Help with substituting through hole with SMD

[sonolink]

Haven't you made a "finger error"? From the same calculator, I get 1.02mm with 2oz copper, and 2.03mm for 1oz.

You're right....my bad

The "thickness" there is, by default, 2oz/sqft, or 70um (70 micrometers, 0.07mm). Change that to 1oz/sqft or 0.035mm and see what you get then.

For 1oz/sqft I get 2mm width....this is weird. No way I'm gonna be able to fit 2mm traces on that board...isn't that huge?

 

[Khron]

Well, 2A isn't something to sneeze at (either). And 2mm for a power trace isn't even all that wide, especially on 35um copper.

BUT on the other hand, you need maybe 300mA for the heater, and (250v x 5mA / 9v) maybe 150mA for the B+ supply, so even allowing for not-fabulous-efficiency for the B+ step-up converter, you'll still be WAY below the 2A of the recommended plug-pack to supply this whole thing.

Just because it's recommended to feed this circuit with a 9v 2A adapter, doesn't necessarily mean it's gonna be pushed to 100% of its limits constantly. Rather to leave some headroom...

 

[sonolink]

Well, 2A isn't something to sneeze at (either). And 2mm for a power trace isn't even all that wide, especially on 35um copper.

BUT on the other hand, you need maybe 300mA for the heater, and (250v x 5mA / 9v) maybe 150mA for the B+ supply, so even allowing for not-fabulous-efficiency for the B+ step-up converter, you'll still be WAY below the 2A of the recommended plug-pack to supply this whole thing.

Just because it's recommended to feed this circuit with a 9v 2A adapter, doesn't necessarily mean it's gonna be pushed to 100% of its limits constantly. Rather to leave some headroom...

Do you mean I could do with 0.3mm traces then or should I stick to 0.5?

 

[Khron]

I'd rather go with "as wide as you can fit". Although it would be interesting to see where you are with the board layout and trace routing...

 

[abbey road d enfer]

Some times PCB designers resort to some tricks, such as charging the trace with solder, or even adding a wire.

 

[sonolink]

I'd rather go with "as wide as you can fit". Although it would be interesting to see where you are with the board layout and trace routing...

Ok, I´ll upload the layout asap, just promise not to laugh ok?

Thanks again for all the help
Cheers
Sono

 

[ccaudle]

Some times PCB designers resort to some tricks, such as charging the trace with solder, or even adding a wire.

Or you just put the connector for the high current input on the PCB right where you need it, and run the power with wires. 2A isn't really high, that would be trivial if you add an extra layer. Just something to keep in mind, I know we all like to save money, but 4 layer PCBs aren't very expensive these days if you are willing to use a predefined stackup so you can share a panel (e.g. jlcpcb).

To be honest I don't REALLY know.

Then you can't REALLY design the PCB properly. You need to have at least a decent idea of how the circuit operates to create an appropriate layout.

I know that B+ will be around 200-250VDC

If you are squeezing the layout that tightly, don't forget to include proper distance between conductors appropriate for the voltage.
Creepage and clearance (Cadence white paper)

I assume these will be external traces. FR-4 dielectric? Will you have solder mask, or bare?
Looks like around 2mm spacing should be enough around the high voltage traces:
chart for high voltage spacing at Altium

Don't forget that at 250V quiescent plate voltage you will get swings above that when operating. Extra margin above the minimum requirements never hurts.

 

[Khron]

I think the B+ is supposed to be ~250v, not the anode voltages.

 

[sonolink]

Ok here goes. I need to explain first that, the tube is mounted horizontally on the socket (the socket is not depicted horizontally) and the socket will be soldered to the 10 pin connector on the left. The switch on the right will have a daughter board to connect it to the 10 pin header on the right. I still need to finish the traces to both headers. The thin traces are audio path and 0.3mm. The rest are 0.5mm.

Cheers
Sono

 

[Khron]

Any chance of a higher-res pair of screenshots? Almost none of the text labels are legible.

And if the point is to move it to SMD, why keep through-hole resistors / diodes / capacitors?

 

[sonolink]

Any chance of a higher-res pair of screenshots? Almost none of the text labels are legible.

Ooops, sorry about that.

