Author Topic: Why am not able to get a grasp of PCB designing?  (Read 15764 times)

0 Members and 2 Guests are viewing this topic.

Online tautech

  • Super Contributor
  • ***
  • Posts: 29813
  • Country: nz
  • Taupaki Technologies Ltd. Siglent Distributor NZ.
    • Taupaki Technologies Ltd.
Re: Why am not able to get a grasp of PCB designing?
« Reply #100 on: December 03, 2019, 08:36:36 am »


Looking better.  :)
How do you feel about progress thus far ?

Can you name the USB socket designator that's on both sides ?
How do you feel about rotating the IC another 45o to the left ?
« Last Edit: December 03, 2019, 08:50:32 am by tautech »
Avid Rabid Hobbyist.
Some stuff seen @ Siglent HQ cannot be shared.
 
The following users thanked this post: redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #101 on: December 03, 2019, 08:50:31 am »
Looking better.  :)
How do you feel about progress thus far ?
Thanks.
This is cool! Awesome. What I once thought I could never do, I am almost there.
Thanks a lot for everyone who helped. :-+
Quote
Can you name the USB socket designator ?
How do you feel about rotating the IC another 45o to the left ?
J5 and J6.
Let me try...
 
The following users thanked this post: tautech

Online tautech

  • Super Contributor
  • ***
  • Posts: 29813
  • Country: nz
  • Taupaki Technologies Ltd. Siglent Distributor NZ.
    • Taupaki Technologies Ltd.
Re: Why am not able to get a grasp of PCB designing?
« Reply #102 on: December 03, 2019, 08:56:47 am »
Looking better.  :)
How do you feel about progress thus far ?
Thanks.
This is cool! Awesome. What I once thought I could never do, I am almost there.
Thanks a lot for everyone who helped. :-+
That's made my day.
Really happy to see you getting your head around it and congrats for sticking at it.  :clap:

If the 45 anticlockwise doesn't look viable it don't matter as you've proved if it is by trying it.
« Last Edit: December 03, 2019, 08:59:15 am by tautech »
Avid Rabid Hobbyist.
Some stuff seen @ Siglent HQ cannot be shared.
 
The following users thanked this post: redgear

Offline thinkfat

  • Supporter
  • ****
  • Posts: 2161
  • Country: de
  • This is just a hobby I spend too much time on.
    • Matthias' Hackerstübchen
Re: Why am not able to get a grasp of PCB designing?
« Reply #103 on: December 03, 2019, 09:00:12 am »
I think it's getting somewhere now. Good job!

Now, I think you can keep the net ties, if they help you staying close to the the sample schematic and if they don't confuse you, just keep in mind to treat them as a sub-part of the mosfets they're attached to and keep them close together.

On the question of thermal vias - yes, you need them. And you need to keep a considerable area of copper below the IC so that the heat can go somewhere. Also, the power pad seems to be the main ground connection, you'll need to keep that in mind.

There's a few other things to consider:

- the VOUT portion is the main power rail for the USB connectors. You need a quite beefy connection there, placing the capacitors on the opposite side of the PCB needs some care taken. I don't know how many amps you plan to source simultaneously, but keep in mind that you need a significant trace width. If the capacitors are supposed to stay on the bottom side, you'll need plenty of vias to keep the inductance low.

- I didn't see straight and suggested to keep J3 where it is, but if you look at the ratsnets, it'll be even easier if you swap J3 and J4.

- Around the switching part of the boost converter, you'll need to think about keeping ground loops very tight. The copper area of the SW node should be kept small. Place L1 close to the IC pins and on the top side. The thing looks _huge_. Which component did you choose? Maybe you can find a different type that exchanges PCB area with height? But I'm not sure about the overall dimensions. Also, treat this area with care while routing traces on the bottom side, make sure to not cut or obstruct the ground loop of the boost converter part. There'll be high switching currents flowing, you need as low an impedance as you can get. It's a shame the chip vendor doesn't provide a layout suggestion.



Everybody likes gadgets. Until they try to make them.
 
