Ground plane misunderstanding

[nounours18200]

Hello,
I have designed dozens of PCB with SL-6.0, but the possible ground interferences were not important.
Actually I try to understand how to create a ground plane on a very simple PCB; it has 3 pins, an Input ("I"), a ground "G" and an output "O".

Without ground plane, the PCB is like this:

sans PDM.JPG (61.35 KiB) 4550 mal betrachtet

When I ask SL-6 to create the ground plane I get this:

avec PDM.JPG (63.5 KiB) 4550 mal betrachtet

Bu it seems to me that I should link the ground plane with the "G" pin, and when I try to add a track, SL-6 does not accept to link them, i get this (look just above the "G" pin):

ne connecte pas.JPG (66.11 KiB) 4550 mal betrachtet

As I have been using SL-6 for years, I know that I am doing something wrong, but how should I proceed ??

Thank you

[abacom]

You can select the track and set the "distance to the ground-plane" (in the lower statusbar) to zero. Then the track will connect to the ground-plane.

The better way will be to change the ground-pad into a "thermal-pad". Just select the pad and check the option "Thermal-pad" in the properties panel on the right. Then the pad will be also connect to the ground-plane automatically.

[nounours18200]

You can select the track and set the "distance to the ground-plane" (in the lower statusbar) to zero. Then the track will connect to the ground-plane.

good ! I have different ground planes due to the parts placement, is it wise to link them with the "star green tracks" like shown on the screen capture below ?

avec PDM relié.JPG (67.18 KiB) 4532 mal betrachtet

The better way will be to change the ground-pad into a "thermal-pad". Just select the pad and check the option "Thermal-pad" in the properties panel on the right. Then the pad will be also connect to the ground-plane automatically.

If I do this, the center "G" pad seems to touch to its neighbour "I" and "O" pads:

with thermal pad.JPG (65.17 KiB) 4532 mal betrachtet

I can of course remove these 2 tracks, but it seems to me that I must link the other ground planes by using the same "star" that I show above ?? sorry if I say something stupid, but it is the 1st time i work with ground planes...

[abacom]

I have different ground planes due to the parts placement, is it wise to link them with the "star green tracks" like shown on the screen capture below ?

Yes of course , you can do this.
Maybe there is sometimes a better way to do this, without the use of vias and tracks on C2.

[nounours18200]

OK, I have removed the via on C2, and here is the result:

avec PDM 2.JPG (66.88 KiB) 4517 mal betrachtet

but I still do not clearly understand the benefit to transform the pin "G" in a thermal pad ??...

Thanks

[hasta]

I think you don't understand what thermal pad means.
A thermal pad is the direct connection between a pin of the component (whether smd or wired) and ground plane. You can define the design of the thermal pad separately for each pad depending on its geometry.

In your PCB you can completely save the conductors of the 2nd level, if you design all ground connections of all components as thermal pad. Do this and then use the test function to check that all the desired pins are grounded.

[nounours18200]

I think you don't understand what thermal pad means.

You are totally right : I have absolutely zero knowledge about the grounded planes in Sprint Layout !

In your PCB you can completely save the conductors of the 2nd level, if you design all ground connections of all components as thermal pad. Do this and then use the test function to check that all the desired pins are grounded.

Sure it would be interesting to completely remove the 2nd level...
I have defined the grounded pins of C1, C3 and R2 as "thermal pad", and then tried to connect these pins to the grounded plane located closest from the pin.
But it seems that there is still no link between the ground plane and the grounded pin, even if I add a track Look at the yellow circle.

Here is the screen capture:

with thermal pad 2.JPG (66.43 KiB) 4510 mal betrachtet

I clearly make a huge mistake in my understanding or drawing (or both), but I don't see where...why the closest plane is not grounded even if I add a track ??

[Sonny1983]

It should be connected. Why do you think these aren't connected? Did you use the TEST function? Activate it and click on one of the grounded pads on a component (NOT on the ground plane itself). All connected items should light up pink.

