USE DISCOUNT CODEEXPERT30TO SAVE $30 USD
About enlarging the tracks of a differential pair without changing the stackup
mulfycrowh , 08-26-2023, 12:23 PM
Hi everyone,
I have a very dense design involving many differential pairs and more particularly dedicated to HDMI.
The target impedance is 100 Ohm.
The matching width and gap are respectively 75 um and 127 um.
To make the PCB cheaper in production I would like to have a width equal or bigger than 100 um.
A matching gap for this width is 250 um.
I would like to know if you already used this technique to achieve this goal.
Thanks.
I have a very dense design involving many differential pairs and more particularly dedicated to HDMI.
The target impedance is 100 Ohm.
The matching width and gap are respectively 75 um and 127 um.
To make the PCB cheaper in production I would like to have a width equal or bigger than 100 um.
A matching gap for this width is 250 um.
I would like to know if you already used this technique to achieve this goal.
Thanks.
mulfycrowh , 08-26-2023, 01:35 PM
Not so obvious: no sufficient distance between pairs...
mulfycrowh , 08-26-2023, 01:36 PM
we can also decrease a little bit the impedance within the tolerance.
What do you usually do?
What do you usually do?
qdrives , 08-27-2023, 03:03 PM
Not that It would help you, but I am currently designing a board with 105um (3oz) inner layer. That requires 0.25mm traces and spacing. I cannot get much above 40 ohm impedance.
However, If you increase the dielectric thickness, you need wider traces too. Is this an option for you?
However, If you increase the dielectric thickness, you need wider traces too. Is this an option for you?
mulfycrowh , 08-27-2023, 03:28 PM
As you can see on the screenshot, it is not possible to increase the thickness to get wider tracks.
I had everything above 75um in the project.
Reaching the target above 100 um is very difficult.
I reached the target everything above 90 um.
For that I enlarged the gap for the DPs dedicated to HDMI.
With a gap of 180 um, I get a width of 90 um.
DONE!
The only remaining that cannot be solved is 5 BGAs with same packages. The balls have 0.25mm diameter with a pitch of 0.5mm.
Impossible to get a space of 90 um: either you choose a track of 83.3 um with a space of 83.3 um or a track of 90 um with a space of 80 um.
I chose the second option.
I had everything above 75um in the project.
Reaching the target above 100 um is very difficult.
I reached the target everything above 90 um.
For that I enlarged the gap for the DPs dedicated to HDMI.
With a gap of 180 um, I get a width of 90 um.
DONE!
The only remaining that cannot be solved is 5 BGAs with same packages. The balls have 0.25mm diameter with a pitch of 0.5mm.
Impossible to get a space of 90 um: either you choose a track of 83.3 um with a space of 83.3 um or a track of 90 um with a space of 80 um.
I chose the second option.
qdrives , 08-28-2023, 03:00 PM
What is the length of the tracks where the impedance does not match?
I though Altium was able to do a "SI" simulation with the actual traces, right? If so, you could see of the effect of your decision is acceptable.
I though Altium was able to do a "SI" simulation with the actual traces, right? If so, you could see of the effect of your decision is acceptable.
mulfycrowh , 08-28-2023, 03:13 PM
@qdrives Do you mean the tracks used to make the fanout?
qdrives , 08-28-2023, 03:18 PM
Yes, if the fan-out is relatively short compared to the rest of the trace and compared to signal rise time, the 'problem' may not be that much.
mulfycrowh , 08-28-2023, 03:28 PM
TI suggest using micro vias but taking account of the problems encountered with many PCB manufacturers when we speak about vias with 0.15mm diameter, I have rejected this option.
Yes the tracks are very short. The IC is 5mm x 5mm.
Yes the tracks are very short. The IC is 5mm x 5mm.
qdrives , 08-28-2023, 04:00 PM
What about Via in Pad, SMD (Solder Mask Defined) and copper filled pads/microvias? For the inner pads.
Does not make it cheaper though.
Do note that I am not an SI expert, nor have I ever done HDI.
Does not make it cheaper though.
Do note that I am not an SI expert, nor have I ever done HDI.
mulfycrowh , 08-28-2023, 04:09 PM
I think it is out of the standard manufacturing. I even received a quote of $85,000 for 5 boards!!!!
qdrives , 08-29-2023, 02:47 PM
$85k, let my check my wallet....
Sorry, no I cannot help you. I do have an old 1000000 Turkish Lira bill, but I don't think they will accept that (it was worth about $0.50)
Question is: did they also provide some 'assistance' on how to produce it more cheaply?
Just looking at my standard fabricator Eurocircuits -- https://be.eurocircuits.com/shop/ass...b-d815c93952de
0.09mm TW/TT, 12 layers, 100x80mm -> €534/pcs for 5 pcs.
Perhaps not your spec, but at least they are willing to give tips on how to do it. However, they do not have microvia support.
we-online.com, 0.085mm inner layer, 0.1mm outer, should be able to do HDI.
Sorry, no I cannot help you. I do have an old 1000000 Turkish Lira bill, but I don't think they will accept that (it was worth about $0.50)
Question is: did they also provide some 'assistance' on how to produce it more cheaply?
Just looking at my standard fabricator Eurocircuits -- https://be.eurocircuits.com/shop/ass...b-d815c93952de
0.09mm TW/TT, 12 layers, 100x80mm -> €534/pcs for 5 pcs.
Perhaps not your spec, but at least they are willing to give tips on how to do it. However, they do not have microvia support.
we-online.com, 0.085mm inner layer, 0.1mm outer, should be able to do HDI.
mulfycrowh , 08-29-2023, 03:15 PM
The true issue with the manufacturers, they never say why it is not doable or why it is $85k or just share a small part of the iceberg.
I was tired about this and went to one of them, had a chat for about 3 hours and they exactly told me what do do to have a complex PCB for a reasonable price.
I was tired about this and went to one of them, had a chat for about 3 hours and they exactly told me what do do to have a complex PCB for a reasonable price.
qdrives , 08-29-2023, 04:02 PM
and they exactly told me what do do to have a complex PCB for a reasonable price.
I would rather go to a fabricator that says: "why do you need 0.09mm tracks?" then the one that states: "no problem, we can make that."
mulfycrowh , 08-29-2023, 05:32 PM
And for the assembly, same type of issue: either they say „we are not interested in such protyping quantities“ or it is expensive.
i found the solution, I have my own stencil printer, my PNP and reflow oven.
Quantities of 100 pieces is no more a problem with components down to 0201.
i found the solution, I have my own stencil printer, my PNP and reflow oven.
Quantities of 100 pieces is no more a problem with components down to 0201.
robertferanec , 08-30-2023, 01:19 AM
don't forget, often you would like to have the single ended impedance of the signals in diff pair around 50 ohms. that will specify the width and based on the width you then calculate space for your diff pair impedance.
the only way to adjust these is to play with stackup, specifically distance from reference plane.
I have some stackup examples, feel free to reuse them: https://fedevel.com/blog/download-pc...-your-projects
the only way to adjust these is to play with stackup, specifically distance from reference plane.
I have some stackup examples, feel free to reuse them: https://fedevel.com/blog/download-pc...-your-projects
qdrives , 08-30-2023, 02:50 PM
Here in the Netherlands we have a company (https://www.deltaproto.com/) that specializes in proto types. In fact, they do not want to do high quantities.
I do not know if what you need is beyond their capabilities.
I do not know if what you need is beyond their capabilities.
Use our interactive Discord forum to reply or ask new questions.