The following users thanked this post: redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #104 on: December 03, 2019, 09:51:18 am »
I think it's getting somewhere now. Good job!
Thanks.
Quote
Now, I think you can keep the net ties, if they help you staying close to the the sample schematic and if they don't confuse you, just keep in mind to treat them as a sub-part of the mosfets they're attached to and keep them close together.
The sample schematic does not use net-ties, @jhpadjustable suggested to add them and helped me around the DRC errors in schematics.

Quote
On the question of thermal vias - yes, you need them. And you need to keep a considerable area of copper below the IC so that the heat can go somewhere. Also, the power pad seems to be the main ground connection, you'll need to keep that in mind.
Ok
Quote
There's a few other things to consider:

- the VOUT portion is the main power rail for the USB connectors. You need a quite beefy connection there, placing the capacitors on the opposite side of the PCB needs some care taken. I don't know how many amps you plan to source simultaneously, but keep in mind that you need a significant trace width. If the capacitors are supposed to stay on the bottom side, you'll need plenty of vias to keep the inductance low.
The max current will be 4A. I was considering something around 100-110 mils. I used a online trace width calculator and the result was 104mils. Nope the capacitors can be placed on the top side too. While the chip's datasheet gives no layout recommendations, a similar chip that i selected previously wanted those capacitors on VOUT network to be placed as close as possible to IC. So, I just put them directly underneath. There is still space for the capacitor to be accommodated on the top side of the board. If that is better, I will flip them to the top.
Quote
- I didn't see straight and suggested to keep J3 where it is, but if you look at the ratsnets, it'll be even easier if you swap J3 and J4.
Done, exchanged them.
Quote
- Around the switching part of the boost converter, you'll need to think about keeping ground loops very tight. The copper area of the SW node should be kept small. Place L1 close to the IC pins and on the top side. The thing looks _huge_. Which component did you choose? Maybe you can find a different type that exchanges PCB area with height? But I'm not sure about the overall dimensions. Also, treat this area with care while routing traces on the bottom side, make sure to not cut or obstruct the ground loop of the boost converter part. There'll be high switching currents flowing, you need as low an impedance as you can get. It's a shame the chip vendor doesn't provide a layout suggestion.
Ok. Does it make sense to flip the mosfets to the back and get the inductor on top near the IC? I went with the one that was recommended in the BOM. Here is the datasheet SPM10102R2MESN. I was not able to find a footprint online so I created one myself, I might have made a mistake if that component looks unsually huge.

Thanks :)
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4705
  • Country: au
  • Question Everything... Except This Statement
Re: Why am not able to get a grasp of PCB designing?
« Reply #105 on: December 03, 2019, 10:31:27 am »
Had a play around trying to reduce how many headaches there where (e.g. trying to keep the switching node at least a little away from the USB differential, and how to lay that out with minimal crossing)

seems to me the best result is if you treat the chip like a switch mode converter first, keeping loop area as small as possible and all that fun, then running the USB in the order you have it assigned (even if the USB is just for signalling, my mind is still clinging to routing it out with minimal crossings,

Also had a play with your battery connection area to keep the connections as short as possible,

next steps from here would probably be to shift the micro more central, to keep those battery connections short, while keeping as much distance as possible from the inductor switching node and the usb pairs.

those 0201 components will be a right pain to solder, if you can, I would recommend larger parts for ease of assembly,

I should also mention, the trace width calculations can be cheated a little, sometimes it is better to have a thinner but shorter connection than a wider but longer one, the big one may reduce the amount of heat per unit distance, but a shorter connection reduces that distance.
« Last Edit: December 03, 2019, 10:37:30 am by Rerouter »
 
The following users thanked this post: redgear

Offline thinkfat

  • Supporter
  • ****
  • Posts: 2161
  • Country: de
  • This is just a hobby I spend too much time on.
    • Matthias' Hackerstübchen
Re: Why am not able to get a grasp of PCB designing?
« Reply #106 on: December 03, 2019, 10:36:36 am »
The correct land pattern is shown on p.83, if you used that one it's likely OK, but also the it's quite a huge component, 11mm x 10mm. Looking at their datasheet, you could likely go with a smaller device, like an SPM5050xxx. I've used Coilcraft XAL5030 inductors for switching converters with good results. For example, the XAL5030-222MEC, it's around 5mm x 5mm, could fit your design.

