Designing spiral or helix [SOLVED]

Deppy · November 25, 2015, 2:24pm

Hello,
I would like to design a spiral in Kicad but I can’t find any tool to do that.
Until now I was creating the spiral in Autocad, then converted it to gerber and then export from GerberView as .pcb.
Is there any way to design it entirely in Kicad?
I’m attaching an image of an older spiral transferred to Kicad.

Thanks

Joan_Sparky · November 25, 2015, 2:40pm

as track, copper zone or one of the other non-copper layers?

Deppy · November 25, 2015, 3:44pm

As track and as soldermask.
But I would like to be able to change the radius, step and number of spirals…

maui · November 25, 2015, 5:01pm

@Deppy
In which way do you convert from autocad (dxf?) to gerber?

Joan_Sparky · November 26, 2015, 12:14am

The only way would be to use a python script to draw track segments in a spiral and then paste&copy the result into a kicad_pcb file with a text editor.
There is no GUI that would allow what you want atm.
Have a read here:

kinichiro · November 26, 2015, 3:52am

Is Bitmap2component available for your needs ?
Convert your spiral into bitmap, then convert it component by Bitmap2component.

Deppy · November 26, 2015, 7:45am

I am using a converter. Here is the link.
I am using the 30-days evaluation version.

maui · November 26, 2015, 8:35am

@Deppy
thanks for the link…
I found also here a nice Lite sw for RF design with dxf to gerb export option…
https://www.sonnetsoftware.com/
https://www.sonnetsoftware.com/products/lite/

Could you suggest me where could I learn some pcb techniques to work with RF?
I mean if would be something like a workshop video or similar…
Thank you
Maurice

Deppy · November 26, 2015, 9:08am

@Joan_Sparky
I’m not familiar with python. Although, I read the post but it’s not what I’m looking for in the moment but I’ll keep that in mind (when I’m in the mood for python).
I prefer to create arcs in footprint editor and then convert them to copper in text editor.

@kinichiro
That is a good idea but I want to avoid using Autocad for this design. Do you know any other program that creates spiral/helix with controllable radius?

@Maui
Thank you for the links. I’ll check them out.
I know nothing about pcb RF designs but I found some guidelines.

Thank you all for your help
Deppy

maui · November 26, 2015, 9:16am

@Deppy
thanx for the link of maxim…

I know that at
https://hackaday.io/project/8117/logs
they organized a workshop on RF techniques:
Simple RF Circuit Design (Sunday Afternoon)
Michael Ossmann will show specific examples from his own designs including Ubertooth One, HackRF One, and YARD Stick One. Participants with prior experience designing non-RF circuits should be able to walk out of this workshop with the ability to design boards to use RF transceiver ICs.
That would be great if the workshop would be available as video, because it is also a talking about kicad RF techniques …

Deppy · November 26, 2015, 9:28am

@maui
That sounds great but I think that it is not going to be recorded.

maui · November 26, 2015, 9:58am

I read at the hackaday posts that has been recorded…
will see if they will publish it…

Joan_Sparky · November 26, 2015, 11:19am

[quote=“Deppy, post:9, topic:1745”]
I’m not familiar with python. Although, I read the post but it’s not what I’m looking for in the moment but I’ll keep that in mind (when I’m in the mood for python). I prefer to create arcs in footprint editor and then convert them to copper in text editor.[/quote]

Well, I prefer to create copper spirals as tracks in python and copy&paste them into a kicad_pcb that has got the basic setup done and then enjoy myself

Code is here:

gist.github.com

https://gist.github.com/JoanTheSpark/e5afd7081d9d1b9ad91a

KiCAD_CopperSpiral.py

import sys, os
import shutil
import math
import itertools
from copy import deepcopy

#              0        1          2      3      4        5    6
LIST_elmt = ["  ("," (start ",") (end ",") "," (layer ",") ","))"]
#LIST_elmt = ["  (gr_line (start 131.571908 182.314571) (end 112.874456 120.68499) (angle 90) (layer Dwgs.User) (width 0.1))"]
#LIST_elmt = ["  (segment (start 118.7 106.7) (end 119.4 106.7) (width 0.25) (layer B.Cu) (net 0))"]

This file has been truncated. show original

Have fun.

Deppy · November 26, 2015, 11:37am

Thank you a lot @Joan_Sparky!!!

Joan_Sparky · November 27, 2015, 8:09am

You’re welcome.
The code might need some polishing for CW/CCW of those spirals and maybe something that would add 1/2 segments per turn as it get’s quite corner-y in the outer turns compared to the inner ones.

Joan_Sparky · November 27, 2015, 8:55am

What are words, right?

gist.github.com

https://gist.github.com/JoanTheSpark/e3fab5a8af44f7f8779c

KiCAD_CopperSpiral_v2.py

import sys, os
import shutil
import math
import itertools
from copy import deepcopy

#              0        1          2      3      4        5    6
LIST_elmt = ["  ("," (start ",") (end ",") "," (layer ",") ","))"]
#LIST_elmt = ["  (gr_line (start 131.571908 182.314571) (end 112.874456 120.68499) (angle 90) (layer Dwgs.User) (width 0.1))"]
#LIST_elmt = ["  (segment (start 118.7 106.7) (end 119.4 106.7) (width 0.25) (layer B.Cu) (net 0))"]

This file has been truncated. show original

Upgrades:

adds 4 segments per turn to the base number
can rotate CW or CCW

Deppy · December 1, 2015, 12:06pm

Hello,

@Joan_Sparky
I’m trying to import your file but it seems that I’m doing something wrong.
I am using BZR 6245 on VM winXP.
Steps I followed :
-Save helix.py (your file) in the directory Program files/Kicad/bin/scripting/plugging.
-Then restart PCBnew and re-open it.
-opened scripting console and typed “import helix”.
-open footprint editor and select “new footprint using footprint wizard” and then select “wizard script to load and run” and nothing is to be shown.

What am I doing wrong?

Thanks,
Deppy

Joan_Sparky · December 1, 2015, 12:17pm

this is not a kicad-python script, sorry… this one runs on itself (or better just with a python interpreter) and the output is to be handled manually…

use the command line and let it parse the output into a txt file like so (Windows)

“helix.py > helix.txt”

have a project + kicad_pcb file where you want the helix to be part of, open the kicad_pcb in a text editor
copy the content of helix.txt into that kicad_pcb file… right before the last braket closes

…
helix.txt stuff goes here
)

close pcbnew if it was open and open it again to load the modified kicad_pcb

Deppy · December 1, 2015, 12:22pm

Ok. I’ll let you know for my progress on this.
Thank you Joan.

Deppy · December 1, 2015, 1:30pm

Sadly I can’t find a way to do this step. Could you please help me?
I have installed python 2.7 in VM and tried to use helix.py in shell and cmd.
Meaning, in cmd I changed the directory in order to read your file. Also, ran python.exe through cmd but I can’t do the “helix.py > helix.txt”… I did pretty much the same in the shell.

I am sorry but I am a dummy in python.

Thank you Joan