Designing PCB adapter: SSOP20/30 to DIP20/30. Need a Glancing over, plz
911 13
korishantalshin 9 months ago
So, I'm using designing an SSOP20 -> DIP20 and SSOP30-> DIP30 adapter boards. The ones on eBay aren't quite designed right from what I can gather. The SSOP20 ones I think would work, but not sure. And there are no SSOP30->DIP30 boards. I want to make clear that I'm creating these PCB adapter boards so that I can plug the TI chips into a breadboard. So, my big question is, can someone look over these files and verify I have them properly to scale and put together correctly? Here's the Datasheet for the two chips: http://www.ti.com/lit/ds/symlink/bq76940.pdf http://www.ti.com/lit/ds/symlink/bq78350-r1.pdf And Gerber/SVG files: https://drive.google.com/drive/folders/1RfmBp-aw6GGOihCcTLQI4TF-DT1vP0XD?usp=sharing Thanks for any assistance. Trying to learn this stuff :) Kori
Comments
andyfierman 9 months ago
If you want the files checking properly, please post the public url to your EasyEDA project. Like this: https://easyeda.com/korishantalshin/New_Project3-58f255f0d89a4bd3ba602185ce189814 * Did you know that you can get low cost, professional quality (i.e. silk screened and plated through holes) PCBs fabricated directly by EasyEDA rather than messing about with films and etchants?
Reply
andyfierman 9 months ago
A quick look at your project shows that the DIP through-holes are not on a standard 0.1 inch pitch in the X or Y directions. Please check and correct against a dimensioned datasheet of the target DIP20 and DIP30 sockets. I suggest that when you lay out the through holes, you: 1. Set the Canvas units to `mil`; 2. either select a 20 pin DIP (and then edit it to create a 30 pin DIP package) from the System library or set the grid snap to `Yes` at `100`mil and manually place the pads; 3. reset the grid snap to some smaller value to adjust the tracks.
Reply
andyfierman 9 months ago
BTW: the TI chips you have posted datasheets for are in TSSOP packages not SSOP. The packages that you have chosen should be OK because they too are TSSOP but they still need to be checked against the TI recommended footprints (for non-soldermask defined (NSD) pads, which is what EasyEDA uses unless otherwise specified).
Reply
korishantalshin 9 months ago
Thanks Andy. I'll make the adjustments you recommend. Learning how to do all this PCB designing is almost as cryptic as learning a programming language (or foreign language, too, I suppose). What made it a little difficult is that the Datasheet shows mm dimensions, and PCB fabrication uses mil. I wasn't quite sure how to use the mil, so I went with mm since I could measure with that.
Reply
andyfierman 9 months ago
You can switch between the imperial (mil, inch) and metric (mm) as you go through the PCB design. You can also reposition the origin to make some of the measurement references easier during construction (though beware that it is not as accurate as it could be when re-positioning it even if the grid snap is turned off). For info: 1 mil is 0.001 inch. 1 inch = 25.4 mm => 1 mil = 0.254 mm DIP and many other packages are based on a 0.1" (100 mil) or 0.05" (50 mil) spacing. More modern package styles are on a metric spacing.
Reply
andyfierman 9 months ago
If you are going to do more complex designs in EasyEDA then may I recommend that you read: https://easyeda.com/andyfierman/Welcome_to_EasyEDA-31e1288f882e49e582699b8eb7fe9b1f :)
Reply
korishantalshin 9 months ago
Thanks andy. I've redone the PCB's and marked them with a 2 on the name. I took a DIP30 for both, and trimmed it down to 10 for the 20pin one. I changed the scale to mil, which did make things a litte easier, since you showed me what it was :) You mind taking another look at the boards? The autorouter works pretty good, but there are some thing it just gets goofy about. Even though the board is set to 45Deg traces, the autorouter ignores that. I had to manually change a few traces to 45Deg because it put in 90Deg traces. There should be an option in the autorouter to set the minimum tracer angle.
