I am a beginner, totally new to PCB design and basic knowledge of electronics, so bear with me
I am working to design a parallel notch filter, I do have the schematic on paper, so I thought to create the schematic with KiCad. Apparently, no issues and no errors so far.
However, I am having some issue with the PCB drawing, and I would appreciate your advice:
I am aware that the 3 terminals are currently reversed, I mean, they should be rotated 180°, but if I do so, then my connections will be reversed and I have to re-design the PCB layout.
Is there a way to change the polarity in the terminals? I thought there was no polarity really in these connectors, but it appears to be the case with any footprint.
I do not fully understand the problem, but perhaps we can get to the bottom of your concerns by asking a few questions and proposing 1-2 ideas. I do not understand your concern quite well enough to tell you what to do. These are only points of discussion to try to get to your answers:
I think you are using terminal blocks which each have two terminals, so you have 6 terminals in 3 terminal blocks. Am I correct?
Are the terminal blocks symmetrical (or symmetrical enough) so that you can physically rotate them by 180 degrees and mount them to the pcb?
I would not recommend this for most ICs (for example) but I think that maybe there is no need to be “locked in” to the pin number assignments of 1 and 2. (??) A vital but easy skill in KiCad is to edit your own symbols and footprints. Would it work to make your own footprint with which you swap pin numbers 1 and 2?
This link explains how the forum works for posting images.
I think you mean “match the terminal numbers”?
You need to correct the Schematic so the numbers on the terminals are connected to wires you wish.
After this, from “Tools” use the “Update PCB from Schematic” function. The fine white “Ratlines” will show you which footprints need to be connected together.
If I am correct, use the “Flip Items” to change pin connections for the terminals in the Schematic.
It seems, your intention is to have “common plus upside” if watching the PCB. Therefore you need to swap pin 1+2 between input and output. If you turn the footprint 180 degree, the upside pin 1 goes down and opposite. This happens with all kind of footprints and connectors and is correct behaviour of Kicad.
If you are bothered by the pin 1 + 2 numbers in the circuit diagramm, Kicad allows to switch them to invisible. Another method to swap 1+2 is to place either input or output to the soldering side of the pcb but doing the assembly on component side. Therefore you have to be aware that your schematic is wrong as pin 1 is defined in the data sheet of the connector and thats always same not regarding from where you look or how you turn
Thank you guys, I edit the footprints as suggested and that resolved the issue.
I finalized the copper tracks, ran a DRC and got 4 violations:
Now, 3 are expected because I modified the footprint, but I do not understand the silkscreen overlap:
Also, if I add 5 mounting holes I get 9 schematic parities, it this because the holes are not part of the schematic? Is this expected?
Another question I have:
Currently the copper track width is 0.25mm, since we are talking about a passive crossover, is this the recommended width, or is it typically bigger?
This is the 3D View, inductor and connectors are missing because: 1) the inductor is not in the library and there is no 3D that exists, while the connectors I will probably go for the typical black ones, but no 3D in the KiCad library.
There are mostly very large components fitted to your board. In the interests of being mechanically robust, I’d increase all the pads and tracks greatly.
All pads except the terminals could be the diameter of the resistor front courtyards (Spread C1 & C3 further apart).
Multiply tracks by 10 or more, to at least 2.5mm.
Increase pads for terminals.
Relocate the track from +C3 to halfway between T2 & T3.
Remove the square holes in the C pads… too difficult to machine , likewise the pin1s for the terminals.
Check the hole sizes in your pads to suit the wire sizes for your components.
Your silk warning means you have drawn a Silkscreen line over something else or something else is interrupting the silk line. I can’t tell from the image posted.
If the silk line is not printed over bare copper it can be ignored.
Thank you very much for your hints, I will work on them tonight and post the results.
In the meantime, I am sharing the original boards of the crossover which will host this notch filter, just to show how they are built, (they are 30 years old), so trying to achieve consistency from a design and technical perspective
Note the plentiful use of copper on the crossover PCB you have posted, that is really the way to go with your PCB. There is current, weight and vibration.
You have already paid for the copper when you order the PCB, you might as well use it.
So, I want to create the connections using filled zones instead of tracks, like in the in picture 11 I posted above.
I have read about filled zones and netlists, but for whatever reason although the ratsnest lines are all connected and show the components, as in the schematic, when I click the copper zone properties, I only see the terminals:
No.
You need to route the board manually.
A Filled Zone is an area of copper that is “flooded” automatically, and connects to pads that are part of the specified net. You need to draw the outline of the zone using the zone tool, then Kicad will do the rest.
This will be a single sided board with the components on the front and the tracks on the back?
If so, replace your ratlines with tracks as you demonstrated 2 days ago. Don’t forget to use the same layer (back?) when creating your tracks and zones.
Then, as @3Dogs mentions, you need to draw, one at a time, areas around each net in the style of the cross-over you posted above.
In case you are not sure: a net is all the footprints that are connected together by an unbroken track.
eg. Pin 2 of J1 is connected to one side of R1 & R2 & L1 & C1 & C2. The other end of these same footprints is connected to Pin 1 J2. This is another net.