About flipping the transistors to the other side - well, you need to make up your mind, I would put each of the transistors closer to the USB receptacles they will switch power to, but keep in mind that you also need to route the sense wires. You need to develop a general idea of where certain nets should go. For example, you could decide that the high-current stuff should stay on the top layer and that you'll route the sense wires on the bottom.

It might be a good idea to route the VOUTP net as a beefy trace on the border of the PCB, out to the right and then up and then to the left along the top edge, and feed the mosfets from there. That keeps the power distribution out of the way of the USB signals that you also need to route. You could then drop the sense lines and the gate signals to the bottom layer of the PCB and route them back to the IC. They have no speed or current requirements and might not mind a few vias.
Everybody likes gadgets. Until they try to make them.
 
The following users thanked this post: redgear

Offline thinkfat

  • Supporter
  • ****
  • Posts: 2161
  • Country: de
  • This is just a hobby I spend too much time on.
    • Matthias' Hackerstübchen
Re: Why am not able to get a grasp of PCB designing?
« Reply #107 on: December 03, 2019, 10:50:23 am »
Had a play around trying to reduce how many headaches there where (e.g. trying to keep the switching node at least a little away from the USB differential, and how to lay that out with minimal crossing)

seems to me the best result is if you treat the chip like a switch mode converter first, keeping loop area as small as possible and all that fun, then running the USB in the order you have it assigned (even if the USB is just for signalling, my mind is still clinging to routing it out with minimal crossings,

Also had a play with your battery connection area to keep the connections as short as possible,

next steps from here would probably be to shift the micro more central, to keep those battery connections short, while keeping as much distance as possible from the inductor switching node and the usb pairs.

those 0201 components will be a right pain to solder, if you can, I would recommend larger parts for ease of assembly,

I should also mention, the trace width calculations can be cheated a little, sometimes it is better to have a thinner but shorter connection than a wider but longer one, the big one may reduce the amount of heat per unit distance, but a shorter connection reduces that distance.

That looks pretty good already. I agree the controller should be more central, close as possible to the battery protection circuit. but still positioned so that the display socket doesn't obstruct the USB traces. Close to the bottom would be good I think.

Also, I don't see a reason for putting all the high-power components on the bottom side, there's plenty of space between the USB receptacles to put e.g. the mosfets and there isn't much more that you need to place. As a general strategy I'd use "power distribution and usb signals on top layer, ground plane, slow signals and sensing on the bottom". The small jellybean stuff can go to the bottom side too.
Everybody likes gadgets. Until they try to make them.
 
The following users thanked this post: redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #108 on: December 03, 2019, 10:59:54 am »
Had a play around trying to reduce how many headaches there where (e.g. trying to keep the switching node at least a little away from the USB differential, and how to lay that out with minimal crossing)

seems to me the best result is if you treat the chip like a switch mode converter first, keeping loop area as small as possible and all that fun, then running the USB in the order you have it assigned (even if the USB is just for signalling, my mind is still clinging to routing it out with minimal crossings,
Thanks. I will try to do it again from scratch.
Quote
Also had a play with your battery connection area to keep the connections as short as possible,

next steps from here would probably be to shift the micro more central, to keep those battery connections short, while keeping as much distance as possible from the inductor switching node and the usb pairs.
@thinkfat suggested I keep the inductor on the top layer but I find it is on the bottom layer in your design. Should I place it on the top layer?
Quote
those 0201 components will be a right pain to solder, if you can, I would recommend larger parts for ease of assembly,
Bigger components takes more space, so I was thinking to go with reflow method.
Quote
I should also mention, the trace width calculations can be cheated a little, sometimes it is better to have a thinner but shorter connection than a wider but longer one, the big one may reduce the amount of heat per unit distance, but a shorter connection reduces that distance.
Thanks for the tip...

