Making of a PCB designer

[gkcbangalore]

Hello Every one
I am a freelance PCB designer for micro and small companies for the past 15 year. After struggling for 12 years I can tell with some confidence I have a hold on designing.
My fight for the following continues
1. How can I know where to keep which component to where so that routing becomes easy
2. How can I reduce the mistakes
3. How can I anticipate the completion time
4. Which strategy to follow   "place and route" is best or" place route place "strategy
5. How can I preserve the mental strength till the end of the design phase
6. How can I upgrade the knowledge and tech advancements.

[free_electron]

Hello Every one
I am a freelance PCB designer for micro and small companies for the past 15 year. After struggling for 12 years I can tell with some confidence I have a hold on designing.
My fight for the following continues
1. How can I know where to keep which component to where so that routing becomes easy

use schematic driven placement.

2. How can I reduce the mistakes

use cad software with realtime DRC and plug design rules from schematic. ( trace width and spacing )

3. How can I anticipate the completion time

experienc.e can't help you there. this depends on person to person ...

4. Which strategy to follow   "place and route" is best or" place route place "strategy

it depends. i work in 'blocks'. place circuitry around a chip ( decoupling caps for digital stuff for example and the associate power ground spiderweb ) , or a quad opamp chip with all the passives around it. then place this block close to the other blocks or connectors it mates with. this is all very trivial if you use schematic driven placement.

5. How can I preserve the mental strength till the end of the design phase

here's what work for me :
   pepsi ( with real sugar as opposed ot corn syrup )
  youtube playlist with some thumping music...  zztop's sharp dressed man ,legs ,  perfect for routing high density boards ....

6. How can I upgrade the knowledge and tech advancements.

read blogs , IPc documents, there's free magazines you can subscribe to that help you stay sharp.

here is my layout strategy.

define board contour, mouting holes , no-go-area's. this is often dictated by the housing.
place 'unmovable parts' : connectors , switches, displays.. anything that sticks its head out of the box , or needs to mate with another assembly.
place 'bulky' stuff like large heatsinks , fat capacitors depending on headroom.
freeze at this point.
take a look at the power supply section first. stick that in its corner of the board, close to the power input and do the layout so you can break out easily on different layers / split planes.

place the 'critical stuff now ( noise sensitive things etc ) . use schematic driven layout. ( select the parts that belong together in the schematic , switch to pcb and place one by one from this selection. use the ratsnest to rotate and get the parts in a setting. rotate and replace parts to get a clean ratsnest. plunk down tracks and freeze this block.

repeat for other blocks.

move blocks into their location on the pcb ( close to their input/output pathways such as connectors etc. )

and so on...

[jerry507]

I tried to find anything to add to free_electron's method, but I can't think of anything off the top of my head. It's exactly the way I do it. I find the "block" method for designing certain areas such as PSU are very helpful. It's at that point that you see very clearly only what is necessary and you can't eliminate mistakes such as forgetting strategic copper pours and such.

It's important to have a very well defined mechanical design done BEFORE you design the PCB. It would be better if this could be collaborative, but in reality you need to know where connectors go, mounting holes, any keepout areas and things like that BEFORE you route. Otherwise you just risk wasting time.

I have never needed help keeping my mental strength up doing PCB layouts. That's the fun part, and I know that I'll be wishing I was doing a layout later on when it comes time to do the software. Sigh.

[gkcbangalore]

Thanks for the reply.
We can divide the pcb design mistakes as
1.Connectivity mistakes such as wrong or open connections
2.Mechanical mistakes such as component fouling, wrong position of components
3. Signal level mistakes such as lengthy tracks, interfering traces, wrong track widths
4. Ground loop errors, and ground plane mixing(for mixed signal gnd plan)
5.  Pin reversal (BEC insted of BCE for sot23 packaged transistor for example)
  May be further more
Most of the times sch driven designs avoid connectivity mistakes. To avoid other mistake types we may have to  have specific checklist apart from general pcb design guidlines

[AnthonyJarmie]

Hello friends,

You've designed your circuit, perhaps even bread boarded a working prototype, and now it's time to turn it into a nice Printed Circuit Board (PCB) design. For some designers, the PCB design will be a natural and easy extension of the design process. But for many others the process of designing and laying out a PCB can be a very daunting task. There are even very experienced circuit designers who know very little about PCB design, and as such leave it up to the "expert" specialist PCB designers. Many companies even have their own dedicated PCB design departments. This is not surprising, considering that it often takes a great deal of knowledge and talent to position hundreds of components and thousands of tracks into an intricate (some say artistic) design that meets a whole host of physical and electrical requirements. Proper PCB design is very often an integral part of a design. In many designs (high speed digital, low level analog and RF to name a few) the PCB layout may make or break the operation and electrical performance of the design. It must be remembered that PCB traces have resistance, inductance, and capacitance, just like your circuit does. This article is presented to hopefully take some of the mystery out of PCB design. It gives some advice and “rules of thumb” on how to design and lay out your PCBs in a professional manner. It is, however, quite difficult to try and “teach” PCB design. There are many basic rules and good practices to follow, but apart from that PCB design is a highly creative and individual process. It is like trying to teach someone how to paint a picture. Everyone will have their own unique style, while some people may have no creative flair at all! Indeed, many PCB designers like to think of PCB layouts as works of art, to be admired for their beauty and elegance. “If it looks good, it’ll work good.” is an old catch phrase.

Best regards
Anthony

[free_electron]

there is a reason that the layout is callec 'artwork' ....

[steve_w]

Thanks for the tips "free"

regards

SW

[JuKu]

Thanks for the reply.
We can divide the pcb design mistakes as
1.Connectivity mistakes such as wrong or open connections
2.Mechanical mistakes such as component fouling, wrong position of components
3. Signal level mistakes such as lengthy tracks, interfering traces, wrong track widths
4. Ground loop errors, and ground plane mixing(for mixed signal gnd plan)
5.  Pin reversal (BEC insted of BCE for sot23 packaged transistor for example)
  May be further more
Most of the times sch driven designs avoid connectivity mistakes. To avoid other mistake types we may have to  have specific checklist apart from general pcb design guidlines

The key issues are schematic driven design, a designer who knows what s/he is doing, good design rules and very good part libraries. If so:

1. Never happens
2. Components will fit to the pattern on the PCB and not touch each other. Components will also solder well. Some interaction with the enclosure designer is needed (potential error)
3. Will not happen, but might require high-end tools for RF, EMC and other interference control (I don't consider track length control a high end feature nowadays.)
4. Needs communication from the sch designer to the PCB designer (potential error) and a tool that knows the difference of digital, analog, chassis and whatever grounds you have (different nets, connected together in a controlled manner)
5. Will not happen

I don't recall the last time when I've experienced a true PCB design error; that is, not originating from the schematic design, error in the libraries, bad data from chassis CAD, a bug in tools or something like that. It is truely an art, but if you know your art, use the features of your tools and have tools that are up to the task, the PCB creation is unlikely to produce any errors of its own. (Rather different from schematics or software creation! :lol:)

[free_electron]

Be care full with 3 and 4... This requires a great deal of specialized knowledge and experience and can not be driven from schematic....  As for the software tools... They are very poor or unusable at best...

Yes you can do things like specifying defferential pairs, max length discrepancy and others, but the routing is still an art where you need to look around the channel you are passing through for potentiaal agressors...
And that requires a pcb designer that is not just a 'polygon pusher' but someone who understands the design , knows the signals and knows signal integrity / emc rules!