This is my first board, so the question may seem very simple, there may be very similar followups which I will handle by replying to anyone kind enough to help.
I have created a schematic, which I am looking to use SMB components on, with a couple of through hole components for jumpers etc. I am looking for guidance on selecting the right type of capacitors footprint for my schema. I don’t want tiny tiny smb stuff (as it is too fiddley to solder by hand, or hot air) so I would like to stick to 2.54mm or larger.
I have the following capacitor(CP1) which is for filtering the vcc going into a 3.3 regulator(AMS1117), what do you suggest my chosen footprint is,? There are elec capacitors, axial, radial, wave, hand reflow etc none of which make particular sense to me. I am however pretty certain electrolytic is the wrong type here.
A 1206 SMD footprint should work. The ams1117 is in a SOT223 package, right ?
Tip : do not use cvpcb, seriously !
Instead make sure what components you are going to use before/while drawing
the schematics and define a component in the library with all the correct settings
like value, type and footprint taken from the manufacturers datasheet. That way
you can always find the correct type when some time has passed.
Also this will make sure that you will be using the same component on the PCB
and not the same value with 2 or more different footprints
Setting up your own libraries is not difficult at all thanks to the text based layout.
I like to use copy/paste and then change for a new component in text mode.
Even with the kicad-sch and kicad-pcb component editors it is easy to create your
own new library.
Selecting footprint for a capacitor (or any other component) depends on many different parameters.
The main decision you will make is if you want to use surface mount or through hole components.
Through hole caps are physically larger, easier to solder for a beginner but have higher series resistance and inductance. (Just because of their size)
SMD is smaller which means less board space required, less series resistance, can be assembled automatically but is a bit harder to hand solder (requires better equipment and a bit of practise)
For capacitors you might also need to check your equivalent series resistance (ESR) requirements. (Tantal caps typically have a high ESR whereas ceramic caps have a low ESR)
After that decision you check what is available for you. (You really need to check with your supplier what you can buy. For every component. Before starting with the pcb!)
As you also state you want surface mount and at least 2.5mm size for your capacitor you can simply check with the EIA size codes given. See: https://kicad.org/libraries/klc/F3.3/ (Section about tantal caps)
But again: Make sure you can buy such
@roelofth68 tantal caps are given in metric sizes not imperial as you listed above.
And no for caps and resistors cvpcb is totally fine (Making fully defined symbols for every cap and resistor will result in thousands of parts in your libs. Which is total nonesense in my mind. Accept that there are multiple different workflows. Sometimes it makes sense to mix them. I would never use CvPCB for ICs or other unique components.)
Yes 1206 sounds right,
But which option is this in the list?
Also – I am not sure what you mean by defining the component in libraries, please bare in mind this is my first ever board in kicad, and I am finding it hard to get to grips with.
He is suggestion you create a so called fully defined symbol for every component you ever use. This will be something you need to decide for yourself. Be aware that his workflow has some benefits when it comes to accountability but has the massive drawback of having a very large library.
I personally have a symbol for every capacitor size and use house part numbers for the material management. For caps (and resistors) a script builds the house part number from the information in the size dependent symbol plus the value i assign to it.
As you see there are a lot of options what you can do. For your first board i suggest you do not worry about that at all.
I would like to help you further but kicad-pcb crashes here (and by a lot of others too)
due to some library issue.
I think you have to do some scrolling in the list to find the correct footprint.
And yes, rene_poschl, the libraries will grow very large if you put every single part in
there known to exist. But I only put the parts in a library which I actually have in stock.
That way the amount is limited to the number of different parts in stock, it is traceable
and most important less mistakes.
You are right with capacitors and resistors (but not limited to), lots of manufacturers
for the same value and footprints. So for some people it is easier to use cvpcb. But
I might argue that also R’s and C’s have specific order numbers and therefore can
have a unique “part” in a library.
