Loading ...
Sorry, an error occurred while loading the content.
 

Best PCB program to use with TinyCAD

Expand Messages
  • jwkaiser
    Hi All, I ve been a TinyCAD user for years and love it but I have yet to use it with another program to create a PCB board. I ve searched this forum and
    Message 1 of 8 , 25 Jul
      Hi All,
      I've been a TinyCAD user for years and love it but I have yet to use it with another program to create a PCB board. I've searched this forum and freepcb and kicad are mentioned. freepcb appears to have mostly abandoned judging by the forum comments and kicad doesn't natively accept any of the netlist outputs that TinyCAD generates. In older posts Magnus Beicher claims to have written a converter to allow kicad to accept TinyCAD output but I've been unable to locate it.

      I don't want to invest the time and effort into learning how to use a program, and I'd prefer an open source program to one which is tied to one PCB company.

      I'd be interested in any comments and recommendations this community of TinyCAD users might have.
      Thanks,
      Jim Kaiser




      [Non-text portions of this message have been removed]
    • jwkaiser
      Sorry, I didn t finish a sentence properly!! I meant I didn t want to invest time and effort in learning to use a program if I would have to abandon it later!!
      Message 2 of 8 , 25 Jul
        Sorry, I didn't finish a sentence properly!! I meant I didn't want to invest time and effort in learning to use a program if I would have to abandon it later!! Must be a little ADHD

        [Non-text portions of this message have been removed]
      • Don Lucas
        Hi Jim - I contacted the developer of FreeCAD a number of years ago to see if he was interested in better integration. He was unhappy with the fact that
        Message 3 of 8 , 25 Jul
          Hi Jim -



          I contacted the developer of FreeCAD a number of years ago to see if he was
          interested in better integration. He was unhappy with the fact that TinyCAD
          doesn't provide permanent net names to unnamed nets. He said that he had
          developed a reader for it that would match differently named nets from one
          revision to another by using the reference designators of components so a
          lot of nets didn't need to be ripped out each time that you make a schematic
          change. Past that, he didn't seem too interested in further work. It is
          possible for TinyCAD to adapt fixed net names internally or at least to do
          something like sort the nodes connected to a net and then use the first
          sorted node (C3pin2, for example) as the net name. That would at least
          reduce the number of differently named nets provide that someone didn't
          renumber all of the designators. It is also possible to use unique guids
          for each net, but then you have the same problem that he has - you have to
          make a "best match" of the components in a net before and after to determine
          which guid you should call an edited and close, but not identical, net.



          As far as netlists go, you can create any custom netlist that you want
          without recoding by hijacking the SPICE netlist features. The SPICE netlist
          is basically a set of macros that determine what gets output for each
          component and each pin.



          Custom netlist formats (involves writing C++ code) are the easiest of new
          features for TinyCAD to implement. There are quite a few developers in the
          TinyCAD community that have developed new netlists. Some have chosen to
          simply write standalone netlist converters, also. The netlists are all
          straight ASCII and a very simple command line program will suffice with
          redirected standard input and output to write a TinyCAD2Whatever.exe type
          converter.



          Another option and the richest, is to write a converter from XML to whatever
          format that you want. Everything that TinyCAD knows about the nets and
          components in a design are output to the XML format built-in netlist. If
          you are comfortable writing an XML to whatever converter, this might be the
          best approach. All parameters of all components are available in this
          format.



          Also, I don't know of any professional PCB CAD ($$$) software that can't or
          won't read in any of the TinyCAD netlist formats.



          Best regards,

          Don





          From: tinycad@... <mailto:tinycad@...>
          [mailto:tinycad@...]
          Sent: Tuesday, July 25, 2017 3:35 PM
          To: tinycad@... <mailto:tinycad@...>
          Subject: [tinycad] Best PCB program to use with TinyCAD





          Hi All,
          I've been a TinyCAD user for years and love it but I have yet to use it with
          another program to create a PCB board. I've searched this forum and freepcb
          and kicad are mentioned. freepcb appears to have mostly abandoned judging by
          the forum comments and kicad doesn't natively accept any of the netlist
          outputs that TinyCAD generates. In older posts Magnus Beicher claims to have
          written a converter to allow kicad to accept TinyCAD output but I've been
          unable to locate it.

          I don't want to invest the time and effort into learning how to use a
          program, and I'd prefer an open source program to one which is tied to one
          PCB company.

