My second ever PCB on Altium. Have a couple questions - Page 1
Forum section: electronics / beginners

author: ExtensionShoe
author_rank: Contributor
timestamp: February 03, 2021, 11:37:10 am
content: Hi so I got my hands on an Altium Designer 21 license. It is legitimate do not worry. I am a student currently and since I'm on a break right now I thought I would mess around with PCB design.So this is the second ever PCB I've ever designed and I have posted the first one here for feedback:https://www.eevblog.com/forum/beginners/my-first-experience-in-pcb-design/This is a simple overcurrent protector with a 0.1 ohm shunt power resistor.The first picture I've attached shows the schematic I've drawn. I made sure to make GND point down and VCC point up. Is there anything you see that are against common design practices.The second picture I've attached shows the PCB design. Here are my questions:1)So I needed to shrink down the silkscreen to meet the design rules. The default height of the silkscreen was 60 mils but I needed to drop it down to 30 mils. Is this OK or is this not recommended?2)Inside the green circle you can see I have put the silkscreen inside the resistor shape, since I could not fit them anywhere, while other components designators are placed outside. Is this acceptable in a professional PCB design?3)Inside the blue circle you can see the long traces from the normally closed switch. Is it bad practice to use long traces that pass through multiple components?4)Inside the purple circle I'm using LM358. You can see that there are tons of traces going all over the place. Some of them are again really long. Is there anything you can spot that can cause problems?I am also attaching an image of the PCB without the circles so you can see it better.Thank you so much.

author: mvs
author_rank: Frequent Contributor
timestamp: February 03, 2021, 12:36:08 pm
content: 1) No reason to do that, you have plenty of space on the board.2) It is not recommended, as you can not see designator after part is installed. You can place designators of this resistors on the right.3) You need to consider speed of your circuit. Buttons are usually low speed and are not so important.4) Opamp feedback usually needs to be short, low stray inductance, low stray capacity. Remove also unconnected ground plane islands.If your board is single layer, you should place through-hole components and silkscreen on one side (usually top layer), traces on the other (usually bottom layer, blue in altium).Your traces are quite thin for TH design. There might be a mechanical issue, if board is low cost / without hole plating.No decoupling on opamp, etc.If you have time, you can try to rearrange components and see if routing gets better.---Input stage of LM358 does not work near V+ rail, so you might lower gain of your differential amp to get it working as high side CSA. Vcc*R3/(R1+R3) should be larger then 1.5V + Vout.If your Vcc is 12V, then set gain to 5 or lower.You can also change logic a bit to save one BJT stage and use NO buttons, since they are more common.

author: E-Design
author_rank: Regular Contributor
timestamp: February 03, 2021, 01:02:43 pm
content: Ditto what was said above.. make sure opamp input nodes are small.. this is usually done by placing your resistors closer to the opamp.Also, if I am understanding your intention (actuate a relay based on a pot setting for a current limit) check that U1 connections.. looks like + and - are not right and it has no negative feedback.You can simulate this circuit - try it in a simulator. Its a good way to find problems right away before you spend the time to build it.

author: tautech
author_rank: Super Contributor
timestamp: February 04, 2021, 07:11:22 am
content: CommentsLooks like the autorouter did this......have they not improved significantly to Summer 09 I use ?I'm giving the autorouter a Gawd awful mark for trace routing.Why ? All the room in the world to run traces and it runs them hard against others or with minimal clearance to pads on other nets.You can turn off displaying the IC power pins in schematics as Altium knows what they are and will connect them to the power nets.Zero bulk or decoupling capacitance on any PCB with active components is never a good idea, you need add some. 100uf for bulk and 0.1uf for decoupling.

author: ExtensionShoe
author_rank: Contributor
timestamp: February 04, 2021, 10:35:56 am
content: I routed it myselfAnyway I will add decoupling caps thank you

author: tautech
author_rank: Super Contributor
timestamp: February 04, 2021, 10:42:48 pm
content: Quote from: ExtensionShoe on February 04, 2021, 10:35:56 amOK some tips to make your life easier.Resist the temptation to run tracks the shortest path so to not run them too close to pads on another net.If a track connects to several pads run it the best route from first to last pad and branch off it at 90% to connect to the remaining pads.Don't stick too rigidly to a component orientation scheme where for example if both Q1&2 were flipped 180 routing would be simpler and tidier.Keep a close eye on hole sizes particularly on pads with small annular rings as if the hole size is overly large the annular ring is susceptible to lifting when performing rework. In the same vain set yourself a minimum size annular ring (I use 100 mil) and if routing is tight be prepared to change their width/height to oval to allow a track to pass between adjacent pads.....a bit like the pads on Q1&2 but wider apart.Consider adding test points if/where necessary especially when you have only ordinary scope probes to use. If you have some tiny grabbers then ensure component layout is such that you can get them onto all devices as needed.Always, always do a PCB layout with ease of rework in mind.Have fun and study commercially made PCB's for tips on how the pros do layouts and never forget you have one of the best tools in the business for PCB layouts.Learning to use the full power of Altium is the hard part.