4 layer daughter board on top of 2 layer board - Page 1
Forum section: electronics / beginners

author: newtekuser
author_rank: Frequent Contributor
timestamp: January 28, 2024, 07:42:30 pm
content: Since I'm too lazy to change my 2 layer PCB into a 4 layer PCB in order to integrate a DRV8825 motor driver and its passive components, I am planning to design a 4 layer PCB and connect it to the main 2 layer PCB via pin headers. (i.e.: DIR, STEP, 12v and GND pins connected to the main board). My main PCB does not need to be a 4 layer PCB and this should keep manufacturing costs down and save me time.Is this an acceptable practice? Are there any performance considerations? I do not need to certify the board to comply with any standards.

author: MarkT
author_rank: Frequent Contributor
timestamp: January 28, 2024, 07:56:39 pm
content: Have you considered a 2-layer layout for the DRV8825 - it ought to be OK.

author: JustMeHere
author_rank: Frequent Contributor
timestamp: January 28, 2024, 08:09:52 pm
content: Just do a full redesign. 4 layer boards are easier to layout. You can improve your original design.

author: newtekuser
author_rank: Frequent Contributor
timestamp: January 29, 2024, 01:57:20 am
content: Ideally I'd like to keep my project to 2 layer, but the placement of components and traces for the DRV8825 IC is an impediment, even if most are 0402s. I would like to avoid using zero ohm resistors.I have circled the problematic area in the attachment, especially traces to the pins that go to the motor will be crossing each other. I can't see any way to rotate components to make room for the traces which are also pretty wide at 0.409mm as they need to carry up to 1.2A.

author: MarkT
author_rank: Frequent Contributor
timestamp: January 29, 2024, 03:40:10 pm
content: Fan them out like wedges from the pins for more current handling (and chip cooling)?There's a 2-layer layout example, figure 11.2 in the datasheet. Its takes the four winding traces through to the other side using multiple vias close to the chip.

author: wraper
author_rank: Unknown
timestamp: January 29, 2024, 03:49:08 pm
content: Quote from: JustMeHere on January 28, 2024, 08:09:52 pmI find it absolutely wasteful approach. Define "improve". If it works the same and complies to regulations, what's the improvement? As of DRV8825, I would not even consider 4 layers for those, you could use them on a single layer with a few jumpers FWIW.

author: wraper
author_rank: Unknown
timestamp: January 29, 2024, 03:54:49 pm
content: Quote from: newtekuser on January 29, 2024, 01:57:20 amI frankly see no issues there whatsoever. Put motor out traces on the top layer and connect everything else to GND plane and VM power rail on opposite side. Or move output traces to bottom side instead. Also you can run a few traces under IC. They even give you a layout in the datasheet.

author: newtekuser
author_rank: Frequent Contributor
timestamp: January 29, 2024, 05:07:05 pm
content: Thanks all for the suggestions!I see in the layout example the output traces have two VIAs each going to the bottom. Why 2?Also both traces from the Rsense resistors use a group of 8 VIAs to go to the bottom. Why that many VIAs for Rsense and not for Vout?Is that because the power dissipated is that much higher from Rsense resistors? In my design these resistors have very small values (i.e.: 92 mOhms)

author: sparkydog
author_rank: Regular Contributor
timestamp: January 29, 2024, 06:23:09 pm
content: Quote from: JustMeHere on January 28, 2024, 08:09:52 pmAside from the OP mentioning cost concerns (and, no, 4-layer boardsaren'tnecessarily the same price as 2-layer boards), I've actually had at least one design — that started as a well laid-out 2-layer design, mind — that I tried to redo as 4-layer and gave up because it was turning into an utter mess. Ialsohave a 4-layer board that would be impossible to do as a 2-layer board. YMMV, but in my experience such blanket statements aren't as universally true as they're typically asserted to be.

