eelik, I am putting these vias in to connect the front and back of the PCB to allow as much current as possible to flow between the two layers. For that reason, I plan to put a ‘wire’ through the via and solder it on both sides. Thinking about this., vias already connect the front and back so maybe I should just add MANY (like 4-6 per pin) vias with the smallest possible drill hole. Then I don’t have to solder anything. With this approach I don’t have to put a wire through and solder it on both sides.
You can use a footprint with one through-hole pad if you need thermal relieves, otherwise it’s identical to a via when manufactured.
Why “smallest possible drill hole”? Let’s say you have a hole with 0.5mm diameter. The circumference is about 3.14 times that, so it’s almost equal to a 1.6mm track. 0.2mm diameter corresponds to 0.7mm track, which is 0.9mm less, but takes only 0.3mm less space in one direction. So, one 0.5mm hole is much more efficient than 2 0.2mm holes but takes less space. If you add four thermal relieves of 0.2mm they will be 0.8mm together and will be a bottleneck.
If a hole has a good size, it’s easy to solder it through without any wire. But it may require thermal relieves which then are the bottleneck.
Ah, I just posted on the manufacturing page about those vias. For some reason I didn’t see a notification of your post and I figured it’s a somewhat different topic. I tried to delete the post but it seems that’s not possible.
In any case, I look at it from a different way. As you increase the diameter of the hole you increase the ‘track width’ in a linear way (‘track width’ = ~6 * radius). However, you also take surface area away and that increases in a quadratic way (lost area = ~3 * radius * radius).
Having said that, you make a good point about soldering, The hole needs to be wide enough so the solder gets wicked through all the way. What is the ideal size for that?
On the negative side you mention the thermal relieves. Why are they even necessary? Can’t you just leave everything copper and to avoid for the copper to bleed out you expose the copper (none of that green/blue/purple color coating) right around the via. That assumes solder will try to stay close to the exposed copper and not get into areas where there is ‘paint’. Then again, maybe the thermal relieves keep the heat within that small area, i.e. the copper outside the thermal relieve is much cooler, hence the solder does not bleed out.
The copper inside a hole has surface area, too
The minimum depends on the manufacturing quality, I think, and on the tin quality etc. I have a board where all 0.5mm holes can be seen through and take tin, but they may be difficult to solder individually. The upper limit, on the other hand, is so large you don’t have to care. For example normal through-hole component footprint pads are easy to fill.
When you solder with iron the heat dissipates everywhere. It’s difficult to work if there’s large copper area because the actual location and tin don’t take enough heat from the iron. You need a more powerful iron and risk overheating. Thermal reliefs keep the heat in one place, in the pad. Take a thrown away board with large copper area and test.
eelik, thanks for your answers. That actually makes a lot of sense.
I was busy with other things but in the meantime I have come to what I think I can send to production. Here are the screenshots.
As you probably can see, the layout changed a lot since my initial design thanks to all your input. If you see any issues with this latest design then please let me know. Some comments:
- I added a bunch of 4x4 vias to stitch the front and back
- I have quite a lot of bridges (they look like transistors) to create wire connections to increase amperage between copper fields and back/front. I might not use them but at least they are there if needed.
- The mounting pads are not in the most ideal position because the biggest strain will be towards the top where all the cables connect to the panel. I guess I could make the PCB 2cm wider and just put mounting pads on all 4 corners.
It seems like your blocks of 4x4 via stitches don’t actually connect to the copper, but the resolution is too small to see it properly.
Just recenly I saw a nice tutorial here to make via stitches by adding a component with a hole to a net.
A search throws up many results here:
I think the “protip” is the one of the best.
That’s much improved, now close to maximal copper.
- The right side jumpers can move higher, closer to the FETs, like those on the left. Even with wide coppers, you do want shortest-distance too.
- Right most 2 jumpers do very little ?
