latigid on Posted January 10, 2016 Report Share Posted January 10, 2016 I'm working on a sort of hybrid DINX6/DOUTX4 board and I have a question on how to treat SC and RC. The BLM is proof that chaining the clock works even when the DIN/DOUT parts are not equal in length. But on DIN/OUTX4 boards sold by SmashTV normally one splits the J8/9 ribbon with an intermediate header. On this board I have the choice to go serial or parallel, so I wonder what the best way is, or if it really matters. Many thanks, Quote Link to comment Share on other sites More sharing options...
TK. Posted January 10, 2016 Report Share Posted January 10, 2016 It does matter! It's important that DINs and DOUTs are chained separately. At the "output port" (J2) the SC line of the longest chain (in your case: DINX6) should be available, RCs are separate anyhow. Best Regards, Thorsten. Quote Link to comment Share on other sites More sharing options...
latigid on Posted January 12, 2016 Author Report Share Posted January 12, 2016 Good to know, thanks again. But RCs on J8/9 are common, perhaps you're thinking of J19? Interesting to note that the SEQ PCB doesn't follow this practice. SC and RC are directly connected from header to header. Quote Link to comment Share on other sites More sharing options...
Hawkeye Posted January 12, 2016 Report Share Posted January 12, 2016 Hm, that (and the lack of sleep ;-)) explains my confusion a few weeks back :-). RCs on J8/J9 do come from different 74HCT541 pins, but... while "beeping through" connections from the core to the SEQ CS, only 6 connections (single RC line) were needed to wire up the SEQ CS, but 7 connections (two RC lines, that are common on the SEQ CS board, but I did not know that then) to wire up the TPD :-). Does it have something to do with the maximum possible serial chain length? Wilba (SEQ CS PCB) connected the RCs, Ilmenator (TPD PCB) kept them separate... Does it make no difference or was it just a violation of well-established norms and standards? :-) Many greets, Peter Quote Link to comment Share on other sites More sharing options...
latigid on Posted January 12, 2016 Author Report Share Posted January 12, 2016 Interesting! I was referring to the SmashTV DIN/DOUT boards and the Core8 module, which I remixed for the BLM. It may be a good time to consider _NG modules for the 32-bit Cores. Quote Link to comment Share on other sites More sharing options...
Hawkeye Posted January 12, 2016 Report Share Posted January 12, 2016 No problem :-). Probably within software, the output pins 13/Y5 (RC1 on J8/9 the STM32F4 board) and 14/Y4 (RC2 on J8/J9 ofthe STM32F4 board) of the '541 are switched in unison/at the same time, but I also have the strong feeling, one should not connect the RCs in the serial chain :-). Many greets, Peter Quote Link to comment Share on other sites More sharing options...
TK. Posted January 17, 2016 Report Share Posted January 17, 2016 In the past J8/9 RC1/RC2 was a common line at the core (MBHP_CORE_PIC, MBHP_CORE_STM32), but always routed as separate lines at DIN/DOUT PCBs. With MBHP_CORE_LPC17 and MBHP_CORE_STM32F4 I introduced separate RC1/RC2 lines at J8/9 core side for future enhancements. This feature isn't used by MIOS32 yet (it just sets both pins at once), but it could be used in future for whatever reason. Best Regards, Thorsten. Quote Link to comment Share on other sites More sharing options...
latigid on Posted January 17, 2016 Author Report Share Posted January 17, 2016 Okay, actually the r5 boards I've got both share RC (bottom pins on the 2*5 connector) but it makes sense to change the convention. Quote Link to comment Share on other sites More sharing options...
latigid on Posted February 2, 2016 Author Report Share Posted February 2, 2016 Here we go: This was my best solution to routing up the DINs. Looks like it will be possible to make a "mini-DINX4" at around 50*50mm in the future. Quote Link to comment Share on other sites More sharing options...
Zam Posted February 2, 2016 Report Share Posted February 2, 2016 Hi Is that a work in progress? because i'm not sure about your ground plane (bottom?) As side note, if you are looking for smallest possible pcb and low profile, I successfully use micromatch connector for my system, still 100% compatible with actual MBHP wire specification, you can have micromatch at one side of the ribbon and header at other side. Best Zam Quote Link to comment Share on other sites More sharing options...
latigid on Posted February 2, 2016 Author Report Share Posted February 2, 2016 Could you be a bit more specific about what you don't like about it? It should be possible to mirror the 5V trace to allow a a solid connection back to the supply, but it's always a toss-up between as few vias/layer changes as possible. Quote Link to comment Share on other sites More sharing options...
Zam Posted February 2, 2016 Report Share Posted February 2, 2016 I think I just understand...74HC165 and pull-up resistor in smd package (which I completely miss) are superimposed. It looks better then For what kind of device are the driver/buffer for ? Best Zam Quote Link to comment Share on other sites More sharing options...
latigid on Posted February 2, 2016 Author Report Share Posted February 2, 2016 Did you mean the 2981 chips? They will provide level-shifted gates as part of a MBCV v2 control surface (here). There could be other uses though, like a more generic NG build. Quote Link to comment Share on other sites More sharing options...
Zam Posted February 2, 2016 Report Share Posted February 2, 2016 Hi Yep the 2981 Tks for info, it make sense Best Zam Quote Link to comment Share on other sites More sharing options...
latigid on Posted February 3, 2016 Author Report Share Posted February 3, 2016 Well, it's still not too clear what you were proposing about the ground plane, but I changed it anyway . Quote Link to comment Share on other sites More sharing options...
Zam Posted February 3, 2016 Report Share Posted February 3, 2016 Hi yes I was not clear because I don't clearly get the layer :) My first thinking was top layer=ground plane Some observation: -At hc595 power distribution, maybe it's better to connect first to caps, then to pin 16 -The remaining 5V trace at bottom layer between the two 165 can bee traced easy at top layer, like you do for other with half din trace at bottom layer -You can simplify rc/sc/so chain at 595. All trace have angle at some point, most of them can be axed X at bottom and Y at top. Also you have some room to move digital trace more left by one or two steps, this will reduce the bottom trace at ground plane -RC line at lower 595 to J8/9 can maybe use the same "pattern" as other ones with X bottom trace, an then top trace (via) // all other digital line. This will reduce a lot the long trace cutting ground plane Just some ideas Best Zam Quote Link to comment Share on other sites More sharing options...
latigid on Posted February 4, 2016 Author Report Share Posted February 4, 2016 Thanks for your feedback. Some thoughts in reply: 20 hours ago, Zam said: -At hc595 power distribution, maybe it's better to connect first to caps, then to pin 16 I see what you mean, but that would involve a layer change of either +5V or the caps. At the moment the IC pin/socket acts as a conduit. 20 hours ago, Zam said: -The remaining 5V trace at bottom layer between the two 165 can bee traced easy at top layer, like you do for other with half din trace at bottom layer It adds a few vias, but I think you're right. I was wondering whether a plane break would actually help to decouple the longer signals running to J8/9A 20 hours ago, Zam said: -You can simplify rc/sc/so chain at 595. All trace have angle at some point, most of them can be axed X at bottom and Y at top. Also you have some room to move digital trace more left by one or two steps, this will reduce the bottom trace at ground plane Not a biggie, but I straightened them. But moving the traces to the left means SC starts to intercept the isolation for the caps = plane break. 20 hours ago, Zam said: -RC line at lower 595 to J8/9 can maybe use the same "pattern" as other ones with X bottom trace, an then top trace (via) // all other digital line. This will reduce a lot the long trace cutting ground plane This would have intercepted the +5V line, but I found another way around. Again, I appreciate your input. Best, Andy Quote Link to comment Share on other sites More sharing options...
Recommended Posts
Join the conversation
You can post now and register later. If you have an account, sign in now to post with your account.