4 Replies Latest reply on Jun 30, 2011 1:38 AM by pcb_layout

    ExpeditionPCB - Gerber generator

    MaBUa

      Good morning everybody,

      is here anybody who fought with a text font generated in gerber format (data)? see my attached picture.

      I'd really appreciated the possibility to be able to set the gerber generator for generating all the text font as an polygon.

      (I heard in PADS it is possible... why not in Expedition.... is it so big problem to include this feature in the ExpeditionPCB ?? )

       

       

      I know that I can choose some other font (in 2007.3) which is not true type font...  -> vf_xxx but I dont' like this fonts.

       

       

      Many thanks for your comments

       

      Best Regards

      Martin

        • 1. Re: ExpeditionPCB - Gerber generator
          strangd

          Hi:

           

          It looks like you are trying to use Arial for your silkscreen refdes.  It is a filled font and the Expedition Gerber generator historically will only draw the font outline.  I like using arial so I increase the drawn line width which will closes in the open space within the characters.  This works if the text height is .050" - .060" or less.  At > .100" it does not work as well.

           

          Some CAM software packages do quick work of flooding an area that is surrounded by drawn borders.  If the there are not a lot of larger, hollow text characters, then this is a good follow-up to finish the silkscreen text.

           

          Dwain

          • 2. Re: ExpeditionPCB - Gerber generator
            yu.yanfeng

            Hi Martin,

             

            If you use any true-type font and set the pen width to a very small value but not zero, you will get the effect. However, the font will be filled iby Expeditionpcb gerber generator using 5mil default D Code if the pen width is zero.

             

            BTW, The silkscreen data generated by Expeditionpcb is bigger compared to other layout tools.

             

            Yanfeng

            • 3. Re: ExpeditionPCB - Gerber generator
              MaBUa

              Good morning boys,

              many thanks for your notes

               

              I know that I can "mask" the space inside the character by increasing the text width option in the Silkscreen generator tool... but as you mentioned it has restrictions.... depending on the text height .... I used it but I need more elegant solution. In this case thers is the space (50um)  between the two lines (border) of the character. I can flood it in some CAM tool but I was not able to flood all the text character in one click.. only each character separately... I tried to do it in the CAM350 ver 6. Can you recomend me the tool which can do it in one click for all the characters?

               

              So, If I'll use this method I have to count with this 50um distance I don't like it.

               

              I would really appreciated the mentor's guy to implement the PADS possibility (generating the polygons into gerber file) into Expedition

               

              Thanks and have a nice day

              Martin

              • 4. Re: ExpeditionPCB - Gerber generator
                pcb_layout

                Hi All,

                 

                If you haven't many text written by true type font

                 

                  You can do this ( It is a bit toilsome -  many work):

                 

                1) Type text with using true type font

                2) Generate silkscreen

                3) Change generated silkscrenn on Draw object

                4) Fill each charakter of the text in Draw object properties

                5) Change the layer of Draw object to Silkscren layer