Drawing PCB using EAGLE Software

Discussion in 'The Projects Forum' started by mermerzac, Apr 23, 2012.

Feb 9, 2012
30
1
Hi all!!!

I'm currently drawing a PCB for high voltage application which consists of some IGBT, capacitors, transformer using EAGLE software.
I will solder the components manually onto the board after the board is fabricated.
The voltage and current rating of IGBT is 300V and 15A.

I tried to draw the trace on board file using EAGLE as shown in file attached.
When I tried on larger trace width which is up to 6.4516mm (as the current rating is so high), the width of trace seems to be so much larger than the diode hole.
Will this bring any problem when fabricating the PCB?

Thanks for advice from you all.

File size:
12.9 KB
Views:
42
2. panic mode Senior Member

Oct 10, 2011
1,328
305
on standard pcb 15A is about 12.6mm for 10degC rise or 8.3mm for 20degC rise.

if this is too wide, you can specify PCB with greater Cu thickness.

standard is 1oz of Cu/ft^2 (or 35um thickness) but you can order 2oz, 3oz or even 4oz of Cu /ft^2.
the thicker the copper, the narrower trace can be.

high current traces normally have cloud of bunch of 'satellite' vias around the pin hole for component. they all get plated through which then dramatically improves conductivity between layers, but this can mean having to design custom parts in eagle

Feb 9, 2012
30
1
Thanks for your reply. But I would like to know how you calculate the trace width for different current?
I'm referring to this link to decide on the trace width: http://www.desmith.net/NMdS/Electronics/TraceWidth.html
I'm afraid it is not relevant to my pcb design.

Thanks again!!

4. panic mode Senior Member

Oct 10, 2011
1,328
305
The formula from IPC 2221 is supposedly:

I=K*(dT^0.44)*(W*H)^0.725

internal traces, K=0.024
external traces: K=0.048
I= max current in Amps
dT = temp raise above ambient in deg C
W,H = width and Thickness in mils (taus)

therefore

W = [I/K*(dT^0.44)]^1.38 / H

what do you mean it is "not relevant"? are you doing PCB design or not?
btw, if you are using traces on same board side for D1, there will be overlap...

Feb 9, 2012
30
1
Oh thanks for your reply. What i mean "not relevant" is because i am not sure whether the information from the link below is correct. I use it to calculate for my trace width.
http://www.desmith.net/NMdS/Electronics/TraceWidth.html

And how can we know the thickness of the trace? I am using EAGLE software and when i search for "thickness" on HELP, it comes out with information regarding trace width only.

6. panic mode Senior Member

Oct 10, 2011
1,328
305
i told you - standard PCBs are 0.5, 1, 2, 3 and 4 oz of copper per ft^2

unless you explicitly specify it, it is assumed to be 1oz/ft^2.

smaller PCB shops normally tell you sizes they use, check their website.
here is some random example (check it out and pay attention to Copper Weight):
http://www.custompcb.com/

there are non-standard ones too (anything for \$).

for fine detail PCBs (narrow tracks) one uses 0.5oz because of erosion of copper from sides during etching whcih affects tolerances. the thicker the copper layer, the deeper the "hourglass" eroding.

but thinner copper layer means lower current capacity.

some PCB manufacturers will just use 0.5oz for anything and after etching, use electroplating to deposit more copper to a specified thickness (within a reason).

using information on copper density, and knowing weight in oz, you can get volume of copper per ft^2. relating that to area in ft^2 (1ft=0.3048m; therefore 1ft^2=0.0929 m^2) you can calculate thickness from volume (divide volume by area).

none of this is secret really. if you never ordered any PCBs, check few sites and see what they suggest on PCB design. unless you follow their recommendation, you will be paying higher price.

some restrictions (if you want best deal per \$) are:
- minimum trace width (precision costs)
- number of holes per inch square (tooling cost)
- selection of drill sizes (unless you use what they prefer, additional tooling cost and setup charges apply)
- number of layers (not all shops do 16 layers)
- type of finish (you pay for everything: number of layers, copper thickness, solder mask, color of soldermask, top and bottom silkscreen, density of tracks, testing, finish, board material, goldplating, panelizing, any routing or fancy board shapes etc.)

if you are looking for bargain, and use 0.1" pitch through hole components, there is little sense in making design that requires 3mil tracks, uses bottom side silkscreen, red or black or golden soldermask, etc.

just go out there and read what they suggest, all the suggestions are to make their life easier and your bill smaller.

Last edited: Apr 23, 2012
7. Siggi New Member

Oct 29, 2012
1
0
I knew that this is an old thread, but i had exactly the same problem yesterday and you guys solve my problem. thanks for your advices here. i also used to read some topics in EAGLE Cadsoft Forums, there are also some experts.
bb