- 4x4 via clusers do not seem to plane-connect, and the inner vias in those tight clusters probably do little.
An alternative is to use Create-Array to paint rectangle arrays of vias across the whole PCB, and then delete the violating ones.
Not sure the loop-over GND traces above the FETS are a nett gain ? - there is plenty of GND below and those loops subtract from the power copper fill.
Paul & PCB_Wiz, thanks a lot for your input. Indeed the stitches weren’t connected to the copper. I am glad you caught this. I actually followed the “protip” video Paul linked to. What I did differently is creating a “4x4 Stitch” footprint in my library so that I can place in various areas. However, I forgot to set the “Net Name”. Since you can’t change the “Net Name” for the whole 4x4 footprint I had to do this for every single pad. Only towards the end I realized that I could have just done this for one 4x4 footprint and then duplicate that footprint. Duh!!!
I also moved the jumpers higher up and added a few more 4x4 stitches. The jumpers on the very right indeed don’t do anything so I removed them.
As for the loop-over, I had to connect the +12V for the FETs and doing this loop-over was the best/only way I saw (I didn’t like that it takes away from the GND copper field, though.) However, I know have the stitches and jumpers so there are other paths and I removed those loop-overs. Having said that, I am having second thoughts. The lower copper fields provide the +12V (and the top is GND). On the right side I am fine but the left side is of some concern. The top has no continuous connection and only the jumpers connect those copper fields. On the bottom layers the width is somewhat limited due to the chips at the bottom.
So with those changes I have the following including a close-up:
3D Top Layer:
2D Top Layer:
2D Top Layer:
2D Bottom Layer:
2D Bottom Layer:
Top & Bottom Layer:
I see you’ve had a lot of suggestions on layout so I don’t think I can add much there. I am curious as to why the Fets are so far apart. I can’t see a reason in the graphics you posted, however I guess there may be some mechanical reason.
The reason for this post is to show the type of drill I used with my dremel when I was making boards. I can’t remember where I purchased them but perhaps the attached photo will help you find some.
John, the MOSFETs are about 19mm apart. Each MOSFET with heatsink is 15mm wide so it really just leaves 4mm (~1/6") between MOSFETs. Why did I place them 19mm apart? It’s because of my connectors at the top. Each MOSFET needs two connectors and two connectors occupy 19mm.
Thank you for sending the picture of that drill bit. My initial idea was to make my own PCB board and I actually already bought some 3oz copper boards, ferric chloride, etc. I finally decided that it might be better to have this board fabricated. I have some other projects in mind that are pretty simple so I might try to make my own board then. At that time I will have to purchase a drill press and a drill. Since my only Dremel is a sander I might actually consider a Proxxon. The cost will be higher than getting something fabricated plus it requires a whole lot more time but it’s all about the experience…
Now the MOSfets / Heatsinks have been mentioned…
What does that combination actually look like?
The TO220 package was not designed to stand loose, it has long wobbly legs.
It should always have mechanical support.
I see no mounting holes for your heatsinks.
How much heat do your MOSfets have to dissipate?
If it is only a little, then soldering the tabs directly to the copper planes might suffice.
Another way is to put the MOSfets “reversed” flat on the copper with the tab’s up.
Then you can lay a long strip of some aluminimum profile with (almost) the same length as the pcb over it.
If you do this you will need a few holes between the MOSfets.
Put screws from the backside through the PCB (Or put the MOSfet’s themself on the back side) and then make a strong sandwitch of the Alu profile, mosfets and PCB.
FR4 is nasty stuff to drill or work with yourself. The glass fibres are very abrasive for the tools.
I tried drilling it with “regular” HSS drills. You can drill 1 or 2 holes before the dril is worn out.
The drill JohnRob showed are made from (tungten) Carbide.
Ali / Ebay is full with these PCB drills, and you can drill loads of holes with them.
But they are very fragile. You can not use them with a hand held dremel or Proxxon.