The correct land pattern is shown on p.83, if you used that one it's likely OK, but also the it's quite a huge component, 11mm x 10mm. Looking at their datasheet, you could likely go with a smaller device, like an SPM5050xxx. I've used Coilcraft XAL5030 inductors for switching converters with good results. For example, the XAL5030-222MEC, it's around 5mm x 5mm, could fit your design.
Yes, I used the same dimensions. Ok, I will try to look for components with smaller footprints. I tried using the Digikey filter before I started but sadly I did not find any.
Quote
About flipping the transistors to the other side - well, you need to make up your mind, I would put each of the transistors closer to the USB receptacles they will switch power to, but keep in mind that you also need to route the sense wires. You need to develop a general idea of where certain nets should go. For example, you could decide that the high-current stuff should stay on the top layer and that you'll route the sense wires on the bottom.
Alright, I will redo it. Hope I develop these over time so I could do it right the first time.
Quote
It might be a good idea to route the VOUTP net as a beefy trace on the border of the PCB, out to the right and then up and then to the left along the top edge, and feed the mosfets from there. That keeps the power distribution out of the way of the USB signals that you also need to route. You could then drop the sense lines and the gate signals to the bottom layer of the PCB and route them back to the IC. They have no speed or current requirements and might not mind a few vias.
Ok, let me try this.

Thanks.
 

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #109 on: December 04, 2019, 05:09:10 am »
For example, you could decide that the high-current stuff should stay on the top layer and that you'll route the sense wires on the bottom.
If I choose to have the high current stuff at the top, should also flip the battery protection to the top layer?
Quote
It might be a good idea to route the VOUTP net as a beefy trace on the border of the PCB, out to the right and then up and then to the left along the top edge, and feed the mosfets from there.
If I am going to do this, can I remove the net-ties?
« Last Edit: December 04, 2019, 05:12:11 am by redgear »
 

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #110 on: December 04, 2019, 06:07:43 am »
I managed to find a Design Recommendations for the chip in Chinese. The document gives me headache. Feels like I hit a roadblock again. I am attaching it with this reply.
 

Online tautech

  • Super Contributor
  • ***
  • Posts: 29813
  • Country: nz
  • Taupaki Technologies Ltd. Siglent Distributor NZ.
    • Taupaki Technologies Ltd.
Re: Why am not able to get a grasp of PCB designing?
« Reply #111 on: December 04, 2019, 06:52:01 am »
I managed to find a Design Recommendations for the chip in Chinese. The document gives me headache. Feels like I hit a roadblock again. I am attaching it with this reply.
If you can copy paste, drop it in here:
https://translate.google.com/

Build a new English doc in MS Word or similar.
Avid Rabid Hobbyist.
Some stuff seen @ Siglent HQ cannot be shared.
 

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #112 on: December 04, 2019, 07:08:05 am »
If you can copy paste, drop it in here:
https://translate.google.com/

Build a new English doc in MS Word or similar.

Here is the translated version.

They have recommended to use a 4 layer board. Will it be possible to do it in a 2 layer board? I feel like it can't be done in a 2 layer board if I were to use the recommended trace width. Also, they recommend to use 8 mils or 10 mils as default trace width but if I use that, the traces won't connect to the ic pins.
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4705
  • Country: au
  • Question Everything... Except This Statement
Re: Why am not able to get a grasp of PCB designing?
« Reply #113 on: December 04, 2019, 07:34:17 am »
It can be done on 2, you just need to avoid crossings under switching nodes or the differential pairs, It makes it harder, but it is still possible. as for the trace widths, it is a recommendation, but you can neck-down the traces where they enter the IC if you wish

there reference layout looks very weird, they have there switching node taking up half of the PCB.

Working on the top layer, its quite possible to lay it all out, just a pain in terms of loop side, seeing as 8-27 need to be escaped
« Last Edit: December 04, 2019, 07:49:06 am by Rerouter »
 
The following users thanked this post: redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #114 on: December 04, 2019, 08:09:18 am »
It can be done on 2, you just need to avoid crossings under switching nodes or the differential pairs, It makes it harder, but it is still possible. as for the trace widths, it is a recommendation, but you can neck-down the traces where they enter the IC if you wish
ok, Let me try. idk if i will be able to.Thanks.

