Actions
Forum Thread Details
  • State Verified Answer
  • Locked Locked
  • Replies 9 replies
  • Answers 4 answers
  • Subscribers 86 subscribers
  • Views 3252 views
  • Users 0 members are here
Related
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

How can I Duplicate a PCB Layer?

jimku

Is there any way to duplicate a pcb layer? I imported a design from PADs where the copper layers came in well but the Overlay came in as a combined Silk Screen layer and Assembly drawing. I would like to duplicate this Overlay layer and make changes to make one a Silk Screen and the other an Assembly drawing. If I use the PCB filter on the Overlay layer to select Components-All then CTRL-A to select all (I can see all is selected) then paste to a new layer (Assembly Drawing Top) nothing happens. Any suggestions?

  • 0

    I asked to fast because I discovered the answer in the CircuitStudio help for copy and paste tools here:

     

    http://documentation.circuitstudio.com/display/CSTU/PCB_Cmd-Clipboard_Composite((Cut,+Copy+&+Paste+Tools))_CS

     

    I did have a problem though in selecting by using the select tool by drawing a box around my selection. Nothing gets selected when I use this tool. I worked around this by selecting all on the sheet, then using the Deselect tool by drawing a box around what I didn't want selected. But I am able to duplicate what I want to a different layer.

  • 0 in reply to jimku

    Actually, it didn't work as stated. It turns out I cannot select only the Top Overlay, copy, then paste to the same layer and then change the layer with the Inspector panel as described in the help. At first it appeared to work but was actually copying the pads of the components too and placing them on the top layer. When I deleted the extra pads on the top layer, it deleted my new layer that I just created. So... I'm still trying to duplicate the Top Overlay to another layer, then make changes to it.

  • 0

    Hi Jim, I'm not sure you can copy and paste selected elements as you are asking. However if the objective is to move the primitive drawing elements to the correct layer that can be achieved fairly easily.

     

    To move drawing primitives, have the PCB Components panel open and the PCB Inspector panel. In the PCB panel select <Top Side Components> (or whatever is applicable to your board), in the next list down select the components that need adjusting. In the third box click the Layer header to sort by layer, select the rows for the drawing primitives you want to change and then in the PCB Inspector panel click on the Layer value to change layer.

  • 0 in reply to e14softwareuk

    Thanks for your suggestion. It gets me part way to my goal. I can select the primitives of the component outlines and move them to the assembly drawing layer but I would also like to duplicate the reference designators. I guess I can just enter text on that layer matching the reference designators. That shouldn't be too bad on this design since there are only 59 components but could be a lot of work on other designs that I may need to do some work on.

  • 0

    The designator text and lines on the overlay and assembly layers are typically associated with the parts decals/footprints.  So they typically cannot be treated as free primitives and copied/pasted as such.  I experimented with this and I was able to select and put them on another layer as Peter mentioned but I could not find a way to duplicate them.  Unless, these have been decoupled after the import from PADS and are treated as separate free primitives.

     

    If you have access to the PADs environment maybe you can export the silk/assy layer as a DXF layer and then reimport them to CS as free primitives and then build an assembly layer.  However, your design would be difficult to maintain as the assembly layer is no longer going to update automatically if you change the design.

     

    If you don't have PADs but you do have the Gerber files then perhaps you can find a third party Gerber to DXF converter and then import the DXF into a layer of choice and edit it there.

  • 0

    If you are not using the component comment field then it would be possible to update these as a copy of the reference designator and place them onto their own layer. The text would be associated with the component and so would move around with it. Not as quick and easy as if you could copy and paste though.

  • 0 in reply to e14softwareuk

    Thanks again Peter. Your first suggestion may be all that I need to get the component outlines off of the silkscreen layer. The outlines were all over the solder pads or made it too tight to put the reference designators in a good place and still be readable. I'll just leave the designators on the Top overlay layer for the silkscreen. I see when I use the managed output generator, the assembly drawing pdf does show up with the outlines that I put on the Assembly Drawing Top layer (using your suggested method) and the reference designators from the Top Overlay. That's not the case for the gerber output for the Assembly Drawing. The gerber Assembly Drawing only shows the items shown on the Assembly Drawing layer. I could probably combine the two gerbers with some gerber tool but would rather not mess with it at this time.

     

    Your suggestion for using the component comment field would also work but could get messy if I didn't remember to update the comment field if changes were made in the future. I also wondered if I could put in something like =Designator in the schematic properties comment field, but that didn't work. It would also get just as messy if I just went in and added text for the reference designators on the assembly drawing layer. So... I think I'll just move the outlines to the assembly drawing layer and keep the designators on the overlay layer and just use the pdf for the assembly drawing.

  • 0 in reply to jimku

    I've discovered there is an option to make the component comment field a live copy of the reference designator. On the component edit the comment field to be ".Designator" (no quotes). Click the LS button, go to View Options and check Convert Special Strings.

  • 0 in reply to e14softwareuk

    Thanks once again! I just experimented with your suggestion and it appears to work just fine. I'm not going to go back and use it on this board as I think I already have what I need with a little more clean up. It's definitely worth knowing about if I need to work on another board like this.