gfxgfx
 
Please login or register.

Login with username, password and session length
logo
 
gfx gfx
gfx
19852 Posts in 1275 Topics by 5182 Members - Latest Member: charbuild March 29, 2024, 09:24:41 AM
*
gfx* Home | Help | Search | Login | Register | gfx
gfx
Breaktru Forum  |  eCigarette Forum  |  Modding  |  Topic: Eagle cad
gfx
gfxgfx
 

Author Topic: Eagle cad  (Read 6413 times)

0 Members and 1 Guest are viewing this topic.

Offline tj138waterboy

  • Full Member
  • ***
  • Joined: Mar 2015
  • Location: Ky
  • Posts: 31
  • Karma: +3/-0
  • Gender: Male
Eagle cad
« on: April 25, 2015, 08:06:59 PM »
Hi guys, just wanted to share a eagle design that I am working on for unregulated mods. Can anyone see any issues with the layout or trace widths?
If I get this figured out I will try to incorporate p-fet for series batt. with all smd parts. Not sure which files to upload so I will post screenshots.

« Last Edit: April 25, 2015, 08:37:57 PM by tj138waterboy »

Offline tj138waterboy

  • Full Member
  • ***
  • Joined: Mar 2015
  • Location: Ky
  • Posts: 31
  • Karma: +3/-0
  • Gender: Male
Re: Eagle cad
« Reply #1 on: April 25, 2015, 09:15:57 PM »

Offline david4500

  • Ultra Member
  • ******
  • Joined: Mar 2014
  • Location: Illinois
  • Posts: 230
  • Karma: +55/-0
  • Gender: Male
Re: Eagle cad
« Reply #2 on: April 26, 2015, 11:46:16 AM »
You have full current going through your fire switch. The traces and fire switch are likely not rated for the current load. The switch is switching the current before the mosfet gets a chance to like it should. The fire switch should be connected to the trace going to the mosfet gate. All of your traces for the atomizer, batteries, drain and source connections need to be the proper width for the maximum current load. Use a trace width calculator to determine that.

You would want your fuses to be between the battery+ and 510+. I'm not aware of any resettable fuses with a 9 amp hold that are available in a 1812 package. Do you have a link or part# for the fuse? They might be quick blow fuses, once they trip they're done for.

For your traces, you have quite a few right angle bends. You should be using 45 degree bends instead. The trace for your resistor going to the GND pad & Source pin comes to a perpendicular/right angle intersection. Create a chamfer there such as shown here http://en.wikipedia.org/wiki/Chamfer#In_printed_circuit_board_.28PCB.29_design. Actually I would just move the resistor to the right so that the right pad is in the middle of the trace, eliminating that intersection all together. Also position components so that trace lengths are shorter.

For your resistor, 2512 is pretty damn big. Try maybe a 1210 or 1206 instead. Although the choice is yours.

You have a power plain on the second layer of your board but it isn't connected to anything. It looks like you plan on securing the drain tab to the board with a screw. I would get rid of that mount. Place pad directly under the drain tab to solder to. You can connect that top pad to that bottom plain you have by placing multiple vias http://en.wikipedia.org/wiki/Via_%28electronics%29. All of that copper will act as a heatsink for your drain tab. Any traces are pads you currently have going to the drain pin, place close to and connect to the drain tab instead (such as 510- and VM-). You can still connect the drain pin to the board put only to secure it.

Consider a surface mount n-fet instead. A properly selected one will have better specs and be much smaller in size. I use this on most of my boards and am able to hand solder it: http://www.mouser.com/ProductDetail/NXP-Semiconductors/PSMN1R1-25YLC115/?qs=sGAEpiMZZMshyDBzk1%2fWi%252bFHavO7hMd5ZCHgcLfhazw%3d

Also your board is dimensionally quite large. Can't imagine it fitting into a decent sized enclosure.
« Last Edit: April 26, 2015, 11:55:24 AM by david4500 »

Offline tj138waterboy

  • Full Member
  • ***
  • Joined: Mar 2015
  • Location: Ky
  • Posts: 31
  • Karma: +3/-0
  • Gender: Male
Re: Eagle cad
« Reply #3 on: April 26, 2015, 01:40:37 PM »
Thanks for the input. I wanted to use smd mosfet but couldn't find n channel d2pak in eagle and tried to make my own for about 3 hours before getting too frustrated.  I understand the using ground plane for heatsink and I thought it was setup to do it that way but I just used the auto route feature after I positioned everything.  Also I know that shorter traces are better but as far as width, I remember someone mentioning oshpark can only do a certain width which is why most people run a solder bead along those traces.  Well I'm back off to redesign this thing and learn more eagle. Thanks for response David. BTW I have ordered one of your boards from oshpark still waiting for arrival.

Offline CraigHB

  • PV Master
  • *******
  • Joined: Nov 2011
  • Location: Reno, Nevada
  • Posts: 2023
  • Karma: +246/-1
  • Gender: Male
Re: Eagle cad
« Reply #4 on: April 26, 2015, 04:22:21 PM »
Yes the library editor can be a real pain in Eagle.  That's a common complaint about that program.  I usually make quick and dirty parts for building boards without setting them up for  the schematic editor as well.  That makes things a lot easier when you don't have to define all the parameters. 

First create your own library file and point to it from the Eagle control panel.  Then when open the library editor either from the board editor or control panel, you can add parts and edit them in the same manner you edit things in the board editor.  There's some non-intuitive button pushes you have to discover to create parts, call them up, and edit them.  There's a bit of hunt and peck there.  Generally speaking, the library editor is probably the biggest point of contention comparing Eagle to other PCB design products.  Though once you get used to the strange way it does things, it's tolerable.

In terms of high current paths, what I usually do is lay down a solder mask along a trace a couple mm wide to allow soldering a bare solid copper wire along its length.  You can use a solder buildup, but the the problem with solder is it only has about a tenth the conductivity of copper.  The conductivity of solder is fine for joints where there's only a thin layer between copper connections, but not so great for extended current paths. 

Offline CUtiger

  • Newbie
  • *
  • Joined: Mar 2015
  • Location: Richmond VA
  • Posts: 1
  • Karma: +0/-0
  • Gender: Male
Re: Eagle cad
« Reply #5 on: April 26, 2015, 06:25:40 PM »
I'm new to eagle as well and navigating the libraries has been one of the hardest parts for me.

If you do some creative searching though I've found layouts for quite a few parts under a different package names. 

For the NXP mosfet linked by David search for "SOT669" and you should find what you need.

Offline tj138waterboy

  • Full Member
  • ***
  • Joined: Mar 2015
  • Location: Ky
  • Posts: 31
  • Karma: +3/-0
  • Gender: Male
Re: Eagle cad
« Reply #6 on: April 27, 2015, 09:04:29 PM »
V1.1 smaller components. Still unsure if ground plane is even being used by the drain/atty- .  I ran 1 trace top and another bottom connecting them as well as naming both wires atm-. I also gave that name to the ground plane. From all trace width calculations I tried, this can handle about 1.2 amps at the smallest trace which is resistor .  Do you usually run trace on top and bottom layer to double current carrying or just use alot of copper wire soldered to the trace on top layer?
https://oshpark.com/shared_projects/TiCThmQg

Breaktru Forum  |  eCigarette Forum  |  Modding  |  Topic: Eagle cad
 

gfxgfx
gfx gfx
Powered by MySQL Powered by PHP Valid XHTML 1.0! Valid CSS!