LMH0030 to buffer impedance

Richard Woodham1

Other Parts Discussed in Thread: LMH0030, LMH0002, LMH0031

We have a requirement to pass the LMH0030 output signal from the middle of a long, thin board to the buffer chip (LMH0002) at the end. Space constraints require this signal to be routed on an inner layer of our FR4 PCB & we are really struggling to find a geometry to give 150 Ohms differential impedance. The LMH0030 datasheet gives dire warnings about driving 50 Ohm loads, yet SNLA196 ("LMH003x FAQs") suggests a method with 100R differential traces. Our board house is suggesting a geometry which will give 138R. Can we work with this? What should the LMH0030 load resistors be? At the moment they are placed at the drive end of the transmission line with the termination resistor across the buffer inputs.

over 10 years ago

0 Michael Peffers over 10 years ago

TI__Mastermind 20820 points

Hi Richard,

One of our applications engineers is looking into this and will respond shortly.

0 Nasser Mohammadi over 10 years ago

TI__Guru* 93670 points

Hi Richard,

How about if you arrange your board stack up such that you would have 75 ohm(not 150 ohm)? If you have multiple planes this should be easier to achieve than 150 ohm? Please check with your fab house and i think they should be able to do this.

Regards,,nasser

0 Richard Woodham1 over 10 years ago in reply to Nasser Mohammadi

Prodigy 210 points

So, If I have 75 Ohm differential, what value of load resistors should I use ? 37.5?

Why not 100 Ohm differential with 50 Ohm load resistors, in flagrant breach of the datasheet advice?

0 Nasser Mohammadi over 10 years ago in reply to Richard Woodham1

TI__Guru* 93670 points

Hi Richard,

I was referring to 75 ohm single ended not differential. In this case, you can treat the load like what is specified in LMH0030 and LMH0031 data sheets. Arranging board stack up to meet 75 ohm impedance is very doable so the thought is that this would be preferred.

Data sheet strongly recommends not using 100 ohm differential since it could involve long term reliability of the device so we should stay within the data sheet recommendation.

Regards,,nasser

0 Richard Woodham1 over 10 years ago in reply to Nasser Mohammadi

Prodigy 210 points

Simply stating that our problem is not a problem is of no real help.

0 Mark Sauerwald88474 over 10 years ago in reply to Richard Woodham1

TI__Genius 13475 points

Richard

What I would do is to use the LMH0030 but use 50Ohm pullup resistors rather than the 75Ohm that are shown in the typical interface circuit - the result of this will be a smaller output swing, and it may not meet the SMPTE rise/fall specs, but since this is not an output from the board, this shouldn't matter. Now you can drive either a 100Ohm differential transmission line, or loosely coupled 50 Ohm single ended lines (matched in length), to the LMH0002 - at the LMH0002, terminate with 100 Ohms across the inputs. Since your swing will be a bit less than nominal, you will have lost some noise margin, but running differential rather than the normal single ended for SMPTE signals makes that back.

Mark

0 Richard Woodham1 over 10 years ago in reply to Mark Sauerwald88474

Prodigy 210 points

Of course, as these signals are only internal to the board I don't need to stick to the standard impedances. The most we can squeeze out of our board is 144 Ohm differential which is within 10% of target, but I still have option of using 71.5R pull-ups & 143R termination.

Thanks.

0 Mark Sauerwald88474 over 10 years ago in reply to Richard Woodham1

TI__Genius 13475 points

If you know that your transmission line will be closer to 140 than 150, then you would be better off terminating in that value, however since it is a bit non-standard, I'd probably annotate the design/layout with a note saying what you are doing.

Interface

Interface forum

LMH0030 to buffer impedance