I have a dual analog output PCBA that I am routing. The analog output component selected is two TI DAC7750IRHAR DACs.

These DACs are controlled via SPI lines. I had originally intended to place both of those on the same layer and route the control signals between them and the controller, but due to space constraints, nearby connectors, etc., I found it quite advantageous from a routing standpoint if I had these two components on opposite sides of the board and placed directly on top of each other.

However, the recommended footprint shown at the end of the datasheet includes thru-vias in the thermal ground pad that are intended to help with heat dissipation.

I haven't yet determined if my circuit will require the extra heat sinking (TI's documentation suggests that it's optional), but this does bring up the question about the feasibility of placing the components like this. Will the thru-vias in the thermal pad cause assembly problems? I'd prefer to avoid having to tent or plug them.

I'm not concerned about the vias from each footprint "interfering" with each other. I have placed them directly on top of each other, so they all line up perfectly. I could also change the footprints so that only one of them has the vias, or so that each only defines half the vias and they don't interfere. I'm only concerned with how the vias showing up in the ground pads will affect assembly.

  • \$\begingroup\$ This really comes down "how is the board assembly cooled"? Is your thermal path DAC->PCB->air? Or is it something else? \$\endgroup\$
    – SteveSh
    Nov 28, 2023 at 15:24

2 Answers 2


Not experienced as a PCB assembler, but as a designer I wouldn't expect having the unplugged/untented vias would be any worse from an assembly perspective with the components directly opposite each other when compared to having a single component on one side with thermal thru vias. In either case, solder will want to go down the plated thru holes.

From a design perspective, I would be concerned about the amount of heat concentrated in that area if the thermal vias are serving two chips. Are you able to estimate how much heat those DACs will be dissipating?

Ultimately, it is a question for your PCB assembler, the sooner you ask them, the sooner they can identify if this and other things on your board are issues.

  • \$\begingroup\$ I'm still working on estimating the heat dissipated by the chips. I certainly agree with your 1st paragraph, that the first chip assembled is no different. I guess I'd wonder if solder might already be present on the 2nd pad when running the other side of the board, and if that would matter. I'll ask my fab house, thank you. \$\endgroup\$
    – rothloup
    Sep 3, 2023 at 19:31
  • \$\begingroup\$ I've estimated that worst case, each chip will dissipate about 1W. Based on the datasheet, I should get about a 35 C rise on the die using only junction-to-ambient dissipation. I would expect the thermal vias to only make it better. They will both have ample area nearby of open ground pours, both on the internal plane and on at least one surface layer, so I think it'll be ok. I put thermal vias around the packages as well to help pull heat out of the internal ground plane and onto the surface. \$\endgroup\$
    – rothloup
    Sep 4, 2023 at 3:11
  • 1
    \$\begingroup\$ @rothloup Ah interesting point on solder from the first reflow travelling to the other side of the board. I suspect it wouldn't be a big issue, but might depend on the how much solder paste is applied; you may be able to reduce the openings in the paste mask to help with that but yeah the assembler will know better than me. That sounds okay with regards to heat, so long as your worst case ambient temperature is low enough to allow for a 35C rise \$\endgroup\$
    – jramsay42
    Sep 4, 2023 at 8:00

Concerning heat dissipation, I would avoid this because both components will be directly "linked" through the vias and will heat each other up without much chance of the heat dissipating into the PCB.

If you decide that the heat dissipation is not a problem and if you stick with the idea, there is a design choice which will greatly influence the manufacturability of the product.

You can choose to simply add vias to the pad, or you can have the via filled and capped. Check out IPC 4761. They describe different types of via filling, capping and plating. Specifically, in your case, it would be IPC 4761 Type VII (Filled and Capped Via).

If you have the components on opposite sides of the PCB in the same location and if you chose to go with a simple via, this will negatively impact the manufacturability:

  • Depending on which side is soldered first, the solder of the ground pad will be pulled into the via through gravity, surface tension and capillary action. You will see that some of the solder actually forms on the bottom pad. How strong this effect is depends on the paste used, soldering temperatures, ambient temperatures in the factory, drill hole size and surface finish of the PCB. The effect of this is very difficult to predict and thus challenging to control.

  • When you solder the second side (previously bottom) you now have to account for the solder that has already wetted the pad. Theoretically, since this is the same component, the assembler would have to reduce the paste amount compared to the first component because some of the solder is already present.

In summary, you have to see if you will face thermal issues from a technical perspective. If that is not the case, you should then choose IPC 4761 Type VII (Filled and Capped Via) which will slightly increase the cost of the bare PCB but will make the assembly of this critical component more consistent and reliable.


Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.