3 Replies Latest reply on Jun 1, 2011 5:39 PM by David Ricketts

    Creating Silk Screen solid areas in PCB Decals

    rkondner

      Hi,

       

      When drawing Silk Screen 2D lines in a PCB Decal I typically draw then on Layer 1. That gets lines into the Silk for a component but how about solid areas?

       

      Is the only way to draw COPPER for Silk Screen to draw the copper in the SIlk Screen Layer? That implies the decals wont work if used in a PADs environment that has the Silk Screen in another layer, right?

       

      Did the reccommended method for drawing Silk Screen lines in Layer 1 change over the last 20+ years or so?

       

      Perhaps Silk Screen 2D lines should now be drawin in the Silk Screen layer? Again, how about the changing PADs layer setup?

       

      Thanks,

      Bob K.

        • 1. Re: Creating Silk Screen solid areas in PCB Decals
          David Ricketts

          Short answer: Just add the silkscreen copper setting, whatever layer it's on, to the silkscreen CAM file.

           

          Long answer: PADS is relatively unique in that it allows silkscreen information on the same layer as the component. So putting it there has been the recommended method. But I don't recommend it, as I find it too limiting. My decals have silkscreen information on the Silkscreen layer and assembly information on the Assembly layer. The silkscreen information is relatively sparse, basically just a visual aid for placement, and clears all of the exposed copper in the decal. The assembly information is as a complete mechanical representation of the part as I can draw. This is also compatible with other CAD systems, which is useful if you ever need to translate a design.

           

          I also tend to avoid using solid copper in decals. It is subject to the same default settings as the PCB copper, so it can be tricky to get it right. It also doesn't have access to the "Solid Copper" setting that board level copper has. For small areas, I just use a rectangle and overlapping lines. For large areas, just be sure to use a wider line than your default PCB copper grid settings.

           

          I don't understand what you mean by "changing PADS layer setup". I've never needed to.

          • 2. Re: Creating Silk Screen solid areas in PCB Decals
            rkondner

            David,

             

            Thanks for the reply.

             

            What I mean by "Changing PADs Layer Setup" is:

             

              Layer 26 is typically the Silk Top layer. If you add copper to a decal in the Silk Screen Layer" it is recorded as Layer 26.

             

            Now anyone could use Layer 26 for anything. Doing a job in 250 layer mode probably changes the layer number for Silk Screen. This would invalidate all the PCB Decals that had lines of copper in layer 36. Not Good.

             

            So if I generate any decals with copper in Layer 26 the decal will not work in 250 layer mode, I think.

             

            Thanks,

            Bob K.

            • 3. Re: Creating Silk Screen solid areas in PCB Decals
              David Ricketts

              I see. I've never needed to go to max layer mode. Going to the max layer mode is an "all in" move, and in over 1000 designs, I've never needed to. As I understand it, all of the documentation layers just get 100 added to them when you do, so the default silkscreen layer will be remapped to 126. I know the PCB and everything on it is automatically updated. I don't know if this applies to adding parts built to the 30 layer standard. I'm not going to, but I bet it wouldn't take you longer than 10 minutes to test it out.