TDR solder mask...

J

John Larkin

Guest
https://www.dropbox.com/s/idwz568o8hfpgzb/TDR_Solder_Mask.jpg?raw=1

The two un-masked patches are not visible on 30 ps TDR. Board
variations are a lot bigger.

--

If a man will begin with certainties, he shall end with doubts,
but if he will be content to begin with doubts he shall end in certainties.
Francis Bacon
 
Am 25.01.22 um 23:08 schrieb John Larkin:
https://www.dropbox.com/s/idwz568o8hfpgzb/TDR_Solder_Mask.jpg?raw=1

The two un-masked patches are not visible on 30 ps TDR. Board
variations are a lot bigger.
Click to expand...

I got similar results on a JLCPCB 4 layer board.
I calculated that 50 Ohms are 11.55 mil, drew it 12 mil in
Altium. Seems to fit.

<
https://www.flickr.com/photos/137684711@N07/51843174578/in/dateposted-public/lightbox/
>

The SMA launcher decal was not so good, but I was interested in the 50
Ohm line only for verifying eps-r and thickness etc.
The launchers were for a 2 layer process. The streamlined boards
for the LMX2594 are on the plane from HK. They also have cutouts
on Layer 2 and shorter SMA center pads. The unpopulated SMA is
better than the populated one. The thickness of the center pin
and the solder seem to matter.

cheers, Gerhard
 
On Tuesday, January 25, 2022 at 2:09:11 PM UTC-8, John Larkin wrote:
https://www.dropbox.com/s/idwz568o8hfpgzb/TDR_Solder_Mask.jpg?raw=1

The two un-masked patches are not visible on 30 ps TDR. Board
variations are a lot bigger.
Click to expand...

Makes sense; the mass of the lacquer layer can\'t be much, and multilayer boards, with glue
layers, might have more material nonuniformity over modest length scales. Fiberglass
cloth, too, can be expected to contain some weave variance.
 
On Tue, 25 Jan 2022 23:40:32 +0100, Gerhard Hoffmann <dk4xp@arcor.de>
wrote:

Am 25.01.22 um 23:08 schrieb John Larkin:
https://www.dropbox.com/s/idwz568o8hfpgzb/TDR_Solder_Mask.jpg?raw=1

The two un-masked patches are not visible on 30 ps TDR. Board
variations are a lot bigger.

I got similar results on a JLCPCB 4 layer board.
I calculated that 50 Ohms are 11.55 mil, drew it 12 mil in
Altium. Seems to fit.


https://www.flickr.com/photos/137684711@N07/51843174578/in/dateposted-public/lightbox/


The SMA launcher decal was not so good, but I was interested in the 50
Ohm line only for verifying eps-r and thickness etc.
The launchers were for a 2 layer process. The streamlined boards
for the LMX2594 are on the plane from HK. They also have cutouts
on Layer 2 and shorter SMA center pads. The unpopulated SMA is
better than the populated one. The thickness of the center pin
and the solder seem to matter.

cheers, Gerhard
Click to expand...

The quickie Chinese board houses default to super thin layer 1/2
dielectrics for some reason. If you use layer 2 as ground, that makes
your SMA pads capacitive anomalies. Even the cutout doesn\'t seem to be
enough; fringing maybe.

Your trace hit 50r pretty good.

We have one 50-ohm SMA footprint that cuts away all the inner planes
and plops a big copper square on the farside.

https://www.dropbox.com/s/hebu7yfzj9mf3lm/Rob1.jpg?raw=1

That connector has a giant center pin. The center pin in free space,
not on a board, is 100 ohms!

https://www.dropbox.com/s/a2weq43lmo1hdch/DSC01527.JPG?raw=1



--

I yam what I yam - Popeye
 
Am 26.01.22 um 04:39 schrieb jlarkin@highlandsniptechnology.com:
On Tue, 25 Jan 2022 23:40:32 +0100, Gerhard Hoffmann <dk4xp@arcor.de
wrote:

Am 25.01.22 um 23:08 schrieb John Larkin:
https://www.dropbox.com/s/idwz568o8hfpgzb/TDR_Solder_Mask.jpg?raw=1

The two un-masked patches are not visible on 30 ps TDR. Board
variations are a lot bigger.

I got similar results on a JLCPCB 4 layer board.
I calculated that 50 Ohms are 11.55 mil, drew it 12 mil in
Altium. Seems to fit.


https://www.flickr.com/photos/137684711@N07/51843174578/in/dateposted-public/lightbox/


The SMA launcher decal was not so good, but I was interested in the 50
Ohm line only for verifying eps-r and thickness etc.
The launchers were for a 2 layer process. The streamlined boards
for the LMX2594 are on the plane from HK. They also have cutouts
on Layer 2 and shorter SMA center pads. The unpopulated SMA is
better than the populated one. The thickness of the center pin
and the solder seem to matter.

cheers, Gerhard

The quickie Chinese board houses default to super thin layer 1/2
dielectrics for some reason. If you use layer 2 as ground, that makes
your SMA pads capacitive anomalies. Even the cutout doesn\'t seem to be
enough; fringing maybe.
Click to expand...