[/quote]
Working on the top layer, its quite possible to lay it all out, just a pain in terms of loop side, seeing as 8-27 need to be escaped
[/quote]
You mean all components on the top layer?
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4705
  • Country: au
  • Question Everything... Except This Statement
Re: Why am not able to get a grasp of PCB designing?
« Reply #115 on: December 04, 2019, 08:59:49 am »
well they say that SW and VOUT should not change layer, which kinda nudges towards also having the BAT caps on the top side to, playing with it now, but very possible, main thing is I should shift it back towards the center, but I am thinking you can route a lot of the VOUT/VBUS traces under the plugs, and place the mosfets for each plug practically next to the USB ports.

I have done the caps for the inductor a little weird, but this was to keep the smallest loop area I could find for this inductor, I would be feeding in the battery connection to both capacitor groups seperatly,

edit: by loop area, you can treat it like drawing a line that shows where the current goes along the power trace, vs how it has to travel on the ground plane to complete that loop, anywhere it deviates from being directly next to or under that power trace is a possible EMI noise source for switchmodes, or a potential antenna for general signal traces (e.g. your KEY pin)
« Last Edit: December 04, 2019, 09:26:14 am by Rerouter »
 

Offline thinkfat

  • Supporter
  • ****
  • Posts: 2161
  • Country: de
  • This is just a hobby I spend too much time on.
    • Matthias' Hackerstübchen
Re: Why am not able to get a grasp of PCB designing?
« Reply #116 on: December 04, 2019, 10:26:17 am »
It can be done on 2, you just need to avoid crossings under switching nodes or the differential pairs, It makes it harder, but it is still possible. as for the trace widths, it is a recommendation, but you can neck-down the traces where they enter the IC if you wish

there reference layout looks very weird, they have there switching node taking up half of the PCB.

Working on the top layer, its quite possible to lay it all out, just a pain in terms of loop side, seeing as 8-27 need to be escaped

Yeah, having a large switching node is not a good idea, specifically for EMI. That thing radiates like crazy. The larger it gets, the more possible modes it has for forming resonances while you pump pulses of energy into it that are rich of harmonics.
Everybody likes gadgets. Until they try to make them.
 

Offline thinkfat

  • Supporter
  • ****
  • Posts: 2161
  • Country: de
  • This is just a hobby I spend too much time on.
    • Matthias' Hackerstübchen
Re: Why am not able to get a grasp of PCB designing?
« Reply #117 on: December 04, 2019, 10:46:55 am »
If you can copy paste, drop it in here:
https://translate.google.com/

Build a new English doc in MS Word or similar.

Here is the translated version.

They have recommended to use a 4 layer board. Will it be possible to do it in a 2 layer board? I feel like it can't be done in a 2 layer board if I were to use the recommended trace width. Also, they recommend to use 8 mils or 10 mils as default trace width but if I use that, the traces won't connect to the ic pins.

Reading the layout recommendations made me smile a bit, they basically reiterate what I've already mentioned ;)

Will it be possible to use only two layers - well, you'll likely get all the traces connected, but as I see it, the question is more if you'll be able to get the thermal design right. Even though they claim 95% of efficiency, let's be conservative and only assume, like, 85% or so, which means at full tilt doing 22 watts, you'll need to get rid of about 3 watts of heat through a tiny 6x6mm chip. The center pad is even less than that, hence their recommendation to put 36 vias into the center pad. But that buys you nothing, if those vias are not connected to a huge amount of copper. With a 4 layer board, you can dedicate a full layer to being a ground plane and they still say you need to keep a considerable window under the chip as an unbroken copper area.

The next aspect a 4 layer board helps with is that you have high-impedance sense wires for voltage and current sensing running around, those will very easily pick up dirt from the switching node. Putting them on the bottom layer and using ground the ground planes as a shield will definitely help here.
Everybody likes gadgets. Until they try to make them.
 
The following users thanked this post: redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #118 on: December 04, 2019, 11:06:54 am »
well they say that SW and VOUT should not change layer, which kinda nudges towards also having the BAT caps on the top side to, playing with it now, but very possible, main thing is I should shift it back towards the center, but I am thinking you can route a lot of the VOUT/VBUS traces under the plugs, and place the mosfets for each plug practically next to the USB ports.

