7 Replies Latest reply on Jul 30, 2013 12:23 PM by michael.weinberg

    How important is in-house expertise in regard to successful EDA implementation?

    michael.weinberg

      I've been a PCB Designer/ECAD Administrator/ECAD Librarian for over 30 years and I've never seen cells built as shown in the image.

       

      This company required the placement outline to encompass the cell's pads as shown in the image.

       

      Cell Placement Outline includes Pads.JPG

       

      I see no benefit to creating cells this way, yet I do see significant drawbacks.

       

      The ECAD system has separate DRC checks for physical items (i.e. placement outline-to-placement outline) and electrical items (pad-to-trace, trace-to-trace, etc.)

       

      With the Placement Outline encompassing the pads, the electrical checks are trumped by the mechanical checks or vice versa depending on the actual design rules. This is an unnecessary limiting of the software's DRC capabilities.

       

      For QFPs (Quad Flat Packs) the corner areas between groups of leads are unavailable for placing other devices unless DRC is disabled. There are false DRC error messages that are generated for devices placed in these otherwise acceptable locations.

       

      Another drawback is with 3D rendering of the PCB when mechanical models are not yet available for mapping. In this case the placement outline is extruded in the +Z axis to the height specified in the cell (1.75mm in the example shown), which looks strange and unfamiliar.

       

      I think this procedure was originally defined by an electrical engineer working as ECAD administrator, someone who had little or no PCB design experience.

       

      This is why electrical engineers make lousy PCB designers or ECAD administrators. Yes, it involves electronics, and the electrical engineer is the only customer I need to satisfy in regard to the PCB layout, but It's a totally different discipline and methodology than electrical engineering.

       

      For this reason, I advocate for a separate ECAD department, call it Engineering Services. There should be representation on the ECO committee for Engineering Services in addition to Engineering. This would enable some advocacy for PCB designers and excellence in ECAD operations.

       

      Although I often open my mouth only to change feet, I might as well voice some other pet peeves that still irk after all this time in industry.

       

      Please read with an implied "In my humble opinion..." and feel free to respond.

       

      1. Electrical engineers should stick with electrical engineering and let experienced PCB design staff define how best to satisfy the engineers' requirements. Companies would be well-advised to bring in ECAD consultants in addition to EDA vendors if the in-house staff does not have expertise in ECAD administration or intimate familiarity with EDA software.
      2. Symbol, padstack, cell, and part creation should be completely documented in unambiguous detail and as concisely as possible. This documentation should be ECO-controlled and is critical when multiple design sites contribute to the corpoarte library.
      3. Companies typically use their less experienced employees as ECAD Librarian. This could work if excellent documentation and training are provided, but it's a train wreck otherwise. The CAD libraries are the foundation of all electronic development. A poor implementation here will soon get out of hand to the point where ECAD administrators are too busy putting out fires to have any time available to fix the problems causing those fires!
      4. ECAD administrators should have a broad and deep working knowledge of the software used, otherwise there is no hope of changing or improving a poorly-implemented ECAD system. Any change or proposal not fully understood by the ECAD administrator will be deemed too risky.
      5. PCB designers are better suited for the position of ECAD administrator than are electrical engineers, but even so may lack an adequate understanding of other parts of the tool such as schematic capture, simulation, MCAD-ECAD data sharing, ECAD library, etc.
        • 1. Re: How important is in-house expertise in regard to successful EDA implementation?
          thad.schultz

          Michael,

           

          When I first saw your post I thought, "Is he talking about my company?".  My company does this.  I am currently the ECAD adminstrator / librarian.  This was done this way before my time so I have inherited this rule.  The librarian before me was not an engineer and was very sharp and I respected her as an librarian.  My thinking is she must have had a good reason for doing this.  Maybe it is because back in the day we were using Mentor BoardStation and this was to make up for some shortcoming in the tool that I am not aware of.  Now we are in Expedition PCB and all of our BoardStation cells were translated to Expedition at one time.  We still have our placement outline encompassing the pads like you show.  Of course my situation now is to go forward with this for new cells created or I will end up with a mix of encompassed pads and not encompassed ones.  Or I modify all of my existing cells.  Ha!  Not likely.  So I just wanted to share my situation as another data point.  One question that I have is do the DRC rules ignore the pads inside of the part outline like you suggest?  I was hoping that the X-to-pad checks still looked at the pads encompassed by my part outline.  But I really don't know.

           

          As far as your 5 points go I agree whole-heartedly with all of them.  Your point two is key!  Like you say make it as unambiguous as possible.  Don't leave anything out or it will be open to interpretation!  I say this from experience.

          • 2. Re: How important is in-house expertise in regard to successful EDA implementation?
            michael.weinberg

            Hi Thad,

             

            Thanks so much for your response and for a data point I was not expecting. I am surprised to find that this method of encompassing the cell's pads within the placement outline has been adopted elsewhere. Do you apply this method to discrete components as well as to the major ones?

             

            I just got off the phone with a friend of mine who works for a big multinational company as Global ECAD Administrator and they use the same method as at your company. It's interesting to note they too have transitioned from Board Station to Expedition.

             

            For this company, it appears the major components are given this treatment but discrete components are not. For discretes, the placement outline represents the maximum dimensions of the component body and does not encompass the cell's pads.

             

            IPC standards used to define a footprint "courtyard", a rectangular outline that encompassed the extents of a device package and its' PCB footprint, resolved upward to a 0.5mm grid. I think the courtyard was used for "floor-planning", a way to provide sufficient room on the PCB for circuit placement and routing back in the days of TTL logic. Perhaps this is a carry-over from that. Maybe placement outlines are functioning as courtyards although I have always considered the two as separate entities.

