need help with SMT layout

[ambertch]

Hi guys,

This is my first SMT layout. I'm converting a through hole design so I've gotten the 1206 and SOIC variants of all possible components and have some questions (using Orcad):

1. What wire width should I use?
2. Any general tips for the routing? I played around with the layout for a bit yesterday, placing components with a rough spatial locality, hit autoroute and it was impossible to route. I then spaced out components a little more and autorouted again. It took a long time and I did not have significant space savings (But partly b/c I still have a couple large components like I/O transformers that can't be shrunk).

Thanks a lot,
Ambert

 

[itsmoked]

Hi ambertch,

1) Typically about 10mil traces. Of course it totally depends on what they need to carry. I generally go with 10mil and when I'm done I will go back and bump up any that I can. A lot of trace width selection depends on whether you need to run traces between pins.

Also if u have high voltages you of course need larger gaps, often called your "design rules".

Remember that SMT parts often can't dissipate the same power as the thru hole parts so you need to watch that. You can help the parts by having wider heat dissipating traces leading to them.

2) Every job has its own special requirements to make a clean layout. I couldn't begin to make suggestions with out a whole bunch of detail information... all of which can change with a single new detail.

I will say the first thing you MUST do is rats nest the design. Take a while moving the parts around. I find good luck by trying to place the parts on the board in the same pattern as the actual schematic, since this generally locates the parts and hence their connections, hence the traces in the locations needing the shortest runs.

 

[sreid]

Are you using both sides of the board for components? This is commonly done on SM boards. Often, small parts are put on the back side and larger parts (IC's) are placed on the front side.

 

[buzzp]

There are many rules to laying out a board. Parts placement should not be a random placement. Analog circuits should be kept seperate from digital. Power parts seperate from rest of circuitry. Signal and return lines should be side by side and approximately the same width (I assume you know all this since through hole layout is no different than SMT when it comes to parts placement). Many, many other rules to this.

Pad sizes should be kept the same size on each part (only the pads for one part) to prevent tomb stoning of parts when they go through reflow oven.

Autorouting has never produced good results for me so I never use it. And when you do use it, it does not care about digital and analog circuits, return lines, etc.

Do a web search and you will find many rules of thumb amongst other helpful information.

 

[itsmoked]

I agree buzzp auto routing does a lousy job. Occasionally it works well if you have a large bus running to multiple ICs. You set up the netlist so only the bus is in the picture then let the router at it. Finish with a hand route.

 

[ambertch]

Thanks for the replies.

"large bus running to multiple ICs. You set up the netlist so only the bus is in the picture then let the router at it." I'm not sure what this means, can someone clarify? I am thinking rails and planes for commonly used signals but not sure.

 

[tuned99]

"large bus running to multiple ICs. You set up the netlist so only the bus is in the picture then let the router at it." I'm not sure what this means, can someone clarify? I am thinking rails and planes for commonly used signals but not sure.

He suggests that the multiple line bus signals can be auto routed by the program rather than by hand to prevent mistakes. A netlist will typically generate the specifications for all signals of your circuit, including power and ground connections. So deleting all entries from the netlist, except for the bus, will isolate the bus for the auto-router to handle. You manually route everything else.

 

[itsmoked]

Thanks tuned99.

Yeah ambertch, large busses like a bunch of data lines D0-D7 and/or address lines A0-A16 going from say a microprocessor to it's memory and and peripherals, timers, A2D converters, D2A converters, flash memory, etc. etc.

This can be tedious and time consuming for a human and relatively easy for autorouters. So this is all I ever use them for. When you get good at boards the first requirement ends up being SMALL which means tight and tough to do. Autorouters never ever manage to *complete* these routes and so leave you with 5 or 6 traces that CANNOT be routed by anyone or thing.. essentially rendering the whole effort a waste.

 

[ambertch]

Please bear a newbie question; this is my first experience with Orcad's layout software: How do I make a drillhole for sending wires to the other side in the main layout (what I am doing now is just creating a testpoint in my capture file and the autorouting seems to go through to the other side of the board), and how do I make a hole when making footprints? (Tried placing a pin and going to its properties w/ no success) Thanks again for the help.

 

[Comcokid]

On through-hole boards, there are enough leads that traces from one side to the other usually can be done at a component lead. With a surface mount design, you will usually have few through-hole leads.

A hole with pads on each side is called a "via". A 30 mil pad with a 18 mil hole might be used.

Trace sizes, via hole sizes, minimum space, minimum annular ring (pad size - hole size) are largely defined by the PCB costs. If you are making a PCB from one of the many PCB companies that will make two to four boards for a low cost, check their web site to see what board "rules" must follow to get their low price.

Generally, prices remain low until you go below 8 mil trace/8 mil space and 18 mil minimum hole size. You can go as low as 4 mil trace/4 mil space and 10 mil hole, but prices quickly increase. Boards are made with sizes below this, but costs quickly go up and fewer board houses have the capability.

 

[itsmoked]

ambertch, as Comcokid said, vias are what you are thinking of. They are a standard part of board layouts and will be accessed easily in ORCAD. Somewhere there is a "put a via here" button.