve been an electronics tech since I left school (45 years) … but always been in the repair side of things. As such I don’t have much experience designing circuits or board layouts.


I’m looking for some pointers in designing and building a circuit board … as replacement for a particular type I fix, that can be difficult and time consuming to repair. Would be nice to be able to offer a brand new board at a comparable price to repairing one … and save myself a lot of time.


The difficult ones are badly corroded and after fixing a few times can take a lot of effort to rebuild.


My thoughts are to recreate the board with the same physical shape, mounting holes, locations for switches, leds and displays etc … so they will be a drop-in replacement.


… but then to use smd components mounted on the rear near the top, for all the active electronics.


The bottom half of the front face is where the majority of the boards problems are … so moving as much as possible to the rear at the top should give it a fighting chance.


I also want to have any tracks and pads that are on the front, to be large and as far apart as possible.


The originals have very heavy copper (compared to most boards I see) … so I want that as well. It’s probably the only reason the originals have been able to hold up to some of the abuse they cop.


Just wondering what is the best software to use … a general idea of what steps to take … and any gotchas I need to look out for.


Thanks for any help.

 

[Pommie]

What size is the board? How many layers? Voltages?

The free version of Eagle handles double sided boards up to 80 square cm. The full version is around $500.

Another free one is Kicad. Not tried it myself but might be worth having a play with.

Mike.

 

[Western]

6"x 4 " ... double sided ... 5 volts

I have played with both at different times of my life ... but never got very far with either.

 

[JonSea]

The free version of Eagle handles double sided boards up to 80 square cm. The full version is around $500.

The free version of Eagle explicitly states it's not for commercial work. But it won't handle a large enough board anyway.

Eagle is only available through a subscription model now. It's about $500 per year for the full version of everything (schematic capture, layout and autorouter) but you can also rent by the month for around $50.

$500 is not unreasonable for the whole package per year, considering the purchase price of the pro version (to be able to make large boards) was about $500 per piece. That's why I use version 5 layout with TinyCad for schematics.

 

[Western]

That's why I use version 5 layout with TinyCad for schematics.

So you prepare your circuit diagram in TinyCad ... then transfer back to Eagle to do the board layout?

I've just spent the last hour checking out UpWork to see if it is worth my while just paying someone to do the task ... and getting some idea how much it might cost.

 

[JonSea]

I create the schematic in TinyCad, then either lay out the board in Eagle "by hand" or I will import a netlist for a more complex boatd. Not the smoothest way go do it, but it works for me.

 

[Western]

I create the schematic in TinyCad, then either lay out the board in Eagle "by hand" or I will import a netlist for a more complex boatd. Not the smoothest way go do it, but it works for me.

Sounds like something I would do ... though if I am going to have to learn something new, it has to be the easiest way possible ... or I'm never going to get it finished.

 

[dknguyen]

Just wondering what is the best software to use … a general idea of what steps to take … and any gotchas I need to look out for.


Thanks for any help.

With regards to "best" software. This will be heavily dictated by price. Name your budget. $0, $500, $1000, or $10k.

Two main pieces in the software package:
1. Schematic capture software
2. PCB layout software

Steps:
1. Make schematic symbols with capture software.
2. Make padstacks (the PCB pads for the physical component).
3. Make the footprint of the component using the PCB pads for use in the PCB layout.
4. Make schematic and label schematic symbols with their associated footprint file.
5. Generate a netlist from the schematic.
6. Import the net list into PCB layout software
7. Lay out the PCB.
8. Generate the gerber files, drill files, and if automated assembly, the pick-and-place files, solder stencil, bill of materials, etc.
9. Open up the gerbers in Gerber software (you can find free ones to use. I use "DFM Now!") to view the physical copper layers, silkscreens, and outlines of the board as they will be manufactured and make sure everything looks right. (You must do this step! PCB layout has a lot of configuration options that can be missed so you must always look at the physical file after it is generated to make sure you didn't mess something up. Seeing the clean layers separately also helps you spot errors that you would otherwise miss in the PCB layout software which can be very crowded even if you turn some layers off since certain things from other layers can still have limited visibility).
10. Send off to PCB fab
11. Hope you made no errors.

