MIL-STD-1553 trace routing

Are you saying the traces on the "outside world" side of the transformer are going through several boards before getting to the connector?  Then, does that mean you have two pair you are routing from the xformer to the connector?  If so, this sort of complicates the purpose of transformer coupling of the "stubs" which are normally intended to isolate the "inside box" connection from the outside world cabling.

I have never ran across a specific requirement to avoid ground/pwr planes with the routing, but then usually that is a pretty insignificant part of the overall bus structure.  I would think that maintaining a consistant impedance of the diff pairs compared to the STP cabling (~120-130ohms) would be more important, so running long lengths over a ground plane could adversely effect that if your stack-up and trace geometry isn't done with that in mind.  Also, pay attention to the "max stub length" specs of 1553.

Otherwise, keeping the 1553 traces along the outer edge of the boards sounds like a good approach to me if for no other reason than to eliminate possible crosstalk issues with other internal logic.  Especially if you're integrating it with newer low-voltage circuitry internally.

IMHO - cheers!

Hi Roger,

Yes, I need to route across several boards before getting outside the box. The bus controller (brick) and xfmrs will be mounted on a "controller card". This card plugs into a backplane. From there the signals go to a transient / EMI protection board(s) which then interface to the outside world connectors. Routed length is going to be on the order of about 7" inside the box. Outside the box there will be approx 6 feet of cable to the bus coupler which is terminated with 78 ohm terminators. Max stub length is on the order of 20 feet, so we are well within this requirement.

There are two dual redundant 1553 busses (Bus 1 and Bus 2) each consisting of a "Bus A" and "Bus B" for a total of four pair. I suppose I'll route the first bus on the top and inner 1. The second bus set on the bottom and the next layer up all along the outer edges to avoid crosstalk. Board will probably be 8 layers.

I'm still working on the hardware design, but looking ahead to the board layout so I can supply the mechanical designers with my electrical needs before they try to manipulate my electrical design to fit their mechanical needs................. We all know how that goes.

Layout starts in a few weeks, so I'm sure I'll be around more often asking silly questions as I try to work in harmony with PCB editor.........

 Tom 

hi Tom,

 I too am facing the same problem for routing the 1553 lines on backplane. Since it carries more current, is it necessary to give thicker traces like 15-20 mil? Is it compulsory to avoid power planes below the traces? Most importantly differential trace length matching, What is the tolerance for the + and - lines.

I have been consulting with the application engineers from the 1553 device company we are using. They recommend keeping the coupling transformer as close to the 1553 controller as possible. This being the case, I will have a fairly long run of 1553 bus signal before it gets to the outside world connector. The FAE's have recommended keeping the 1553 bus signals away from any power/gnd planes as the capacitance induced by the planes will have an impact on the signals.

Since I am designing most of the circuitry that is going into this product, I have the freedom define the connector pin outs and locate the signals at the edge of the backplane. I can easily route them along the edge without having to deal with any planes. I'm planning on using 15 mil traces.

I have worked on designs in the past where we had planes under 1533 signals, but these had a very short run before they hit the coupling transformer, maybe 1.5" or so. This new design requires the 1553 to run almost 8" from the outside world connector to the transformer. With such a long internal run, 1553 signals can easily be affected by routing them over any planes.

Of course the proof will be when I finally get the board back and hook a scope up and see the actual signal.

Tom 

Tom, 

Thanks for the reply. The trace impedance preffered is 78 ohm differential right?