Schematic Review Rev 4 PDB

Owned by Farris Matar
Last updated: Aug 21, 2022 by Ari Wasch
13 min read

 

Part Reviews

Reviewer Name

Manufacturer Part Number

Sheet Number

Symbol Name

Footprint Name

Comments

Reviewer Name

Manufacturer Part Number

Sheet Number

Symbol Name

Footprint Name

Comments

<Reviewer Name>

<Part Number>

 

<Symbol Name in Schematic Libs>

<Footprint Name in PCB Libs>

  • Every single new part that was used in the PCB and added to the libraries must be reviewed by both the designer and one other person, following the Part Review Checklist. This can be excepted for ceramic capacitors and chip resistors

  • If the reviewer notices any problems with the symbol or footprint, comments should go here, and the problems will need to be resolved by the designer

@Paul Kokhanov

UT336M100HGKTA

SH2,SH3

CAP_33uF_100V_ALUM

RADIAL_Aillen

Schematic

  • Maybe merging issue but footprint is not linked

  • Manufacturer Part Number different in Parameters then one listed here in table

  • No Supplier Link

Footprint

  • The footprint name as listed here is not following the footprint naming convention in the library.

  • Corner Radius for Pads should be 15%

  • Assuming ~10mm wide A1 (as per datasheet), need:

    • Pad Y-value to be ~3.2 mm

    • Pad X-value to be between 0.7-1.3 mm

    • Separation between pads should be ~4.7 mm

@Paul Kokhanov

UT476M100HGKTA

SH2,SH3

CAP_47uF_100V_ALUM_1

RADIAL_Aillen

Schematic

  • Maybe merging issue but footprint is not linked

  • Manufacturer Part Number different in Parameters then one listed here in table

  • No Supplier Link

Footprint

  • See above comments for footprint

@Paul Kokhanov

TPSD157K016R0060

SH2,SH3

CAP_150uF_16V_TANT_1

CAP2917

Schematic

  • Manufacturer Part Number different in Parameters then one listed here in table

Footprint

  • No Slikscreen visible

  • As per datasheet, need:

    • Separation between Pads 4.40 mm

    • Pad X-dim 1.3 mm +- 0.25 mm

    • Pad Y-dim 2.4 mm +- 0.2 mm

 

@Ari Wasch

TPSD226M025R0100

SH2,SH3

CAP_22uF_25V_TANT

CAP2917

Schematic

  • Get rid of design part number

  • Include digikey part number

Footprint

  • Looks good

@Logan Hartford

MWLA1707S-100MT

SH2,SH3

IND_10uH_16.5A

Inductor MWLA1707

Schematic

  • Missing supplier link

Footprint

  • Not following the library naming convention

  • Should add a lines on top overlay layer to show the outline of the 3D body and a mechanical 15 layer 5-20mils outside of the 3D body to indicate how close this part can be placed to other parts without issue

  • Pads should be at least 3.825mm wide according to the datasheet, yours are only 3mm

  • Distance between pads should be 16.23mm according to the data sheet, yours is only 14.7mm

@Logan Hartford

PCEC1308-220M

SH2,SH3

IND_22uH_7A

Inductor PG0936

Schematic

  • Low stock on digi-key--watchout

  • Missing supplier link

  • This is a 3 pin inductor and you schematic symbol only has two pins.

  • Add a third pin to the schematic symbol and place it so it is clear that the pin is for mounting purposes only and does not need an electrical connection. You could connect this third pin to ground for better heat sinking of the part.

Footprint

  • Not following library naming convention.

  • Need to add the third pad the the footprint. Just because it is not electrically connected does not mean you can ignore it. It if for properly mounting the part and as mentioned above can be used for better heat sinking.

  • Should add a lines on top overlay layer to show the outline of the 3D body and a mechanical 15 layer 5-20mils outside of the 3D body to indicate how close this part can be placed to other parts without issue

@Farris Matar

AONS66923

SH2,SH3

NMOS_100V_15/47A_1

AONS66923

Schematic

  • Remove the _1 at the end of the name

  • Since the part has 3 source pins and 4 drain pins, make a pin in the symbol for each of those pins (should be total 8 pins). Each pin should have a unique designator number as well (match the numbers in the datasheet symbol)

    • This is something new we’re doing so it isn’t implemented throughout the library yet, which is why you wouldn’t have seen this before

  • Otherwise, symbol is all good

Footprint:

  • Be sure to update the pin numbers to match the symbol once you add the missing pins

  • Use the pad dimensions in the recommended land pattern page of the footprint datasheet, pads need to be a bit bigger

  • There’s an additional pad that needs to be added as a heatsink for the drain pins, this is an irregular/hard to describe pad so I’ll help you with it next time we call

  • Draw a circle next to pin 1 on the silkscreen to indicate it’s location

@Farris Matar

MB10H100HE3_B/I

SH2,SH3

DIO_SCHOTTKY_100V_10A

D-PAK3

Schematic:

  • Hide the supplier part number, show the manufacturer part number instead

  • Show the forward current parameter

  • The heatsink pin (K) needs to be included in the symbol

  • Change the pin designator numbers to match the datasheet (pin 1 should be the cathode or front of the diode, pin 2 the anode or the back)

Footprint:

  • Pad sizes and locations are incorrect. Double check the datasheet for the mounting pad layout

  • You’ll also need to replace the 3D model with the correct one (can be found here, the DD pack file)

  • Draw a circle next to pin 1 on the silkscreen to indicate it’s location

@Farris Matar

LM20BIM7

SH7

IC_TEMP_SENSOR_NEW

SOT65P210X110-5N

  • IC is no longer in stock, so a new part will have to be selected

    • Use the same process to select the new part: check for similar parameters and footprint to minimize the amount of work for updating the symbol/footprint and schematic

@Ari Wasch

IRF5210STRLPBF

SH1

PMOS_100V_38A

DPAK5_PMOS_FOOTPRINT

Schematic:

  • Package/footprint should be D2Pak instead of TO-263

  • Show current parameter

  • what is the 120A id parameter?

Footprint

  • 2nd pin should be wider

  • 2nd pin top solder and top paste not centered

  • top solder and top paste look odd and don't follow pin 2 well

 

@Ari Wasch

TCAN334GDR

SH8

IC_CAN_TRANSCEIVER

SOIC127P600X175-8N

Schematic:

  • Make manufacturer part number visable

Footprint:

  • Pads are bigger than data sheet example, but still looks good

  • Change name of footprint to match the IC

@Logan Hartford

LT3845AIFE#PBF

SH2,SH3

BUCK_LT3845A

SOP65P640X120-14N

Schematic

  • Your pin designators should not be hidden. The pin number is a very important piece of information.

  • None of you pins have their pin types set. While this is not necessary it can help avoid errors. For example, altium will give you and error when you compile if you leave and input pin floating or if you connect two inputs together. Set the type of each pin according to its fuction.

  • Missing supplier link

Footprint

  • Change footprint name to match library naming convention for buck IC

  • This part is a 16 pin package and you footprint only has 14 pins. It is also missing the thermal pad which should be designated as pin 17 in the footprint.

  • Pin pads should be 1.15mm long and 0.5mm wide

  • The x-distance between the two columns of pads should be 4.95mm, yours is 5.74mm

Schematic Sheet Reviews

POWER.SchDoc (@Farris Matar )

In addition to the lists below, each individual schematic sheet should be reviewed by another person for correctness and clarity
Check Stock and Connections on Diodes

17V Buck Converter.SchDoc (@Logan Hartford & @Paul Kokhanov )

In addition to the lists below, each individual schematic sheet should be reviewed by another person for correctness and clarity
Pretty Much Entire Thing was made from Scratch so Everything should be verified

@Logan Hartford 's Comments:

Schematic Readability/Neatness

  • This is not a clear way of representing a voltage divider:

Voltage dividers should be vertical with the positive voltage at the top of the divider and the reference voltage at the bottom, as illustrated above.

  • You should not have this many connections crossing each other, the schematic should be easily readable, I’ll make some suggestions for how to clean this up.

    • Move the VCC pin above the BOOST pin so that you don’t have to route that across all of the other connections.

    • Move the CS+/- pins to the top or bottom of the right side of the IC to those lines can be routed up and away from the rest of the circuit instead of going through.

    • Pull this circuit out and away from the IC and expand it if you need to make it cleaner.

    • You don’t need to route power, you can just drop a GND port

    • Make the IC symbol larger if you need to, to make these changes. Space is not a constraint in schematic and readability is most important.

  • Bring this is in

  • Again, this is not a proper way to represent a voltage divider. Pull it out from the IC and make it vertical.

  • If you are doing this you are not allowing enough room for the circuit, pull it out and expand it.

  • I would prefer to see this part of the circuit being organized vertically with all of the grounds placed vertically

  • IC part number should be listed here

Schematic Readability/Neatness (Post-Update)

  • Might as well move CSS below BURTS_EN to remove another crossed wire

From the IC Datasheet:

  • I’m not sure what this is but I think BURST_EN should be shorted to GND or VFB. This voltage divider should be to GND should it not?

  • You are missing SGND. I don’t think you need to create a signal GND just be careful with how you place and route the high noise and high power components relative to the IC. You do need this pin to give the thermal pad the proper connection though.

     

  • I may be doing the calculation wrong but it seems like your IC power dissipation will be too high

  • The indutor you have selected has less inductance than the minimum inductance indicated by your calculations

  • Based on Rb as 10k and Vsupply at 36V, I’m gettin 256k for Ra. Double check this. also the divider is missing a ground port in your schematic

  • The voltage rating of your capacitors is not high enough. Your caps should be rated to 2x the expected voltage therefore the minimum acceptable voltage rating would be 34V.

