Platform forum

Opinion about 10 layer board

manishbuttan , 09-03-2015, 10:07 AM
Hi Robert,
I wanted your opinion on this stackup. We have followed your video for the 10 layer stackup, but the PCB manufacturer is saying it will be difficult to manufacture for the SODIMM 200 connector at 1mm. We have kept the same layers as you have specified for 10 layer board

Would appreciate it if you can let us know if we are doing something wrong. Thank you for your help.

(Attachment sent to you by e-mail).
robertferanec , 09-03-2015, 10:34 AM
@manishbuttan this may help you. This is one of our stackups we used for some 10 layer SODIMM projects:

manishbuttan , 09-03-2015, 07:46 PM
Hi Robert, this is the feedback from the PCB Manufacturer. Please let me know if 8 layer board should be used instead? or should I ask him to continue with the 10 layer build?

As the thickness is critical (due to the PFA SODIMM Connector datasheet)
We suggest to reduce the number of layers to 8 layers if possible.

We have made a similar product. The yield is low for such critical design and most of offshore companies will decline to manufacture this job as it is. Therefore, we suggest to review the design by reducing the number of layers if you have to use PFA SODIMM Connector.

For us, it is not a problem to manufacture prototypes as it is but it would be really expensive as the yield is low.
robertferanec , 09-04-2015, 12:23 AM
The projects where we used the 10 layer stackup which I attached above have been manufactured in 10 000+ pcs, no problem. Did you check with your PCB manufacturer the stackup which I suggested? I don't know what connector you exactly use, but I believe for SODIMM, the PCB thickness is 1mm - can you confirm that?
manishbuttan , 09-04-2015, 02:08 AM
This is the same stackup we have used. I have also forwarded this link to Exception PCB Solutions. Can you confirm that you used them for the 10K + pcs without any problem? I am trying to understand why you had no problem and why we are being told that it would be difficult to manufacture? Yes, the SODIMM connector is 1mm.
robertferanec , 09-04-2015, 02:16 AM
Please, could you take screenshot of your stackup and place it here? Thank you.
manishbuttan , 09-04-2015, 03:48 AM
These are the details:

PCB Description : 10 layer board
L1 – Signal
L2 – GND
L3 – Signal
L4 – Power Plane
L5 – Power / Mixed
L6 – Power / Mixed
L7 – GND Plane
L8 – Signal
L9 – GND
L10 – Signal

-- Required impedances:

Single ended: 50 OHMs (L1 ,L3(Ref: L2); L8(Ref: L7,L9); L10 (Ref: L9) )
Differential: 100 OHMs (L1,L3 (Ref: L2); L8(Ref: L7,L9); L10 (Ref: L9) )

– Used VIAs:

Through hole VIA: 0.45mm (pad) / 0.2mm (drill), Start layer: L1, End layer: L10

Start layer: L1, End layer: L2; 0.3mm (pad) / 0.15mm Start layer: L3, End layer: L2; 0.3mm (pad) / 0.15mm Start layer: L8, End layer: L9; 0.3mm (pad) / 0.15mm Start layer: L10, End layer: L9; 0.3mm (pad) / 0.15mm

Buried VIA:
Start Layer: L3, End layer: L8; 0.45mm (pad) / 0.2mm (drill)
manishbuttan , 09-04-2015, 03:49 AM
This is the response from Exception PCB:

On Robert stack up, he has not got 1oz copper weight on layers 4 and 7.
He is using 76um cores instead 50um cores on our build.
He is using different prepregs pressed thickness to ours.

Saying that, I would appreciate if Robert can advise you what was the yield of this part?

We have made SODIMM part for different customers but with different stack up structures.

As I said, we can manufacture the proposed build but it is not the most cost effective option.
manishbuttan , 09-04-2015, 03:57 AM
And then they recommended that we should use 8 layer instead, as it will be more cost effective and easier to do for SODIMM 200. The problem with this is that we will need to re-do the entire layout again, which I want to avoid. These are the notes:

This build would more cost effective comparing to the 10 later build. Also, you will not find issues to find offshore suppliers for volume production.

Please let me know if that is feasible for you to layout the job with 8 layers instead of 10 layers.

robertferanec , 09-04-2015, 04:08 AM
@manishbuttan it's your choice. Of course 10 layer PCB will be harder to make within 1mm than 8 layer PCB

If I was you, I would ask them for their 10 layer / 1mm stackup suggestion, but do not forget to check impedances.
manishbuttan , 09-04-2015, 04:12 AM
This is their 10 layer Stackup. Do you recommend we move forward with this?
robertferanec , 09-04-2015, 04:33 AM
I would play with it. For example:
- If I have a signal layer inside PCB, I personally prefer to have Solid GND plane closer to this signal layer, rather than the other plane (in your case, distance between L2-L3 is bigger than distance between L3-L4). It is just my opinion. I am not saying you have to use it this way.
- The dielectricum 51um - wow, that really is quite thin, but maybe it's not really possible to do much about it and also maybe it would not have big influence on the design.
- The 100 OHM impedance geometry "75/250", that 250 is a quite high number, it may be difficult to route signals around this differential pair (ideally I always try to keep clearance around diff pair signals bigger than the gap between them).
manishbuttan , 09-04-2015, 05:27 AM
Hi Robert, this is the feedback on your comment -
I agree with his comments and make sense. However, we don’t have much room in your case in order to consider Robert’s comments in our proposed build.
As Robert said, I am forced to use 50um cores which are not the ideal knowing they affect yield during production (handling issues).

The 75/250um are the consequence of the dielectric separation 2-3 and 3-4: I have to either reduce the track width (75um is already very thin) or increase the gap (250um is already very large). I cannot meet 100ohms if I reduce 2-3 to 74um, and I cannot increase the dielectric between 3-4 as I have exceeded the overall thickness limit.

Can you deal with 0.5oz (17um) copper weight on layers 4 and 7 instead of 1oz (35um)? This will allow me to increase the dielectric separation between 3-4 and 7-8.

We are using 35um on ground and Power Planes since most designs we have seen have this settings. The board runs at 5V and 2Amps. Do you feel that 17um would work? Is there a calculator we can use to confirm this?

robertferanec , 09-04-2015, 06:10 AM
I am sure you can handle this
Use our interactive Discord forum to reply or ask new questions.
Discord invite
Discord forum link (after invitation)

Didn't find what you were looking for?