1 2 First Previous 24 Replies Latest reply on Mar 16, 2012 8:09 AM by jmatthews

    solder mask on wrong layer


      Here's a strange one.  I created two fiducial decals, one for the top layer(FIDTOP) and one for the bottom (FIDBOT).  The top fiducial pad stack defines a pad (on 'mounted side') of 50 and a pad on the TOP side solder mask of 150.  The bottom fiducial also has a mounted-side pad of 50 and a BOTTOM side solder mask pad of 150.  BUT when I place the bottom fiducial, there's no pad on the bottom solder mask.  BUT, miraculously, there's a pad on the TOP side soldermask. In other words, regardless of which soldermask layer I place a pad on, it ends up on the top.   After wasting 2 hours of my life on this, I discovered the following:  If I place FIDTOP on the bottom layer, the pad explicitly defined for the TOP side soldermask appears on the BOTTOM side soldermak. It appears that when generating soldermak layers, PADS interprets "bottom" solder mask as "OPPOSITE" soldermask


      Is that the way this is supposed to work? What's the point of explicity telling a pad what layer to go to, when the software is just going to stick it wherever it wants?

        • 1. Re: solder mask on wrong layer

          I use one Fiducial decal  (top pad and top soldermask) and place this part on the bottom for a bottom fiducial. Keeps it simple.


          • 2. Re: solder mask on wrong layer

            "The bottom fiducial also has a mounted-side pad of 50 and a BOTTOM side  solder mask pad of 150.  BUT when I place the bottom fiducial, there's  no pad on the bottom solder mask.  BUT, miraculously, there's a pad on  the TOP side soldermask."


            that's because you placed the soldermask pad on the bottom soldermask layer and when you place the part on the bottom side, the bottom side soldermask pad is now on the top (and your top side pad is on the bottom since that is the side of the board you placed it on


            IOW, it is acting exactly as it is supposed to, your error was placing the solder mask pad on the bottom side, should have been on the top side solder mask if your intent was to place the part on the back side


            you could have placed the part on the top side, but defined the pads on the bottom layer, and bottom layer solder mask, but I agree with previous poster, keep it simple

            • 3. Re: solder mask on wrong layer

              You are starting to understand how PADS works.  If the part is mounted on the TOP side the top mask is on the top.  If the part is mounted on the BOTTOM side the top mask is on the bottom.  'Mounted side for TOP and Opposite sdie for BOTTOM would make more sense.


              The trick to remember is that the decal editor only defines TOP mounted components.  It is up to the user to flip them with layout if they want them on the bottom.  Keepin' it simple...

              • 4. Re: solder mask on wrong layer

                Our team have experienced similar situation having the solder mask placed on the wrong layer.

                After you have developed your PCB decal correctly as per your requirement on the paste mask or solder mask etc..

                you might want to check the "Component Layer Association" of these layers on the Layer Definition in PADS Layout.

                Be sure to check that the Top Layer is associated to the Paste Mask Top, Solder Mask Top, and Assembly Top layers.

                Same applies to the Bottom Layer is associated to the Paste Mask Bottom, Solder Mask Bottom, and Assembly Bottom layers.


                Have a look at the attached files...

                • 5. Re: solder mask on wrong layer

                  "IOW, it is acting exactly as it is supposed to"


                  I beg to differ.  When you identify a layer as BOTTOM SIDE SOLDER MASK, it should be on the BOTTOM, not the top.  There would be no confusion if it was identified as OPPOSITE side Solder Mask.  Pads are identified as MOUNTED side and OPPOSITE side, why then aren't mask layers consistent with this methodology?????  They are mixing relative and absolute references.

                  • 6. Re: solder mask on wrong layer

                    Hey All, new here, new to PADS, longtime Altium user.  Found this post and would like to re-visit it since I'm having the same issue.  New hired, first task is rebuilding the company library in PADS.  My parts are defined properly, s/m added on s/m layer, p/m added on p/m layer.  But when I place my part on the board, the parts on the top side have s/m on the bottom side.  Flip the part to the bottom, the s/m flips to the top.  Spent several hours trying to figure it out.  Any suggestions??





                    Bruce N.

                    • 7. Re: solder mask on wrong layer

                      See my 6/29/2009 post about 'mounted' side vs 'opposite' side.


                      Check your pad stack in the decal editor, and then check it in Layout to see if that gives you any clues.

                      • 8. Re: solder mask on wrong layer

                        I've checked the decal, I have a copper pad on Mounted Side, which I would take to be Top.  Solder Mask on Solder Mask Top.  But now it gets strange.  On my board, I double click on the part, it says R1 on top.  Double click on Pad Stack, it says shape on Mounted Side and Solder Mask Bottom.  The part is on the top, has always been on the top.  I'm confused.





                        • 9. Re: solder mask on wrong layer

                          Select <Setup><Layer Definition...> and then click on your Top layer.  Press 'Associations'.  Here you can associate your top side parts with the bottom solder mask, but I don't know why someone ever would.  Maybe you have a legacy issue that someone fixed something the wrong way a long time ago.