You will need an accurate low play drill press.
Have I already said these drills are very fragile and brittle?
Buy them in boxes of 10. Without the right tools you WILL break loads of them.
Drills > 1.2 mm can be used with a hand drill (if a bit carefull / experienced) but the very thin ones… No way.
I’ve had the 0.3mm drills break on me by simply dropping them on the carpet floor.
You also do not want the glass fibers on your hands or on your clothes. They will stick as needles into your skin and are very itcy. Wear gloves, and/or use a vaccum cleaner to suck the dust away.
I have NDP6020P MOSFETs that are driven by darlington transistors (12V input). The MOSFET is logic level with Rds=0.06 ohm with Vgs=-4.5V and 125 degree celcius. I drive I drive about 6A. So in the worst case scenario (100% duty cycle, 125 degrees, etc) that’s about 2W per MOSFET. The heatsinks I use are those small aluminum heatsinks that have pretty little weight. I hope they won’t require some additional stabilization/mountings.
Btw, what drill press do you use?
I forgot about that particular model of heat sink.
These are actually quite good because they provide a lot of support around the TO220 to keep it from wobbling (which may result in metal fatigue and breaking).
The question about the drill press is a difficult one to answer.
I myself have a custom built CNC router, which is not for everyone.
The Drill Press does not have to be very stiff or strong, but it has to be low play. No slop in the axis, and accurate machined stuff is usually expensive.
If you are handy and willing to spend some time on it you can make something fairly accurate with Alumunimum profiles such as MakerBeam and a Dremel/Proxxon
Lineair rails used to be prohibitively expensive, but if yo look at Ali / Ebay / China nowadays they seem to be a good option to make something accurate for a fairly low price.
Quite some years ago I found a picture of a frankensteined “upside down” drill press, which I liked a lot.
The “demel” like tool has a much higher rpm and is much better fit for PCB work than the original.
There is quite a lot of slop in these cheap drill presses, but turning the table upside down creates a “gravity assist” that always pushes the slop to the same side so it wil not hinder you during drilling.
I do not have much confidence in cheap mini drill presses.
This instructable is for such a cheap thing, and he solved it by using some rubber bands to always pull the slop to the same side so it can be used for PCB work:
It’s not the weight that matters, it’s the leverage. - it looks like they have provision for self-tapper securing, so I’d add those holes to the PCB.
Also, clips are far better for attach of heatsinks than screws, if you can find one that uses clips.
I ordered PCBs just before I got the comments about securing the MOSFETs. More about the MOSFETs below. Unfortunately, I messed up. The drill holes for the 8 and 3 position terminals are at least 0.5mm off (they are 1.2mm but probably should be around 1.7mm). In any case, I have some questions about the boards I got. I had several 4x4 stitchings with 0.3mm drill hole, 0.6mm size, all copper layers, solid pad connection. However, the connections seem pretty inconsistent. In most cases there is nothing around the pad so I doubt it makes connection to the copper field. Is that assumption correct? In one case the hole is filled with solder (which I guess is good) but in all other cases it is not (I guess that’s still ok). Also there is a dark area around all the vias. Is that of any concern or is it just something optical?
As for the MOSFET, I don’t quite get what the comment “they have provision for self-tapper securing” means. Some clarification would be helpful. In any case, below are a couple of images of the MOSFET with heatsink. I was going to have the MOSFET a bit above the PCB. That way I can have the jumpers closer to the MOSFET (below the heatsink). In addition, the heatsink is separated from the PCB and won’t transfer any heat to it. However, considering the concerned voiced, maybe I should just have the heatsink touching the PCB which would give it more stability. That means I also have to move the jumpers further down (and anything else below). Any input is appreciated regarding stabilizing the MOSFETs.
I probably will also extend the PCB about 5mm to the left and right so that I can have mounting holes all the way in the top left and top right corner to support the pull from cables wired to the connecters at the top.