Gotchas? Ummmm...
1. Solder masks should be a little bit larger than the copper pad due to tolerances (0.1mm or 4mils larger on each side seems to be standard)
2. Solder paste masks (for automated assembly) should typically be a bit smaller than the copper pad. 0.1mm or 4mils smaller on each side is standard.
3. But some people just use the same size for the copper pad, solder mask, and solder paste mask
4. Be aware that heavy copper boards can't have traces that are as fine or as closely spaced together as lighter copper boards.
5. Ground and voltage planes make routing much easier since those connections go everywhere and without those planes, it's an artform to get those connections jumping over every other trace to get them to go where you want.
6. 0.3mm seems to be the standard minimum via size before you have to jump to start using more specialized processes
7. Make sure your all your net names for ground and other voltages are generated properly in the netlist and PCB layout. I've heard of buggy schematic capture software (big names) that sometimes generate multiple ground net names in the netlist. (e.g. instead of "GND" for eveyrthing, some are "GND", some are "GND_0129938", others are "GND_28375739", etc.)
8. Via stitching is cool
9. Make sure your vias connect to the plane they are supposed to connect to I know that at least PCB layout in OrCAD has a peculiar way of handling the net that a via is connected to (vias don't necessarily retain their net when copied and place onto another plane, they either take the net of the new plane or lose their net altogether and become isolated) and you can't just click on a via and arbitrarily change it's net. The net must be added onto the plane it is intended for and never be moved off that plane.
10. Make sure your PCB silkscreen designtations for components don't get covered up by pads...this was not obvious to me even when examinig the Gerbers. It only became obvious after I received the PCBs.
11. Always check the footprints files made by someone else against at least one datasheet for a component you are using of the same package. I've even had times where the footprint data on the datasheet was incorrect.
12. You can print the PCB out 1:1 on paper and test it against real components before you send the PCB off.
13. Don't have unconnected sections of copper on your PCB. (e.g. a section of copper plane on an outside layer has become disconnected from everything else by traces surrounding it. Either remove it using the function in the PCB layout software or put a via in it to connect it to an internal plane. Or else it can act like an antenna.

Do you need basic electrical design pointers like:
1. placing decoupling capacitors (0.1uF of ceramic X5R or X7R type if you don't know any better) as close as possible to the power pins of all ICs?
2. Keep traces to ground and power planes as short as you can.
3. PCB planes, grounding, and plane partitioning. Really good stuff:
http://www.hottconsultants.com/tips.html
The most important stuff IMO, are the following sections:

• 2. Slots in Ground Planes
• 4. Grounding of Mixed Signal PCBs
• 8. PCB Design Guidelines (pdf file)
• 9. Decoupling (Bypass Capacitors)
• 10. PCB Stackup
  • Part 1. Introduction
  • Part 2. Four-Layer Boards
  • Part 3. Six-Layer Boards
  • Part 4. Eight-Layer Boards
    
  • Part 5. Ten-Layer Boards
  • Part 6. Return Path Discontinuities
• 14. Red Flags

It would really help if we knew what kind of PCB it was since that would narrow down pointers a lot.

 

[AnalogKid]

1. PHOTOS of the board.

2. Do you have a schematic?

ak

 

[Nigel Goodwin]

You might like to check out DesignSpark, which is free and fairly well featured.

However, the viability (and cost) of your requirement really depends on how complicated the board is, and how important it is - recreating a replacement PCB is likely to cost far more than the item is worth, UNLESS the device is important and irreplaceable.

Basically, such a solution is for when 'price is no object' (and get a big wedge of cash upfront!).

 

[Colin]

I still use the very first PCB CAD program created by two engineers in Tasmania.
It does everything you need and has never fallen over or created frustration. All these other program "drive you up the wall" with limitations and "grouping" and "can't do this."
A 100mm x 100mm panel is only $10.00 I make everything to this size and if a larger board is needed, they can be joined with jumpers.
Take some photos and we will be able to let you know the level of complexity and the chances you have in doing the job.

 

[Western]

With regards to "best" software. This will be heavily dictated by price. Name your budget. $0, $500, $1000, or $10k.

Two main pieces in the software package:
1. Schematic capture software
2. PCB layout software

Steps:
1. Make schematic symbols with capture software.
2. Make padstacks (the PCB pads for the physical component).
3. Make the footprint of the compon........ .

Wow wow wow wow ... I am staggered at your reply. That must have taken ages to type ... and years to learn ... amazing.

Looks like I have 3 choices ...

1) Start learning/doing
2) Pay someone to do it for me
3) Forget about it and keep fixing them

As far as budget ... I'm unlikely to be doing this sort of thing too often, so I don't know that it would pay me to spend too much on software that I'll never use again.

It would really help if we knew what kind of PCB it was since that would narrow down pointers a lot.

Ok ... the board is the front panel of a 2 board set ... quite basic ... roughly 4"x 6" ... has 16 x keyswitches, 10 leds, 4 x 7 segment displays and 3 x ICs to drive them ... plus a small handful of other components.

They are only available as a pair at over AUD$1100 ... and while the rear board has it fair share of problems ... they are rarely at a point where you wouldn't bother fixing them. Out of hundreds, I only have one on the shelf where I gave up ... deep burn channels across the back under some power traces.

