1 2 First Previous 20 Replies Latest reply on Jul 23, 2012 7:36 PM by dmeeks

    Output Gerber files are not Aligned

    bhojaraj.go

      Hi Everybody

                           I am user of Pads 9.2,I designed 6 Layer PCB in this and i created gerber using cam options,after that i imported those in CAM350 but gerbers are not aligned from top to bottom and also nc drill file not aligned,Anyway i sent that to manufacturer he also sent the same thing.Please anybody give solution for this.

       

      Thanks in advance

        • 1. Re: Output Gerber files are not Aligned
          jduquette

          Check your Gerber plot setup <File><Cam...>(select a plot) (Edit), (Options), (Justification section).  If the plots are centered they probably won't align.  The offset is not global, and needs to be set for each Gerber file.  If one has an incorrect offset, it will not align with the others.

          • 2. Re: Output Gerber files are not Aligned
            bruce.northrop

            I had the same issue when I started using PADS.  To fix it, I loaded the gerbers in a CAM viewer, I use Altium's CAM viewer.  Pick a layer to start with where you want your stackup to be.  Pick a point that is easy to identify on all layers, corner of the board is usually best.  Measure from that point on your first and to that same point in the next layer.  This will be your offset that you need to manually to enter in PADS.  Under File--CAM--Layer Edit--Options.  You will need to do this for each layer.

             

            Bruce N

            • 3. Re: Output Gerber files are not Aligned
              bhojaraj.go

              Hi thanks a lot for the replay,I tried it worked 100% .

              • 5. Re: Output Gerber files are not Aligned
                max_clark

                What has been described in this thread is a typical data exchange process challenge that is resident in the use of traditional CAM data exchange formats, one of which was Gerber.  The truth of the matter is all CAM systems in use by PCB fabrications have had to develop tools answering this exact shortcoming within these formats.  It is admirable that you are attempting to send Gerber data in a manner that is the best as it can be, but is that really enough?

                 

                Existing today is an alternative to the lower-level task driven formats such as Gerber and Excellon. The ODB++ format has the ability to transfer all, or user-selected portions, of the PCB product-level intelligence required to support the PCB manufacturing processes (fabrication, assembly, test).  Therefore, the ODB++ format enables design-to-manufacturing integration within the fabrication, assembly and test processes, while still protecting the design’s intellectual property (IP).  In doing so, the ODB++ format eliminates the daunting and risky tasks required to reconstruct the product-model from multiple legacy formats and the processing of additional information received in non-standard formats.  These same product-model reconstruction tasks are often repeated multiple times within the PCB manufacturing supply chain.

                 

                As part of PADS 9.4 is an updated ODB++ output process developed specifically to enable the quick adoption of the ODB++ format in support of intelligent data transfer into manufacturing.  The ODB++ export functionality enables a fully automated ODB++ comparison to the traditional CAM formats of Gerber 274X, Excellon and IPC-D-356A.  Users can use the CAM Compare functionality to not only view the ODB++ data, but also compare and view the other CAM formats simultaneously.  The functionality built into PADS 9.4 eliminates the need to use any other Gerber viewing solution in the support of manufacturing, while enable the use of ODB++ as a viable format replacement.

                 

                I politely ask you consider whether to continue correcting traditional CAM format legacy issues is the right place to invest or whether a more intelligent data exchange process support by the ODB++ format may be a more sustainable solution. To learn more about the ODB++ format, please visit the ODB++ Solution Alliance at www.odb-sa.com.  This site can provide you access to resources that further describes the ODB++ content and how the format solves a variety of data exchange issues.  You will also find a free ODB++ Viewer that can be used independently from PADS, complements of Mentor Graphics.  Finally, the detailed ODB++ format description is available for download.

                 

                Regards,

                Max Clark

                • 6. Re: Output Gerber files are not Aligned
                  jim.granville

                  max_clark wrote:

                   

                  To learn more about the ODB++ format, please visit the ODB++ Solution Alliance at www.odb-sa.com. 

                  ODB++ is a good idea, but anyone literally following your advice will be greeted by this message at that web site :

                   

                  This is what it said, when I went to learn more about the ODB++ format, by getting the specification.

                   

                  ODB++ Format Specification

                  Sorry, the requested resource(s) are only available to registered Solutions Partners of ODB++ Solutions Alliance Website.

                   

                  A format where a CAM user cannot even obtain a copy, is not going to impress many potential users.

                  It is also not quite what the FAQ suggests

                   

                  1. Is ODB++ available to the whole industry?

                  Yes, ODB++ is available to all, both in terms of the format definition and

                  implemented via commercially available interfaces and CAD/CAM tools.

