Questions from Learn Altium Essentials Second Edition

[Jetstream4]

Hi everyone,

My first post here. I have recently completed Learn Altium Essentials Second Edition course and I have the following questions. I have tried re-watching the videos multiple times but I missed the explanation for the following. I would appreciate if someone can clarify these questions.

1. Logic behind using ground planes - How many should be used and where they should be used.

2. Why are certain signals routed in Layer 3 in the course - Is there any requirement/good practice? How would I know which signals should be routed in layer 3 (i.e. not on top/bottom layers). Did Robert carefully choose not to route the signals he routed in layer 3 in the beginning of the layout, so that he can route them in layer 3 later or did he randomly route the signals until that point and then decided to route the remaining signals in layer 3

3. How does a layer get attached to a net - If no vias are placed in the PCB? (In the course we assign GND net to layer 2 and layer 5 before any VIAs are placed in the PCB. Does this connection happen through the pads we already have on the PWA. How will this connection happen if we don't have any pads or vias on the PCB?)

Thanks,
Siva.

[qdrives]

To answer question 1: https://www.ninedotconnects.com/vide...c-board-design

[robertferanec]

1. In ideal world, you may want to have GND planes above and below each signal layer. Also in ideal world you may want to have GND plane close under components (the second layer and before the last layers). Also you may want to have GND planes as neighbor layers around power planes.

The question is not how many, but why we need them. Solid GND planes help fields do not spread all over the board or escaping board. I recommend to watch some of my videos about how signal travels and how power is delivered. It will help you to understand what GND planes do in PCB.

Of course, we don't live in ideal world and you will need to make compromises e.g. often you may be able only use one solid GND plane - in this case place it close to the signal layer.

2. It's related to my answer at point 1. We placed the noisy signals inside of the PCB so we can control how the fields will travel. This means, we make the board less noisy

3. you connect the layers via through hole pads and vias.

[katepalmes]

Ground planes are crucial for providing a solid reference point for your signals and helping manage electromagnetic interference. Typically, you'd want to have at least one solid ground plane (like a bottom layer) and possibly a power plane (like a top layer) if you're using a multilayer board. The ground planes should be strategically placed to ensure good return paths for your signals and reduce noise. It's often recommended to have a continuous ground plane on the layer adjacent to your signal layers. Navigating the realm of business communication can be a complex dance, and that's where business writing services like no other come into play. These services are more than wordsmiths; they're architects of impactful communication. As a business professional striving for clarity and influence, I've found these services to be a compass guiding me through intricate strategies and persuasive pitches. Their knack for transforming ideas into polished narratives is a testament to their expertise. Here's to the business writing services that elevate our communication game and empower us to thrive in the competitive world of commerce.

[gyuunyuu1989]

The capacitor that goes onto the LDO pin was chosen to be a "Low ESL" feature capacitor but the ones before it. Why is that so?

The capacitor that goes to the SMPS output pin is specified (in datasheet example) as having ESR of 4mohm. Isn't this just the minimum value ESR and one can use this or larger value. Or does one need to use this specific value?

The ISL6236EVAL2 BOM lists some manufacturers as "GENERIC". What does this really mean?

During creation of the 200k resistor, there are features that contain terms "AEC-Q200" "High Voltage" "Moisture Resistant". What do these really mean?

The datasheet example schematic for ISL6236A only gives the part number for a single component on the page itself. This is the transistor SI4816BDY. Why did they mention the part number itself while this was not done for the inductor?

[gyuunyuu1989]

I have finished lesson 1 of the Learn Altium Essentials Second Edition. The lesson 2 is still locked. Why is this so?

[robertferanec]

Maybe you signed up for Online version? You can double check if you send an email to [email protected] then Marcela or Dominik will check your account and help you.

[qdrives]

The ESR of the capacitor highly depends on the regulator. There are some regulators that cannot have a low ESR, there are some that require a low ESR.
If the ESR on the output capacitor is low, it can more easily supply transient currents.

Often, it does not matter which manufacturer make the resistor, capacitor or inductor as the differences between them are not important for the design.
Take a 4.7k pull-up resistor - if it has a tolerance of 10% it is no problem.
If it is used for a precision measurement and needs to be 0.1%, does it matter who makes it? Probably not.

AEC-Q200 is an automotive quality system. One could argue that they are a bit more reliable.
High voltage - guessing here as I never needed one (that I know of), but consider how resistors are made. This could be a film that is laser trimmed. "High voltage" could mean that that trimming would not cause a problem with higher voltages.
Moisture resistance - again a guess that the resistor is less hygroscopic, which could alter the resistance.

For FETs there are a lot of parameters that can influence the result. Naturally, that is also true for other parts, but in this case the FETs are driven by the controller. For most other components the specifications are not so strict, or, in the case of the inductor, are less of a concern to Renesas. However, do not forget "politics" here.