You can find the names of the nets that Kicad has assigned to your PCB by zooming in on any pad connected to a net. The net name is shown on each pad.
When you start to create a zone, highlight the correct net when the “Copper Zone Properties” panel opens and choose/change any other setting you wish in that panel before “OK”.
NOTE: you will probably have to move and modify your thin tracks after each zone is created to keep those tracks inside their correct zone.
Good luck!
Thank you for your instructions, that helps a lot to understand the Nets.
I did not have time to work on the project during the last three days, but I wanted to ask you regarding the pads of the terminals. You mentioned in a previous post to increase them.
I increased the ones of the R, C and L to 8mm, but how much should the ones of the terminals be? 4mm?
Also, since I am gong to use only the B.Cu for the connections, I only need to have the pads plated on the B.cu side for soldering, how do I remove the plated part on the F.Cu?
In the meantime I made the tracks 3mm and next step is to create the zones.
I have removed the 3D as per previous images because my components are crossover specific, therefore I cannot find the 3D models anywhere. I mean, you do not find those parts on Digikey or Mouser together with their 3Ds.
But at least I do have now the right dimensions (I have measured them), so I can be precise with the footprints I create.
Seeing you are going to produce a board in the style of the cross-over board where the pads are in large areas of copper, you do not have to worry too much about pad size, BUT, you do have to consider your Solder Mask.
It is probably best to change your pad size to something similar to the cross-over board. Sorry, the pad size I had mentioned earlier was before your board had the extra support of the large areas of copper using zones will create.
Your terminal pads can also be made in a similar way to the cross-over terminal pads.
I found some time to continue with my project this evening.
So I created the zones by net, but I get those violations and I cannot understand the problem.
The 5 errors relate to the keepout area, which I have created to facilitate the task of adding the filled zones.
I take this opportunity to ask you why, in the original PCB from the manufacturer, 2 mounting holes are on the copper layer, and two are not. I assume there is an electrical reason?
The other warnings are related to the footprints. They do not match a copy in the library, and that is true, because I had to customize them,none of the library ones are a fit, so what’s wrong with it?
Apart the above, I tried to do my best with the filled zones, and give as much copper areas as possible to all the components. I am sure a pro would do a better job.
How do I adjust the clearance of the filled zone that goes to J2 pin 2 and J3 pin 1? It is the only zone with diagonal lines, not easy to make it 0.5000 mm like the H or V lines. Is there a feature that allows all the zones to have the same default clearance?
I also attach an image of the copper zone properties, just for you to know the settings I used.
The DRC is following the Kicad procedure for making PCBs. It is not very smart and cannot understand your method.
The kicad procedure is to assign a footprint to a symbol. You have placed a modified footprint onto the PCB. Kicad doesn’t like that.
The Kicad way is to place a Kicad footprint into a personal library, save it as a new footprint (and probably rename), modify that footprint to the specifications you require,save, assign that new footprint in your personal library to your symbol in the schematic, then update your PCB from the Schematic with the new footprint.
You will have to do this with all the similar warnings about footprints not matching.
The alternative is, if you are confident with the footprints you have placed, ignore the warnings about this problem.
Not that I can think of.
The two mounting holes are attached to the -ve terminal of the amp. output. If that crossover was mounted in a metal box this would be a SUPER DODGY way of attempting to earth that box.
Long answer:
First, go into File / Board Setup / Design Rules / Constraints / and place a “Copper to Edge Clearance”… .5mm, 100mil, something like that.
Next, instead of using pads, use mounting holes. Find them in the Schematic library in “Mechanical”, then associate the required footprint from the “Mounting Hole” footprint library. Choose a hole footprint without pads.
Next, in the Rule Area Properties of the Keep Out Area only tick “Keep out Copper Fill”, then create your 5 Keep out areas.You will have to increase the keep out area of the inductor hole or offset the two top zones or use an insulator washer because the bolt holding the inductor may cause a short. Check the others for screw clearances also.
Now the zones. The shapes are good.
In the Copper Zone Properties: Layer - good. Each zone was assigned a Net - good.
In General, give each zone a name (or number) and a priority level.
Smoothing as you wish.
Electrical Properties: Clearance. This gives you the distance between each zone, whether diagonal or not (to answer one of your questions). Make the clearance similar to your crossover board.
Pad Connection: If you have a largish soldering iron, select solid, If not, select Thermal Relief. If you select thermal relief, you will need bigger pads and wide thermal spokes (for physical strength of the board with large, heavy components).
Solid fill - good.
Back to Priority level. When creating adjacent Zones, the second zone can overlap the first when drawing, but, there will always be the the clearance between them. The Priority level decides which zone wins where the two overlap. The higher priority zone gets its drawn border respected.
eg. If the first zone is drawn with a 20mil gap and priority 5, the second zone, where drawn over the first, if it has priority 4 or lower, will have move its border 20 mil further from the first zone border.
Experiment to find out. Note this will only show once you have filled the zones. Also, zones do not have to be drawn accurately around the edge of the PCB, they can be drawn outside the Edge Cut, but they will respect the Edge Cut clearance when filled.
, likewise the pin1s for the terminals.
