Criticize my first big PCB - Page 1
Forum section: electronics / projects

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 26, 2018, 01:45:19 pm
content: Hello all,Don't blame on me if you see something stupid. Below are attached the layers of a 160x114 mm PCB that I'm working now. It's a big PCB for me, since I've always worked with small projects. I'm doing this mainly for educational purposes, to get involved with SMD components, different packages, get to know some new products, learn how to draw a medium scale PCB from schematics. I don't intend to put into production, but I intend to make it real. It's about a DC motor controller for 90-130VDC motors. I have drawn the high current traces by myself (you can see some copper pours), and let the autorouter make some signals traces. The dashed line that you see is to indicate a separation between high and low power. Those ICs in the line, all of them, have isolation. They are optocouplers, isolated gate driver, isolated DC/DC converter, and galvanic isolated hall current sensor. If you strictly need deep details about the project to advice me on something more specific, let me know. I know I might be exaggerating the project idea of a DC motor controller, but don't take that into account.

author: Gribo
author_rank: Frequent Contributor
timestamp: July 26, 2018, 01:59:37 pm
content: C1 and other high side components have no thermal relief for their vias, you might want to add those, otherwise, hand soldering will be more difficult.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 26, 2018, 02:07:19 pm
content: Thank you. I'll fix that.

author: Nusa
author_rank: Super Contributor
timestamp: July 26, 2018, 03:38:44 pm
content: While not wrong, it seems weird to split the circuit touching AC1 and AC4 between top and bottom layers when there's no obvious reason to do so.Ditto for the two right pins of F1.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 26, 2018, 03:45:24 pm
content: Thanks. I will review them now. They are some of the traces that the autorouter made.

author: Phoenix
author_rank: Frequent Contributor
timestamp: July 27, 2018, 01:52:07 am
content: You might need to rearrange some tracks to improve the isolation distance. The auto-router has placed tracks between the HV and LV sides of the isolation components reducing the creepage and clearance. I'm not sure what voltages you're applying, but looks like mains... You'll want to keep the gaps between the isolation ICs clear of tracks.You can move the current measurement chip up to reduce the high power track length and loop inductance. It's OK for the isolation line to be a wonky shape.

author: qwaarjet
author_rank: Regular Contributor
timestamp: July 29, 2018, 08:12:02 am
content: The lack of thermal on some of your component is definitely a problem but most likely that would only be a real issue in mass production. without more details it hard to say if there anything fundamentally wrong.While not technically wrong these some things I would call you on if I were your lead.I see a fair bit a dead copper on your bottom layer pours generally unless there's technical reason for them being there get rid of them they just make extra EMI issuesyour polygons look sloppy since they are not at strait or at 45deg angles.There are number of acute angles in the copper. This can be an issue at higher frequency but is also not good from a mechanically as it create stress constentions. This is also non ideal from a fabricator standpoint since the exact geometry will be variable by process used. ie you don't know exactly what those angle will look like in the copper. you might want to look into teardrops.On a plus though your silk looks very good.

author: ocset
author_rank: Super Contributor
timestamp: July 29, 2018, 08:36:51 am
content: your bototm diagram shows pth and smd copmponents very close to each other........this could be nmore expensive to asseble.....they say 4-5mm needed really...have you got that?

author: tautech
author_rank: Super Contributor
timestamp: July 29, 2018, 09:45:37 am
content: The hole and annular ring sizes are all over the place.Mostly annular rings are way too thin and thereby susceptible to rework damage.Are all single diode cathodes clearly marked ?All polarized caps too ?

author: mariush
author_rank: Super Contributor
timestamp: July 29, 2018, 10:14:52 am
content: I would ...shift mov1 f2 c4 and all that a bit to the rightrotate F1 90 degrees and move it between the AC# header and those componentsrotate that big resistor R28 or whatever by 90 degrees and move it where the fuse was, but shift it a bit to the right (move TR1 and the other stuff a bit more to the right if needed) - if you want distance between TR1 and the big cap to keep it cool or whatever, you can move that cap also to the rightmove the AC# headers / terminals a bit higherrotate that big rectangle on the bottom left , relay or transformer or whatever that is , by 90 degrees and move it up enough to have the AC connections above that dashed linemaybe have those ledsconsider having that thick trace under the capacitor that's now making a 90 degree angle, a 45 degree angle... it will allow you to keep the thickness of the track throughoutthose JP1, JP2 ... J2, J3 look to me like a mess there , prone to make mistakes ... maybe try to shift the controller a bit more to the left and move at least those JP jumpers to the right? At the very least it could allow you to add some silkscreen, some legend text near them, so if you forget a few months later what those are for, you can just look on the pcbdo you have to break that big ground thing with U5 by having those traces on another layer, can't you keep them on same layer?the bridge rectifier looks like it's taking an awful lot of space on the circuit board and you have alternatives like those SIM style (4 pin in line) rectifiers, maybe you could have one of those arranged in line with the TR1 and have them both attached to one heatsink if needed ?You have big capacitors which would make your board tall, so I don't see why you'd have to resort to those big square flat rectifiers with big terminals that are harder to create on the circuit board, compared to regular through holes? Looks like if you replace that rectifier, all the board can be made with regular drills. Do you need the amperage of that rectifier?Don't see the actual schematic so that's all that jumps to me from the pictures at the moment...