Reply
korishantalshin 9 months ago
I'm actually thinking about doing a little redesign. The Arduino Nano is 700mil wide. My current designs are 900mil. So what I was thinking is having Even pins on one side of the board, and Odd pins on the other side. This would allow me to narrow the width to about 700mil. What are your throughts? Also, are my traces still too big? They are set 8mil. What are the widths of the Nano traces?
Reply
korishantalshin 9 months ago
Ok, so I've made 2 more revisions with through holes. Do I have to connect a path from the IC pad to the hole, or could I just put the hole 1/2 under pad? I'll leave the "BQ78350 SSOP30 DIP30 PCB 2 Dbl Layer" with 1/2 under to show what I mean.
Reply
korishantalshin 9 months ago
Ok, so I've redone the "BQ78350 SSOP30 DIP30 PCB 2 Dbl Layer". I think I got it this time :) I had to redo the IC layout for the BQ78350 as it was the wrong dimensions. The pads where in the wrong location for my model chip. I got the BQ78350006, which has .65MM pad spacing. It makes the footprint for the IC larger, but that makes it easier to run the traces, too :) I think I got it this time.
Reply
andyfierman 9 months ago
What has the Arduino Nano to do with a TSSOP-20 to DIP-20 or TSSOP-30 to DIP-30 adapter PCB? Are you saying that you are actually trying to make TSSOP-20 or TSSOP-30 to Arduino Nano adapter PCB? That is not the same thing as a TSSOP-20 to DIP-20 or or TSSOP-30 to DIP-30 adapter. If you want it for an Arduino Nano then you need to find a dimensioned drawing of the pins on that PCB. Or turn an existing PCB layout into a 1:1 image and import that into the Document layer of your adapter PCB as a template from which to lay out your pins. The Tutorial shows how to import an image into the PCB Editor or this: https://easyeda.com/forum/topic/Image_as_copper_zone-ldJDUc6oG and then set the layer to **Document**. **Copper widths:** You need to check the currents being carried by each trace and use an online trace width vs current and temperature rise calculator to decide widths in careful consultation with the TI device datasheets. Note that in your PCBs, 1. you have put text into copper. This is bad practice when you have a silkscreen layer to use. 2. there is no point in putting an outline on the yellow Silk Screen layer because the outline is actually determined by the magenta Board Outline.
Reply
andyfierman 9 months ago
Why are you using the Autorouter when you had already achieved a much better layout - and probably quicker - by hand? It looks like using the Autorouter has messed up what should have been a perfectly direct set of connections that only ever needed to be on the top layer: ![enter image description here][1] [1]: /editor/20180111/5a57266e6b08d.png
Reply
korishantalshin 9 months ago
The nano was only reference, really. I just happen to have it to use as a reference for placing on a breadboard. I noticed the original layouts were quite large width and would of used a good chunk of the breadboard so I was trying to narrow down the board. The nano is 700mil wide and fits perfectly on the center of a breadboard and I am trying to match that small size. The TI chips are tiny, so I don't see why I couldn't. I used the autorouter to see what it would do. I left it last night as it was getting late and didn't get it finished. The autorouter did a decent job on the smaller 20pin board of both sizes. Was trying to get a similar look on the 30pin board, but no go. I will probably end up hand drawing the 30pin board traces. And yeah, I know text with copper traces is bad. That wasn't intentional. I'll be fixing the board later today.
Reply
Login or Register to add a comment
goToTop
你现在访问的是EasyEDA海外版,使用建立访问速度更快的国内版 https://lceda.cn(需要重新注册)
如果需要转移工程请在个人中心 - 工程 - 工程高级设置 - 下载工程,下载后在https://lceda.cn/editor 打开保存即可。
有问题联系QQ 3001956291 不再提醒
svg-battery svg-battery-wifi svg-books svg-more svg-paste svg-pencil svg-plant svg-ruler svg-share svg-user svg-logo-cn svg-double-arrow
We use cookies to offer you a better experience. Detailed information on the use of cookies on this website is provided in our Privacy Policy. By using this site, you consent to the use of our cookies.