BTW: Why dou you use tracks to connect the mounting hole, pin 7 and 18 on IC1, the "G" connection and the left side of R2 to ground? Just use thermal pads or adjust the clearance of the items to the ground plane to 0.

Info: While you can simply let the solder pad or via connect to the ground plane by adjusting the clearance to 0 (then it just sits in the plane directly), this takes away the heat when soldering. Soldering with an iron takes longer on those pads, and hot air or IR reflow can cause a small part like an 0603 resistor to "tombstone" (it stands up on the non-grounded pad, because the solder paste on it melts faster and pulls it up).

[nounours18200]

I apologize: I found my error just after posting my reply, and there was also an error due to a first wrong schematic... I have corrected it, and it seems OK , here is the latest version:

avec PDM 3.JPG (66.37 KiB) 4457 mal betrachtet

BTW: Why dou you use tracks to connect the mounting hole, pin 7 and 18 on IC1, the "G" connection and the left side of R2 to ground? Just use thermal pads or adjust the clearance of the items to the ground plane to 0.

I understand that I do something wrong by using these tracks, but there is something I still don't understand with the thermal pads and the ground links...
do you mean that I should change the nature of the pins 7, 18, G and Left side of R2, and transform all of them in thermal pads ?
This transform means editing the makros (IC-1 and R2), but if it is the way to do, I can doit

[Sonny1983]

Yes, I think you should change all pads that should connect to ground to
a) thermal pads
or
b) set the clearance to the groundplane to 0 (if you don't mind taking a second longer to solder)

You don't have to dissolve the macro into its pieces, edit a pad and then make a macro out of it again. There is a much simpler way in SprintLayout: Just hold the ALT-key and left-click on a solder pad (without moving the mouse). Now the pad is selected (pink). You can now either set the pad as a thermal pad (using the properties-sidebar on the right) or set the clearance to the ground plane to 0 (the active layer must be the top copper layer before you mark the pad). The setting fot the clearance is a little to the right down where the layer-selection of SprintLayout is. After you're done, click anywhere on the PCB to stop editing the selected pad. This way, you can edit all parts of a macro easily, but it still stays a macro.

I would suggest you use the thermal-pad-method for all pads and the 0-groundplane-clearance-method for the mounting hole. When creating a thermal pad, select the sides where you want the pads to connect to the ground plane (for example: on pin 7 of IC1 you would choose only top and bottom). There is a "selection-star" in the properties-sidebar where you can turn on and off the connections. Just do it the way it makes sense.

To clearify again: The pro of setting ground-clearance to 0 is, that the item (solder pad, via) has the maximum possible connection to ground. But, since copper conducts heat very good, soldering is a little harder, because the groundplane works as a heatsink. Thermal pads restrict the heat flow but still provide a good ground connection. Rule of thumb: When you try to get high currents into the ground plane (example: a via where you solder in a wire on a power supply PCB), you set ground clerance to 0 (soldering just takes a bit longer). Where only decent currents flow, you can use thermal pads.

Of course, before doing the steps above, you have to delete the unneccessary ground tracks, because they will get replaced by groundplane connections.

[Sonny1983]

I made a little tutorial video on YT.

https://www.youtube.com/watch?v=W2WSnqgrmaM

[nounours18200]

Thank you very much Sonny1983 for this video: it is a bit late tonight but I will watch it tomorrow ! it will be a big help for me and a lot of people.

Meantime I have learned a lot of things regarding the ground plane and I have achieved what I consider to be the final version of my PCB: I will post it tomorrow. It is perhaps not perfect, but much better than initially !

Nevertheless it would be nice if you can have a look at it before I send it to the manufacturer.

SMD parts with a thermal square below are totally new animals for me, so I am sure to have more things to learn...

[nounours18200]

Hi Sonny1983,

I have watched your excellent video, and it allowed me to improve my PCBs.
Here is my final version:

Capture2.JPG (65.3 KiB) 4345 mal betrachtet

I believe it should work.
I have implemented the ground plane on the C2 layer (because a "commercial" clone of what I plan to design uses the C2 layer as a ground plane), and unless I have made a mistake, it should work and is more "sexy" than having a lot of tracks going around the parts...

