Parallel routing of tracks - Page 1
Forum section: electronics / projects

author: Ribster
author_rank: Frequent Contributor
timestamp: June 24, 2015, 09:39:26 pm
content: Hey guys,I'm designing a board that has 2 FFC connectors for pin breakout.Therefor i am routing all my GPIO from my MCU out to those FCC connectors.I know that when passing 2 busses, it needs to be as short as possible, and perpendicular.But somehow, my tracks seem very lengthy, and very susceptable to noise pickup.Can someone with experience give me tips ?Can i add some gnd traces between ~5 tracks to get the crosstalk lower?Is it usefull if a make my traces over a ground plane as much as possible, or is that a no go like with a transmission line..Would love some input, so if you have any..Cheers

author: Tabs
author_rank: Regular Contributor
timestamp: June 24, 2015, 10:30:38 pm
content: a simple change you may wish to try is to rotate U1 through 45 degrees counter clockwise (or even 90). 45 Seems better in my opinion.Place the rotated U1 (at 45 degrees) on the centerline dividing your two FFC connectors. This should let you have most tracks equi-distant (not sure if you need length matching - looks like no).After that, try pin swapping. You seem to have assigned pins to make layout easier, so I'm assuming you can optimise further.Also, do yo want to create a double sided board only? The most effective way for you to reduce crosstalk (if you're worried about it) is by using a ground plane so switch to 4 layers.Worrying about lengths and crosstalk suggests this is hi speed. Would recommend ground plane in that case.The extra layer will help with the routing if you need to keep traced short.You may also consider tenting your vias (I noticed most are not tented).

author: rs20
author_rank: Super Contributor
timestamp: June 24, 2015, 10:37:04 pm
content: Quote from: Tabs on June 24, 2015, 10:30:38 pmWhy? Other advice I've seen on the forum says only tent vias hidden under packages, tented vias make good test points, and PCB software has vias not tented by default.

author: Ribster
author_rank: Frequent Contributor
timestamp: June 24, 2015, 10:48:29 pm
content: Hey Tabs, thanks for the input!This design is a breakout of all the gpio. This makes it easy to change processors. So i can use STM32F0, and switch to F4 with the same daughter board connected via FFC cables.The 45 degree angle seems the best fit.I was considering length matching, and that is possible if the tracks are in the same ballpark. 45 degrees makes that possible.4-layer ups the cost a bit. I'm planning a version with a BGA version, that will need 4-layer.The board is a kind of universal thing. I want to push 8080 interface through the FFC's, also some analog stuff.I'm assuming placing a groundplane is to reduce the return-path? Or does the extra capacitance help, that takes the maximum frequency down i assume..I'm doing the via tenting always at the end. Does this give any benefit?If you have some good appnotes on your mind, that could be usefull too.I'll change the rotation and post an update.I also added the 2 other chips that i've made a breakout for. (not fabbed yet)Can be a good idea to change the LQFP into 45 degrees too..Cheers

author: Ribster
author_rank: Frequent Contributor
timestamp: June 25, 2015, 12:44:17 am
content: This is the new design with the STM32F4 at 45 degrees...

author: tron9000
author_rank: Frequent Contributor
timestamp: June 25, 2015, 08:02:17 am
content: what is it about a nicely routed board to a 45oQFP IC? It just looks more interesting!

author: Ribster
author_rank: Frequent Contributor
timestamp: June 25, 2015, 08:15:59 am
content: Quote from: tron9000 on June 25, 2015, 08:02:17 amI agree. It looks cooler. But they said to me at school that 45° is not good for pick and placing / reflowing..So i try to avoid it where i can..

author: tron9000
author_rank: Frequent Contributor
timestamp: June 25, 2015, 08:28:42 am
content: Quote from: Ribster on June 25, 2015, 08:15:59 amI've seen loads of boards with 45oIC's, I'm sure there are plenty of PCB's houses out there that can accommodate this providing you give them requirements and BOM notes, the pick and place can be set up correctly? not made such a board myself but my experience with 3 PCB production houses I would think they would be quite helpful to produce a board like this.reflowing though - I'm not sure why that'd make any difference, if its been pasted correctly, why would that cause an issue? once you heat it up the solder just "grabs" the IC's pins to the pads regardless of orientation.

author: Scrts
author_rank: Frequent Contributor
timestamp: June 25, 2015, 08:49:16 am
content: - Add ground every 5-7 signals. Your signals have to have a proper current return path.- Leave at least 2x trace width between data lines and clock. Or surround clock with 2 ground signals.- The IC should be rotated counter-clockwise, so the signals would be routed better.You didn't mention the frequency. If it's in kHz range, then it should work anyway.

author: Ribster
author_rank: Frequent Contributor
timestamp: June 25, 2015, 12:26:26 pm
content: Okay, i tried it out. I rotated the MCU. Because the proof is in the pudding, i think this one is better.I'm thinking about length-matching each broken out bank (per 16 GPIO's).I'll also have to add those groundings in between 5~7 signal tracks.The frequency is dependant upon the application.I think driving an 8080 interface will be my main focus. So i'd say about 25-ish MHz?It know it's pushing it. But with length matching, it should be able to hold that kind of frequency ?Cheers

author: tron9000
author_rank: Frequent Contributor
timestamp: June 25, 2015, 01:20:26 pm
content: does the pinout of the connector have to be in that order? cos the pins in the 20's on K7 are looping round each other through vias. If you could re-order the pinout of K7 that could neaten it up a bit? it would keep it all on one side.i know someones asked this already but I couldn't see your answer, apologies if had.

author: Ribster
author_rank: Frequent Contributor
timestamp: June 25, 2015, 01:38:32 pm
content: Hey Tron, thanks for your input!I can choose everything, because i'm designing the MCU boards as well as the expansion boards.As you can see in the attached image, i chose to route the bank out sequentially.This is a choice, to make the expansion boards easy and simple, while complicating the MCU board.I could just route the pins straight out to the FFC connectors, thus moving the problem to the expansion boards.Since the hardware functionality on the STM32F4 is coupled to specific pins on the MCU, and these are mostly grouped by pins on the same bank, it seemed sensible to do it this way.Moving 7 pins back to front, to match the pinout of the MCU, seems a bit silly. Then i'd rather opt for the easy routing of the MCU board.What do you think after this input ?

author: tron9000
author_rank: Frequent Contributor
timestamp: June 25, 2015, 02:50:07 pm
content: Ahh I see, your grouping all of the ports essentially, yeh that's a pretty user friendly way of doing it.I agree, it would seem a bit silly to have them mixed up, and most of them seem to be routed both aesthetically and electrically sound.in which case, ignore my last!

author: T3sl4co1l
author_rank: Super Contributor
timestamp: June 25, 2015, 03:03:01 pm
content: Avoid routing buses over each other (the best way is to cross buses at right angles, so the overlap area is minimal). Always leave open space, above or below, so that ground plane can fill in around them. Stitch the ground wherever possible.Tim

author: free_electron
author_rank: Super Contributor
timestamp: June 25, 2015, 04:35:14 pm
content: Quote from: Ribster on June 25, 2015, 08:15:59 amschool

author: Ribster
author_rank: Frequent Contributor
timestamp: June 25, 2015, 05:20:25 pm
content: Quote from: free_electron on June 25, 2015, 04:35:14 pmI agree. I'm a highschool dropout that got a 'graduaat' (bachelors in evening school) in electromechanics. Now doing my bachelor in electronics.Experience > school, but they go hand in hand.. That's why i'm learning by doing..