[gyuunyuu1989]

Thanks qdrives.

When the resistor says high voltage, the confusion is that high voltage means high current. This means high power dissipation. But SMT resistors are only rated for very low power. So what significance does "high voltage" have? Does high voltage mean millions of volts or hundreds of volts?

Is there ever any need to use other than 100 mil grid during the schematic creation? During schematic symbol creation, Robert used all grid sizes during creation of the symbol graphics using the line tool.

For IC schematic symbol, should vertical spacing between pins be 100 mil or 200 mil? Robert created the SMPS IC to have 200 mil spaced pins in the schematic symbol.

From the course it seems that the schematic symbol comment field is set during component creation and then it never changes in the schematic. Is this correct or there are exceptions?

Sometimes we show things other than component value in the comment field e.g MLCC voltage rating, inductor DC resistance, resistor power rating. At other times the comment field will only mention the component value and nothing else. Why is this so?

What does "soft termination" mean for MLCC?

Finally; Robert did not go into why we are using certain type of resistor or capacitor. I am referring to the material. We are using mostly ceramic capacitors and then some tantalum I believe. The resistors I believe are thick film resistors. On digikey I come across these options under composition: Carbon Composition, Carbon Film Ceramic, Metal Element, Metal Film, Metal Foil, Thick Film, Thin Film Wirewound. How does one know which material resistor to use?

[qdrives]

High voltage resistors

Lets do a search on Digikey for high voltage resistors... So all that are high voltage in the feature, lets limit to 0603 types.
The first 3 resistors in the list were 25M, 100M and 50M ohm. That is Mega ohm. With 100V and the 100M the resistor only dissipates 10mW. So power wise, no problem.
Now the 4th on the list is a 1k resistor. There 100V would give you a power issue (10W!)

I can tell you that the 350V limiting element voltage is twice what most other resistors have.
Now you may ask "But if the voltage cannot be across it because of the power limit?" True, for 1k power would be the limit. However, this family resistors can also be 10M. So, 100mW, the rated power. Now do a short time overload, that is only possible with a higher voltage.

If we look at the datasheet of the first in the list, we see the resistive element of the resistor.
Notice the zig-zag pattern? If a spark would jump, how much would it 'cross' the resistor? If this pattern would be 90 rotated, it would almost completely skip the resistive element.

High voltage is also to prevent sparks from crossing the resistor. It should go through it, not across it.

Grid
For drawing the schematic in general there is no need to have anything other than 100mil grid. Especially for placing symbols, you want them on 100mil grid.
When designing the symbol, there are reasons, like adding the 'curls' for schottky or zener diodes. Or details in FETs, bipolar transistors, etc.
Pins should always be on the 100mil grid.


As you may have noticed I did not make it hard on the schematic. However, for esthetic reasons I have some text (like designator) on a 50mil grid in the symbol.
Altium has a bug that if you move that text, even an undo does not restore it to the original position, but on the grid.
At such times I set the grid to 50mil to restore the text to the correct position.

100mil vs 200mil
There are times when it is convenient if the pins are 200mil or more apart. 100mil is for MCU, CPU, etc., but for (SMPS) regulators or other drivers, 200mils may create a more clean schematic.
Take the next bit of schematic.

Here the pins are either 200mil or even 400mil apart. This reduces the number of direction changes the lines in the schematic need to make.
Take a look at pin 2 and 3 going to R1003 and R1005.
If the schematic would be more clean and you have the space, go for 200mil.

Symbol comment change in schematic
In part that is a personal preference. I too set the comment when I create the symbol and do not change it in the schematic.
There are 2 parameters that I change in the schematic (2 that I can think of):
1) Label - used for connectors to state what is connected to it (ie. power in, motor, programming, etc.) These are created in the library with a "?" and changed on the schematic.
2) Remarks - For special remarks like gluing the component after assembly or a resistor that needs to be mounted off board (raised) due to the heat it produces.
But I do not have any exception on the comment field.

Symbol comment change in schematic
Again that is a personal preference. I still vary a bit with the comment field. Mostly because I have no real use for it.
But for resistors I have i.e. "Res 0402 10E"


Soft termination
When a board flexes, stresses are exerted on the components. With capacitors they have a tendency to create a short when it goes bad in if flexed to far.
With soft termination that the capacitor should be beter able to withstand such stresses, or at least, not cause a short.

Material
Thick film resistors are the cheapest. Wire wound have more inductance (often problematic) but higher power(?) and metal film are often more accurate. And we (or should I say others) could go on with all the pro's and con's of the various resistor elements.