@Paul Kokhanov Comments:

Schematic Readability:

  • Logan Touched on all the main points, please refer to his suggestions

  • potentially make these come to one ground

  • Could make overall IC larger in size just to space everything out, but that’s up to you

Schematic Correctness:

  • Footprint not linked for MOSFETs

  • Should you include the SGND pin?

  • May need to look at BURST_EN pin and confirm which operating method you are intending to use, it looks like you do want the BURST_EN enabled so make sure to short it to GND

  • In terms of Vc, it seems the best method in order to determine the optimal RC network connection would be to create and order the PCB and test how well the transient response is depending on various values of the capacitor and resistor, hence for now the values should be fine but this is something that will need to be tested later

  • This voltage divider for the SHDN pin should be grounded

  • I’m getting a Ra of 256.6 kOhms using the following equations with Rb as 10Kohms and our V Supply of 36 V

  • Just to be confident could I get an explanation why we chose 0.1 V for our Delta Vout? Is that a fairly typical value?

  • Potentially chose a larger voltage rating for the output capacitors as we are expecting 17 V of output, 25 V should be reasonable but maybe put it to over 30 V to be safe

  • Overall MOSFETs seem to be reasonable, if you want you could look and see if there are any other MOSFETs with a smaller RDS(ON) but if the difference is less than 5% I’d say don’t worry about it

  • You will need to chose an inductor with a larger inductance, currently you have 22uH but need it to be larger than 23.5uH

  • As Logan mentioned, the power dissipation of the regulator seems too high, from the datasheet of the MOSFET we get a Max total gate charge of 35 nC which causes the Power dissipation to be 1.24 W instead of the maximum of 250 mW. So a new MOSFET could be selected, or if there is a chance to reduce the input voltage then you could lower the power dissipation. Or you could potentially lower the switching frequency.

  • Also I notice the input voltage range is 36-50.4 V, how did we determine the 48 V input voltage?

5V Buck Converter.SchDoc (@Logan Hartford & @Paul Kokhanov)

In addition to the lists below, each individual schematic sheet should be reviewed by another person for correctness and clarity
Pretty Much Entire Thing was made from Scratch so Everything should be verified

@Logan Hartford 's Comments:

Schematic Readabiltiy/Neatness:

  • Same as above, I can see several ways you could clean up this section of the schematic and not have so many wires crossing each other

From the Datasheet:

Since the ICs are the same for the 5V and the 17V, most of my comments from above will apply but I will state them breifly here again.

  • Missing a GND on the SHDN divider and I think you should double check the calcualtions for Ra for that divider.

  • Your output capacitance target is 660uF but you only have 600. 600 is probably enough, but if you want to push it to >660 I would use some of the 22uF caps from 17V converter. Caps with different capacitances will filter different noise ranges better, thus improving your overall noise filtering.

  • Inductance looks good

  • IC power dissipation looks good

 

@Paul Kokhanov Comments (WIP):

Readability:

  • Connect these grounds

  • Similar comments to those on the 48 - 17 V converter

Correctness(Similar comments as per 17 V converter):

  • Footprint not linked for MOSFETs

  • include SGND?

  • GND needed on SHDN pin voltage divider

  • Ra calculations need to be looked at

  • Footprint for inductor not found

  • in your part Selection document you mention you are using the same MOSFET here as you did for the 17 V Converter, however in the schematic the part seems different

  • Still concerned about power dissipation of the regulator

  • increase output capacitance on schematic

  • I’m getting 3.75 uH for inductor value

 

Load Monitoring 2.SchDoc (@Farris Matar )

In addition to the lists below, each individual schematic sheet should be reviewed by another person for correctness and clarity
Verify stock on the 17 V Load Monitoring Switch, Mouser says 756 Expected 17-Aug-22 which means it may have stock in time, but I may just need to replace it altogether with BTS5016SDAAUMA1 for example
In stock at Mouser now so it should be good

MicroController.SchDoc (@Ari Wasch )

In addition to the lists below, each individual schematic sheet should be reviewed by another person for correctness and clarity

  • The SPI connection below can be removed unless there is something that uses SPI. it used to connect to BMS, but BMS is going to be a separate board

  • BMS and Battery Balancer pages can be removed

  • Can we include a few more VBAT_FUSED output connectors?

 

why a diode for the output of the temperature sensor? an output capacitor is recommended from the data sheet

 

 

  • in layout example, all NC are connected to GND

CAN.SchDoc (@Ari Wasch )

Generic Schematic Reviews

Net Naming (@Farris Matar )

Wiring and Connections (@Paul Kokhanov)

Component Labels (@Logan Hartford)

  • See 17V buck comments

  • Diodes are not showing part number

Design-for-Test (@Ari Wasch )

 

 

 

 

where does the below connect to?

 

Temperature_ADC_INPUT needs a test point

testpoints for all the ultra sonic sensors inputs and outputs?

 

 

Supporting Document Links if Needed

Part Selection.xlsx

Buck Converter 5 V Calculations Simplified.xlsx

Buck Converter 17 V Calculations Simplified.xlsx

https://www.analog.com/media/en/technical-documentation/data-sheets/3845afa.pdf