First pcb layout/routing using orcad

Hello,

I am using orcad capture and pcb editor to make a small pcb (around 4 by 4 inches). First time making a pcb.

There is about 30 components and big connectors

I am having a hard trouble routing all the components in a double layer pcb (price matters)
It will be for digital signals and some measurements, nothing requiring high frequencies or top performance.

Here are some of the questions

Are there any good books or sites for routing tips?
Does the ammount of vias I create matter for the manufacturer? Does via size matter? I am using the default ones in pcb editor.
Is Wire width of 5 mil too small?

Even using the autorouter some netlists are not connected when using the limit wraparounds option. However from what I gathered it is always better to route it yourself without the autorouter.

Any tips for first time pcb really appreciated! Right now routing all the components just seems overwhelming

Figuring out how to route a dense circuit is something learned by experience. That said a few tips:

1. Contact your board house to see what their min trace width and spacing are. A high end board house would be able to do 5 mil traces w/ 5 mil spacing, but an economy fab will not -- for example, Sunstone specifies a minimum of 6 mil trace w/ 6mil spacing for their quick-turn prototypes. I prefer not to push the limit of the board house unless absolutely necessary (i.e., if they say 6 mil, I try to do at least 8) -- operating right at their limits increases the risk of shorting in the board (although, if you pay for electrical testing at the board house, this is not an issue).

2. Vias: again, this is a function of your board house. Certain standard drill sizes are usually included in a quote. Specialty holes are usually extra. Also ask your board house what their maximum via density is. They should give it to you in terms of vias per square inch. There are also physical requirements. Higher current traces require larger vias. Different sized vias also have different parasitic capacitances and inductances. These need to be considered in higher speed designs (note, both clock rates AND rise times need to be considered --> a clock rate of 100kHz w/ a 1ns rise time constitutes a high speed design).

3. Many people who have only worked on relatively small designs rail excessively against the evils of autorouters. However, like just about everything else, there are appropriate times and places to use autorouters -- try hand routing every single trace from end point to end point on a board with three 1500 pin FPGAs. The argument for manual routing is about control. Sometimes autorouters do really stupid things (like use 10 vias and run a trace three times around a board rather than make a direct connection). However, carefully setting up design constraints and autorouter options can usually alleviate this. If you are having a hard time with this, I would recommend manually routing any critical traces and locking them down. Then try to run the autorouter with a few different settings and see what you get. The autorouter is intended to be used with boards with more than 2 layers (i.e., 4, 6, 12, or more). It may choke on the fact that it only has two layers to work with. If you still can't get the board routed, consider the cost tradeoff between 2 and 4 layer boards compared to the amount of man-hours you are putting into the design.

* better to go for 8/8 mils trace/ clearance ( 6/6 is also common- consult fabricator)
* via size can be 12 mil dia/25 mil annular ring ( annular can be reduced)
* you may use jumper wires if routing is too tight for a bpoard for test purposeses.

How critical is price, as I've sourced 4 layer PCBs from China, where the price is minimal. The problem with modern digital devices is not so much the ultimate clock frequency, but device rise times. These coupled with EMC compatability requirements make a multilayer board a requirement for any digital design, with at least one contigous ground plane. This is basicly my opinion, but years of trying to get products through EMC etc has biased my view, so much that it is 2002 since I last did a 2 layer digital board.
The most important part of routing a PCB is COMPONENT PLACEMENT. Place the compoents and look at the paterns formed by the rubber banded connections, try to create as many point to point connections as possible. If you are stuck on a two layer design, use the compoent placement to minimise the use of vias. Placeing discretes can be a big factor in achieving this, so dont restrict the orientation of SMD discretes.
A big part of being a PCB designer is laying out boards, you develop an eye for placement and subsequent routing from looking at the connectivity, this is learned by experience. So the best way is learn the basics rules, clocks first etc and try it out, route the design and look for improvements as you route. It is an iteritive process.
Auto-routers like all tools require using correctly, again you learn to get a feel for them the more you use them, and the more you learn about adding design constraints.
So welcome to the land of PCB design, it is a world of PAIN

marce said:

The most important part of routing a PCB is COMPONENT PLACEMENT.

Click to expand...

Absolutely - I agree with that. Maybe you can show your layout - you may get some advice on how to re-arrange things.

Keith.

Thank you so much for the tips, Ill try to post the layout when I get to the pc with orcad

I will try the 8 mil width/spacing

I am in the US and only need 1 board, the best price I have seen is the 4pcb.com

going 4 layer they require min qty of 4 boards which is 264$

Boards are made in panels, and most board houses will charge your for an entire panel's worth of material, regardless of how much of it you use. Panels come in different sizes, but even the smallest should be able to get at least two 4" x 4" pcbs on it -- at most houses, you should be able to get two boards for exactly the same cost as just one. Besides -- it's always a good idea to get at least one spare PCB, in the event of a problem with assembly (i.e., a pad delaminating, or components getting assembled incorrectly).

A word of caution: be careful going with extremely low priced board houses. For a really simple design, they should be fine. However, sometimes "you get what you pay for." You could get bad substrate, poor layer registration or drill precision, or a whole other host of problems that will make your board not function at all. Better to pay a little more and get a working board then to pay less, and still have nothing. Obviously, some board houses are set up for large production runs, and gear their efforts (and prices) for that. However, there are some basic costs that can't be avoided with precise PCB fabrication. I get a little nervous when I see really low prices on a website that doesn't explicitly list all of their manufacturing capabilities.

elpajuo said:

I am in the US and only need 1 board, the best price I have seen is the 4pcb.com

going 4 layer they require min qty of 4 boards which is 264$

Click to expand...

That's expensive. I use PCB-Pool in Europe but their USA prices are lower than here. 4"x4" would be around $70 in 2 layer and $102.50 for 4 layer + delivery, depending on options chosen.

Keith.