I have 2 remaining questions:

Q1: what is the best way to connect(to ground) a side of a part : is it to use a via to the ground plane like I have done, or is it to define this side as a thermal pad ?
Q2: I have not defined a ground plane on the C1 layer : is it necessary ? or more precisely, when is there any advantages to also define a ground plane on the CA layer ?

Thank you !

[Sonny1983]

First, I'll try to answer Q2:
Since you're already using the top copper layer C1, I would also make it a groundplane. Why?
a) You can use thermal pads to connect an SMD pad to the top copper layer directly (you can't connect it directly to the lower copper layer because an SMD pad is only on one side)
b) Whether you need it (sensitive signals or OPAMPS etc.) or not: You'll get nice shielding around traces, ICs, ....
c) The PCB manufacturer doesn't have to etch away so much copper from the base FR4 material.
d) It doesn't make to much sense to go to the effort of putting down vias next to SMD pads just to use the other side as groundplane. What is accomplished by not using the empty space on C1 to fill it with copper? If that is a copy of a commercial PCB then, to be frank, the commercial one is somehow stupidly designed. It's like if you want to add another sink near the existing one in the bathroom. Sure, you can pull a new water pipe from the basement to the faucet. Would you? No, you would put a T-joint in the pipe unter the existing one. It's just.... no.
e) It doesn't cost you anything!

Q1: If you set the groundplane clearance of a via to 0 (like you did), it will do this for both layers. So, it works. But regarding of my answer to Q2: I would not do this. I would use a groundplane on both sides and connect the SMD pads via thermal pads to the top groundplane. Then I would stitch the top and bottom groundplanes together with a couple of vias with 0 clearance, placed in areas that make sense. And of course, in areas where you would otherwise have floating copper (isolated "islands" of groundplane).

Also, make the mounting hole a via (throughhole) instead of a one sided soldering pad. Reason: A via has also copper on the inside "walls" of the hole which make it more durable when using screws. For an M3 screw for example, make the via hole 3,2mm.

[Sonny1983]

An example:

GP1.JPG (223.93 KiB) 4333 mal betrachtet

As you see, i put more vias near the capacitor grounds to stitch them dowm for lower resistance. All stitch-down vias are tented vias (with soldermask over them).

[Sonny1983]

I just saw that the "gorundplane island" I have marked isn't a real island, since there is a small strip of copper between the right two big solderpads, and there is a connection through the bottom 3 IC pads. But because a capacitor should have good grounding, the three vias still make sense.

[nounours18200]

Thank you so much Sonny, you are a Professor for me !

Tracks shielding is not important for this small PCB, but it will be of the highest importance for my next project, so your explanations are a golden tips !

Although I globally understand what you explain, there are unclear things for me:

U1: you set the ground plane on the top (excellent for tracks shielding in my next project) and the vias are supposed to establish a link With the bottom C2 layer. But how does the software "defines" that the C1 layer has to fill all the bottom surface ? (maybe it is define by default ?).
U2: what does "tented" vias mean: does it mean that their internal diameter is zero ?

I have tried to build a PCB according with your last tips, see attached, but I feel more comfortable with my previous one, i feel a lower risk of error...

Here it is:

pour sonny.lay6

(138.42 KiB) 55-mal heruntergeladen

Can you have a look at it ? (I know that the bottom left pad of the IC is not yet defined as a thermal pad, but it will in my final version)

[Sonny1983]