             

            Still, I see only disadvantages to applying this method and no advantage. I look forward to hearing more from others on the topic. Here's an image to illustrate how physical and electrical DRC rules may be effectively applied during placement. I believe the effectiveness of this approach may be diminished (depending on the actual design rules) when placement outlines encompass the pads.

             

            Using Physical and Electrical DRC rules.jpg

             

            Thanks for weighing in on my 5-point rave. I agree with you that clear documentation is critical for CAD library work, and that consistency should be maintained in CAD library work whether right, wrong or indifferent. Consistency informs, inconsistency confuses.

             

            In response to your question "...do the DRC rules ignore the pads inside of the part outline like you suggest?" I say no, nothing is ignored by DRC, but in the case of two conflicting DRC rules the one with the greater clearance will prevail, as it should.

             

             

            Regards,

             

            Mike

            • 3. Re: How important is in-house expertise in regard to successful EDA implementation?
              yu.yanfeng

              There are different requirement to component' Profile and indeed may companies prefer to create component outline which including pin extrudes. I agree that a well-quality libary should consider every things such as data integrity, easy of use for schematics entry and pcb layout, supporting visual DRC/DFM check , suppoting better MCAD-ECAD data change, associated CAE models, and should also consider the limition of various ECAD systems.

               

              I have helped our company to establish an library infracture which is based on neutral data, support both Allegro flow and ExpeditionPCB flow and the most challenge is that the limitions of various ECAD system. I really appricate Mentor and our industry to push EDX ahead and make it a reality that

              every part' libary data be pushed and distributed in XML format, ported to dedicated ECAD system based on your policies to support versitle requirements from different user/usage or ECAD limitation.

               

              yanfeng

              • 4. Re: Should Placement Outlines include the pads of the cell?
                michael.weinberg

                A neutral XML-based library data paradigm sounds like a good idea once a standard has been created and adopted by industry, which seems to be a very difficult thing to do. But that does not answer the question, should the placement outline include the pads?

                 

                What do you do at your company with Placement Outlines? What are the advantages or disadvantages that you see with either approach?

                 

                I see only disadvantages to including the pads in cells (see original post) and so I ask, "What good does it do to include the pads in the placement outlines"? Is there some benefit to doing things this way?

                 

                It seems as if many companies do this so there must have been some paradigm established somewhere by someone. Was it an EDA vendor? IPC?

                 

                Mike

                 

                p.s. I'm changing the subject line to be more in line with the active discussion.

                 

                Message was edited by: michael.weinberg

                • 5. Re: How important is in-house expertise in regard to successful EDA implementation?
                  David_S

                  I agree on a lot of things you are talking about, but as to why you have to include pads in the placement outline, see the picture below.  This is 100% legal during placement, and will only show an error, if you set rules that will flag errors on about 99% of parts.  (ei. in the picture below, pins 1-4 on the IC will be errors!)

                   

                  why.jpg

                   

                  We had been using Boardstation, which has a flag to alway include the pads in the placement outline, which fixes this issue.  Also, if I remeber correctly, there was also a rule for pad to another's part placement outline to pads.  Expedition does not have a rule like this, or not one I can find.  Now maybe they've fixed this in a newer version, but as far as I know, they haven't.

                  1 of 1 people found this helpful
                  • 6. Re: How important is in-house expertise in regard to successful EDA implementation?
                    michael.weinberg

                    Hi David,

                     

                    Thank you for your response. Your comments and example really helped bring clarity to the issue.

                     

                    BoardStation seems to be a common thread among those who include the cell pads in the Placement Outline.

                     

                    I've never used BoardStation. Does BoardStation use Placement Obstructs as well as Placement Outlines like Expedition? Can you define several non-overlapping Placement Outlines of differing Height properties within the same cell as in Expedition?

                     

                    If not, perhaps this was the "shortcoming" in the software that Thad mentioned as a possibility for the development of this paradigm. It makes total sense then to include the pads in the Placement Outline.

                     

                    Your example shows a situation where the tool will allow the placement but an error would be flagged only when DRC is run (if there exists a "placement outline-to-other cells' pads" design rule check). This is clearly unacceptable as we need realtime feedback during placement and should not have to run DRC to find these kind of errors.

                     

                    Expedition's rule matrix can check placement outlines against SMD pads or through hole pads, but unfortunately that check also applies within the same cell, so many false errors would be generated. This, too, is unacceptable.

                     

                    Now I understand the point that Yanfeng made regarding the different requirements in the use of Placement Outlines across the spectrum of EDA tools. I agree that a quality library will consider all aspects in how those cells are used including DRC, MCAD-ECAD interface, DFM requirements, etc.

                     

                    In regard to those criteria, the MCAD-ECAD interface is not optimum when including the pads in the cell's Placement Outline for the reason stated in my original post. This issue goes away if an accurate MCAD model has been created and mapped to the cell. In any case this is a minor consideration in contrast to allowing an illegal placement.

                     

                    If I were to start a new library for use with Expedition, I would use Placement Obstructs in those locations where the pads extend beyond the Placement Outline as shown at the right in the attached image. It is important that the Placement Obstructs do not overlap the Placement Outlines within the same cell, otherwise "false" DRC errors will be generated.

                     

                    Placement Outline Issue 1 - 3.JPG

                    Thanks eveyone for a great discussion.

                    • 7. Re: How important is in-house expertise in regard to successful EDA implementation?
                      michael.weinberg

                      One might consider converting the Placement Obstructs into Placement Outlines with a width equal to the lead thickness. This would give a more WYSIWYG extruded rendering in the absence of a mapped MCAD model.

                       

                      Further testing is needed to check for any potential downstream issues when using Placement Obstructs or multiple Placement Outlines for component leads which extend beyond the component body.