Creating a printed circuit board (PCB) from a PADS net list.

In the previous section we produced a schematic called Parixt01.sch and we also made a netlist out of it called Parixt01.asc. In this chapter we are going to convert the netlist into a copper layout on a carrier material. This gobbledygook is tech speak for a printed circuit board.

The essence of this lesson is to get familiar with the multitude of options PADS gives you to do the job. We will not use the autorouter since single sided PCB's are more suited for the home-PCB-brewer. It's very difficult to align both sides of the PCB.
Also, the autorouter just puts all horizontal tracks on the component side and the vertical tracks on the solder side. I can do better than that. The trick is to make a PCB with less than 3 wire bridges. And even a eurocard sized PCB with 6 wire bridges isn't that bad. It's a lot cheaper and more accurate than a double sided board with 20 traces on it.

Some explanations before we get started.

It was a hell of a job to create this lesson, take my word for it. Any sane person would not have undertaken this job. Lucky for you, I am not sane.
In this lesson, a lot of mousing around and clicking is done. Therefore I want to set the following rules/conditions:

I will present this lesson in big tables. Process these tables from left to right and from top to bottom.

When reading the lesson, sitting next to an old DOS computer running PADS, try out as much as you want. There's only ONE way to get used to ANY router: Trial and error. MANY errors. Get used to your router and get used to the properties and idiosyncrasies of the components.
So if you ask yourself "Why is he doing this?", look around and try your approach. In most cases it will be better than mine. In all cases you have learned from it again.

Starting the PCB router.

In order to get started you must be sure that:

• the file 'parixt01.asc' is in the LOGFILE directory
• the file 'euro2.job' is in the FILES directory
• PADS is setup properly

1.1: Load an empty PCB.

In my libraries I have defined empty PCB's for the most widely used formats. The most widely used PCB's are euro.job and euro2.job which contain a full and a halfsized Euro-style card. A eurocard is 10 x 16 cm or 4 x 6.2 inches.
We will now load the half sized eurocard and immediately import the netlist from the previous lesson:

• F1 [In/Out]
• F1 [Job in]
• "euro2"
• F3 [ASCII in]
• "parixt01"
• "error.log"

1.2: Place the components for easy routing.

Now that we have a lot of garbage on screen, we're gonna place the components such on the bare PCB that the connections are easy to route in 2D copper.
This job can only be learned by lots of trials and lots of errors.

Repeat this last step until all zener diodes are placed above the PCB borders. Stack the zeners one below the other. The second zener comes at (-200, 3500). Place 6 zeners below eachother, then commence to the right. The second group of 6 zener diodes is stored from location (500, 3600) down.
The names of the zener diodes is offset from the parts, so you'll have to trial-pick some zeners before you get to Z12. But you'll learn that soon enough.

By this time you have untangled the zener diodes from the rats nest. They all are placed above the PCB.

Repeat this series of steps for R15, R14, R13 and R12. All these resistors handle in the same way. When we reach R11, we have another situation: R11 is not oriented and connected like the others.
What we'll do is use length minimisation by pressing F4. The length minimisation function makes the connections as short as possible. For some routing this is handy, for other it's not. But we'll see that when we get to the actual routing section.
If you're clearvoyant, you can force certain connections by moving a component around, pressing F4 until it connects to what you want and then bring the part back to the place where it's supposed to be.

Now place all resistors, up to R2 in the way as we did before this. You end up with 15 resistors, each 600 mils wide, right above eachothers.

Resistor R1 has a missing link. No problem. This is a FREE package, remember? We'll fix that later using the paper copy of the schematic. For the time being do as follows:

Now place all 2 pole connectors below the PCB, like we did with the previous two.

We now have a neat, packed, concept. But still, there are a lot of crossing connections. But we'll pass that bridge when we reach it.
Time to place the Jx 2 pole terminal blocks. We are going to arrange them side by side. We'll just do as if these are side to side stackable terminal blocks: 2 pin terminal blocks with small, mating, rails which enable us to only buy 2 pole connectors and make 4, 6, 8 or whatever size out of them.
In reality, one stocks up on 2, 3 and 4 pole terminal blocks of this kind. With these, we can then build every conceivable size terminal block.

Repeat this for J3, J2 and J1. Close this action with a 'Num-1'.

The status quo.

Things look good, so far. Except....

• probably too little space below the PIC chip
• probably too little space between PIC and resistors

Move all resistors R2 - R16 300 mils up and 100 mils to the right. In the case of R16, this means it is moved to (2100, 1900). By now, you should be familiar enough with PADS to do this on your own.

Fixing the dangling components.

This free trial version of PADS sometimes makes small mistakes. One of these mistakes is problems during transfer from schematic to netlist. The result is a component with missing connections, like, in this case, resistor R1 and zener diode Z16.
We're gonna fix this error with the help of the original drawing and a very powerful option of PADS PCB: the 'On the fly' function.

Using 'On the fly' function is so powerful, that (for small projects) you could skip the schematic capture and immediately load a PCB and add parts and tracks.
On the printed schematic we see that R1 is connected to Z16. So now we are going to lay a new connection from the open end of R1 to the (also open) cathode of Z16:

We return to the 'Place' 'Move' menu.

Pouring the first copper.

First make sure you are in the main menu (that is: when you press F10 once more, the program asks confirmation to exit to DOS; we don't want this, so we do not confirm this).

Repeat this sequence until R6 is connected to the PIC by copper tracks.

