I barely know what is an arduino. Don’t amadillos eat a lot of arduinos? Or maybe it is the other way around.
2 Likes
@ Robert_Loos: thank You very much for Your valuable time and continuous support to bring this project to the next level. 
I sincerely appreciate Your schematic in the last post. I found it very helpful. 
I updated the topology of the junction terminal & the Shield. Kindly check and give your comments.
I’m not sure: is the grounding of “R3” & “Cap” correct (see point “A”) or shall be somewhere near to point “B” or “C” ? Thank You very much for any kind of help in advance.
Almost perfect, I think. I’m still not sure why there are two pcbs, the green power pcb and the yellow shield which has almost no parts. Can’t they be simply combined? If not, I would take R3 and the cap to the yellow one to bring it closer to the MCU. This reduces the loop area of the connections and thus the induced noise. You may also provide a small cap (a nanofarad or so) at A1 to GND, again as close to the MCU as possible.
If you read Naib’s post, you are surely away from a 3mm track. I would use copper pour in the high current area to create a massive connection between battery and motors. I sketched that in your picture. If you have those pours on both sides, you have twice as much of copper. (But you need a good soldering iron 
)
@ Robert_Loos: Thank You very much for your quick answer and the suggested modifications. Especially the sketch helped a lot to understand a little bit this “black magic”.
“Can’t they be simply combined?” Very good question ! I would like to put a lot of connectors on the Shield, but as per my understanding the high voltage part will disturb the MCU and signal lines (signal GND vs. motor GND) .
Therefore the “all in one” solution can’t be or maybe I’m wrong ?
I would give it a try. If you can keep the power part in one corner of the PCB, separated from the signal and analog lines and put a ground trace or grounded via fence as a shielding between imho it should work. The motor controllers surely have their own filter capacitors so the load is relatively ‘clean’. But 30A and motors are not my daily business, maybe I underestimate their effects. Separate PCBs may also introduce problems because of long wires between them that catch up EMI.
Are the 30 A the continuous current or just the peak? If it just the peak you can get away with much smaller wires and tracks. If it is continuous you need at least 3 mm² wires and the tracks should be as wide as they can (side note: this will make it hard to solder).
johannespfister: Fortunately it is a peek current.
Robert_Loos: Okay, I will put all in one board. The power part will be in the corner.
In addition, I will make 2mm width grounded traces around the power part on the front & back layers.
Those will be connected with 1mm OD & 0.6 drill vias. The vias will be on the traces in approx 5mm distances.
(I hope the above via fence parameters are fine. )
You have to mention this. The requirements will be lower in this case, depending on the continuous current and the duration of the peak. I think everyone assumed you where talking about continuous current.
What is the maximum continuous current and what is the longest duration of the 30A peak?
did a quick FEA for fun… This will mean very little to your project/interest except to indicate what you/user could do… I’ve posted info on FEA Thermal analysis on this Kicad forum, look for it if interested…
Garbage-In = Garbage-Out
Meaning, I threw it together from a few pieces of info from above comments and assumptions
PCB Material = FR4
Trace Geometry: Width=3mm, Length=80mm, Thickness = 70uM
Trace Material = Copper
Temperature, Initial/Ambient = 273º K
Temperature, Final = 333º K Imposed on Trace, only. ∆T=60ºK)
Trace Constrained to X, Y (No Movement in X or Y)
PCB Constrained to No Movement
(Thus, Only the Trace can move in Z direction. Assumes contact pins, vias and process bonding of Cu to FR4 board ignored)
Time of run is for 1 Second
Did not include interest in what happens to the surrounding FR4
Results:
Two Plots (Temperature & Displacement) Plus, one in ParaView without exaggerated displacement
Trace lifts off PCB 28uM (0.028mm = 0.007inch)
Exaggerated in the View for clarity
@ johannespfister: You are right and sorry for this kind of mistake, but honesty say, it is just an estimated value. As present, the things like a chicken egg situation. This is my first design/prototype, so unfortunately I don’t know the actual loads.
This is the one of the reasons, why I would like to measure the current as well.
For prototype we can over-design the traces and later can be optimized.
The rover will be in outdoor application, so later I can log the data and give the actual load circumstances.
@ BlackCoffee: Wow ! I’m very impressed ! Thank You very much !
It meas with 70uM thickness the 3mm width trace is lifting with 0.028 mm.