          I'd be interested in any comments and recommendations this community of
          TinyCAD users might have.
          Thanks,
          Jim Kaiser



          [Non-text portions of this message have been removed]





          [Non-text portions of this message have been removed]
        • Cris Harrison
          Hi. I have used tinycad for a while and have found it OK for one page diagrams but when you have multiple pages well it does not do a good job also it does no
          Message 4 of 8 , 25 Jul
            Hi. I have used tinycad for a while and have found it OK for one page
            diagrams but when you have multiple pages well it does not do a good job
            also it does no net verification, IE missing resister on open collector
            outputs.
            I found a group of packages under the banner of gCAD runs on Linux maybe
            Windows. On the finger scale it's about a five or six difficulty it was set
            up presently for terminal interface but it's quite usual there are some
            great tutorials on YouTube for it as well.. thanks and cheers


            On Jul 25, 2017 2:34 PM, "jkaiser@... [tinycad]" <
            tinycad@...> wrote:


            >
            >

            > Hi All,
            > I've been a TinyCAD user for years and love it but I have yet to use it
            > with another program to create a PCB board. I've searched this forum and
            > freepcb and kicad are mentioned. freepcb appears to have mostly abandoned
            > judging by the forum comments and kicad doesn't natively accept any of the
            > netlist outputs that TinyCAD generates. In older posts Magnus Beicher
            > claims to have written a converter to allow kicad to accept TinyCAD output
            > but I've been unable to locate it.
            >
            > I don't want to invest the time and effort into learning how to use a
            > program, and I'd prefer an open source program to one which is tied to one
            > PCB company.
            >
            > I'd be interested in any comments and recommendations this community of
            > TinyCAD users might have.
            > Thanks,
            > Jim Kaiser
            >
            >
            >
            > [Non-text portions of this message have been removed]
            >
            >
            >




            [Non-text portions of this message have been removed]
          • m_beischer
            Hi Jim, I have used kicad for a lot of professional PCB designs based on TinyCAD schematics. The issues that Don mentions about net names in FreeCAD does not
            Message 5 of 8 , 26 Jul
              Hi Jim,

              I have used kicad for a lot of professional PCB designs based on TinyCAD schematics. The issues that Don mentions about net names in FreeCAD does not apply to kicad. Renaming nets just works like it should.
              I did write a converter from TinyCAD netlist format to kicad. Have been using it for years. You find it here: https://github.com/beischer/netconv https://github.com/beischer/netconv
              If you can't bild it from source (requires Qt 5) I can put the Windows exe on Github as well. Just let me know.
              Magnus





              [Non-text portions of this message have been removed]
            • m_beischer
              Added a small wiki to the github project: https://github.com/beischer/netconv/wiki https://github.com/beischer/netconv/wiki Magnus [Non-text portions of this
              Message 6 of 8 , 26 Jul
                Added a small wiki to the github project: https://github.com/beischer/netconv/wiki https://github.com/beischer/netconv/wiki



                Magnus




                [Non-text portions of this message have been removed]
              • Jim Kaiser
                Thanks, Magnus, for putting up the binary installer for Windows as well as the wiki. That helps a lot. I ve got netconv installed and running so now I can
                Message 7 of 8 , 26 Jul
                  Thanks, Magnus, for putting up the binary installer for Windows as well as
                  the wiki. That helps a lot. I've got netconv installed and running so now I
                  can start playing and deciding whether this is the best way for me to go!!

                  I think I understand the issue Don brought up about changing net names and
                  how a schematic revision coulld potentially mess up a board design. I don't
                  quite understand how kicad's handling of netlists differs from freepcb's.
                  The only thing I've used a netlist for has been to create a wire-wrap card.
                  I'll figure this out eventually!

                  Jim.

                  On Wed, Jul 26, 2017 at 3:59 AM, magnus@... [tinycad] <
                  tinycad@...> wrote:

                  >
                  >
                  > Added a small wiki to the github project: https://github.com/beischer/
                  > netconv/wiki https://github.com/beischer/netconv/wiki
                  >
                  > Magnus
                  >
                  >
                  > [Non-text portions of this message have been removed]
                  >
                  >
                  >


                  [Non-text portions of this message have been removed]
                • m_beischer
                  Jim, KiCAD adapts to the net names that are used in TinyCAD. Both manually named nets and automatically named nets (the ones that you haven t put any label
                  Message 8 of 8 , 26 Jul
                    Jim,

                    KiCAD adapts to the net names that are used in TinyCAD. Both manually named nets and automatically named nets (the ones that you haven't put any label on).

                    If the net name changes when you import an updated net list (generated by TinyCAD/Netconv) in KiCAD, KiCAD match the wires already connected to that pins and adapts. It just works as you want it to work.


                    Please note that my workflow requires you to use the extremely good feature in TinyCAD - "aliases for symbols". If you have a symbol för a resistor, you have to make an alias for that resistor and name it for instance "Res-0603-10k". This will be your "internal art.no." for that resistor. Add more fields to that alias like "Digi-key order code" etc. and you will get a very nice BOM out of your schematics.


                    When creating your map file to support the component above, write a line in the map file like:
                    Res-0603-10k 0603


                    (this says that "Res-0603-10k" maps to the layout symbol "0603" in KiCAD. You have to browse/search the library in KiCAD to find the layout symbol name (or create your own layout symbol/foot print).


                    Magnus







                    [Non-text portions of this message have been removed]
                  Your message has been successfully submitted and will be delivered to recipients shortly.