That is needed to get some signal out from under a BGA.
They also have a process for thicker lines. I think I will
test it with a UHF LDMOS power amplifier.

<
https://www.flickr.com/photos/137684711@N07/51844498620/in/dateposted-public/
>

one of the next tries. Red is top = 1, blue = 2,
yellow = 3 (not in this area) 4 = bottom = green.


Your trace hit 50r pretty good.

We have one 50-ohm SMA footprint that cuts away all the inner planes
and plops a big copper square on the farside.

https://www.dropbox.com/s/hebu7yfzj9mf3lm/Rob1.jpg?raw=1

That connector has a giant center pin. The center pin in free space,
not on a board, is 100 ohms!

https://www.dropbox.com/s/a2weq43lmo1hdch/DSC01527.JPG?raw=1
Click to expand...

Looks like the center pin on my board. I also have recovered
some SMAs from junked wafertesters; they have REALLY small
center pins and a ground tunnel / bridge with 2 hex nuts.
They might fit the 12 mil line directly. Probably a solder
problem even with the finest METCAL tip.

Probably Rosenberger.

The plane with the new boards has landed in .de in the night. :)

Cheers, Gerhard
 
On Wed, 26 Jan 2022 10:28:15 +0100, Gerhard Hoffmann <dk4xp@arcor.de>
wrote:

Am 26.01.22 um 04:39 schrieb jlarkin@highlandsniptechnology.com:
On Tue, 25 Jan 2022 23:40:32 +0100, Gerhard Hoffmann <dk4xp@arcor.de
wrote:

Am 25.01.22 um 23:08 schrieb John Larkin:
https://www.dropbox.com/s/idwz568o8hfpgzb/TDR_Solder_Mask.jpg?raw=1

The two un-masked patches are not visible on 30 ps TDR. Board
variations are a lot bigger.

I got similar results on a JLCPCB 4 layer board.
I calculated that 50 Ohms are 11.55 mil, drew it 12 mil in
Altium. Seems to fit.


https://www.flickr.com/photos/137684711@N07/51843174578/in/dateposted-public/lightbox/


The SMA launcher decal was not so good, but I was interested in the 50
Ohm line only for verifying eps-r and thickness etc.
The launchers were for a 2 layer process. The streamlined boards
for the LMX2594 are on the plane from HK. They also have cutouts
on Layer 2 and shorter SMA center pads. The unpopulated SMA is
better than the populated one. The thickness of the center pin
and the solder seem to matter.

cheers, Gerhard

The quickie Chinese board houses default to super thin layer 1/2
dielectrics for some reason. If you use layer 2 as ground, that makes
your SMA pads capacitive anomalies. Even the cutout doesn\'t seem to be
enough; fringing maybe.



That is needed to get some signal out from under a BGA.
They also have a process for thicker lines. I think I will
test it with a UHF LDMOS power amplifier.


https://www.flickr.com/photos/137684711@N07/51844498620/in/dateposted-public/


one of the next tries. Red is top = 1, blue = 2,
yellow = 3 (not in this area) 4 = bottom = green.



Your trace hit 50r pretty good.

We have one 50-ohm SMA footprint that cuts away all the inner planes
and plops a big copper square on the farside.

https://www.dropbox.com/s/hebu7yfzj9mf3lm/Rob1.jpg?raw=1

That connector has a giant center pin. The center pin in free space,
not on a board, is 100 ohms!

https://www.dropbox.com/s/a2weq43lmo1hdch/DSC01527.JPG?raw=1

Looks like the center pin on my board. I also have recovered
some SMAs from junked wafertesters; they have REALLY small
center pins and a ground tunnel / bridge with 2 hex nuts.
They might fit the 12 mil line directly. Probably a solder
problem even with the finest METCAL tip.

Probably Rosenberger.
Click to expand...

Some of the high-end connectors don\'t need solder. Substitute money.

>The plane with the new boards has landed in .de in the night. :)

New boards are always fun.

Cheers, Gerhard
Click to expand...

This is a nice part:

MUELLER BU-1420701851
DIGIKEY 314-1703-ND

We\'re paying less than $4.

A 35 mil wide trace matches the pin width, and you can bury one end of
an 0603 part in that trace without adding any pad capacitance.

There\'s room for a couple of small parts or some silk text inside the
footprint, which can be handy.



--

I yam what I yam - Popeye
 
You must log in or register to reply here.

Welcome to EDABoard.com

Sponsor

Back
Top