7 Replies Latest reply on Aug 7, 2010 8:48 AM by TBD

    CAM350 netlist verification errors

    aakula

      Hi,

      I am kind of new to CAM350 and having trouble with doing the netlist  verification.
      I am using CAM350 v8.6.2

      I have imported the Gerber files into CAM350 (using  File/Import/AutoImport).
      Run the Draw to Flash, filled in the layer info, extracted the netlist  (Utilities/Extract netlist).
      Imported the IPC-D-356 netlist (created by Allegro).

      When I do Compare netlist (Analysis/nets/compare external nets), I get  two types of errors.

      1) No Copper
      2) No Point On Cam Net

      I do not understand what the "No Copper" means

      Also I have tried to export the Gerber netlist as a IPC-D-350 file  (file/export/IPC-D-350) and compared some of the nets (starting and  ending points) with error 2 with those in the Allegro created netlist.
      They look correct (i mean i can look at them with correct positions in  the Gerber files).

      Could some one suggest me how to proceed with the "No Copper" error?


      Thanks in advance,
      Regards,
      Aditi.

        • 1. Re: CAM350 netlist verification errors
          yu.yanfeng

          Do you check the layer types?  To make CAM350 extractes netlist from your gerber data, first you should correctly set layer types(signal, copper etc).

          BTW, CAM 350 is weak in netlist verification. I suggest you move to Vsure.

          Yanfeng

          • 2. Re: CAM350 netlist verification errors
            TBD

            Hi Aakula,

             

                  Dont worry about these errors.  when you check IPC in CAMV350 should be care Short, Open errors. Ignore all other errors, i dont know exactly that why but maybe there are some different between IPC cordinate since generated and net list export from CAM.

                  Believe me, dont care other errors except Short/Open.

            • 3. Re: CAM350 netlist verification errors
              aaron.palomar

              Hello Aditi,

              There is a bit of a process to get ipc netlist into CAM350 (any version)

              It has been awhile since I have done this but from what I recall it goes like this:

               

              1. import gerber data and drill file.  (all layers and drill need to be exactly aligned) Also, make sure origin in cam350 exactly matched origin of ips netlist or allegro data.

              2. define layers in cam350

              3. convert polygon draws to flash.  (this is a bit fuzzy in my memory but I think you want to end up with flash)

              4. convert pads to padstacks.

              5. generate netlist to compare to in cam350.

              6. import ipc netlist.

               

              After cam350 generated netlist comares to ipc netlist and you have no errors you be good to go.

               

              Regards,

              a-

              • 4. Re: CAM350 netlist verification errors
                aakula

                Hi All,

                 

                Thank you for your answers.

                 

                Now, when I check, I have composite layers (4) and my Gerber data is in 274X format.

                So, do I need to Convert the composite layers into a single layer?

                If so, I have another question, when I convert the composite layers into single layer (Utilities/Composite to Layer/New layer)

                I am getting the converted layer onto a new layer. So do I have remove the original composite layers and reorder my layers?

                 

                Also, if I do that and Draw to Flash and compare netlists, I have 2 errors.

                !) Open

                2) Short

                 

                The Shorts are shown along the fingers of my module (module is similar to SIMM memory).

                It looks like the spacing between the fingers is about 4-5 mil and CAM350 is not able to recognise the

                spacing and shows them to be shorts.

                Is there a place where I can mention the tolerance and the minimum spacing to look at?

                 

                Regards,

                Aditi.

                • 5. Re: CAM350 netlist verification errors
                  aakula

                  Hi all,

                   

                  Looks like I have found the problem.

                  I am attaching a screen shot of the problem.

                  It appears that the fingers are getting shorted by the outline.

                  The outline is present on the top and the bottom layers and

                  CAM350 somehow thinks the outline is copper. And hence gives the Short errors.

                   

                  Can somebody tell me how to remove or enlarge this outline?

                  Is there any setting in CAM350 which I can set tto mask the outlien or something.

                   

                  Is there a particular reason the layout house has added the copper outline to a SIMM module that has an edge connector.
                  Is that a standard procedure?

                   

                  Regards,

                  Aditi.

                  • 6. Re: CAM350 netlist verification errors
                    aaron.palomar

                    Yes,

                    It sounds like board outline was included to each routing layer when gerbers were generated.

                    The easiest way to fix this is to remove outline from etch layers  when generating gerbers and output board outline on its own layer.

                     

                    If this is not possible you will have to manually delete outline from etch layers in ca350 before importing netlist

                     

                    a-

                    • 7. Re: CAM350 netlist verification errors
                      TBD

                      Hi Anula,

                      Thats good, really difficult to see where is Short/Open in CAMV350 (i used ver. 9.2).

                      You can move the board outline to the other layer if needed. Because of the CamV350 environment can't understand Board Outline, thats reason causing Short Error above.

                      I just want to inform you that you can change thickness of Board Outline to smaller or larger instead of move to other layer. In this case, try to reduce the thickness (Change Dcode) untill you see Board Out line dont touch to Finger pads. then, regenerated Netlist and check IPC again.

                       

                      Adding more (if you dont know how to change Dcode):

                           1. Press Q --> touch Board Outline --> the Dcode will be appeare. take note this Dcode, shape, value , Ex: Dcode100, Round, value:10.

                           2. Define other Dcode: press A --> Dcode table will be appear --> you can see all Dcode were defined here, be careful, if you change any Dcode here the data gerber will be wrong. Kindly press other Dcode (such as 1234, remember 1234 is not value) --> select Shape (Round) --> value :5 (if you want to reduce the Board Outline from 10 to 5) --> Enter ---> ok.

                           3. Edit/Change/ Dcode : Click Board Outline --> Right click --> Enter Dcode 1234.

                           Now , you changed from Dcode 100 to Dcode 1234.

                       

                      good luck !