I'll put together some photos to make it clearer.

Thank you very much for your input so far.

 

[Western]

1. PHOTOS of the board.

2. Do you have a schematic?

ak

This is what I start with ...



This is a finished batch ...



Closeup of partly done - front



Closeup of rear




I do have a circuit ... a very rough hand drawn one.

I should say segments of circuit ... as to keep it manageable I have separated the display and drivers from the keypad side etc.

 

[Western]

You might like to check out DesignSpark, which is free and fairly well featured.

However, the viability (and cost) of your requirement really depends on how complicated the board is, and how important it is - recreating a replacement PCB is likely to cost far more than the item is worth, UNLESS the device is important and irreplaceable.

Basically, such a solution is for when 'price is no object' (and get a big wedge of cash upfront!).

Thanks Nigel, I will check out DesignSpark..

As mentioned above, the board is fairly simple ... but is part of a set and only available at AUD $1100.

I'm not sure of actual numbers, but this is certainly not a one off.

A lot of boards are easy to fix and I wouldn't even consider offering a replacement in those cases ... but if you look at the Before photo above ... you get some idea of what I have to go through.

With boards in this condition ... with pcb and parts on hand I could build a new board myself in less time than it takes to fix the harder ones ... though I do lean towards having batches built for me.

I have colleagues overseas who face the same problems ... so there are potential outlets there as well.

edit ... add closeup of faulty board

 

[Pommie]

Do you know how it interfaces with the other board? What is the big chip on the board? It might be programmable and therefore a problem.

Mike.
Edit, where are you based?

 

[AnalogKid]

Those are all low power circuits, so there is no explicit reason for extra thick conductors. I suspect that the actual copper weight is a normal 1 oz or 2 oz, with extra solder plating hanging onto the wider traces.

That looks like 70s/80s technology. What is the device that is so old, yet still in such demand as to have you rebuilding them in bulk?

ak

 

[Western]

Do you know how it interfaces with the other board? What is the big chip on the board? It might be programmable and therefore a problem.

Mike.
Edit, where are you based?

Hi Mike,

The electronics on the board is very basic ... nothing sophisticated at all. The first versions of these came out probably 30 years ago and the only difference with these newer ones is the style of switch!

The board at the rear is a different matter ... I wouldn't be thinking about replicating them in a hurry.

The big chip is the display driver ... M5450 ... and is available cheaply in an smd version ... which I would mount on the rear to help protect it.

I'm down in South Aust.

 

[dknguyen]

Yeah. That looks totally doable if you know what the board is supposed to do and what the ICs are. Only 3 ICs and doesn't look high speed or anything special so you can probably ignore most of the nitty gritty ground plane return crap in my post. It's just good to follow when you can.

Also looks like it's a 2 layer PCB though you could go with 4 if you really wanted to make routing the power and ground connections that go everywhere easier. But looks low speed so you don't even need ground planes and use jumpers where needed to cut cost.

 

[Western]

[QU
Sounds likeOTE="AnalogKid, post: 1325478, member: 175399"]Those are all low power circuits, so there is no explicit reason for extra thick conductors.
[/QUOTE]

Agreed ... unless the designers were expecting constant drownings and for corrosion to eat them away. Then thicker ones will last longer.

I suspect that the actual copper weight is a normal 1 oz or 2 oz, with extra solder plating hanging onto the wider traces.

Not sure of the actual thickness ... the extra solder plating is from a previous repair. I do know when I have peeled away some of the tracks I have been amazed at how thick they are compared to many modern boards. Maybe twice the thickness at least.

That looks like 70s/80s technology. What is the device that is so old, yet still in such demand as to have you rebuilding them in bulk?

Sounds like a riddle doesn't it.

I don't know if you have milk on your cereal for breakfast ... but these things are used to collect it.

That's not BS on the front of those boards ... that's CS.

Reason they want them fixed is that many of them are used on farms with 40, 50, 60 ... maybe as many as 120 of them. To put in something newer they have to buy a complete new batch ... along with the associated hardware. Absolutely megabucks.

 

[Western]

Yeah. That looks doable. Only 3 ICs and doesn't look high speed or anything special so you can probably ignore most of the nitty gritty ground plane return crap in my post. It's just good to follow when you can.

You're right ... it certainly isn't high speed or anything.

I don't know who designed the originals but just about every bit of space between tracks is filled with areas connected to ground. Absolutely nightmare when re-tinning everything as whiskers catch me out every time.

And apart from that, trying to decypher a circuit on a board like that is nigh on impossible ... especially the rear one ... takes forever. Me anyway!