Side A: F2-B-Side-A

Side B: F2-B-Side-B

And if the point is to move it to SMD, why keep through-hole resistors / diodes / capacitors?

I kept the anode load resistors as TH because they are rated 2W and to be able to tweak the split load in case I need to adjust the values. I kept the 4 diodes belonging to the soft clipping part of the circuit as TH to be able to use different kind of diodes for different sounds and textures. The idea is to socket these to be able to replace them easily. TH caps are because of Voltage rating basically.

 

[Jen]

Race to the bottom! Why are so concerned about absolute minimum trace width? If you are making 2,000,000 of something, the cost of copper and plating materials might come into play, as we saw in low cost mass produced goods. In the course of my 70 years I have seen the evolutionary transition from point to point components all the way to now. The worst part of that was when being really cheap was job one. I saw hundreds of items made with the narrowest possible traces fail in service thanks to blown up melted traces. They are also far more difficult to do repairs on, even with intact traces, because of the poor adhesion to the board. If you are making an ultra miniature smart phone or laptop/tablet circuit, you have to go small, and watch Louis Rossman make a video about repairing the shitty thin traces and running 32 gauge wire jumpers.. For anything else, stop racing to the bottom.. try to design and build with the idea of low resistance instead of the absolute minimum possible where traces are one breath away from fusable links.

 

[sonolink]

Race to the bottom! Why are so concerned about absolute minimum trace width? If you are making 2,000,000 of something, the cost of copper and plating materials might come into play, as we saw in low cost mass produced goods. In the course of my 70 years I have seen the evolutionary transition from point to point components all the way to now. The worst part of that was when being really cheap was job one. I saw hundreds of items made with the narrowest possible traces fail in service thanks to blown up melted traces. They are also far more difficult to do repairs on, even with intact traces, because of the poor adhesion to the board. If you are making an ultra miniature smart phone or laptop/tablet circuit, you have to go small, and watch Louis Rossman make a video about repairing the shitty thin traces and running 32 gauge wire jumpers.. For anything else, stop racing to the bottom.. try to design and build with the idea of low resistance instead of the absolute minimum possible where traces are one breath away from fusable links.

You're missing the point, sorry. It's not about cost or about the minimum possible width. It's just about if I can use 0.3 instead of 0.5 to be able to FIT certain traces on the board. That's all...

 

[abbey road d enfer]

Race to the bottom! Why are so concerned about absolute minimum trace width? If you are making 2,000,000 of something, the cost of copper and plating materials might come into play, as we saw in low cost mass produced goods. In the course of my 70 years I have seen the evolutionary transition from point to point components all the way to now. The worst part of that was when being really cheap was job one. I saw hundreds of items made with the narrowest possible traces fail in service thanks to blown up melted traces. They are also far more difficult to do repairs on, even with intact traces, because of the poor adhesion to the board. If you are making an ultra miniature smart phone or laptop/tablet circuit, you have to go small, and watch Louis Rossman make a video about repairing the shitty thin traces and running 32 gauge wire jumpers.. For anything else, stop racing to the bottom.. try to design and build with the idea of low resistance instead of the absolute minimum possible where traces are one breath away from fusable links.

Actually, narrow traces do not cost less that wide ones; they are just a necessity when real estate is limited. There may also be performance motivations, such as minimizing X-talk and shunt capacitance.

 

[JohnRoberts]

Actually, narrow traces do not cost less that wide ones; they are just a necessity when real estate is limited. There may also be performance motivations, such as minimizing X-talk and shunt capacitance.

this is an old story but why not... Back last century at my day job, my employer used single sided PCBs that we etched in house. To conserve etchant, our PCB designers were instructed to leave copper everywhere even if not connected to anything.

Some times PCB designers resort to some tricks, such as charging the trace with solder, or even adding a wire.

Back then many of our high current power amp PCB traces had no solder mask so the solder could increase the cross sectional area of traces and lower resistance.

JR

 

[sonolink]

Side A: F2-B-Side-A

Side B: F2-B-Side-B


I kept the anode load resistors as TH because they are rated 2W and to be able to tweak the split load in case I need to adjust the values. I kept the 4 diodes belonging to the soft clipping part of the circuit as TH to be able to use different kind of diodes for different sounds and textures. The idea is to socket these to be able to replace them easily. TH caps are because of Voltage rating basically.

