I am trying to finish a PCB design for an interface board. The board is designed to take 3.3V and convert it to 6V for the Low Noise Amp for a GPS. To do this, I am using the voltage regulator LM622, which needs the circuit laid out in the below schematic to deliver the proper output power.
I am able to get all the other components to route to their respective traces, on the PCB, but I cannot place a trace on pins 5 and 6 on the booster and route it to the 3.3V line that the inductor is on. I have run the DRC and nothing appears wrong, it just wonât connect. I canât figure out what I have not set up correctly. Could someone please offer a few ideas for debugging?
@sroger13 needs to read some application note suggested layouts. Switcher component placement and tracking is critical if you ever hope to pass CE.
Also D4 is huge and L1 looks too small
This is the full layout. I reduced the traces on the diode and inductor (L1) to be 15 mils, while the other traces are the default 20 mils. IT seems like the components are far enough away from each other for thermal relief. The board is meant to take a V TTL signal (6 position header) and convert it to 3.3V, which is the power input needed for our GPS (pin 2 of the longer 20 pin header). The LD117 will convert the 5V input to 3.3V.
The LM2622 converts the 3.3V input from the board to 6V, which is needed to power the GPS LNA. Various LEDs on the board allow you to see when the GPS is transmitting or receiving information to a PC, or when it receives a valid location position. The extra circuitry around the LEDs (270 ohm and 1.0k ohm resistors allow the LEDs to get enough power to operate.
The 6 position TTL header and 2 of the 3 LEDs are then connected to the Tx and Rx lines on the 20 position GPS header in order to send and receive information. Are you suggesting that I need to move some of the components around the LM622 closer to one another or to another location? I understand that a few of the traces are a bit long. Do you have any other suggestions on how this might be best updated?
Here is the schematic, if anything doesnât make sense. Iâve never made one of these before, so Iâve been trying to read up on how to improve on how the schematic can be communicated.
Unusually the datasheet doesnât have a suggested layout, but the linked article on smps layout has more general guidance http://www.ti.com/lit/an/snva021c/snva021c.pdf
You need a closed core inductor, with a high enough current rating not to saturate at any time -startup can be much higher than normal operation as capacitors charge. These are much bigger than the L1 footprint
For more detail on switching power supply layout considerations see Application Note AN-1149: Layout Guidelines for Switching Power Supplies (SNVA021).
And, it is a clickable link.
I think Sarah found the main issue I was curious about. The LM622 has a weird desciption.
With the ability to convert 3.3V to multiple outputs of 8V, -8V, and 23V, the LM2622 is an ideal part for biasing TFT displays.
Page 9 of the datasheet has the formula for setting the output voltage. With the values in the schematic the output voltage will be 8 volts, not the 6 volts specified.
Yes, it IS unusual that the manufacturerâs Data Sheet doesnât show a suggested layout, with accompanying discussion about circulating currents, inductor coupling, radiating loop area, etc. Do you suppose itâs a conspiracy by T.I. execs to make the former National Semi parts look less attractive than T.I. counterparts, by omitting applications guidance from the Data Sheets?
Even the Userâs Guide for the âLM2622 Step-Up DC/DC Converter Evaluation Boardâ ( AN-1198 ) doesnât show anything like a layout. But it DOES include a suggested Parts List. The recommended inductor is Sumida p/n CDRH5D18-100NC. A quick scan of this inductorâs Data Sheet shows that it is MUCH larger than the 1206-package part selected by @sroger13 .
Thank you all for your help! The hardware accepts anywhere from 6V-12V on the LNA pin, so the default layout should be acceptable to use. Is C2 supposed to be that large? That seems a little off to me. I was going to try to find other components
@dchisholm It looks like this is the part that you were referring to?
Alright - after some re-work, I have changed the inductor to be the CDRH5D18 which @dchisholm suggested. I applied the design rules from @davidsrsbâs article as well and put the capacitors acap to the IC. The 5V to 3.3V regulator was moved to the other side of the board to make the power lines less complex and smaller to reduce noise. Should I try moving anything down further than it is? I am using 15mils by the diode, 25mils for the 8V output, and 20mils pretty much everywhere else for my traces, but should I make these larger? The article said to make them as large as possible, but Is there a good size you would recommend for eithre 5V 3.3V or 8V?