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 31, 2018, 06:32:47 am
content: Thank you all for your suggetions. I have slightly modified some traces [see new attachment]. Some changes seem to be unnoticeable for you according to your recommendations. Of course, I would have to redesign almost the whole circuit to take into consideration some of the things you've said.Quote from: mariush on July 29, 2018, 10:14:52 amWow, it just made me rethink the whole design idea, but I'm glad you've pointed out valuable information. I will see what I can do, as I do not have much time to finish the project.

author: tautech
author_rank: Super Contributor
timestamp: July 31, 2018, 07:24:50 am
content: Youwilldiscover the folly of fine and thin annular rings, if not immediately on this PCB further creations you will make.Just noticed now how some of your corner mounting holes have little clearance to the traces. You need to shift traces further away if using metal fastenings.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 31, 2018, 02:25:08 pm
content: Quote from: tautech on July 31, 2018, 07:24:50 amSo do you strictly suggest to increase the annular rings in this design? I mean, the concept is new to me, that's another thing I have to learn.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 31, 2018, 02:44:29 pm
content: Quote from: qwaarjet on July 29, 2018, 08:12:02 amDo you mean removing the copper pour at the bottom side (below the dash line)?

author: tautech
author_rank: Super Contributor
timestamp: July 31, 2018, 08:01:46 pm
content: Quote from: XaviPacheco on July 31, 2018, 02:25:08 pmYou can address this issue in 3 ways.Decrease TH lead hole size as the annular ring OD will remain as before.Increase annular ring ODDo both. ( my preference)#1 and most important benefit, a more robust design thatwillwithstand rework without the risk of pads lifting.For home etched designs I reduce hole size to 20mil (0.5mm) to provide more accurate drill centering.Everywhere I can I use 100mil pads, round and square. Square is reserved for indication of polarity in my designs.Only when clearances are required do I make them smaller often by making them rectangular or oval.

author: BrianHG
author_rank: Super Contributor
timestamp: July 31, 2018, 08:36:38 pm
content: On TR1, pin 1, you have such a thigh trace. Pin 1 is usually the Gate or Base, and on pin 3 you have the thin trace, this is usually the Emitter or Source. Are you sure you have wired this device correctly?Unless TR1 is a SCR or Triac, then yes, pin 3 is the gate.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 31, 2018, 08:39:34 pm
content: Quote from: BrianHG on July 31, 2018, 08:36:38 pmSorry if I haven't used the right nomenclature. TR1 is a Triac.

author: BrianHG
author_rank: Super Contributor
timestamp: July 31, 2018, 08:41:23 pm
content: The trace on TR2, leaving pin 1 going just above pin 3 is way too close to pin 3. Give it a better centering/breathing room.

author: BrianHG
author_rank: Super Contributor
timestamp: July 31, 2018, 08:47:51 pm
content: Also, what looks like and Allegro isolated current sensor to voltage converter, you shouldn't have one of the traces going under the package as when you look at the current sensor IC's bottom/internals, there is a loop near there from the high voltage side to measure the current. You have room to draw that trace straight down from it's IC and slightly push/move the other traces close by the MCU so you may access the via down there without looping that trace under the IV sensing IC.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: July 31, 2018, 08:59:16 pm
content: Quote from: BrianHG on July 31, 2018, 08:41:23 pmGood. I will fix that.Quote from: BrianHG on July 31, 2018, 08:47:51 pmMy current sensor is the TLI4970 from Infineon. What exactly do you mean by having one of the traces going under the package?I think I've fixed that in my last attachmentEDIT: Oh, I see. I will make all the digital pins go straight down, instead of having that line under the sensor.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: August 01, 2018, 02:56:50 am
content: I have made some adjustments. See attachment. I have reconsidered some of your ideas. But not all of them. I would have to make a whole board again taking them into consideration. Of course, for future projects, I will consider all of them.Quote from: mariush on July 29, 2018, 10:14:52 amI know. But changing the rectifier, will drastically change the design. For a next project, I will use a regular through hole rectifier.What I really want for now is to be sure, at least, that my circuit will do something expected. And, if I have to change something, it would have to be something that I could easily modify. It's very time consuming for me to redraw the whole board again. I intend soon to order the PCB prototype. For a first design, it's not so good, but acceptable I think (for a student). I really appreciate all your suggestions, and they make me more mature for a next design.And indeed, I know that your suggestions are based on the layers that I have uploaded, because you haven't seen the actual schematic. So, you all are assuming that the net connections are right.I will see what else I can easily modify before ordering the PCB. It's not for production, I will just order the minimun quantity. So I don't expect something extremely cheap for now.

author: Thewafflication
author_rank: Contributor
timestamp: August 01, 2018, 09:54:44 am
content: Just a thought. May be make the trace on the top side near the hole in the bottom right corner thicker, only because it is heart breaking for a board to slip and the stud/fastener destroys the trace.

author: XaviPacheco
author_rank: Regular Contributor
timestamp: August 01, 2018, 02:08:40 pm
content: At this point, assume the net connections are okay. Would any of you redesign the whole PCB? Would you attempt to order the PCB prototype? I plan to order it in China, do you think they might have issues with this PCB? If redesigning the circuit avoids any kind of potential problem, so I don't have more options to do so.