In a recent blog entry, I introduced a new type of nixie tube power supply that is powered from 5v, Designing a Small Footprint, Low Profile 5v to 170v Nixie Tube Power Supply (Part 1). The design achieved a footprint size less than 14.5cm^2 and the efficiency was optimized in (part 2) of the blog. A good question to ask is how much smaller can the power supply get while keeping the same efficiency and layout objectives? The combination of high transistor currents (i.e. 2.9A max) and high output voltage (i.e. 170v) make the challenge of shrinking the PCB footprint by hand a rather time-consuming task. The high currents require wide PCB traces to minimize losses and keep the efficiency high, and the high voltage of the supply requires large trace-to-trace spacing to avoid voltage breakdown and arcing. Keeping both constraints satisfied to the very limit would be difficult without computer-aided design (CAD). In this blog, I’ll show you two CAD power tools I used to get this done quickly and efficiently. As a result, the new “mini” nixie tube power supply footprint was reduced 27% to just 10.5cm^2. The explanations of the steps are explained using the open source KiCad PCB layout software, but most PCB layout software will have similar features. And as an open source hardware design, the complete KiCad schematic, layout, and BOM are available at GitHub for download so you can try it with your next nixie tube project.
Step 1: Minimize spacing with Design Rules Net Class definitions
By setting up Net Classes and assigning them to each of the nets, the PCB trace layout routines and DRC checking in the software will ensure that ensure that critical traces are wide enough to handle the higher currents and have enough space to avoid high voltage breakdown. For this design, five net classes were defined.
- Default: 0.1524mm clearance and 0.381mm trace width
- High Voltage: 0.8383mm clearance and 0.381mm trace width
- Low Power Low Voltage: 0.1524mm clearance and 0.381mm trace width
- Power High Voltage: 0.8382mm clearance and 1.0mm trace width
- Power Low Voltage: 0.1524mm clearance and 1.0mm trace width
KiCad has a nice built-in PCB calculator tool with a trace resistance calculator and trace spacing table to determine the minimum trace width and trace distances for the defined net classes.
Trace Width Calculator
The minimum width of the input traces of the power supply can be calculated with the trace width calculator. In this design, 1amp was used as the RMS value of input current and a 10 deg C temperature rise is a conservative value to reduce power dissipation. The calculator shows that External layer traces will need a trace width of greater than 0.58mm. For our net class definition, I increased this to 1mm to add some margin.
The exact spacing required between two traces to avoid voltage breakdown is a complicated engineering problem with many variables. Fortunately, there are some good resources available. The Association Connecting Electronic Industries, IPC published a standard on Printed Circuit Board Design that is widely accepted for non-regulatory trace spacing. And KiCAd placed the IPC-2221 trace spacing table from this report into the PCB Calculator to simplify our work.
Traces covered with a solder mask (i.e. permanent polymer coating) are covered under the B4 column above. The 170v traces need a minimum spacing of 0.4mm. For the high voltage trace net classes, I set this to 0.8383mm to provide some margin.
In KiCad, the Design Rule Editor is where the nets are assigned to a particular net class. Other PCB layout software will have other methods to do this. In truth, the KiCad method below is a little time consuming and could be improved to help identify the net names on the schematic. I’m hoping that version 5.0 of KiCad will start to improve this.
To set a net to a particular net class, select that class in the pull-down menu on the right (see the *(Any) pull-down menu). Then select the net on the left scroll window that you want to define and press the “>>>” button to assign it. The difficulty in this step is to trace the net names back to the schematic. Use the reference designators and pad numbers in the net names to help with this.
The high power nets for this power supply are attached to the nets associated with L2, L3, Q1, R10 and D1.
The ground connection of R10, and two of the mounting holes also need to have a wide traces, but the ground net was not assigned to a high power net class since many low power devices were also attached to this same net. A special copper pour was placed on this R10 connection, and the trace width was manually set to 1mm or higher for the mounting hole trace connections. Can you find these wide traces on the layout below?
The high voltage net class was assigned to the nets connected to the anode of the cathode of D1 and the output +160v trace. CAn you also find these in the image above?
Step 2: Quickly find free PCB areas with the 3D viewer
With all the net classes defined and assigned to the critical nets in the layout, the fun part is to find the open room and simply squeeze things together. For this, the built-in 3D viewer (press alt-3 while in PCBNew) is a great tool to quickly identify where open space is located. Check out the original nixie tube power supply and identify where components can be moved closer to one another. There is a lot of room around U1, Q1, D1, J1 that were readjusted.
As you get the components close to one another, the DRC rule checker will let you know when you have gotten too close. The net classes will keep you from violating the trace distances while you move them, not allowing the operation to complete if you are in violation. I like this feature. 🙂
After some work, check out how close the components were able to be placed. Can you find more room?
Do you see a difference in the output capacitor size and output connector? These were the two major component changes I implemented to shrink the board size. I was able to find a smaller sized ceramic output capacitor at the same voltage rating (i.e. 250) and same value (1uF) to help with the shrink exercise. The pin spacing of the output connector was reduced from 3.5mm to 2.5mm.
Remember to run the DRC rule checker and ensure any violation is handled. It is good to remove all the errors, but not always required. Engineering judgment is acceptable sometimes. 🙂 Let me know your comments below or @surfncircuits on Twitter and Instagram.
Here are links to the other blogs in this nixie tube power supply series:
- Designing a Small Footprint, Low Profile 5v to 170v Nixie Tube Power Supply (Part 1)
- Optimizing the 5v to 170v Nixie Tube Power Supply Design (Part 2)
I’m wondering when the surf will pick up….
Output Connector For more Clearance
No product is perfect, and the mini version of the Nixie Tube power supply is no exceptions. Since the initial release of the blog, I updated the layout of the mini version of the nixie tube power supply to improve high voltage clearance on the 170v connector pinout. At the connect, the high voltage clearance was just not as large as I wanted, so I modified them to have more clearance. To do this, I modified the original 4 pin connector with a 3 pin connector and a 2 pin connector. The Kicad, BOM, and schematic files on Github and the gerbers on Oshpark both have these improved layout updates, but the pinouts are different from the images above. In the improved layout, there is a J6 with the following pinout.
- N_ENABLE (NOTES: pull this pin to enable supply)
J1 is a 2 pin connector where both pins are connected to +170v (i.e. 160v in the layout).
Have fun building your own 5v to 170v power supply. Let me know if you have any questions.