Andy, For example, as you can buy a certain IC in a so14 or dip14 footprint
you can have two different parts in a library which are recognizable by the
unique part number. In the kicad-sch library you can enter the two parts :
(only a part of the definition shown)
tl084cd
DEF ~tl084cd IC 0 40 Y Y 5 L N
F0 “IC” 50 200 60 H V C CNN
F1 “tl084cd” 0 200 60 H I C CNN
F2 “so14” 0 100 50 H I C CNN
F3 “/media/data/datasheet/opamp/ST/tl084.pdf” 0 0 60 H I C CNN
F4 “tl084” 50 -200 50 H V C CNN “Waarde”
F5 “1260022” 0 -100 50 H I C CNN “ITH nummer”
F6 “OpAmp” 0 -200 60 H I C CNN “Type”
tl084cn
DEF ~tl084cn IC 0 40 Y Y 5 L N
F0 “IC” 50 200 60 H V C CNN
F1 “tl084cn” 0 200 60 H I C CNN
F2 “dip14” 0 100 50 H I C CNN
F3 “/media/data/datasheet/opamp/ST/tl084.pdf” 0 0 60 H I C CNN
F4 “tl084” 50 -200 50 H V C CNN “Waarde”
F5 “1070048” 0 -100 50 H I C CNN “ITH nummer”
F6 “OpAmp” 0 -200 60 H I C CNN “Type”
The above can be done with the kicad-sch part editor, I tend to use a text
editor when I can because I find that easier.
But like Rene wrote, do not worry to much about this for now.
The first step in choosing a component is to choose one you can actually buy. There is no point laying out a board for components you can’t purchase. Therefore you should be looking on your favorite vendors website and finding an appropriate component that is available and reasonably priced. You will usually find several, then you can choose the footprint you want. You may then want to record this part number and footprint on your schematic. Then you can use CvPCB to match the components with footprints in the library. Once you’ve done the legwork using CvPCB is typically quite easy and straight forward.
My mistake in reading the component value of 22 uF and writing a footprint
of the 1206 size. The footprint size is of course also dependent on voltage
rating, type of capacitor (ceramic, electrolytic, polymer, tantalum) and
capacitance for instance.
If you have the voltage rating you can find the correct type for you circuit and
from that the footprint.
I still can’t find a 1206 SMB capacitor footprint in my list, there are hundreds of options, nothing references 1206 though? Which would be suitable for me?
What makes you think you want a 1206 footprint? Just because it was mentioned earlier? No one can tell you which footprint to use as we don’t know the voltage rating of your 22uF capacitor or what type you want, aluminum electrolytic, ceramic, tantalum, … Define the component before you choose it’s footprint or you’ll end up with a board you can’t build.
You placed the symbol of a polarized cap. This is why you only get polarized caps in your filter list.
CP_ELEC are cylindrical electrolytic caps for surface mounting (Size code in the v4 library is [diameter]x[height])
CP_Tantulumn are tantal caps (size identified via manufacturer case size codes plus metric EIA size codes. See my link above.)
Axial, Radial are also electrolytic capacitors but these are through hole components. (Size in the v4 lib is given with prefixes d for diameter, l for length, P for Pitch)
This communicates for what manufacturing process the footprint has been designed. Hand soldering footprints typically have slightly larger pads than reflow/wave.
The new naming convention (used for the version 5 library) includes the pad size if it is enlarged. (plus the suffix HandSolder to indicate that it is enlarged for easier hand soldering)
Tip: read the FAQ entry about footprint assignment (I posted it above) There is a way to get a preview of the footprint from within cvpcb (is described in that FAQ topic)
I want a 22µF solid tantalum, I don’t believe I need a polarised cap here – my mistake. I like 1206 because they are larger and easier for me to handle!
AS for choice of size, I don’t really know why somebody would pick an 805 against a 1206 unless board size was a consideration(and for me it’s not). Are there other factors I should consider here?
I’ve read at least one person argue you should always use a polarized cap symbol because sometimes the reason for choosing one cap over another boils down to cost over all else so the original engineer doesn’t know if it will be polarized or not. Here it doesn’t make a difference, but for people that will be handing off the design to others it might.
I know I went down this road on one of my designs. The 1206 package is pushing the limits of physical size (to small) to achieve 22uf. This may not be a reasonably priced purchasable part.
Are you sure? I used farnell (austria) searched for 22uF and sorted by price. The cheapest 22uF ceramic is 0805 imperial (2012 metric) Admittedly 6.3V (For 16V it is a 1210. Or 1206 if you do not want to pay for delivery from the us)
For tantal the cheapest 22uF is a 10V 1206 imperial (3216 metric)
For tantal 16V the cheapest option is a 1411 imperial (3528 metric)
The cheapest option has approximately (+/- one size code step) the same size (depending on voltage requirement) no matter if you pay for a full reel or if you want to pay only 10 pieces (but there is a factor of 10 between the price for a single cap between buying 2000 or 10 at once)
So it really depends on the voltage requirements. (As multiple people already stated.)
Ceramic generally is cheaper for the same size, voltage, capacitance.
Are you making these choices based on electrical design considerations or purely for package size?
)
Not very sensible and completely irrelevant however.