Connect R5 by LMB and F9. PADS now routes his own track and makes a square angle in the track. Repeat this with R5. By now, PADS has layed two copper tracks over eachother, so we must erase it. We don't like right angles anyway, so we don't loose too much anyway.

You now layed your first interactive trace!

Now route tracks between R2 and the PIC and between R3 and the PIC. That doesn't look all too difficult. But we loose a lot of space in the lower left part of th PCB.
So we must unroute the copper tracks between R2 - R5 and the PIC. Touch F7 with the mouse cursor, LMB on all four tracks and confirm each. Now reverse the position of resistors R2, R3, R4 and R5 (i.e. R2 and R5 change places and R3 and R4 change places) via the 'Place' 'Move' menu.
Now, that looks much better: parallel diagonals between Rx and the associated PIC pins. But J6 still looks like shit. Which isn't a wonder since we designed the wrong connector in....
We're going to lay some more copper. Make sure you are in the 'Route' menu.

Yikes, that looks awful. The tracks don't flow as we would like them to. We're gonna fix this. First RMB to quit this track. Then enter "g50".
The "g50" command sets the dotgrid to 50 mils. You can see that in the top left section of the screen.
The grid is some kind of snap-lock. If you place components they are put on the nearest grid point. They snap into a grid. With the "Gxx" command we can change the grid spacings.

Anyway, we changed the routing (AND the placing!) grid to 50 mils. This enables us to make nicer turns in our tracks. If you don't believe me (which I hope), just try to route tracks with grids of 25, 50 and 100 mils. 25 Mil works nicest, but it gets a bit nervous. 50 Mil is a good compromise value. When routing tracks between IC pins or when putting as much tracks as possible between the pin-row of an IC, the 25 mil grid can be very convenient.

We're going to make fancy traces now:

Placing the zener diodes.

Enough routing for the time being. Let's go back to the 'Place' 'Move' menu.

Now, this already looks good, but the lowerleft of the PCB is still a bit empty. So we're going to place the zeners there. See how far we get.

Press 'Num-1' to refresh the screen.

When looking at the terminal blocks J1 - J5, we see that they have the wrong orientation for matching with the Parinocard Input section. So we will turn each terminal block 180 degrees.

Now make sure we are in the 'Router' menu again.

Fixing routed tracks.

Now we see that the traces from Z15 are a bit out of line with the others. No problemo. We're gonna fix this immediately.

That looks 'MUCH' better, amigo!

Grounding the route track.

Now this all looks superb. We're going on with the ground tracks (GND). Press F10 and touch 'Route Conn'.

Place the remaining zener diodes.

Route the zener diode connections.

First we zoom in by using Num-Del + (900, 0) + LMB + (2850, 500) + LMB.

Hmm. Conductance will not suffer from it, but it doesn't look very nice. We're going to modify the traces a bit so they look better.
In theory this should be a bit better too since now the capacitances due to distances between tracks gets more even.

Repeat this last operation (the line width alteration) for the other three tracks between resistor and zener diode.
I like fat tracks. I -payed- for that copper you know!

See that? We can change the line width while routing! This opens lots of opportunities for us. Now you can lay lines with several line thicknesses without afterwards having to go to the 'Modify' menu.
The "w" command works from the last set corner until canceled by the operator.

Now is the time to place Z16. Pick it up at (-200, 3600), rotate twice and place it at (1100, 2300) after length minimisation. You see? You get the hang of it.

Now we're gonna place the remaining components. Make sure we are in the 'Place' 'Move' section.

Route the voltage regulator.

Now it's time to route the voltage regulator section. Select the Routing function.

Go to 'Place' 'Move' and do: (1700, 2800) + LMB + (1600, 2800) + LMB
Go back to 'Routing'

That damned no-good connector.

By this time, we can no longer pretend as if the header connector is still suitable for us. It's a design error and they should sack the guy who put it in in the first place! Nah, no matter who did this, is a three time loser!
Now, we -could- reconnect all pins, no problem, but we keep on working with a no- good connector. What we need here are SIP headers. If only we could change that, on the fly. On the Fly? That's it! We can do it On-The-Fly!

Here goes.... Not in a table this time, just on a line: RMB F1 F8 F5 F2 "con\sip\8p" Select Accept
That's it. We now have a SIP connector on the mouse pointer. Rotate and drop it at (3350, 2000). F1 (3200, 1200) F1 F1 (3200, 400) F1 RMB <Del Part>
Click anywhere on J6. LMB LMB LMB and J6 is gone forever.

Repeat this last step for the other 13 resistors.

We now must move resistor R1 100 mils up. Go to 'Place' 'Move' and do so. Then return to 'Routing'.

Done. Press Num-1.
Now move C5 from (3100, 2100) to (3050, 2200). Remove the corner from the (now angled) trace.

Go to 'Route' 'Route Conn'.

By now, there's only one connection left. Can you see the yellow line? Go fix it yourself. You can do it. I will give you onw clue: use the south passage.
Now we're gonna finish up a bit. It's been good until now.

What we did with 'Sizes' is replace all lines with a width of 12 by lines with a width of 50. 50 Mil is a nice value. And why throw away copper?
The last operation performed was a 'space check'. The program calculates the distances between tracks and if tracks are too close you get a warning.

Save your design for later.

   <In/Out> 
   <Job Out> "parixt" 
   

In this lesson you learned how to use PADS PCB. Please try all the options available. You cannot destroy anything, so go ahead and test things. For example: try to make text, move the names, create copper planes.

Page created September 2004,

Page equipped with FroogleBuster technology