Planar Spiral Inductor Design Process

Hi maybe this can help you. It is a very good tool. http://www.saturnpcb.com/pcb_toolkit/

You may already be aware but your are talking very low inductance for these types of inductors typically in the nH range. If you wanted to figure out the actual inductance of the finished inductor you either need a VNA or some higher end simulation software such as Agilent ADS. In the case of Agilent that can also generate the artwork which can be easily imported into Allegro.

As a matter of interest, Whats your desired inductance ?

The typical flow is.
Figure out the required inductance first. If your in the uH range then any printed inductor is out without ferrite loading. If in the nH range it may be possible.
Simulate it and verify its inductance. You could get fancy and do an em simulation but below 1Ghz linear simulators offer very predictable results so in that regards EM is probably over kill.
Generate an etch profile based on the simulation.
Export the artwork to Allegro.
For your schematic symbol you will have to fake it out because you only have one net for the corresponding copper trace. Maybe draw a rectangular box with one wire "Net" running through it.

BTW: at 10Mhz it does not really matter if you use spiral or rectangular, you actually don't have to use either topology. A way to think about this is that your copper trace is in itself an inductor. The rectangle or spiral form
just lends itself to getting a longer copper trace in a small area. The main thing is the physical length of the copper trace.

If you have access to a VNA "Vector Network Analyzer" then what you could do is take a length of wire say 20awg and twist it into a spiral form. Short one end to ground and measure from the open end with the VNA.
This will give you instance results without having to twiddle figuring out any copper traces. When you get those results then you could go about creating the etch.

There are a few companies making these planar inductors these days, typically they take on the form of stacked PCB's loaded with ferrite. Maybe you might get lucky that one would be available for the inductance you need.
Have a look here. https://www.power.pulseelectronics.com/inductors/planar

All the best. 

Give this free app a try orcadmarketplace.com/.../Default.aspx

Thanks for this! The biggest challenge for me is always on the software-usage side because there are so many tools available. It's nice hearing what people actually use and how they use it. 

I was actually hoping to get uH out of it. I've prototyped a pancake coil using 24 AWG wire and got an inductance of 1 uH. It's about 20mm in diameter. I was hoping to do a similar size on the PCB as well. I have access to a VNA so I made a Tx and Rx circuit and measured s11 and s21 to get an idea of my system efficiency. I simply made the circuit on a high-quality breadboard because it's only 10 MHz. I'm working on impedance matching the entire system as an exercise, but I'd like to get a bunch of PCB's ordered so I can try them out. 

I've never used Emag simulation before. Is this something you think might be useful? I'm essentially trying to achieve maximum coupling of a large planar inductor (20mm diameter) with a much smaller spiral or planar inductor (diameter ~5mm). 

Hi Steve,

I watched a demo of this add-on and it seems excellent. 

I've been trying to get this app to load with no luck. Do you have any insight as to what I might be doing wrong?

I've checked my allegro site which is "C:/Cadence/SPB_17.2/share/local/pcb"

Inside the above directory is a "skill" folder. I have placed the allegro.ilinit file in there with the following contents: 

printf"Start Loading Skill files:"
load("./nsWare/nsware.il" "nsware" )
printf("done Loading Skill files:")

When I start up PCB editor, I see no print statements and I don't see the nsware menu at the top of the screen.

Do you know what I might be doing wrong? Could this be an issue with the LITE version of PCB editor? I have read that the LITE version is not equipped with a skill cmd ability, but skill files can be loaded "at start up", whatever that means. I should mention that I'm using 17.2 2016

Best Regards,

Mike 

Hi there. When it comes to laying out a board Allegro will deliver. Instead of using traces "Clines" you will get more precise results using shapes to represent the etch of your transformer.

With planar transformers the word "Planar" can somewhat distract from what it is. Planar just means flat. What you might want to look at is "Mutually Coupled Coils" First, perhaps you already have. Another thing to think about is would a planar transformer be the best solution. There not very efficient. They are difficult to make because you have the variable of K and how to control the distance between the primary and secondary coils.

I don't think Emag will really help you. You have all you need with access to the vna.

You mentioned impedance matching. I was wondering what you are trying to match and what ratio of impedance you are after ?. I attach a small pic of allegro doing the etch as a shape. Try out the shapes in allegro... There amazing.

Skipping ahead. Skill files work in the lite version. If you have a skill file you want to try then maybe try this and see if it will load.

Create a folder on you HDD and put the skill file in there. I use c:\allegro-skill-files

Next go to your "pcbenv" folder, it normally gets installed under C:\SPB_Data\pcbenv

Inside that folder you will need to have your "allegro.ilinit" file. This file is just a text file named ..ilinit, You could make one using notepad and save the file as allegro.ilinit.

here is what I use inside the file.

setSkillPath(buildString(append1(getSkillPath() "C:/Allegro-Skill-Files" )))
  foreach(dir getSkillPath()
    when(isDir(dir)
           foreach(file rexMatchList("\\.il$" getDirFiles(dir))
        when(
           printf("Loading Skill file: %s\n" file)
           load(file)
      )
    )
  )
)

When you start allegro it will read all the skill files in the folder. After allegro starts look in the command window and it will tell you what skill files got loaded. You might want to have allegro start up with the command window enabled so you can see at a glance what got loaded.

To launch a skill file in allegro just type its name in the command window and it should start. A word of caution, you need to know the actual name inside the skill file that will call the routine. A skill file could be called hello.il but to actually run it you might have to type 1234 :)

Most skill files are text based so you can open them in a text editor. Usually near the top of the file the author will let you know how to call the routine from within allegro. Or if the file is encrypted then the accompanying documentation should let you know how to load it.

All the best.