I assume that RST, 3v3out and VCCIO are all connected together.
How does the chip get power? I don’t see a connection between VCC and VBUS.
If it’s like the FT232RL, 3V3OUT should have a capacitor for the internal regulator’s output.
I see VCC is fed from VBUS through a fuse element, so I would normally expect this to work.
Do you have your layout available for sharing? I get nervous seeing net labels directly on pins instead of on wires, as it’s easy for a net label to get disconnected from a line as things get moved around.
The fact that you don’t see power on 3v3out makes me think your FTDI is not wired correctly or is damaged.
Thanks for helping all!
@ChrisGammell that’s correct, I followed the example in FT231X datasheet for USB powered operation. Diagram for reference:
.
@phil_from_seattle Apologies if it’s unclear, I went a little crazy with the net labels. It’s connected via the VBUS net label through fuse F1.
@ToyBuilder Here is the layout for the PCB:
One thing I noticed while going through the datasheets again and comparing against SparkFun’s breakout for the same board (http://cdn.sparkfun.com/datasheets/BreakoutBoards/ft231x-breakout-v11.pdf) was that I connected the TX/RX LEDs to 5V instead of the VCCIO pin (normally 3.3V) from the chip. Not sure if this would effect the operation of the chip, but I’m going to desolder those LEDs to see if anything changes.
Oh, wait, you do have a capacitor on 3v3out – you just placed it schematically at VIO and also hooked it up to RST from there…
This is what I have for a FT232RL design. Largely the same, but reset is fed directly off VBUS through a voltage divider; VIO comes from the system’s 3V3 instead of the FTDI’s onboard 3V3 output. The 232RL incorporates the R and C on D-/D+ which are externally added (like yours) on the 231X.
I think your routing needs cleaning up. However, functionally, I don’t see anything that is jumping out at me to explain why it is not working.
5V into the LED… Don’t know your Vf on the LEDs, but it might be possible you’ve put in a few mAs into the chip’s VCC through the ESD diodes. Probably not enough to damage, though?
1 Like
I use the FT231X all the time in both bus-powered and self-powered applications, with the circuits recommended in the data sheet as you show. Never had an issue with one not enumerating on the bus, but I’ve never used USB-C connectors, either.
Running the LEDs to +5V is definitely not a good idea, but abs max for VCCIO is 4V, and you have probably not exceeded that, so as Joseph says probably no damage. Could be driving the chip crazy, though, so I’d pull the LEDs or their resistors and see if it works then.
Random comments on your design:
- Your use of copper floods for ground connections is sub-optimal in terms of inductance and common-mode noise. Much better to use a 4-layer board and get grounds to things like decoupling caps with vias to an inner plane. But probably not the reason your device is not enumerating.
- I don’t see the point of a fuse in this device.
- AC coupling DTR is a weird thing to do.
1 Like
Those leaded resistors are in series, right? So it is 474k instead of 5.1k?
4K7 + 470R. But their junctions do not appear to be soldered…
It’s been quite a while since my last build log post, but finally got some time over the past couple weeks to finish up the Current Sink or Swim schematic + PCB. This one took a little longer since I was spending time trying to understand how everything works, especially going deep into Op-Amps which was a super interesting topic to dig into.
@ChrisGammell, I think there might be a bug with the course, some pages weren’t viewable when logged in, I noticed it on these pages but there might be more:
Some things I did differently:
- I opted to use a fixed output voltage regulator (TPS709) vs the adjustable LM2931 that was used in the video.
- No hierarchical sheets for the schematic.
Here is the schematic:
And a shot of the PCB, note that there is a ground plane on the back which I’ve turned off for this view:
And for fun, the 3D view:
I’m still tweaking the PCB, but should be able to order the parts + PCB by the end of the week. Any feedback is super appreciated!
1 Like
Fun project
One thing you might need is to close the high frequency feedback loop, adding a zero from the output of the opamp to v- (capacitor)
Reason is that you have added a FET to the loop, so it won’t be stable any more
Thanks for letting me know! I have been chasing similar issues with other users and still trying to find the cause of this. I might ping you via DM to find out more about your situation.
Great build so far! I think if I were to do this course over again, i would also skip the hierarchical schematics, as I don’t think it is complex enough to require them.
1 Like
@kvk, thanks for taking a look!
Would you mind elaborating on what you mean by adding a zero? Does that mean connecting the opamp output & v- with a capacitor?
Yes, like described here:
Although in your case you are pulling back on the gain due to the added gain of the FET
1 Like