SMD components and track size.

[ThomsCircuit]

My first time using these tiny things. My soldering skills are good. Ive read that 63/37 is a good idea so i have a roll on order. i just need your input on track sizes. In my PCB ive made them as wide as the SMDs leads. Just want to know if i might run into any unforeseen issues. this s a TTP223

 

[eTech]

My first time using these tiny things. My soldering skills are good. Ive read that 63/37 is a good idea so i have a roll on order. i just need your input on track sizes. In my PCB ive made them as wide as the SMDs leads. Just want to know if i might run into any unforeseen issues. this s a TTP223

Best practice is to make the track smaller than the SMD pad. This will prevent solder from migrating away from the pad when soldering the component. If you don't do this, then the track can act like a heat sink and draw solder away from the pad and cause poor solder joints.

I typically use 8 mil tracks for signals unless there is a compelling reason to use larger tracks.

Be sure to perform a DRC on the routed board to verify rules have not been violated.

 

[KeepItSimpleStupid]

#1. Don;t make the traces the same size as the pads.
#2. Don't use a via, hole and component at the same time unless you have to Damage can more easily occur during repair.
#3 Mounting holes (usually unplated thru)
#4 Use a copper pour. It makes the board easier to etch. The tracks would essentially be islands.

63/37 is "BEST" for surface mount stuff. Solidus and liquidus point is the same.
This essentially means you can drag the solder across multiple pins one once you tack the corners.
A wierd technique I used for larger IC's (processors) is to solder them upside down.


60/40 "better" for thu hole

A solder paste and a stencil. See proto-advantage.com for single stencils and squeegees.. The PCB manufacturer can provide stencils for the entire board. An alloy containing Bismuth (Bi) is much easier to use.

 

[ThomsCircuit]

I typically use 8 mil tracks for signals unless there is a compelling reason to use larger tracks.

Be sure to perform a DRC on the routed board to verify rules have not been violated.

it was recommended to make the tracks (on another project) as wide as allowed. Then the DRC was throwing a "drill back off" error so i researched it. Says that "check" is for older machines that manually drill holes. Suggested that it was safe to ignore that error. your thoughts are greatly appreciated. In this modification i reduced the tracks to 10 and voltage rails are 30-40

 

[ThomsCircuit]

#3 Mounting holes (usually unplated thru)
#4 Use a copper pour. It makes the board easier to etch. The tracks would essentially be islands.

i dont understand #3
Yes Copper pours top and bottom. thank you

 

[ThomsCircuit]

I would also like to know what component i could use for a 2 pole jumper. In my PCB i used a few PADs. I thought they were a bit large (85) so i reduced them to 70.

 

[KeepItSimpleStupid]

Mounting holes:

Everything you need to know about drilling PCB mounting holes

Mounting holes seem simple enough—they let you mount your PCB to an enclosure or...

resources.pcb.cadence.com

PTH and NPTH

Plated Through Holes | Non-Plated Through Holes | Printed Circuit Boards | PCB Assembly | PCB Unlimited

Depending on their application, and the design of a Printed Circuit Board, the holes in it can be Plated or Non-Plated. Read this article to learn more of them and how are they used during the PCB assembly process

www.pcbunlimited.com

You "usually" need a way to mount the physical board. A hole, a screw and a standoff. Sometimes newbies forget.

There are edge mountings and there are even locks for the PCB. There are even handle accessories that can be added.
You can put the PCB on a hinged standoff.

 

[KeepItSimpleStupid]

I would also like to know what component i could use for a 2 pole jumper. In my PCB i used a few PADs. I thought they were a bit large (85) so i reduced them to 70.

There is a part with 0.1" centers and square pins, that accept a "shunt". Some of the shunts have handles.
it's best to use 3 pins, so the jumper can be stored.

Shunts and jumpers

Shunts and Jumpers | DigiKey Electronics

Easily search Digi-Key's large variety of through-hole and surface-mount shunts and jumpers by type or supplier.

www.digikey.com

These https://www.digikey.com/en/products/detail/molex/0022284030/313788 can come in a strip of 40 or so pins that you break apart.

You can also make "split pad" where a solder bridge provides the jumper. There are "zero" ohm resistors and single sockets.

You can also use DIP switches.