That’s likely ok, you can carefully scrape off the green solder mask, and copper should run right to the hole, and then be plated thru.
You can also feed 1-6 Amps into the pcb, and measure the millivolts drop, to get the milliohms of the total paths.
Many extruded heatsinks, have shaped slots that can also accept a self-tapper screw.
The image you posted before looked like it might have those, this latest one rather less so.
Hmm… trying to use the PCB you have already…
- maybe the jumpers can fit from the underside, and trim flush on top.
- Then you can place some mylar+double sided tape, along all the mosfet line, (cut slots for pins) and press heastinks onto that.
You cannot rely on the solder mask for insulation, with the sharp edges of the heatsinks, some quite serious insulation will be needed between them and PCB.
If the heatsink is insulated, you do not need the insulated-package fluff.
You could also look at clip-on heatsinks.
If you were starting from scratch, or want to make many of these, I’d suggest ditch the heatsinks entirely, and lie the fets down - either TO220 or I’d expect you can find smaller SMD packages, for less $$
Spend a few cents more on lower Rds FETS - 6A per FET is not high, but 60mOhms is not great.
If you can drop that to sub 20mOhms, the power drops to < 720mW, 10mOhms is ~ 360mW
Digikey lists P-MOSFETS all the way down to 2.4mOhms.
SQJ407EP-T1_GE3 Vishay Siliconix MOSFET P-CH 30V 60A POWERPAKSO-8 8,984 - Immediate $1.47/1 30V 4.5V, 10V 4.4 mOhm @ 10A, 10V
TSM085P03CS MOSFET P-CHANNEL 30V 34A 8SOP 4,865 - Immediate $0.80/1 30V 34A (Tc) 4.5V, 10V 8.5 mOhm @ 13A, 10V
I’m guessing the self-tapping comment suggests some heatsinks have holes in the extrusion so screws from the other side of the board can hold the extrusion tight to the board so the MosFet leads are not stressed.
Looking at the photo you supplied I’m not sure the extrusion contacting the board is a good idea (I’m sure you know what the extrusion could touch). And I don’t see any holes.
With the board and heatsink as shown, I would add a non corrosive RTV or some other non Rigid adhesive at the base of the heatsink.
The Heatsink below is very similar to your’s, but has a pin pressed into it.
This pin is to be soldered to the PCB for stability.
Your heatsink also has a narrow slot in the middle for such a pin, or for a screw in the same place.
Strangely though, the U slot is only 180 degree around.
Often it is more of an Ohmega with a 270 degree circle for centering the screw better.
As a workaround for you , just solder the jumpers first and then use some filling glue to mount the Heatsinks a few mm higher. You could also add some strips of wood / plastic to fill the gap.
Or you could hollow out the heatsink in the middle to make room for the jumpers.
@mulu In addition to the non corrosive RTV to help stabilize the heatsinks (not too much, you don’t want to cover the radiant surface of the heatsink rendering it impotent) you might also want to slip some sort of tough insulating material between the heatsink and the board. One option that might work well in this situation (thin, tough, electrically isolating, thermally conductive) is mica. Mica sheets are often used as an electrical insulator between active electronics and heatsinks. While is is abrasion resistant, it can be cut and trimmed to shape with scissors. Also, if it is a little too thick, the basal cleavage allows you to peel it apart in layers to get thinner sheets.
You can get sheets of the stuff from McMaster Carr, for not much money. For example, here is a product page for 4mil thick sheets, 3" x 5" for $2.75/ea: https://www.mcmaster.com/#8802k16/=1chtvu8
Looking at the photo of the heatsink installed again I notice a “U” shaped groove. I think you could use a screw through the board into that “U” shaped area to fasten the heatsink. I’m guessing the PCB hole right below it is not for that purpose so a layout change would be required.
BTW Thank you for your post. I am new to Kicad, reading the forum to learn. So I welcome the opportunity to help in other areas.