0

Which Regulator is used in the VL53L0X module?
Moderators: adafruit_support_bill, adafruit

Please be positive and constructive with your questions and comments.

Which Regulator is used in the VL53L0X module?

by TheAliw1 on Sun Aug 18, 2019 2:19 pm

Hello there,

A question came up when reviewing the VL53L0X module data sheet on the Adafruit site. More specifically page 21 of this data sheet, the "Schematic & Fabrication Print" section.
https://cdn-learn.adafruit.com/downloads/pdf/adafruit-vl53l0x-micro-lidar-distance-sensor-breakout.pdf
I see that the regulator specified on this page is the "MIC5225_2.8v" LDO.

adafruit_products_schem.png
The Adafruit VL53L0X module schematic
adafruit_products_schem.png (61.77 KiB) Viewed 173 times


After consulting the MIC5225 data sheet:
http://ww1.microchip.com/downloads/en/DeviceDoc/mic5225.pdf

I found on page 2 of the data sheet that a 2.8V version does not exist!
2.7V and 3.0V do however exist.

Looking further I found that the VL53L0X chip tolerates voltages from 2.6 - 3.5V.
My question is if I could use the 2.7V regulator safely here as it is cutting it close (perhaps too close) to the lower voltage margin the VL53L0X chip accepts.
Furthermore if I do use the 2.7V regulator does the schematic change at all? Do any capacitor or resistor values change?

What would be even more convenient, if I could use a 3.3V (perhaps cutting it too close to the upper 3.5 limit?) output from a FT232RL USB to serial converter chip I already use in this project. In this case could I just connect the 3.3v from the FT232RL through two 10K Ohm resistors to pin 5, 7 of the VL53L0X chip and 1, 11 with a 0.1uF capacitor connected to ground and skip the voltage regulator and BSS138 N-Channel transistors all together?

I am quite new to PCB design and circuits so please give elaborate answers. Hope you guys can help me out here :-)

Kindest regards,
Alex

TheAliw1
 
Posts: 6
Joined: Sun Aug 18, 2019 1:23 pm

Re: Which Regulator is used in the VL53L0X module?

by TheAliw1 on Sun Aug 18, 2019 3:08 pm

After more time I am pretty sure there is no way around the N-Channel Transistors I think.

I created the following schematic:

The 5V is supplied by an ATMega328P, the 3.3V is supplied by pin 17 of the FT232RL. SCL and SDA are connected to the ATMega328P.

Please let me know your thoughts! Also If this looks good like this, I am not sure!

Screenshot 2019-08-18 at 20.55.25.png
Screenshot 2019-08-18 at 20.55.25.png (411.13 KiB) Viewed 164 times

TheAliw1
 
Posts: 6
Joined: Sun Aug 18, 2019 1:23 pm

Re: Which Regulator is used in the VL53L0X module?

by zener on Sun Aug 18, 2019 3:30 pm

On the ST eval board it appears they are running it on 3.3V, so you should be good there:

https://www.st.com/content/ccc/resource/technical/document/data_brief/group0/4e/4d/0b/66/36/46/4c/63/DM00285093/files/DM00285093.pdf/jcr:content/translations/en.DM00285093.pdf

*****EDIT, on further reading of the above link they mention the satellite board used "2.8V"... so that is where the whole 2.8V business likely started. You could always use the adjustable version of the regulator if you want exactly 2.8V for some reason. I would have to read the actual sensor data sheet to see exactly what they are saying about the allowable Vcc range.

The ATMega328P can run on 3.3V also I think so you could consider using 3.3V for everything.

zener
 
Posts: 4416
Joined: Sat Feb 21, 2009 2:38 am

Re: Which Regulator is used in the VL53L0X module?

by zener on Sun Aug 18, 2019 3:47 pm

Here's the data sheet:

https://www.st.com/resource/en/datasheet/vl53l0x.pdf

It gets more interesting on page 22:

4.2 Recommended operating conditions...

zener
 
Posts: 4416
Joined: Sat Feb 21, 2009 2:38 am

Re: Which Regulator is used in the VL53L0X module?

by TheAliw1 on Sun Aug 18, 2019 4:06 pm

Hi Zener,
Thank you for your quick reply!
I also stumbled upon this data sheet but there is not much clarification in there.
Assuming this range 2.6V to 3.5V I should be ok with the earlier posted schematic using 3.3V right?

