6 Replies Latest reply on Feb 14, 2017 12:49 AM by malgumhasan@gmail.com

    Having difficulties on designing Micro-USB connector in PADS

    malgumhasan@gmail.com

      Hello,

      Do anybody has experience on making such Micro-USB connector decal/footprint in PADS ? I am talking about similar parts like ZX62D-B-5P8. I have managed to download this part from a website, but unable to use it in my design.

       

      The downloaded design file says when you open in PADS layout,

      Bad drawing width size 0 CLOSED 9 0 1 -1

      Let me explain you in detail, I am trying to design like

      usb_con_mech_dsn.PNG

       

       

      Until now, I manage to design like

      con_dsn_pds.PNG

       

       

      1. Dont you think, it needs "keepout" areas?
      2. How to draw LAND pads inside pad-stakes area?
      3. Let me know about dimensioning toolbar application here.

      Hope you will help me.

       

       

      Regards

      Hasan

       

       

       

       

       

        • 1. Re: Having difficulties on designing Micro-USB connector in PADS
          wcowles2

          Hasan,

          To fix downloaded component export library component to a .d file. Edit in text editor. Search for string “CLOSED 9 0 1 -1”. Change 0 to 1
          or any number greater than 0. This line as written is saying closed shape with 9 coordinates with a width of 0 is on layer 1 and not associated to any pad.

          Question 1 adding a rectangle on layer 20 tells system this is placement zone to keep out other parts.

          Question 2 draw copper rectangle on top layer, add fillets then associate copper to pin.

          Question 3 not sure I can help with this.

          William

          1 of 1 people found this helpful
          • 2. Re: Having difficulties on designing Micro-USB connector in PADS
            malgumhasan@gmail.com

            Dear Sir William,

            Nice to have your response here. Lets introduce me as new born designer. Take a look my feedback,

            To fix downloaded component export library component to a .d file. Edit in text editor. Search for string “CLOSED 9 0 1 -1”. Change 0 to 1 or any number greater than 0. This line as written is saying closed shape with 9 coordinates with a width of 0 is on layer 1 and not associated to any pad.

            Its a reasonable advice, dont you mean edit in notepad/text editor ? Or you mean Edit text in PADS layout? Search it for where? Let me try more.

            The website where I have been download this design file, they said this issue like "Our PADS support is actually in Beta".

            Dont you think this 2 different environment is conflicting ?

             

             

            adding a rectangle on layer 20 tells system this is placement zone to keep out other parts.

             

            Do you mean I have to work in Layer_20?  Do we need any Layer setup at "Layer definition" tab?

            keep_outs.PNG

             

            draw copper rectangle on top layer, add fillets then associate copper to pin.

            Nice, I got it that associate option can keep it tightly on pad stack, but how to add fillets ?

             

             

            not sure I can help with this.

             

            I do mean this following, It works , but only for mid point option.

            dimensioning.PNG

             

             

            Beside this activities,  this guy has done the job well, Create a PCB Footprint by Tracing From a PDF - YouTube

            Kindly explain this process can add together with PADS layout or not.

             

            Regards

            Hasan

            • 3. Re: Having difficulties on designing Micro-USB connector in PADS
              wcowles2

              Hasan,

              Your right I was not clear enough. Here I’ll try to expand.

              Yes edit text file in text editor.

              Choose “File” then “Library” to get library manager dialog box.

              Select decal filter.

              Use library list at top and text in filter area to get your part to show up in items list.

              Highlight your part in items list.

              Click “Export…” button. This opens a file dialog box to create a .d text file in a chosen directory with chosen name.

              Open .d with text editor. I use notepad for this. Control-F finds the text. Control-H will search and replace. Both will get you to the text from you error box so you can change the 0 to 1. Save changes

              In pads library manager click “Import…” to bring updated part back to library.

              I would then edit part and look at pad to see if width looks right. I usually associate copper to pins to make sure it fills.

               

              Somewhere a while back I read layer 20 is used for body to body space in rule checking. A simple 2D box on this layer is the same as component keep out. Both top and bottom mounted components are on this layer and system keeps them straight. Pads router separates them into top and bottom.