                          • 10. Re: solder mask on wrong layer

                            Hello Bruce,


                            When you create Decals in PADS you have number of way to configure your padstack, solder mask and paste mask openings. By default you do not need to specify S/M and P/M because during Gerber creation you can specify over/undersize created from padstack itself. Also you can build into Decal actual pad with particular size for that layer and lastly you can create an attribute that control that and override the default (see attached).


                            You can also look at the supplied Library that came with PADS installation for examples how the padstack are handled.


                            Without seeing your part it is not easy to troubleshoot your particular problem. Best is for you contact our Support Group and they will help you in no time.


                            Regards, Yan

                            • 11. Re: solder mask on wrong layer

                              Now that I just read the help for the Associations page, it says it is only for the CAM output.  Did something get crossed in two places?

                              • 12. Re: solder mask on wrong layer

                                If you post a .d file  (v9.x) we can take a look.

                                • 13. Re: solder mask on wrong layer

                                  You've got some good answers here, but I'll try a simple (though long-winded) answer/explanation....


                                  A NOTE - I've changed my default naming conventions from the PADS defaults to "Primary" for what is called Top ("Mounted" in the Decal pad stack window) and "Secondary" for what is called Bottom ("Opposite" in the Decal pad stack window). So bear with me on that.


                                  And yes, the different terminology in the different areas is confusing....


                                  Part creation in PADS is intended to done as if it is mounted on the "Primary" (aka "Top", "Component", or "Side A") Side. So forget about what side it will wind up on in the board.


                                  When you build a part, just assume that it is on the Primary side. If you do pad stacks, place for the primary side for SMT parts. The Secondary side soldermask and solderpaste pads (and in some rare cases, silkscreen and assembly layers) would normally only be used for THT parts when building a decal. Though there is an occasional (rare) SMT part that will require some of the Secondary-side stuff.


                                  So, you build one Fiducial (not two different ones ), then push to the secondary side if you want it there.


                                  DO NOT mess with the layer associations unless you do some VERY specialized boards where that stuff can be permanently left changed. FYI, the fiducials (and any mounting holes that do not have an electrical connection) do not have to be in the schematic, build them as "non-ECO" and place them in your board using the ECO mode.


                                  Personally, other than the base library for IC pins, and other similar basic items, I wouldn't use the supplied libraries for anything other than as a starting point/example. And even then, they have some things that aren't good (unless they've changed them, I haven't looked at the default libraries in years). For instance, among other things schematic symbols(Parts) and Decals aren't always correct and/or are poorly done. Also, text sizes and line widths aren't consistent from part to part..


                                  Some tips (note most of this is based on how I do things - to each his own of course) on decals -


                                  - DO NOT put ANYTHING on "All Layers" in a Decal.


                                  - Personally, I use "Primary Side" for my silkscreen outline and associated designator only. Any added text needs to be either a  Primary Side attribute (don't forget to make Attributes visible in your colors and in your CAM setups if you do this) or on the Primary Silkscreen layer. I personally only use the Primary Silkscreen layer for non-attribute text, I do not use the Primary Silkscreen for my silk outlines or designators, but some folks do.


                                  - Personally, I create a to-scale, even somewhat detailed (depending on the part and/or whatever minimum detail is needed), part image on the Primary Assembly layer, with its own ref des (center-center, orthoginal), usually centered inside the image, no matter how small (execept for stuff smaller than the equivalent of an 0402 R or C). If you place the designator properly, any cleanup to the assembly image will be none to minimal (which is why I place it on the inside of the part).


                                  - I do use pad stacks, with the solderpaste set at 1:1 to the pad, and the soldermask nominally at 5 mils (yes, I do stuff in mils - so sue me) over the pad size. Obviously, in some cases (like BGAs) the mask is reduced, in other places it will get larger than the 5 mils (generally for THT parts - but not by much,  Fiducials, and for mounting holes - or on some parts as indicated in a data sheet). I will customize these at times to meet a customer's needs. The reason I leave the paste at 1:1 is that I find a lot, if not most, assembly shops like to modify these to meet their requirements/processes/procedures.


                                  - You can build in some keepouts on Decals, like copper pour, TP, Via - but not all keep-out types can be assigned.


                                  - I set aside a couple of layers in my boards, 19 and 20 for "standard" layer count for title blocks and notes respectively. I will include stuff on the "notes" layer in decals for things like board edge alignment, center line(s), part center marks, multi-part-pattern configuration marks, special placement or routing notes (obviously), etc.

                                  • 14. Re: solder mask on wrong layer

                                    Hi All,


                                    Thanks for all the replies.  Still no luck getting this resolved.  I realize that I can leave the S/M out of the padstack and specify it in the CAM, however I always like to be able to see my S/M openings when I'm designing a board, just a personal preference I guess.  The engineers I work with could care less about it.  I have been building library parts for years in Altium, have a very large library in that system, so I very familiar with how parts need to be built.  Just for the fun of it, I opened a NEW schematic, dropped a couple parts, ran an eco into a NEW pcb and everything worked as it should.  Parts placed on the top side have S/M on the top side, flip the parts to the bottom, the S/M flips to the bottom.  So maybe as mentioned above I have a legacy issue going on in my production board?  There is a mix of libraries being used, my new parts, some parts built by the engineer, and who knows where the rest came from.





                                    1 2 First Previous