TheAliw1
 
Posts: 6
Joined: Sun Aug 18, 2019 1:23 pm

Re: Which Regulator is used in the VL53L0X module?

by zener on Sun Aug 18, 2019 4:23 pm

For me, page 22 of the data sheet raises so many questions that I would want an answer from ST. There is the whole 1.8V "mode" vs 2.8V they talk about there, and if it can run on 3.5V then why are they using 2.8V, and why 1.8V logic on a part that can't run below 2.5V?? I would want a apps engineer to 'splain it to me. Maybe the admins can cast some light on this. For example, if you run it at 3.3V, can the IO take higher than 2.8V?? It seems unclear. ST.com has various support, community and contact options you could use. You should be able to contact an application engineer who is knowledgeable about that part.

zener
 
Posts: 4416
Joined: Sat Feb 21, 2009 2:38 am

Re: Which Regulator is used in the VL53L0X module?

by TheAliw1 on Sun Aug 18, 2019 5:11 pm

Dug deep into the ST Community forums and found that someone brought up the exact same topic as I did.

https://community.st.com/s/question/0D50X0000Awa6k6SQA/vl53l0x-avdd-voltage

3.3V seems to be alright.

Zener if you're still around, does the schematic in my previous post look alright now we know the chip can handle 3.3V?

Thanks for your efforts and help!!

TheAliw1
 
Posts: 6
Joined: Sun Aug 18, 2019 1:23 pm

Re: Which Regulator is used in the VL53L0X module?

by zener on Mon Aug 19, 2019 12:04 am

Very good research! That is the exact kind of answer I like - from the "horse's mouth". That person seems to be an engineer on the design team for that part. That is the kind of info you need.

As far as your design, I can't check every connection... But I will give you the same advice I usually give:

1) Make sure you have enough capacitance on your power rail(s). I see a couple of .1uF. Put a 1uF ceramic on there too.
2) PCB layout is just as important as the schematic. Use bigger traces on the power runs. Use copper fill. Try to have some power plane and some ground plane. Use plated-through holes, and mind your hole and pad size(s). Double-check your pinouts.

Someone else might have other/better commentary on your schematic. It looks basically OK to me. Good luck!

zener
 
Posts: 4416
Joined: Sat Feb 21, 2009 2:38 am

Re: Which Regulator is used in the VL53L0X module?

by TheAliw1 on Tue Aug 20, 2019 4:37 am

zener wrote:I see a couple of .1uF. Put a 1uF ceramic on there too.

In parallel like this?
Screenshot 2019-08-20 at 10.30.49.png
Screenshot 2019-08-20 at 10.30.49.png (49.57 KiB) Viewed 109 times

Could you elaborate a little bit on the use of capacitors or link me to some useful resources? Can I have too much capacitance?

TheAliw1
 
Posts: 6
Joined: Sun Aug 18, 2019 1:23 pm

Re: Which Regulator is used in the VL53L0X module?

by zener on Tue Aug 20, 2019 11:59 am

Yes, that is fine. But the PCB layout and placement of the parts, and caps, is just as important. I would say the next step you should take is lay out your PCB and post a pic of that for review. If you want to learn about capacitors my best advice is search the posts of adafruit_support_mike and search on the word capacitor. He has some very informative posts about that subject and a lot of other things.

zener
 
Posts: 4416
Joined: Sat Feb 21, 2009 2:38 am

Re: Which Regulator is used in the VL53L0X module?

by adafruit_support_mike on Wed Aug 21, 2019 2:05 am

TheAliw1 wrote:Could you elaborate a little bit on the use of capacitors or link me to some useful resources? Can I have too much capacitance?

Debounce capacitors like the ones you're using basically act like rechargeable batteries.

It takes time for current to move through wire, so when the amount of current a load uses changes suddenly, it takes a little while (a few nanoseconds) for power from the supply to catch up. During that delay, the voltage at the load can drop sharply (if the current load increased) or spike to a higher voltage (if the current decreased).

Capacitors store energy in fixed electric fields between their plates. It's basically like blowing air into a balloon: you have to push the air in, but once it's inside, it stops moving. The energy you used to make the air move into the balloon turns into pressure acting on the air that's standing still. Capacitors do pretty much the same thing with electrons.

Formally, a capacitor's value is defined by how much its voltage changes when you send electrons into it or pull electrons out of it at a given rate. A 1 microfarad capacitor's voltage will rise or fall by 1 Volt per second if the current flowing in or out is 1 microamp. If you use 1 milliamp of current, the cap's voltage changes by 1000 Volts per second.

That sounds like a lot, but remember that voltage spikes are really fast.. usually only a few nanoseconds. 1000V/s is 1uV/ns, so a 1uF capacitor exposed to 1mA of current for 1ns will only have time to change voltage by 1 microvolt. If you crank the current up to 1A, the same 1uF cap will only have time to change voltage by 1mV per nanosecond.

That means capacitors are really good at making voltage spikes smaller. The bigger the capacitor is, the more current it takes to make its voltage change, but there's a point of diminishing returns. If you have a 1uF capacitor reducing 1A voltage spikes to a few millivolts, it usually isn't worth the cost to use a 1000uF cap to reduce them to microvolts.

A good rule of thumb is to use 1uF of capacitance for every 1mA of current your load needs.