 

[KeepItSimpleStupid]

In this https://www.electro-tech-online.com/attachments/smt-advice2-png.131993/ pic, the top left hand corner, it would be best to make the trace continuous with a pigtail to the connector pin. The connector, if replaced woud require a lot more effort to do so like it's done now.

It also requires more heat to solder and unsolder.

there is something called a thermal relief. https://en.wikipedia.org/wiki/Thermal_relief It's the lft most pad in the center of the pic. Very difficult to see the spokes.

 

[ThomsCircuit]

make the trace continuous with a pigtail to the connector pin.

as such?

 

[eTech]

it was recommended to make the tracks (on another project) as wide as allowed. Then the DRC was throwing a "drill back off" error so i researched it. Says that "check" is for older machines that manually drill holes. Suggested that it was safe to ignore that error. your thoughts are greatly appreciated. In this modification i reduced the tracks to 10 and voltage rails are 30-40

Holes are still drilled with drills (or slots with routers) ...
But I understand what you mean. Its takes some experience with the tool to recognize meaningful DFM errors.

So...when routing, use a common track width for each signal type (example: PWR=20mil, GND=20mil, Signals=10mil) then stick with the track width for the whole track path unless there is a compelling reason to change the width. You've done this on most of the PCB, but I noticed one track on your PCB where the track was wide and then narrowed(?).

Generally, signals carry a very small amount of current (as compared to pwr and gnd), so 10 mils is fine for those. The exception, for example, would be a driver output. Then this would be defined as a PWR track, so its track would be wider.

Sorry if i got a little long winded, but in general your PCB looks good.

 

[ThomsCircuit]

You "usually" need a way to mount the physical board

oh yes. i will. i have added 4 pads from the PCB design screen.

 

[eTech]

Here is a picture of the header and shunt mentioned in post #8

This shows a 5 pin header with a 2 pin shunt. The shunt jumpers two of the header pins.

 

[ThomsCircuit]

but I noticed one track on your PCB where the track was wide and then narrowed(?).

it was suggested. ill undo all of that. i like your approach better.

 

[KeepItSimpleStupid]

as such?

Yes. The connection has less thermal mass and will be easier to solder and remove if necessary.

 

[KeepItSimpleStupid]

You could re-route the green trace too.

 

[ronsimpson]

The connection has less thermal mass and will be easier to solder

Think about how big most soldering irons are and how small parts are (now days). I don't think mass is a problem.

 

[ThomsCircuit]

#2. Don't use a via, hole and component at the same time unless you have to Damage can more easily occur during repair.

My circuit has 2 SMDs chips as shown. I noticed when i went to connect the ground track the program added a via right on the pad. i did not think that was a good idea so i moved that ground trace to the top layer. I try to avoid using vias but here i see i have to. So what would be best. a via before the pad or just change layers on the pad like i did at the cap?

If i could inquire about another concern. The cap in the circuit. I added one for each SMD. I initially thought the cap was acting as a filter so i needed only one but perhaps it is for the IC and one for each SMD in necessary. I included the original diagram. CAP = 104

 

[KeepItSimpleStupid]

hink about how big most soldering irons are and how small parts are (now days). I don't think mass is a problem.

He has big connectors compared to the rest of the parts. Now, you pretty much need a temperature controlled iron these days. The connectors, you usually never have to replace.

 

[eTech]

My circuit has 2 SMDs chips as shown. I noticed when i went to connect the ground track the program added a via right on the pad. i did not think that was a good idea so i moved that ground trace to the top layer. I try to avoid using vias but here i see i have to. So what would be best. a via before the pad or just change layers on the pad like i did at the cap?

If i could inquire about another concern. The cap in the circuit. I added one for each SMD. I initially thought the cap was acting as a filter so i needed only one but perhaps it is for the IC and one for each SMD in necessary. I included the original diagram. CAP = 104

Use a ground plane (pour) on the bottom side then use the thru hole device pins as "vias" for SMD ground connections.
--or--
Use a ground plane (copper pour) on both sides. Then all ground connects will be made automatically when the pour is applied.

C1 and C2 are "bypass" caps used to stiffen the supply voltage for each IC and should be placed as close as possible to each IC's supply pins. I would use an SMD type cap for C1/C2. 0.100uf is fine but I wouldn't use anything smaller than a 0805 type SMD cap. Smaller caps arn't made to be soldered by humans.