PROTEL Autotrax - known issues

You must size strings in multiples of 12 thou, if you don't they will display as if they WERE multiples of 12 thou, until you come to manufacture, where they may change.

The hole sizes in all the protel PCB libraries are not really correct. They are often odd values like "23 thou". I believe that what was intended was that a designer could layout their board, and AT THE END decide that they wanted, for instance, to use no IC sockets, so 28 thou was the best size, or IC sockets, so 32 thou was the best size - and then they could do a global hole size edit of just hole sizes matching "23 thou" to these new, real, sizes. Actually, a far better technique is to make them all 32 thou and be done with it, as often this last step get reliably missed in the rush to get prototypes made! Check all your hole sizes.

You should not select autoroute "pre-route" while you have SMT pads on the board - it will often add little PTH via pads beside the SMT ("stringers") even if they don't need them, and even if they short to neighbouring pads.

In Autotrax, SMT pads will only be produced without a hole if the hole size is set to 0. Be careful that you specify a hole size of 0 for SMT pads

Octagonal pads are rotated by 22.5 degrees in gerber plots. Most australian manufacturers then rotate them back again for you. I elect not to use octagonal pads for this reason. This issue may be duplicated in other versions of Protel software

Sometimes when you rotate components with rectangular SMT pads on PCBs - or perhaps when you rotate block selected areas, I'm not sure - you will get the X and Y values for the pads swopped. That is, everything will rotate by 90 degrees, but if the longest dimension of the pad was horizontal it will still be horizontal. This is usually immediately obvious. It is not random - it happens when you do something unusual first (I can't quite remember what - perhaps it happens when the pads are not part of a component, but are "exploded" or primitives - email me if you know what causes this!)

The "netlist:length" command in PCB does not seem to yield a useful measurement

The PCB design rule check is pretty reliable - but reading the report takes some experience - it tells you that there is a fault, but often twice, and often in a way you are not expecting. (For instance if you reverse the ground and VCC connections on an IC, you may get hundreds of reported errors on a large PCB, when there is only, really, two.)

DRC sometimes shows an error for strings in copper when there is not one - be careful though - some manufacturers somehow screw up translation of copper stings - I have had shorts. I tend to leave a bit of extra room around copper strings now.

If you have two pads with the same pin number in a component (which happens with some tactile switches) then PCB DRC will throw up a lot of errors, - especially if you then use the tactile switch as a jumper. The only solution is to show the four pins on the schematic - or make a PCB library component with two pins and two soldered unnumbered pads.

When producing a multilayer board, Vias cannot be connected to the Ground plane or VCC plane. The solution is to use individual pads as vias, as any pad can be individually edited to connect to the ground plane or VCC plane as required. However, be very careful with any translation of the final multilayer PCB file to other formats - while Protel V2.8 generally handles the translation correctly, many other Protel versions lose the plane connection information saved in an Autotrax file, although the outside layers of the PCB will seem to be correct. Have any translation done by someone who knows what they are doing!

The Autorouter included in Autotrax is not really very good. You are much better off manually placing tracks. I find the autorouter most useful as a yardstick test after I finish placement, before I begin manual routing. (Remember to do this on a COPY of your work!) If the autorouter can achieve 95% routing, I know the board will be a very easy manual route job. If the autorouter can achieve 85%-90% routing, I know the board will be a moderate manual route job. Also, using the autorouter to process just preroutes cleans up the "rats nest" that is used to guide placement during manual routing.

Issues for Schematic

Sometimes you can manage to save highlighted tracks in Schematic. Not really a bug - but it does surprise you when it happens.

If you make very large multipart components in schematic, you will chew through the available memory very quickly. One such component that is tempting is an mutlipart DB25 RS232 connector, where you can place the individual pins one at a time, and the program automatically knows the signal name. A few of these and you will run out of memory. The standard connector pins that schematic provides need the pin name entered every time, but they use virtually no memory.

Issues for Schematic Libmake

Issues for Plot

I think that covers it. I've laid out hundreds (no exaggeration) of boards in Autotrax 1.61. I think I would know of any other bugs by now - but then again, maybe there are some things I just don't do, so I just haven't discovered. Email if you find something we should add.

Links to other Autotrax material

• Protel Autotrax free download page
  
• Protel Autotrax Printer drivers - print to pcx format
  
• Protel Autotrax Video drivers - to improve on 640x480
  
• Short Autotrax PCB layout tutorial, by AirBorn.