                   

                   

                   

                  • 7. Re: Output Gerber files are not Aligned
                    yu.yanfeng

                    For ODB++ Specification, just go to http://www.odb-sa.com/ where you can download the spec after registering.

                    Yanfeng

                    • 8. Re: Output Gerber files are not Aligned
                      max_clark

                      Jim,

                       

                      Thanks for point this out.  What you found is an incorrect setup on the ODB++ Solution Alliance website.  We will correct and you WILL be able to download the ODB++ format.

                       

                      I appologize that you found what you did.  I would have not directed you to the site unless I believed you will be able to download the format specification.

                       

                      Regards,

                      Max

                      • 9. Re: Output Gerber files are not Aligned
                        max_clark

                        Jim,

                         

                        The ability for ODB++ Solution Alliance members to download the ODB++ Format specification has been returned.

                         

                        I hope you accept our apology and return to the ODB++ Solution Alliance website, www.odb-sa.com, and download the format specification.

                         

                        Regards,

                        Max

                        • 10. Re: Output Gerber files are not Aligned
                          jim.granville

                          max_clark wrote:

                           

                          Jim,

                           

                          The ability for ODB++ Solution Alliance members to download the ODB++ Format specification has been returned.

                           

                          I hope you accept our apology and return to the ODB++ Solution Alliance website, www.odb-sa.com, and download the format specification.

                           

                          Regards,

                          Max

                          wow, that was quick!  thanks.   I figured it was more of an oops. ( DXF specs are freely downloadable)

                           

                          Nice spec, I can see they have an attribute defined/allocated for

                           

                          .comp_height

                           

                          I would suggest they should also define/allocate one for

                           

                          .comp_height_offset

                           

                          which then covers the common 3D CAD ability, and allows to have a correct ODB++ file for any part that appears above and below the board plane.

                           

                          There are many parts where this happens, and define of a field name, will allow CAD flows to better support this.

                           

                          PADS even has this data available, now, in the old legacy system of

                          $hh oo

                          text on decal layer 30.

                          ( eg  $200 -100  defines a part 200mils high, 100 mils above, and 100mils below, the board plane )

                           

                           

                          but the importance of the height_Offset has got a little watered down over time. Strange, as it actually matters more and more as designs get tighter.

                          • 11. Re: Output Gerber files are not Aligned
                            dmeeks

                            Getting back to the original issue of the Gerbers being misaligned, it seems that Pads aligns each Gerber according to that layer's contents. So I can't see any way to align all layers so that they are in perfect alignment when the Gerbers are generated, unless every layer in the design has some element that is at, say, the bottom left of the board, in the same place. So a "corner" feature on every layer maybe. Then, in the Cam setup, align the outputs to the bottom-left, and all layers should be aligned.

                            Sheesh! Is there a better way to do this?

                            Note - I tried adding a "target" on each layer, and placed it outside the board outline, on the bottom left, but apparently features outside the board outline are ignored when Gerbers are generated, so it made no difference to my outputs.

                            I have a board house asking me to "fix" my Gerber alignment... is that possible?

                            Thanks

                            Dan

                            • 12. Re: Output Gerber files are not Aligned
                              David Ricketts

                              jduquette answered this in the second post, so to expand a little on that reply, set all the gerber alignment types to offset, and give them all the same offset, including the drill file. The amount of the offset will be the distance from the origin of the PCB to any point in the lower left quadrant that is outside the extents of the gerber data.

                              • 13. Re: Output Gerber files are not Aligned
                                dmeeks

                                Thanks, but that does not align the Gerbers.

                                 

                                The first point in the lower left of the Silk layer is in a different place than the Top Copper layer.

                                 

                                I’ve confirmed that this is how it works. So unless every layer has the exact same feature as its most-lower-left point, they will not line up.

                                 

                                Right now I am putting a small “corner” on the lower left, right on the board outline, for every layer, and that does align the Gerbers, but now I expect to get a complaint that there is copper on the edge of the PCB.

                                 

                                Dan

                                • 14. Re: Output Gerber files are not Aligned
                                  jim.granville

                                  dmeeks wrote:

                                   

                                  Thanks, but that does not align the Gerbers.

                                  Are you sure you selected CAM.EditDocument.Options.Justification[offset] ?

                                  That offset choice is an Origin offset, and it does not care about Gerber content.

                                   

                                  The five options on the CAM Justify list above [offset], are margin offsets, and they DO care about content.

                                   

                                  A new PCB Design project, looks to default to origin [offset] 1000,1000 mils in CAM options, which is what we always use.

                                  ( I guess centered et al are legacy options, from way back when you created films and then worked from there.)

                                   

                                  Some Gerber tools will attempt to Auto-align plots, which they can do quite well on round thru hole pads.

                                  1 2 First Previous