TSSOP 38 routing problems

Question

Hi,

I've created a dozen or so through hole boards with Eagle (mostly Arduino shields), but I need to create a surface mount board. The DAC I need to use is a TSSOP 38 package (AD5348).

I created a custom library following an online tutorial for the DAC and copied the TSSOP 38 package for a different existing library.

I laid out the board (with the DAC and some op-amps) but the auto route couldnt get past about 75%.

I played for a while, but couldn’t get any further. So, I thought I'd test the part with a simple breakout board. I created a board with just the TSSOP 38 device, fanned out to 0.1" headers.

However, to my surprise, the auto route failed to route this simple board as well. See below. Why would the auto route not be able to fan out this simple board ?

What am I doing wrong ? Or am I expecting too much ?

I'm using the free version of Eagle v6.3.0 with a two layer board.

Thanks.

Jon.

Former Member · Answer

Jon Russell wrote: Files attached. Any advice welcomed (my first SMD board, first TSSOP 38, etc). Ideally I want to understand what I need to do to get the auto router to route this board. I have a couple of iterations I want to make, and I don't want to have to re-route it by hand every time ? THANKS ! Jon. -- To view any images and attachments in this post, visit: http://www.element14.com/community/message/69363#69363/l/re-tssop-38-routing-problems Attachments: DACShield.zip I managed to have it route 100% most of the time. Initially it would route 100% but drop back after the final rats nest as the GND polygon could not reach some pins. Change the normal grid millimetres and set the grid size to 0.1mm Then move the DAC package onto that grid by holding down the CTL key when you click the package. That gets the pins of the DAC chip onto the 0.1mm grid so when we make the routing grid 0.1mm also, the traces will be optimally placed. Then select the autorouter and change the routing grid to 0.1mm The best results were attained with preferred directions for the traces set to none (*) The trace size in your DRC of 10mil is fine and the spacing of 8mil is fine as well these sizes are similar in scale. Try removing the GND polygons initially and let the routing takepalce without them. Then add them. You dont have a board outline on the dimension layer(20) so the GND pour goes to the edge of the board. Decide if thats what you really want. Once done you can see a lot of changes that can be done manually to improve the routing result e.g swapping pins on resistors. HTH Warren -- Viewed / responded via the newsgroup at news.cadsoft.de