5 Replies Latest reply on Feb 13, 2009 6:06 AM by yu.yanfeng

    Problems with Gerber data from Expedition

    charles.ietswaard

      Hello  All,

       

      For some of our customers we have to create Gerer data. We create this data from the Expedition Output menu.  When importing  the generated data into a gerber viewer like Pentalogix's Viewmate we find that the generated gerber data contains so-called 'self-intersecting polygons'. As a PCB-designer I simplie ignore these errors and perform a visual check of the generated data.

       

       

      If i send these files to the pcb manufacturer, the moment the manufacture finds these errors, the production stops and I receive an error report and a request to 'repair' the gerber data. The only way I can do this right now is by importing the Gerber data into Gerbtool (Wise) and perform a save.

       

      Does anyone recognize this problem and , more importantly, how do you deal with this ?

        • 1. Re: Problems with Gerber data from Expedition
          yu.yanfeng

          Hi Charles,

           

          This symptom is very common in Expeditionpcb 2007.X, especially when you use 5:5 mm data format and using positive plane. Self-intersecting polygon also is common in most or gerber data where including planes.  CAM tools have a robust algorithim to process  SIPs, but Valor's Trilogy 5000 or Genesys 2000 will fails when translate it into the system when your data in 5:5 data format and somtimes Trilogy 5000 7.6.3 will wrongly raster out the data.  Following method may be helpful to eliminate SIPs:

           

          1 Never change the desing unit from mm to inch or versa after you have placed shapes

          2 Never using a different unit with layout unit to ouputput gerber data

          3 avoid to use 5:5 mm or 5:5 mil data format.

          4 It's better to add Gencad netlist  into your cam data.

           

          In fact, this sympotom also be in other CAD systems . Hope Mentor can improve it soon.

          Yanfeng

          • 2. Re: Problems with Gerber data from Expedition
            yu.yanfeng

            Use x:2mm or x:3 mil data format can make Expedtionpcb to ouput gerber data with no SIPs.Pls let me know it'effectness to your design.

            • 3. Re: Problems with Gerber data from Expedition
              charles.ietswaard

              The gerber data is generated using the following settings;

               

               

              Data type : 274X

              Data Mode : Non-modal

              Step mode : absolute

              data format 3.5

              Zero truncation : Leading

              Character set : ASCII

              Arc Style : Quadrant

              Delimiter : *

              Comments : On

              Sequence numbering : off

              Unit : mm

              Polygon fill method: raster

               

               

              The design is also in mm.

               

              Changing the settings does not affect the polygon created. But, you can overcome this problem by loading the data into Gerbtool and do an "Export Gerber". This is nice as a workaround, but the data generated in the first place should be without any problem. I have created a SR on this issue and we will see what happens next.

               

               

              Charles

              • 4. Re: Problems with Gerber data from Expedition
                yu.yanfeng

                Very thanks. Yeas ago, I have logged SRs and attached test data,but Mentor never give me any reply. I think SIP problem was caused by Mentor's plane date generating algolithm. Because We used to use 5:5 format and positive planes, so Valor always warning SIPs to 60%+ gerber data . After changing to 3:2(mm) and regenerated all plane data(setting all plane type to dynamic), most should be OK.

                 

                 

                Yanfeng