There's a catch though: all the information above is based on the assumption of using an ideal capacitor. There are about twelve different kinds of capacitor in common use, and none of them are ideal. They all have some amount resistance through their lead wires, and that resistance limits the amount of current that can flow into the capacitor.

If a capacitor's parasitic resistance is 0.01 Ohms, 1A of current will produce 10mV as it flows through that resistance. Even if the capacitor can reduce the 1A spike to 1mV, you get another 10mV across the leads.

Worse yet, all capacitors and wires have parasitic inductance, which is the electronic 'dual' of capacitance. Where capacitors turn voltage spikes into pulses of current that change the cap's voltage slightly, inductors turn sudden changes of current into voltage spikes. A real capacitor's parasitic inductance acts like a barrier that keeps voltage spikes from ever reaching the capacitor.

At some point, the parasitic inductance's ability to keep sudden changes in current from reaching the capacitor will be just as strong as the capacitor's ability to absorb voltage spikes, and any signal moving faster than that will send more energy past the capacitor than the capacitor can absorb.

That's why we put capacitors of different sizes in parallel: a 1nF capacitor can absorb energy from signals that will go straight past a 1uF capacitor, but it can't reduce the size of a voltage spike very much.

It doesn't need to though.. a 1nF capacitor can slow a 1A spike down to a slew rate of 1V/ns. A 33nF capacitor whose parasitic inductance would deflect most of the original pulse can absorb energy from a 1V/ns pulse, slowing it down to 30.3mV/ns. A 1uF capacitor that couldn't handle the original pulse at all can absorb a 30.3mV/ns pulse and reduce it to 1mV/ns. Each smaller capacitor slows the pulse down far enough for the next larger one to handle it.

The point about wire having parasitic inductance is important: a 1uF capacitor a few millimeters from a chip's VCC and GND pins can absorb voltage spikes much better than one a few centimeters away. The PCB traces themselves keep energy from reaching the capacitor, so keep your capacitors as close to the load as possible.

adafruit_support_mike
 
Posts: 58799
Joined: Thu Feb 11, 2010 2:51 pm

Re: Which Regulator is used in the VL53L0X module?

by TheAliw1 on Wed Aug 21, 2019 10:43 am

Thank you for your amazing post adafruit_support_mike!
keep your capacitors as close to the load as possible

Thanks for pointing this out! I wanted to place the VL53L0X perpendicular relative to the main PCB on a small PCB stub with a male/female header as I will be measuring distance in line with the main PCB. With this information, I know now that it is best to place the capacitors on the same smaller stub of PCB as the VL53L0X.
This is how I imagine placing the header:

original:
Screenshot 2019-08-21 at 16.19.22.png
Screenshot 2019-08-21 at 16.19.22.png (115.18 KiB) Viewed 73 times


after header placement:
Screenshot 2019-08-21 at 16.33.47.png
Screenshot 2019-08-21 at 16.33.47.png (89.71 KiB) Viewed 73 times

TheAliw1
 
Posts: 6
Joined: Sun Aug 18, 2019 1:23 pm

Re: Which Regulator is used in the VL53L0X module?

by adafruit_support_mike on Thu Aug 22, 2019 1:04 am

That looks sensible.

Don't put too much effort into making the schematic look like the final board though. The schematic's job is to provide a logical and readable view of how the components work with each other. Whenever possible, it's conventional to put positive voltage at the top of a schematic, GND at the bottom (or the center if you have a negative voltage supply), inputs on the left side, and outputs on the right side.

The layout's job is to arrange the components efficiently on the PCB. The convention there is to keep the long axis of all chips on the same axis, and to arrange things so the traces between components are as short as reasonably possible.

You almost always have to make tradeoffs.. moving some components farther away so you can move others closer. In order of shortest to longest, you want to prefer:

- connections for anything that has an effect on the accuracy of your input or output
- connections that carry the fastest signals
- connections that carry a lot of current
- connections between parts of the same subcircuit
- connections between subcircuits that communicate most of the time
- connections between subcircuits that communicate occasionally
- connections that carry low current
- connections that carry the slowest signals

Debounce capacitors fall in all four of the top categories, so it takes something pretty impressive to shove in ahead of them.

Also remember that all signals need two traces: the signal itself and a GND connection (or a 'balanced' opposing signal for AC applications). The same rules apply to both.

That's why 2-layer boards with a ground plane are so popular. An unbroken sheet of copper has very low resistance between any two points, and the current will follow the shortest possible path. Making GND connections for through-hole components is trivial, and with surface-mount layouts you can drop a via anywhere and bring a GND connection up to the component side. That leaves the component side free for non-GND signal connections.

adafruit_support_mike
 
Posts: 58799
Joined: Thu Feb 11, 2010 2:51 pm

Please be positive and constructive with your questions and comments.


cron