U1: When the groundplane option for a layer is turned on, the software looks for all copper elements on that layer (pads, tracks, solder pads, vias, ...) and fills the remaining area with copper, while retaining the set clearance around each element (which of course you can set to 0). The groundplane option is layer-specific: You can turn it on and off separately for C1 and C2. In your layout file, you forgot to turn on groundplane for C2 (to turn it on, select layer C2 and klick on the groundplane button in the lower menu bar [next to "?"]).
U2: A solder pad (also called "Non-Plated-Through-Hole/NPTH") is a drilled hole in the PCB with a copper ring around it, usually only on one side of the PCB. Over that ring, the soldermask ist removed (SprintLayout does that automatically), so you are left with a solderable surface instead of the soldermask (green by standard). Of course, you can put another NPTH on the other side and align them, but until you solder a wire through them, both sides won't be connected, because the inside wall of the hole is not plated with copper (it's just FR4 epoxy). A via (also called "Plated-Through-Hole/PTH") is a hole in the PCB with a copper ring around it on both PCB sides. But, in a via, the inside wall of the hole is plated with copper, so even without soldering a wire through the hole on both sides, there will be a connection (so you can jump between layers of the PCB). Also, over the copper rings, the soldermask is normally removed, so you can solder a wire or component leg into the via. On a tented via howeyer, the soldermask over the copper rings (and the hole) is NOT removed. So, you cant solder on a tented via. It is used only to jump between the layers and not for connecting a component or wire. It is not neccessary to ma a via tented, you can just leave it "naked". But it just looks cleaner to cover it with soldermask. You can make any via a tented via by selecting the "Soldermask"-function in the left menu bar (icon is a little red circle). Then, all solderable elements of the PCB (vias, SMD pads, ...) light up white. You can tent a via by klicking on it; then it will not be white in this mode anymore. You can also remove the soldermask from tracks to leave them naked by clicking on a track. Check the Photo-View later, to see the effect.

A via without a hole cannot work (so the small vias in your file won't work too, you have to set a hole diameter). Use at least a hole diameter that your PCB manufacturer supports (DRC=Design Rule Check, a great function in Sprint layout. Just fill in the data from your manufacturer and you can check in SL6 if you PCb can be produced).

To see how many current a specific via diameter or track can support, I recommend the following free software:
https://saturnpcb.com/saturn-pcb-toolkit/

It is a "must-have" tool for making PCBs.

So, turn on the groundplane option on layer C2, set a hole diameter for the vias and check if the clerance for the groundplane-vias is set to 0. Check the Photo-View to make sure. Also, use the Test-function. Make the groundplane vias tented if you want.

And: Clean-out the groundplane line between R1 and Cff (either set a bigger clearance, move the parts a little away or set a "barrier zone" (don't know the english term). You find this unter the groundplane on/off-button in the lower menu bar.

[nounours18200]

Thank you very much for this lesson ,

In your layout file, you forgot to turn on groundplane for C2 (to turn it on, select layer C2 and klick on the groundplane button in the lower menu bar [next to "?"]).

True: here is the file with a ground plane both on C1 and C2:

Sonny2.JPG (62.55 KiB) 4268 mal betrachtet

but it looks less readable to me: I am sure to make mistakes on a more complex PCB, whereas with only 1 GP on C2 (and the thermal pads and vias, I feel more secure.... It looks too confusing to me...

A via without a hole cannot work (so the small vias in your file won't work too, you have to set a hole diameter). Use at least a hole diameter that your PCB manufacturer supports (DRC=Design Rule Check, a great function in Sprint layout. Just fill in the data from your manufacturer and you can check in SL6 if you PCb can be produced).

I have read 0.1mm minimum (if my memory is OK) so I have modified all the vias to have an internal diameter of 0.2mm

So, turn on the groundplane option on layer C2, set a hole diameter for the vias and check if the clerance for the groundplane-vias is set to 0. Check the Photo-View to make sure. Also, use the Test-function. Make the groundplane vias tented if you want.

Done

And: Clean-out the groundplane line between R1 and Cff (either set a bigger clearance, move the parts a little away or set a "barrier zone" (don't know the english term). You find this unter the groundplane on/off-button in the lower menu bar.

Here I am lost: since I have the ground planes on both C1 and C2, I am no longer able to be sure of the circuit !

here is the file, but I believe that I have no more choice than having a GP on only 1 side, if not I don't clearly see what I am doing !

example by Sonny1983_2.lay6

(107.8 KiB) 57-mal heruntergeladen

I am sure to make errors in a more complex PCB with GP on the 2 sides....

[Sonny1983]

I sent you a PM