Circuit Board Design: Will this work? Thanks!

[jeffserv]

See Picture:

Circuit Board Design: Will this work? Thanks!

For output, I want to use the JP5. This will control 8 relays, via 470 ohm resistor and the DSS4240T (Same as used on Konnect Board); as recommended before. If I set the JP5 to all outputs... and turn on that output, will this work?
_______________________________________

For Input, I am proposing using the 3.3vdc from the Kflop; and simply sending back when I want an input. Should I do more for the inputs, or will this work?

_______________________________________

Thanks so much... This will give me 8 inputs and 8 outputs... which I will use as my main board, for my BlueCNC4 Software setup.

Similar Threads:

• Fanuc 10T keypad/circuit board exchange with 10M keypad/circuit board?
• Need Help!- Printed Circuit Board Design Software
• Need Help c2 sieg mini lathe old circuit board to new board conversion
• Circuit-board, design software.
• Help w/ e-stop circuit design

[TomKerekes]

Hi jeffsev,

That looks reasonable to me. Regarding inputs: connecting JP4 inputs to 3.3V should technically work but may be very noise sensitive. Normally inputs are run at 24V and through opto couplers so that all the wiring is isolated and doesn't couple into the logic.

If you do decide to use 3.3V signals I'd suggest adding a 0.1uF Ceramic Filter Capacitor to GND as close as possible to KFLOP.

HTH
Regards

[jeffserv]

OK, if I go 24vdc with my relays...
Then put in the LTV-846's x 2 and 10K resistors... for the input?
Do I need a PNP version of that chip, in order to switch the 3.3vdc to the Kflop?
Will I need the capacitor, if using that type of Photo Coupler??

Any help would be appreciated...

Thanks,

[jeffserv]

Here is what I mentioned above... should I add a capacitor between IDC-8 and 3?
Will this be good for inputs?

Thanks again...

[TomKerekes]

Hi Jeff,

I don't think that will work. The LTV-847 only has a guaranteed CTR (Current Transfer Ratio) of 50%. That means the output can only drive 50% of the current going in the input (actually even that isn't always true). The input current is based on 24V (ignoring the LED voltage drop) and the 10K

24/10K = 2.4ma

The KFLOP inputs have 150ohm pull down resistors. To pull them up to the required 2.4V would take:

2.4/150 = 16ma

That's about 10X too much. Some type of buffer would be needed.

Regards

[jeffserv]

Hi Jeff,

I don't think that will work.... Some type of buffer would be needed.

Regards

Ok, I see what you mean... I will come up with a buffer setup... and then get a new review. May be a few days... before I can get to it.

Thanks,

[jeffserv]

OK,

Here is a buffer setup for the input to the Kflop...

The LVC chip is 3.3vdc powered and 5vdc input tolerant. Don't know that I need the capacitor... the application note seemed not to show it, if powered this way.

I like the 5vdc board... this allows me to interface a MPG and its buttons... fairly easy.

Thanks again for your time in reviewing this... see new design picture below.

[TomKerekes]

Hi Jeff,

That looks reasonable but:

#1 it looks like you forgot to connect pins 1 and 19 on the buffer

#2 you lost the 24V noise immunity

#3 you lost the optical isolation

#4 those inputs will be very fast (nanoseconds) similar to the original KFLOP inputs. The optos that you had before were relatively slow devices (microseconds) so they inherently provided filtering. So you may need filter capacitors on each input.

Normally you can connect an MPG directly to KFLOP JP4. Even though the MPG is a 5V device it doesn't drive high enough or hard enough to be a problem for the 3.3V inputs. 5V TTL signals are only required to drive to 2.8V.

It would be easier to read if you posted the schematic rather than the layout. And no point of going through the trouble of layout until you finalize the design

HTH
Regards

[jeffserv]

Ok,

Here is a proposed schematic, showing single circuit chips: Photo Couple with Buffer. Let me know if you think this will need any capacitors?

[TomKerekes]

Hi Jeff,

I like that. Except I think you need a pull down resistor at the input of the 74LVC1G125. When the LVT-817 turns off the output will float and not necessarily go low. Maybe like 5-10K. I think you can just GND the /OE signal (no need for a resistor).

I think the LVT-817 is relatively slow (more than 4us) so it will provide enough filtering. But it wouldn't hurt to add capacitors in series with the pull down resistors in case you need them. You can always not populate them.

You should add some power supply bypass capacitors (something like 0.1uf ceramic and 10uF Tantalum) on the 3.3V supply.

HTH
Regards

[jeffserv]

Ok,

I hope this is a good interpretation of what you said above... thanks again for the review...

[TomKerekes]

Exactly

[dgiller]

Just a suggestion... if you're going to make a PCB like the layout in #7, make sure there is space to the right and left of the dual-row header that connects to Kflop JP4. An IDC (ribbon cable) connector sticks over the side (or I guess the "ends"... past pins 1/2 on one side and 15/16 on the other) by at least another 0.1", and preferably 0.2". In the first layout I think the connector would have run into the RJ45 jack, and in the second one, I'm not sure what you would be using to connect the inputs to the board (screw terminals?), but the JP4 header is awfully close to that row of pins. Unfortunately in many cases components stick out past what the PCB program says it will when you drop the part on the board. I am using a shrouded header on my BOB, so it's even a little longer yet, but it uses 0.2" more past each end of the headers... the 26-pin male header on the PCB is 1.6" long. Simple 2-row header footprints in PCB programs are only 1.3" long.

Intuitively your mind wants to believe that a 16-pin header is 0.8" long, but it's actually 1.0" long. And a shrouded header takes up 1.1" on the board (and is 0.36" wide, not 0.2" or 0.3" as you might reason).

Maybe you're not done with layout yet, or know all of this already... I'd just hate to see you get a board fabricated and then have to deal with that highly-annoying problem, so I thought I'd mention it.

[jeffserv]

Thanks Tom, now back to laying this out.

dgiller,

Thanks for that input. I will look at that again, and make sure I have enough room. Maybe change the component drawing to reflect this.

Layout to follow...

Thanks again.

[jeffserv]

Greetings,

Got the new layout, based on the above schematic for Input to the Kflop.

Made board a bit wider, for the extra components. Size is still reasonable, and useful.

I believe this will be it... unless someone see's something else??

See picture below.

[TomKerekes]

Hi Jeff,

Looks ok to me. An reason for using 0.12uF caps instead of 0.1uf ?

Regards

[jeffserv]

I usually buy through mouser, and the .1's are surface mount, but the .12 is Radial... so I can mount them through hole.

Also the .12 was like .60 cents each... whereas the .1 was 2.35 each in the same type. So went with the less expensive one.

- Jeff

[TomKerekes]

Hi Jeff,

Strange. 0.1uF caps are probably the most common and least expensive passive component on earth. We pay about $0.004 for surface mounts

Regards