I tried to place he inductor at a reasonable distance away from everything, but I took it from the article that this should still be close to the diode? Is the current placement of this alright?
I would appreciate any affirmation or other suggestions you guys could give me. You have all been very helpful!
Is there a reason the parts are scattered on the board?
Why is the board so large?
Why use THT LEDs with all else being SMD?
The parts would only take a board a quarter of the size you have now, probably even less.
One of the first steps of layouting a board should always be to think through where you will have high frequency signals and high currents. You then place the components to what makes sense from this. In cases where you have the combination of high currents and high frequency content you will need to take some extra extra care. A trace will always have some resistance, inductance and stray capacitance which scales linearly to distances. With the current design you will have a lot of current switched at high frequency going through long traces with a huge loop area.Not only will this make the circuit radiate a lot of energy, it will also severely impact the performance and ripple of the boost converter, and since you are feeding a low noise amplifier youâd want the powersupply as clean as possible, even though it might have decent PSRR. Read up on how a boost converter works, understand where the currents are going and place the component accordingly.
Here is an example of a good design, all high current components are connected through short low impedance paths (i.e filled zones, not thin traces)
In general, itâs good to keep power carrying paths as wide as possible and use zones where you can to avoid common mode noise.
There is a tone of information out there on both general guidelines of pcb routing as well as guidelines for boost converters. Dave from EEvblog on youtube is one example of a great source of information, he has done a couple of videos on pcb layout and routing.
One final word about thermal relief which you mentioned previously, normally this refers to cutouts in for example a ground plane around a pad, so that if you reflow a board the solder paste will melt at about the same speed on all pads, preventing tombstoning of small parts. As your parts grow bigger this will become less and less of a problem as their mass will fight against the surface tension of the molted solder. If you are not reflowing parts it is less of a concern, although some thermal relief will make it easier to solder, especially if your soldering iron has limited thermal capability.
Iâm guessing that you were referring thermal relief to spacing the components to that they get enough cooling. The only parts that will have a lot of power dissipation and therefore heat will be the LDO and the boost controller. You havenât specified the current draw on the 6V line, but Iâm guessing it will be in the range of tens of mA, so not very significant. If you want to be sure you could always increase the thermal pad on the ld1117 to get more cooling.
Edit: I forgot your question about voltage and trace width. The width is decided by current carrying requirements, voltage is irrelevant
I suppose the parts donât have to be so far apart from one another. I can fix that. The lower half of the board is for mounting the GPS, which is why it is so large, but I think I might change this to just be a header interface, since the board will be light. I just had THT LEDs on hand, so I figured I could use those. I can find a few to order however. Thank you for your resources. I will rearrange this accordingly
I would suggest you restart this layout from scratch and give a little more thought to component placement. Those two connectors probably do not need to be on opposite sides of the board, routing would be simplified if they were closer together or even side by side. Keep all tracks as short as possible unless there is a very specific reason not to. Many of your tracks are far longer than they need to be. Why do you have so many tracks joining at 45 degrees? I would also consider using the +5V as the input to the LM2622. And change the values of your feedback resistors if you havenât done so already.
But above all else, double check the pinout of the LM2622 footprint!
Edit: Also, the footprint for C2 is much larger than it needs to be, find the part you plan to order and then use the appropriate footprint. Footprints for C1, C3 and C4 are much smaller than they should be. These should be bulk capacitors not MLCC. L1, D4 and C3 should be much closer together and closer to the LM2622, as others have already stated.
Yes, that is the component called out for T.I.'s evaluation board. Inductors of similar construction are available from several suppliers. You have plenty of acreage on your board to accommodate the larger footprint of this part - donât overlook the fact that it is significantly taller than the other parts on your board. I believe Coilcraft has an on-line tool that estimates efficiency of switching supplies for various inductor styles from their catalog.