               

              To add fillets;

              While in decal editor click “Tools” then “Options” then “Design”.
              Change diagonal miters to arc.

              Select corner to fillet. You will do one corner at a time.

              Right mouse click menu “Add Miter”. This should prompt you for a radius in the current units setting.

              William

              1 of 1 people found this helpful
              • 4. Re: Having difficulties on designing Micro-USB connector in PADS
                malgumhasan@gmail.com

                Hello Sir,

                Thank you once again.

                Click “Export…” button. This opens a file dialog box to create a .d text file in a chosen directory with chosen name.

                Open .d with text editor. I use notepad for this. Control-F finds the text. Control-H will search and replace. Both will get you to the text from you error box so you can change the 0 to 1. Save changes In pads library manager click “Import…” to bring updated part back to library.

                I think I am missing something which skipped my eyes. Otherwise, folder is corrupted. Take a look the files here. I think layer commends on files as you have mentioned need to understand.

                 

                I would then edit part and look at pad to see if width looks right. I usually associate copper to pins to make sure it fills.

                Did you see whats wrong in my previous design, I am selecting 2 more big size pad stacks , dont you think these should be copper only?

                Is it not  a mistake , I am trying to draw a LAND pad on pad stack ?

                All of your answers are logical I think.

                Now let me ask you few things.

                1. For total  footprint, how many layer I have to consider?

                A simple 2D box on this layer is the same as component keep out. Both top and bottom mounted components are on this layer and system keeps them straight. Pads router separates them into top and bottom.

                2. Does keepout is necessary here, dont you mean 2D plane is enough?

                3. Did you see the mechanical design carefully, some round shape land pad is also necessary.

                4. Did you consider the video clip I have mentioned, if I use this software, cant it linked with pads layout?

                5. In which layer the LAND pad should stay?

                • 5. Re: Having difficulties on designing Micro-USB connector in PADS
                  wcowles2

                  Hasan,

                  Company blocks me from viewing sip files from internet. Maybe someone else could comment on files.

                  To understand the layer comments better goto PADs help menu then “Interface Specifications” then “Library ASCII Specifications”. Your error
                  is in the “Piece Entry Format”

                  I have used a connector in this series. There is a tab that goes thru the slot and gets soldered to the pad. I put the land pad on top and
                  bottom layers over the slot.

                  1. In library only top and bottom layers are shown by default. Will match board when inserted.
                  2. PADs works with outline on layer 20. No keepout necessary.
                  3. Yes you have different pad shapes; rectangles, round, and rectangle with rounded corners.
                  4. Did not watch the video. Not sure what software you are talking about. Mentor Graphics could answer about software linking.
                  5. I would use top and bottom. Tab will be soldered to back side.

                  William

                  1 of 1 people found this helpful
                  • 6. Re: Having difficulties on designing Micro-USB connector in PADS
                    malgumhasan@gmail.com

                    Mr. William,

                    Take look these quick reply.

                    Company blocks me from viewing sip files from internet.

                    Its a common issue in here also. I do agree with you, security s/w could not allow you to open files, helping people is helping GOD we know.

                     

                    I have used a connector in this series. There is a tab that goes thru the slot and gets soldered to the pad. I put the land pad on top and bottom layers over the slot.

                    Could you kindly  put some screen shot here?

                     

                    Mentor Graphics could answer about software linking.

                    Could you specifically tell me any source in this website?

                     

                    Let me ask  ask you few questions those are little bit away from this topic.

                     

                    1. In case of PCB design in PADS layout, manually routing is  bit time consuming, cant I depend on auto routing ?

                    2. When you connect PADS logic with layout, what things you keep in mind in component placing? Do you follow the schematic array? I mean from left to right cascaded circuits?

                    3. What benefit you get, from "via mode", "layer toggle", "Angle Mode" when you do routing ? For design circumstances what you keep on mind? Always control "option" ?

                    4. When do you feel to add Flit components ?

                    5. After significant setting in "Option", take a look this view and leave comment on what we could do for routing ,(its a reference design I am trying to re-design )

                    display.PNG