1. Blog>
  2. Increasing PCB clearance in HV circuits: Low Inductance Capacitor Bank

Increasing PCB clearance in HV circuits: Low Inductance Capacitor Bank

by: May 21,2021 3117 Views 0 Comments Posted in PCB Design Tutorial

DesignSpark PCB Design Tutorial

Summary:       Creating PCBs with high voltages or currents creates additional requirements to keep PCB tracks/pads further apart than normal. We also look at using using copper pour to create low inductance paths. In this case, increasing the clearance around the pads of selected components. For this tutorial I'll be using Design Spark PCB (9.0), but the process for other software will be much the same.

How to create greater PCB clearance around higher voltage (or current) components.

In most PCB software there is just one track/pad clearance setting.

Obviously this is a problem if your board is a mixture of logic/analog circuits and higher voltage parts like mains, SMPS, 400V capacitor banks, or event Tesla coil drivers.

For this tutorial I'll be using Design Spark PCB (9.0)

But the process for other software will be much the same.

I'll be showing how to create low inductance HV capacitor bank on a PCB.

Will be using the measurements from a commercial product for both the PCB clearance, and the 500V capacitors themselves.

count:       12 (3x4)

voltage:     500V

capacitance: 470uF

height:      63mm

diameter:    35mm

pitch:       10.5mm

pin diameter: 2mm

pad width:   5mm

pin clearance:13mm

Start by creating/downloading the component CAD data, then place the capacitors in the schematic/PCB.

As the default libraries don't include capacitors of his size we need to make one.

From the Library Manager in your own library, create a new part using the Wizard.

Use mm as the unit.

component type 'CAN'

2 round pads, PW=5.000 (5mm pad width), HD=2.2 (2mm pin plus some wiggle room in the hole), R=5.25 (half of 10.5mm pitch)

The tricky part was creating the silkscreen for the radius of the capacitor can itself.

As the program for some insane reason uses "Outside Pads" distance rather than total radius/diameter.

Of note, the pad itself isn't part of this calculation.

OutsidePads = (diameter - pitch) /2

           = (35mm - 10.5mm) /2

           = 24.5mm /2

           = 12.25mm - 0.75mm

           = 11.5mm

So where does this -0.75mm come from, you'd have to ask DesignSparks programmers that one.

No Footprint needed.

Finally for the last page, call it something descriptive like "CAPP_35x93_500V", save, then edit the completed part.

Also take the time to add the + symbol to avoid insering the capacitors in backwards when assembling the PCB, explosions are bad.

Change units to mm, and then create a new Circle that is 35mm diameter.

Move the two pads to the center, the use Coordinate Offset to move them +/- 5.25mm in the X direction, 5.25m being half of the 10.5mm pin pitch.

Set the two pads to 2.2mm hole and 5mm outer

Finally Create the capacitor component, using the Wizard.

1. Type Conventional Component

2. Component name, Package, Default Reference, pins, gates as shown.

3. From the Schematic Library "discrete" choose the symbol "CP"(capacitor polarized).

4. From the Library Manager in your own library, choose the symbol "CAPP_35x93_500V"

5. Pin Assigment, use "Assign 1-to-1"

6. Save the component to your own library. Also edit it to check the measurements, and to change a few things.

7. If you want the capacitors to be the correct height in the 3D view, edit the value height= to "63mm"

Create a schematic using the new component "CAPP_35x93_500V".

Connect the pins together so all the positive side and negative sides create two common voltage rails.

1. Rather than connecting the capacitors together with wide copper tracks, we'll create two localized copper pours, one on the top most layer, one on the bottom most layer.

To save time, create one, copy/paste the other layer later on.

2. Pour the copper, notice how we only have 1mm or so clearance between the copper and the pad it doesn't connect to.

At 400-500V this will arc over, start a fire, or just ruin your PCB.

Simply altering the programs clearance setting alters everything, and messes up the current sensor and related circuits.

3. Create a Keep Out Area around each capacitor pin, on both sides of the PCB.

  For DesignSpark, this is a 3 step process.

  Create a circle using Add Shape Circle, change it's diameter to 13mm.

  Change it to be on Layer Top Copper (or Bottom Copper).

  Change Shape Type from Shape to Copper Pour Area

  Properties > Area tab, tick the box Pour Keep Out

4. Copy the shape you created in step 2, multiple times until you have it around half the Capacitor pins, on the top layer.

5. Select one of the large rectangular Copper Pour outlines from step 1.

  Choose Pour Copper from the right click menu.

6. Copy the entire layer, paste to to one side, and select all the shapes and change them to the bottom layer.

7. Now move the bottom copper pour shapes to line up with the capacitor pins/pads.

8. Finally shift the top and bottom edges of the rectangle to line up with the top layer

9. Select the two rectangles that make the edges of the copper pour, and press "Pour Copper"

10. Override the default "Design-Level Thermals" to remove the spokes for increase current capability, "Adjacent (Touching)" does this.

To make the entire process easier, I recommend the following.

A. Hide the other layer, so you can only see/edit one layer at a time.

B. Create the first Keep Out circle off the edge of the board, to make it easier to select/copy/move.

C. Copy/paste the X/Y coordinates of the pins to make the placement faster/more accurate.

Join us
Wanna be a dedicated PCBWay writer? We definately look forward to having you with us.
  • Comments(0)
You can only upload 1 files in total. Each file cannot exceed 2MB. Supports JPG, JPEG, GIF, PNG, BMP
0 / 10000
    Back to top