What about my Layout...?

Back at the calculator Khron provided, if I put Current: 1.5A, Thickness 1oz, I get 0.525 mm width on air layers. To get it to 0.3 or less I'd have to use a 2oz outer copper weight...

 

[MidnightArrakis]

What about my Layout...?

Back at the calculator Khron provided, if I put Current: 1.5A, Thickness 1oz, I get 0.525 mm width on air layers. To get it to 0.3 or less I'd have to use a 2oz outer copper weight...

You do what you have to do.....regardless of how you want to do it!!! I once designed a PCB that required the use of 6-Oz copper in order for the PCB to carry >>> 600-Amperes!!! <<< of current!!! This was for a military power-generator. Right at the moment, I do not recall how wide the routing tracks were for that layout, but you can calculate it out using the "PCB Current Trace Calculator".

You may also wish to implement the suggestion someone made previously of placing a piece of 24GA or 28GA wire along top of the current-carrying tracks and soldering it down onto the track. That will help out considerably.

The next step would be to increase your enclosure size so you can increase your PCB size so you can increase the PCB track widths.

The other alternative, which has also been previously suggested here, is to go to a 4-Layer design and use the 2 inner-layers as "Power & Ground" layers. I have done that myself on maybe.....OH-H-H-H-H-H-H!!!.....several -- HUNDRED -- PCB designs!!! It works out especially well when designing SMD circuit boards. I once did a PCB-design for The Dept. of Homeland Security that was an 8-Layer PCB of only 1.25" (31.75mm) square in size and it required 2-Power and 2-Ground layers in order to get that thing routed. I had to use a 4-mil "track and space" setting as there was a 256-Pin micro-BGA along with over 200 "0201-sized" components that were placed on - BOTH SIDES - of the PCB!!! Talk about a "Routing Challenge"!!! That was a tough one!!!

So.....don't be afraid to go 4-layers. (NOTE: Since this is an "audio" forum.....this Homeland Security PCB also had a special IC-chip on it that contained its own microphone within it!!! Obviously, this teeny-tiny little PCB that I had designed was being used for some kind of covert surveillance device)!!! How "COOL" is that?

/

 

[MidnightArrakis]

What about my Layout...?

Back at the calculator Khron provided, if I put Current: 1.5A, Thickness 1oz, I get 0.525 mm width on air layers. To get it to 0.3 or less I'd have to use a 2oz outer copper weight...

[What about my Layout...?] -- I just got around to viewing your newer high-resolution PCB-design images after I had posted my recent reply and I happened to notice that you are using several "vias-in-pads" on your capacitors and resistors. While.....YES!!!..... you can do that, it is also something that is -- NOT -- recommended that you do, especially with you being a novice PCB Designer. Using "vias-in-pads" can cause you to have -- soldering issues -- such as "solder-wicking" and "tombstoning", if you are not careful.

It is recommended that you place the vias just off of the component pads and use a short stub-route to connect the two together. The same goes for routing to your IC-pads. But.....what do I know about PCB-design and routing??? Do whatever you want to do!!!

Should you want to send me your GERBER and N/C Drill file data, I have a special program that can import those files and then I would be able to provide you with a much better analysis. Just make certain that your PCB-design software outputs "RS-274X" data, as it is -- MUCH EASIER -- to import than the older "RS-274" files. The "RS-274" files also requires an "Aperture" output file.

/

 

[sonolink]

It is recommended that you place the vias just off of the component pads and use a short stub-route to connect the two together. The same goes for routing to your IC-pads. But.....what do I know about PCB-design and routing??? Do whatever you want to do!!!

I think I know what you mean and it makes sense. I will correct that. Thanks

Should you want to send me your GERBER and N/C Drill file data, I have a special program that can import those files and then I would be able to provide you with a much better analysis. Just make certain that your PCB-design software outputs "RS-274X" data, as it is -- MUCH EASIER -- to import than the older "RS-274" files. The "RS-274" files also requires an "Aperture" output file.

I only have one export option. I hope you will be able to import it. I've attached the gerbers+N/C Drill file to this post. Thanks again for your help

 

[sonolink]

So I guess it's "Much Ado About Nothing" then.....