For capacitors there is the ESR, ESL, safety, DC and AC bias, aging, humidity, temperature stability, accuracy next to capacity, voltage rating, price and availability.
I use 3 types of capacitors:
- Hybrid Aluminum - Polymer Capacitors -- for the bulk capacitance.
- X7R/X7S -- for the medium high capacity (HAS DC+AC bias, aging ~3%/decade hour and temperature offset ~15%)
- NP0 -- for timing, low capacitance or where I do not want DC bias effect.

[gyuunyuu1989]

thanks qdrives,

With this topic of reflow soldering and wave soldering that has been mentioned in lesson 3. I can see that both are done by machines in factory setting. One thing I am confused about is, are both applicable to SMT and Through Hole components or wavesoldering is only used with through hole and reflow is only used with SMT? Also, is there a tendancy to apply some sort of glue under components when PCB goes into machine upside down so the components do not fall off due to gravity?

[qdrives]

Better start a new thread in the future.

Wave soldering can be applied for both SMD and through hole components. However, there are limitations to SMD like pin pitch and orientation. So resistor, capacitors and SOT23 are no problem.
From experience, do not try a SC88 package with lead free -- you get about 10% shorts.

For through hole there is also the PiP or THR, Pin-in-Paste and Through Hole Reflow are techniques that solder TH using paste in the reflow over. This is mainly used for connectors so that there is a single soldering action (thermal stress).

If you do SMD and wave soldering the components need to be glued.
When doing two sided reflow, it often is not necessary.
In all my cases the assembly contractor wants to control the gluing of the components (or not).

[gyuunyuu1989]

Thanks qdrives.

I have reached lesson 3 already.

I have found that while Robert is creating a unique schematic symbol for each specific part, it is possible to assign multiple footprints to a single schematic symbol in Altium. Robert has not used thie feature though. A single part number from manufacturer defines a specific component which also includes its package. What does it mean when Altium designer makes it possible for a user to add multiple PCB footprints for the same component? It does not make sense at all.

The Altium PCB Footprint Wizard contains a list for which it guides the user through a step-by-step process culminating in a PCB footprint. This wizard shows options (among others) for capacitor, resistor and diode. All three of these are two terminal components with almost the same type of footprint (only silkscreen might differ to show polarization). What is the point of having different options for capacitor, resistor and diode footprints and then not even mention inductor? This is also a strange observation.

Robert created the PCB footprint for the ISL6236A IC. He changed the solder mask expansion to 2mil. I can see that this makes the gaps between the solder mask cut-out larger and this will make it easier to manufacture the board. But, where did he get the 2mil value from? Some datasheeet or IPC standard or just personel preference?

[qdrives]

I have assign multiple footprint to a symbol in past. One was for reflow soldering and another for wave soldering.
Components need bigger pads when wave soldering then for reflow.
Naturally it is possible to use the large wave solder pads also for reflow, but then the component can be soldered at an angle and it just does not look nice.

I create different footprints for resistors and capacitors too.
1) The height of the components are different. The height is a footprint parameter and may change the size of the pads.
2) I use a different 3D model
3) Even use a different color for C0G compared to X7R capacitors as in reality this is often the case too.

0402 resistor, 0603 X7R cap, 0402 res, 0603 res, 0402 C0G cap, 0402 X7R cap, 0805 cap.

You PCB fabricator should be able to tell you what the limits are.
Take this one: https://www.eurocircuits.com/pcb-des...es/soldermask/
For green LDI soldermask, the minimum expansion can be as low as 0.03mm
However, some fabricators (perhaps even most), kind of ignore the soldermask expansion you provide and just set their own.
The only time I can think of when this would be a problem is when you have SMD (here Solder Mask Defined) pads. They have a negative expansion.
Also, normally you do not set the soldermask expansion in the footprint, but let the board design rules dictate it. That way you can easily change for a different fabricator or technology.

[gyuunyuu1989]

I had missed the fact that height is also an important factor for the pad size.

Robert used a single document which listed the footprint details for different packages of resistors and capacitors. The size list was split into two parts, wave soldering pad dimensions and reflow soldering pad dimensions.

This document did not take into consideration the height of the component. It just said for 0805 package use this pad size and for 1206 package use this other pad size. Won't the same package size (e.g 1206, 0805 e.t.c) chip resistors and capacitors, have the same height?

[gyuunyuu1989]

I have progressed to the part where Robert created the last footprint required for PCB creation, in the lesson 3.

Robert did not create and use any "testpoints" although this would be considered highly important. Why is this so?

Robert did not create any mounting holes. The holes that have been created are solely to make connections I believe. Why is this so?

Although Robert marked components with large NF in red, I believe there is a built in method in Altium to specify what PCB variant to create. Robert did not teach this in the lesson series so far. Is this topic covered?

For the tantalum capacitor T530X337M010ATE004, the document T2076_T52X-530 contains footprint information for Density Levels A, B and C. Woudn't any designer just go for the smallest footprint (level C) since a Level C footprint could be used in all cases but a level A footprint cannot be used in levels B and C?