author: Siwastaja
author_rank: Super Contributor
timestamp: January 29, 2024, 06:30:59 pm
content: Two-board design, one of which is 4-layer board, is almost certainly more expensive than just making the sole board 2-layer. By going 4-layer, you don't have to change much anything of the original 2-layer design. This being said, I'd agree with wraper; gazillion of stepper controllers have been made on two layers. Just dedicate bottom layer for ground, which means you probably have to use a few jumpers, not a big deal. Remember local bypass caps and tight layout, but that is important on 4 layers too.

author: Smokey
author_rank: Super Contributor
timestamp: January 29, 2024, 08:00:02 pm
content: Quote from: newtekuser on January 29, 2024, 05:07:05 pmVia current calculator:https://www.protoexpress.com/customer-portal/vccw-cal/Reasons for multiple vias:1) Current capacity. Typically around 2A/via, but run the numbers for your board through the calculator.2) Redundancy. Vias have less plating than the rest of the board. Can sometimes be uneven. If thermal expansion is an issue, it could crack a via in a way that's hard to detect.3) Thermal conduction. More vias can do a better job of thermally coupling the heat source on top to the heatsink plane/pour on the other layers.4) Inductance. More vias = less inductance. Also lower resistance.

author: Smokey
author_rank: Super Contributor
timestamp: January 29, 2024, 08:09:20 pm
content: On the question of 2 layer vs 4 layer, I used to always try to cram a design into 2 layers whenever possible, but I don't really do that much anymore considering the price of 4 layer boards has come down so much.6 layer is the new 4 layer!This design actually potentially has two of the main reasons I would use at least a 4 layer board from the start:1) Thermal considerations. 4 layers let you have much better thermal heatsinking when there are parts generating lots of heat. Both the internal ground plane and big top/bottom heatsink pours will be much more effective than a broken up 2 layer design.2) High current switching power elements. Creating a low noise design with two phases of a stepper driver switching 2.5A on 24V at 30kHz without a ground plane would be tough. If it's for a hobby project then 2 layers would be fine since you don't really care about EMI. If you need to get it tested to sell to people, then that might be rough without a ground plane under all that high current switching.

author: mawyatt
author_rank: Super Contributor
timestamp: January 29, 2024, 11:22:58 pm
content: Quote from: newtekuser on January 28, 2024, 07:42:30 pmBeware of the TI DRV Stepper type controllers, we evaluated these long ago and selected the Trinamic (now ADI) types. Our application was ultra-precision use with 400 step motors operating in micro-steps driving THK 1mm pitch linear rails for sub-micron positioning. Back then the TI DRV had a horrible transfer function, you can probably find something on line, recall a video showing such on Hack.... Also found out a Toshiba controller (can't recall the part number) had a significant dead zone in the transfer function.Anyway, we went with the Trinamic types and they worked superbly, once you went thru all the features and documentation (Trinamic CS was no help), and figured out how to set them up properly.BTW they offer various controllers on small plug in PCBs BOBs, check here.https://www.digikey.com/en/product-highlight/t/trinamic/bob-breakout-boardsBest,

author: newtekuser
author_rank: Frequent Contributor
timestamp: January 29, 2024, 11:31:59 pm
content: I managed to route all traces and only use one zero ohm resistor, but DRC fails due to clearance violation due to one of the traces I've routed under the IC. The 12V traces (i.e.: VMA/VMB) sit at width of ~0.387mm to handle the 1.2A load of the motor.

author: newtekuser
author_rank: Frequent Contributor
timestamp: January 29, 2024, 11:54:10 pm
content: Quote from: newtekuser on January 29, 2024, 11:31:59 pmActually it's not that, but not sure what it's referring to, clearing within itself?

author: mawyatt
author_rank: Super Contributor
timestamp: January 30, 2024, 02:18:09 pm
content: Quote from: mawyatt on January 29, 2024, 11:22:58 pmGot an inquiry and recommended this:At $13 for a complete PCB with 2.8A 36V stepper controller/driver, some folks might find useful. We've used the TMC5160 for some larger steppers in the past, they worked very well indeedhttps://www.digikey.com/en/products/detail/analog-devices-inc-maxim-integrated/TMC5160SILENTSTEPSTICK/9990281Best,