I have done the caps for the inductor a little weird, but this was to keep the smallest loop area I could find for this inductor, I would be feeding in the battery connection to both capacitor groups seperatly,

edit: by loop area, you can treat it like drawing a line that shows where the current goes along the power trace, vs how it has to travel on the ground plane to complete that loop, anywhere it deviates from being directly next to or under that power trace is a possible EMI noise source for switchmodes, or a potential antenna for general signal traces (e.g. your KEY pin)

This looks great! Do you have the SW1 on the right side? I'm not able to find room for the IC if I have it there.
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4705
  • Country: au
  • Question Everything... Except This Statement
Re: Why am not able to get a grasp of PCB designing?
« Reply #119 on: December 04, 2019, 12:21:37 pm »
Can do, just had to shift around the IC a little, whats mainly left is the mosfets and sense lines, but with some fiddling there silly guide can be followed for a 2 layer fitout
 
The following users thanked this post: tautech, redgear

Offline thinkfat

  • Supporter
  • ****
  • Posts: 2161
  • Country: de
  • This is just a hobby I spend too much time on.
    • Matthias' Hackerstübchen
Re: Why am not able to get a grasp of PCB designing?
« Reply #120 on: December 04, 2019, 12:35:04 pm »
Another hint: They want the battery terminals as far apart as possible, to avoid shorting them out during assembly or when a wire comes loose. That means two things: follow that advice, or use a battery with built-in protection and drop the protection circuit from your design.
Everybody likes gadgets. Until they try to make them.
 
The following users thanked this post: redgear

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4705
  • Country: au
  • Question Everything... Except This Statement
Re: Why am not able to get a grasp of PCB designing?
« Reply #121 on: December 04, 2019, 12:49:45 pm »
And this gets in to why the selection tools in PCB editors are such a nice thing, drag from left selects only what you fully overlap, drag from right selects everything the area overlaps,

them "m" to move and "r" to rotate, or "f" to flip the entire group in one go, means shuffling around chunks is not as much of an issue. "backspace" removes only the segment under your mouse, "delete" removes that segment and any connected segments back to a pin or a junction,

and finally you can edit traces by starting routing on an existing segment, if you end the trace overlapping a segment on the same trace it can auto-delete the old trace and replace it with your new one (button on the left side turns this on or off)
 
The following users thanked this post: jhpadjustable, redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #122 on: December 05, 2019, 07:31:05 am »
The next aspect a 4 layer board helps with is that you have high-impedance sense wires for voltage and current sensing running around, those will very easily pick up dirt from the switching node. Putting them on the bottom layer and using ground the ground planes as a shield will definitely help here.
Since this is my first board, I am afraid 4 layers will make it more complex.

Can do, just had to shift around the IC a little, whats mainly left is the mosfets and sense lines, but with some fiddling there silly guide can be followed for a 2 layer fitout

I am trying to duplicate what you did, How do you do those beefy traces? Do you draw polygons on the copper layer?
I am not able to pour copper on the board. If i try fill it with GND I get only hatched lines and not solid green layers like yours.
 

Offline Rerouter

  • Super Contributor
  • ***
  • Posts: 4705
  • Country: au
  • Question Everything... Except This Statement
Re: Why am not able to get a grasp of PCB designing?
« Reply #123 on: December 05, 2019, 08:28:06 am »
some copper pours, but the BAT trace is a 2mm trace, trace settings are under file/board setup

The pours I have attached my usual settings,

to change how the pour appears, there is a green button on the left hand toolbar, it and the 2 beneath it control what a copper pour looks like, as its easier to lay things out with it hidden sometimes,

edit: you can also change your trace width and grid while routing by right clicking
« Last Edit: December 05, 2019, 09:04:32 am by Rerouter »
 
The following users thanked this post: redgear

Offline redgearTopic starter

  • Frequent Contributor
  • **
  • Posts: 286
  • Country: us
Re: Why am not able to get a grasp of PCB designing?
« Reply #124 on: December 05, 2019, 09:57:45 am »
some copper pours, but the BAT trace is a 2mm trace, trace settings are under file/board setup

The pours I have attached my usual settings,
Thank You!
Quote
to change how the pour appears, there is a green button on the left hand toolbar, it and the 2 beneath it control what a copper pour looks like, as its easier to lay things out with it hidden sometimes,

edit: you can also change your trace width and grid while routing by right clicking
I tried toggling it but no change.
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf