DMX2REN design

[Macrosill]

I am in need of converting my ren64s to dmx. I have desgined an all-in-one solution. The Ren64, the way I have it set up is to take in the zc signal via pins 7 and 8 of the input rj45 and 5v power at U1. So I need two connections. In the design below I have tried to emulate that by injecting the zc signal through the Renard rj45 on pins 7 and 8 along with a separate 5v power connection. This required a regulated 5v supply which I tried to configure on this pcb along with a zc circuit.

This is the 1st time I have attempted something like this. I think I got my head around the 3 separate circuits, zc, 5v and control. I would ask all of you to look it over and confirm if it will work. I have attached the pcb along with the BOM in case I have picked a few incorrect components.

As always Thanks for your time.

The BOM is in excel, the pcb is in ExpressPcb as well as a bit map image for those that do not have ExpressPCB.


I still want to add some fuses on the 110v input side of the pcb and maybe on the regulated 5v side.

edit: New pcb attached below, in post #5.

[budude]

Don't know how much 5v power you need but your layout doesn't really allow for a heat sink on the regulator. You may want to free up some space around it even if not using one.

[Macrosill]

In taking a closer look it appears I am going to have to take the supply for the 5v from between the secondaries of the transformer and the zc diodes and utilize another set of diodes to isolate the caps on the 5v side from smoothing out the zc signal. According to the wiki I need .5a for the ren64 using PWM firmware without the leds on the pcb.

I should be able to get a heatsink on after I move a few things around a bit.

[budude]

You may want to move the 5v output away from the mounting hole area a bit or turn it 90 to go out the side - just a liittle too close to it maybe.

[Macrosill]

I re worked the pcb based on the above posts. It is attached below. One thing I am not clear on though is the gnd for the 5v output. I currently have it connected to the CT of the transformer since the + side is coming from the other 2 secondaries. Is this correct? Does the gnd need to be tied to the gnd of the DMX and REN rj45s? Again the ExpressPCB and a BMP are attached.

[P. Short]

This is for use with an XB-rev board, right?

A couple of things (looking at the DMX2REN_3.0.1.bmp file).

It's not clear to me how you intend to bring power and ZC into the Ren64-XB board, since current .bmp file shows a mixture of several different ideas.

Pins 7 and 8 of the RJ45 connector are tied together on the Ren64-XB board, which would tend to short out the power supply on the DMX2REN board.

I think that there should be four diodes on the DMX2REN board. Two of them will provide power to the input of the regulator (as the .bmp file currently shows), and the other two should provide the ZC signal (going to either pin3 or pins 7/8 of J1, depending on how you want to provide the ZC signal to the Ren64).

[P. Short]

OK, now looking at the 3.1.0.bmp...

Most of my prior comments still apply, except that I see that you added the extra diodes.

[n1ist]

I would grow all of the low-voltage power traces. I would also look into a lower voltage transformer to reduce the dissipation in the regulator. It will be dumping a few watts there.
/mike

[Macrosill]

Phil,
So the zc is just a single feed and not closed circuit? So the output of the diodes goes to both pins 7 and 8? Like this?

[P. Short]

n1ist - That is the correct transformer voltage. That particular circuit does not use a full-wave bridge rectifier, rather it uses the center tap as the ground reference. So the input to the regulator is about 8V (6.3V * 1.414 - 0.7V), ignoring the ripple.

Brian - that looks much better. I'm debating whether the ground on the RJ45 connectors should be tied to ground on the DMX2REN board, or whether it should just rely on the ground connections on the Ren64-XB. Perhaps it would be best to make provision on the DMX2REN board for a jumper (or a 0-ohm resistor) between the two grounds, so that you have something that is easy to play around with.

The RJ45 cable (and the power connections, for that matter) from the DMX2REN board to the Ren64-XB should be kept as short as possible to avoid creating electrical disturbances on the DMX cable. I would try to keep that cable under 6" long, even shorter if possible.

I also think that it would be a good idea to add a power-indicator LED to the board, since the board does have 110VAC on it (or perhaps a neon indicator and any required resistor on the 110VAC side of things).

[Macrosill]

Below is the latest revision 3.1.1. It has a fuse for the 110v input, heatsink for the voltage regulator and a shunt to connect the gnd from the controllers to the CT of the transformer. Both the ExpressPcb file and the bmp are attached.

[Virtus]

Not a technical comment but a potential end user simplification... I would change the use of "+" and "-" designations on the AC input connections to "hot" and "neutral" to eliminate anyone misreading/interpreting it.

[Macrosill]

That sounds reasonable.

[Macrosill]

From the lack of any more suggestions I am assuming my layout appears correct and I have chosen the proper components.

[budude]

Just a couple comments on the layout. I'm not sure if you're planning this for a particular enclosure but you may want to move your mounting holes a bit if so since the transformer makes this fairly heavy you'll probably want all four mounts used.

One other thing is the 5V traces - not sure how much current you are planning to carry through the 5v runs but they may be a bit thin if using 1/2oz copper boards. I'd use 1oz copper if you are home etching otherwise boost those up a bit. This (http://circuitcalculator.com/wordpress/2006/01/31/pcb-trace-width-calculator/) is a great trace width/current calculator.

I'm assuming you are using top-entry RJ45 jacks otherwise you'll want to move them past the edge to insert/remove the cables.

[Macrosill]

The mounting holes are to fit a particular enclosure.

The 5v traces are .02 inch on 2oz copper. They need to carry between 500 and 1000ma. The .02 trace should be capable of carrying 2.1 amps with a 10c rise in temp.

Yes, vertical rj45s all around.

[DynamoBen]

...I'm debating whether the ground on the RJ45 connectors should be tied to ground on the DMX2REN board, or whether it should just rely on the ground connections on the Ren64-XB. Perhaps it would be best to make provision on the DMX2REN board for a jumper (or a 0-ohm resistor) between the two grounds, so that you have something that is easy to play around with.


A DMX receiving device's shield/common should be floated and not tied to common. A DMX transmitter grounds (AC ground) the shield for the entire system, which prevents ground loops.

[scorpia]

Brian,

looks like you are makign this board so it cant be easily made at home, fair enough, but a couple of simple changes would make it possible,

running the ground trace though the middle of the DMX out RJ45 makes it pretty hard to make at home. i would run the ground vertical parrallel with R2 and then add a second jumper to get it to the ground trace between the next two rj45's.

also i would assume 1/2oz copper or at best 1oz. assuming 2oz makes it a hard board to make. and being that the extra copper costs money i think you will find slightly wider 1/2 oz or 1oz traces would be easier.

As for the fuse it looks like you have added a fuse like in the classic SSROZ board. the only issue with those is the height. but being it is beside the transformer then it shouldnt be an issue. you might want to talkt o WJOHn about the hole spacing he uses due to the different fuses available in the states and here in aus. While you looking at that side i would add some more width to the AC side as well. you never know who might want to run 240v though this board. oh and keep an eye on the track spacing. should be fine but now is the time to think about it.

anyway thats something to think about

[lbro]

Okay, here is a question, can I use this board with 595's? Trying to look at ways to still use them.

[Macrosill]

Brian,

looks like you are makign this board so it cant be easily made at home, fair enough, but a couple of simple changes would make it possible,
I am making this board for me to etch at home.


running the ground trace though the middle of the DMX out RJ45 makes it pretty hard to make at home. i would run the ground vertical parrallel with R2 and then add a second jumper to get it to the ground trace between the next two rj45's.
I have done it b4


also i would assume 1/2oz copper or at best 1oz. assuming 2oz makes it a hard board to make. and being that the extra copper costs money i think you will find slightly wider 1/2 oz or 1oz traces would be easier.
I only have stock of 2oz copper so that is what I use.


As for the fuse it looks like you have added a fuse like in the classic SSROZ board. the only issue with those is the height. but being it is beside the transformer then it shouldnt be an issue. you might want to talkt o WJOHn about the hole spacing he uses due to the different fuses available in the states and here in aus. While you looking at that side i would add some more width to the AC side as well. you never know who might want to run 240v though this board. oh and keep an eye on the track spacing. should be fine but now is the time to think about it.

anyway thats something to think about
I have about 50 of those fuse holders so I am using them. I will only be running 110v on this board.

Again, this is not a coop board, just a pcb I need as a solution for my current hardware and future direction. But those are all valid points if this was going to be made by others. I can incorporate all of those things into a new file if others will use it, provided my layout and BOM will work.

[ErnieHorning]

Everyone seems to want to use small traces. Even though I usually mill my boards, the reasoning is still the same.

The fatter the traces are, the less copper you need to remove. In my case, the tools last longer and your case the etchant last longer. The cooper is basically free. Fat traces have minimal heat rise and resistance. I also try to flood my board with the ground potential. This also leaves more copper and shields noise.

I try for best and hope for less problems.

[scorpia]

very true ernie,

i do like the idea of why run a small trace when a thicker trace will fit.

for home etching thicker traces allow more room for error. if you over etch or your resist didnt quite work then you have alot more room for error. just because you can etch traces down to .01 or what ever doesnt mean that you should try to when you dont have to.

Brian,

im sorry i though the idea was you were getting some of these boards made. If you are only expecting them to be made by you then you can ignore alot of what i said. but having said that i do like the idea of allowing for 240v mains voltages on any design shown here as one day im sure someone will copy it without knowing what they are doing for there own design.

also with regards to the trace though the RJ45. as i said, it would make it easier to etch at home if it wasnt run though the center, i didnt say it couldnt be done. the clearences are very small once you start doing things like that. but if your happy that you can do it then great.

btw as a general comment its good to see more people playing around with different designs, this was something this site was missing for a while there.

[Macrosill]

I plan on etching the boards later tonight or tomorrow. I have ordered the BOM from mouser. A couple pieces are on back order so I will have to wait to test this.

I may make some traces thicker and add a ground plane.

Thanks for all the suggestions, 2 or more heads are better than 1.

[Macrosill]

I just made some more tweaks to the pcb. I made the 110v traces .100 wide. I made all the other traces .030 wide. I added a second jumper to eliminate the trace in between the pads of the rj45. I also added a large ground plane. I made the clearance around the traces and pads .020. The ground plane is not currently connected to anything, it is just floating. Should I connect it to the CT or the transformer, which is the gnd reference for the 5v output or the dmx gnd? I think it should go to the 5v gnd but wanted to ask to be sure. I also moved the mounting holes so I could flip the board orientation in the enclosure. It made for a neater wiring layout. Let me know what you think. The ExpressPcb fila and a jpg are attached for your viewing pleasure. Thanks again for all the input.

[Wayne J]

that will etch faster

[DynamoBen]

Should I connect it to the CT or the transformer, which is the gnd reference for the 5v output or the dmx gnd?

The data side of DMX shouldn't have a ground.

[ErnieHorning]

The ground plane should have the best connection to the 5 volt regulators ground and the capacitors that are filtering it. This is what makes ground quiet. Think of the ground plane as a big lake and noise as waves. The bigger the lake, the less that waves will have any affect on it.

[budude]

You may want to leave a bit more gap between the ground plane and the pads because I can already hear the cussing when you create your 15th solder bridge... :rolleyes::p

I'm not sure a ground plane will have a large effect around the DC components of this but then again it can't hurt either...

[Macrosill]

After the suggestions above and a conversation with Wayne James I have the latest revision for review. I have made the clearance around the traces and pads .030". I have eliminated the gnd trace and connected the gnd pads via the thermal pad to filled plane option. I have also connected the regulator heat sink to the gnd plane. I also eliminated the gnd plane from the area around the 110v traces. I also added the gnd plane in the area below the rj45 jacks.

[ErnieHorning]

I use ground clearance of 20 mils if I have the room and 15 mils if I need the space. I find that typically the pad will heat up and wet before the ground place can heat up enough to even melt solder. It can happen and has but I’ve found that I can re-heat the pad and break the connection. If not then solderwick the ground and remove the excess. Of course when I’ve purposely wanted a bridge, I couldn’t and had to add wire.

I guess it depends on your soldering skills. I’ve only met one guy that couldn’t do it, but I swear that he couldn’t solder a fender on a car either.


During writing this, you’ve increased the clearance to 30 mils and it’s next to impossible bridge the solder, even you want to.

Looking at your new layout, the only question is at the mounting holes next to traces. It depends on what you’re using for standoffs but looks like a potential short if they’re metal to a metal case.

[Macrosill]

I have moved the traces away from the 2 mounting holes in the ground plane. Again a .jpg and the ExpressPCB file is attached.

[ErnieHorning]

I’m not using ExpressPCB so I’m just going by the pic. Verify that R1 and jumpers have the right size holes, they just look smaller that the rest, no other reason.

The rest looks good as far as layout; I’m assuming the connections are right.

[Macrosill]

Ok, then the design is complete, maybe. Thanks again to everyone.

[Macrosill]

On a side note, once I etch and test the design I will be uploading the ExpressPCB file along with the pdf of the bottom copper and mirrored silkscreen for printing to the
File Library (http://www.doityourselfchristmas.com/forums/dynamics/index.php)

[Macrosill]

The etching should begin tomorrow. Had a small toner issue.

[Macrosill]

Update : 6 pcb's etched

[Wayne J]

Update : 6 pcb's etched

What, no pics????

[fkostyun]

http://www.striped-bass.com/Stripertalk/images/smilies/this_thread_is_worthless_without_pics.gif

[Macrosill]

OK, OK, here are some pics. Now I have to go solder!

[Wayne J]

Looks great!! Post some pics when they get populated too!

[Macrosill]

Patience my good friend. Here it is minus the rj45s and heatsink that are on back order from mouser. Oh, and I screwed up, I accidentally deleted the 5v power connection from my cart when I placed the order.

If it works or not is a different story.

[Wayne J]

I don't like it..... make it again.














LOL J/K Looks great, can't wait to know how it works.

[Macrosill]

Well the planets finally aligned themselves yesterday. The converters are functioning properly. They are a success! I now have a single enclosure containing a ren64 xb, zero cross, 5v psu, dmx passthru and termination all in one box. Pictures to follow.

I am using RPM's dmx dongle, my REN2DMX board with Ren64 xb boards. 320 channels worth. I still need to convert my Ren24s to dmx and I may stick a Ren SS16 in there if I need the extra channels. Almost 400 channels of DMX blinky flashy.

[lbro]

I don't like it..... make it again.














LOL J/K Looks great, can't wait to know how it works.

LOL that was great!

Great job Brian, glad to see you worked this out for yourself.

[Wayne J]

Great job!

Now... get some sequencing done!

[scorpia]

Well the planets finally aligned themselves yesterday. The converters are functioning properly. They are a success! I now have a single enclosure containing a ren64 xb, zero cross, 5v psu, dmx passthru and termination all in one box. Pictures to follow.

I am using RPM's dmx dongle, my REN2DMX board with Ren64 xb boards. 320 channels worth. I still need to convert my Ren24s to dmx and I may stick a Ren SS16 in there if I need the extra channels. Almost 400 channels of DMX blinky flashy.



nice work,

now do you have any pics? i would like top see a completed box.

thanks

Peter

[Macrosill]

I just put the camera away, took a pic of the ssr boards I have for sale. Give me a few minutes.

Picture added.

[Snowmizer2]

So would this would with any Renard board?? would be intested in converting my SS24's to DMX

[dirknerkle]

Brian,

Did you ever post the final PCB file? I can't find it in the file library. Also, the last picture doesn't look like the completed board. It appears as if there's a D3 in the layout but not in the finished etching.

I'm just curious -- this could be a neat board for folks to have!

[Macrosill]

hmm, not sure. I will look into it and let you know.

edit:

You are right, I never did post the final layout. Good catch on D3.

Here they are.

edit 2:

All files uploaded to the file library under the Copper category.

[dirknerkle]

Thanks, Brian! You're the best! :cool:


-dave

[Macrosill]

My pleasure. Thanks for catching me on this one. I hate it when I read threads and they end result is never posted.

[Jrd]

Great design Brian, but how do you keep the Renards from using the same channels over and over again? I do not remember the Renard DMX firmware being addressable.

[budude]

Great design Brian, but how do you keep the Renards from using the same channels over and over again? I do not remember the Renard DMX firmware being addressable.

The DMX code is addressible - it defaults to '1' - I haven't had a need to use that yet but it will probably come up sooner or later - especially if something wireless comes up for it.

[Macrosill]

Pic code addressing. Each Ren64 board is addressed. The board with channels 1-64 gets all the pics programmed with a start address of 1. The board with channels 65-128 gets the 1st pic programmed with the start address of 65 and the rest of the pics on the board get programmed with a start address of 1. The board with channels 129-192 would get the 1st pic programmed with a start address of 129 and the rest in the board would get a start address of 1. Then so on and so forth. Only the 1st pic on the board gets a start address, every other pic gets a start address of 1.

You can have 2 controllers do the exact same thing by addressing them with the same start address.

Here is the line in the code:

#define DMX_START_ADDRESS 1

I believe it is line 53.

[Jrd]

Ahh I see, thanks.