So I will do definitely some extra soldering with copper wire on he critical traces.
Can you do a favor for me: kindly run the FEA with he following parameters:
105uM thickness, 5mm width trace 10A
105uM thickness, 5mm width trace 5A
I’m very curious: How much will be the lifting ? Thank You for Your help in advance.
@ Robert_Loos: thank You again for Your continuous help and guidance. I made the Shield.
Apart from 12V->5 all in one board.
The 5V come from the Buck converter and I have
3V3 (LM7803) on board regulator.
The reason: thre are 5V & 3V3 logic level MCUs
5V MCU : set buck to 5V and use 3V3 (LM7803).
3V3 MCU : set buck to 3V3 and by-pass 3V3 (LM7803)
I attached some pictures (far from optimum):
As said, “garbage-in = garbage-out”. Thus, it’s all about the input conditions.
In particular, The Max allowable Temperature based on:
• Board material (different suppliers use different materials
• Board thickness = 1.6mm (?)
• Conformal coating covering the traces (type and thickness)
• Other materials close-by that receive heat
• Internal layers underneath/in-close proximity
• Packaging & ventilation…
FEA does only what user inputs
Using the ∆T of 60ºK = 140ºF = 60ºC isn’t bad, I’ve melted plenty of boards using Motor drivers at high power/higher temp’s (230ºF) doing failure testing.
Take a look at the Calculator Tool in Kicad and do some “What-If” conditions to help dial-in what you want.
In the Kicad calculator, you can set and Iterate on concept values(*):
Temperature Rise = 60 C
Current = *
Trace Width = *
Trace Thickness = *
You can use the Formula in a Spreadsheet and dial-in what you want for design…
The following conditions used are:
Trace width = 5mm
Trace thickness = 105um
∆T = 60ºK (Max T=333ºK)
FR-4 board, Cu trace
Board thickness = 1.6mm
(ignore the color blending on PCB, I didn’t bother to reset it…)
@: BlackCoffe: Thank You for the analysis,
I was thinking to make the +12V & GND lines on top and bottom layers and stitch them with vias (see below the traces with red dots).
This can have two advantages:
- Double the cross section of the traces
- Keep the traces stronger together -> less lifting.
But may be, am I causing bigger trouble ?
Drilling holes through the tracks makes them narrower and lessens the available copper and your electrons will get crowded in those area’s.
Use a PCB calculator for the amount of copper you need for your current (KiCad has a built-in calculator 2nd icon from the right in the project manager window. For high currents, more copper is better, but also make sure there are no narrow spots in the tracks such as when drilling holes through them.
Hey, sounds like a cool project!
Looking at your initial schematic, I see no reason why you would route the 30A across the board. Avoid it at all costs, in my opinion. As you can see from the long discussion, it will make your board complicated, expensive, and probably prone to problems.
Instead, you have the option to just use cheap and readily available hardware to connect battery and motor controllers - take a look at either your local hardware store’s electrical department (you will find fuse boxes, banana connectors, heavy duty wire, and mounting fixtures, and can set it up more like a “fuse box”), or your local RC-hobbyist store (you will find XT90 connectors, heavy duty wires, etc, and can set it up like the power distribution of a quadcopter or high performance RC car). Either way, no 30 A traces needed on the PCB…
Note that you don’t lose anything, since your motor controllers will still be connected to your PCB for the control wires…
Another point: the fuses… what are they for? Most motor controllers should include over-current and over-voltage protections, fancy ones have advanced current control. So normally, protecting the motor and the driver from too much current should be a function of the motor controller…
Also, is the 15A a peak value, or the RMS-continuous current? Are the fuses protecting against spikes or continuous over-current?
I’m asking out of interest about your design as I’m also working on a rover type robot…
Regards,
Richard
Agree - realise the high current paths in decent gauge hookup wire and suitable in line connectors. As I said quite a few posts back!
Me too.
High currents through a PCB are a nuisance, they also need big (expensive) connectors, and bigger tools to torque them down, which can result in a lot of stress on the PCB itself. Making a star point for GND near the power supply is usually a more sensible path.
There is one extra thing you have to keep in mind:
If you route the 30A GND cable has a fault (disconnected) then there should be no possibility that the 30A gets rerouted through the PCB in such events. Flat cables and other thin wires release a lot of smoke @ 30A.
This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.