メインコンテンツへスキップ

Making connections to powerplanes

コメント

14件のコメント

  • Brad Levy

    From the menu, select Settings > Design Technology

    Click on the Layers tab of the Design Technology dialog.

    Look in the Net column of the settings on that tab, on the Ground and Power (plane) layers.
    They are probably blank (not yet assigned to a Net).

    Enter the names of your Ground and Power nets in those two boxes in the grid of settings.

    Click OK.

    From the menu, select View > Powerplane > Regenerate.

    You should be good to go.

    Explanation: It can only attach the vias to planes of the same Net as the trace the via is connected to. So until you tell it the names of the nets the power and ground planes are being used for, it leaves the vias unconnected to those planes.

    I've highlighted the net names assigned to those planes in this set of Design Technology settings from an example board:

    -Brad

    0
  • Col Dedman

    Thanks for your comprehensive replies. In the end I have used copper pour instead, actually on all 4 layers, and can control what does and does not get connected to the poured copper by specifying the electrical net for the copper pour.

    The application is unusual, being a DC to 20 MHz power amplifier capable of providing 14 amps, achieved by paralleling 16 of ADA4870 op amps that provide about 0.9A each. The "output buss" needs to be ultra low inductance or, to put it another way, have an ultra-low  characteristic impedance of about 0.7 ohms. To achieve this, the bottom layer (layer 4) is ground, and layer3 (also occupying the entire board area) is dedicated totally as the live output conductor. That leaves top layer and layer2 for the other connections, and while I'm about it I'll pour copper on those as well for the +20V and -20V rails. Hope that all makes sense. Let me know if I'm doing anything obviousy silly. 

    Col 

    0
  • Col Dedman

    Minor correction. Layer3 is dedicated ground plane, and bottom layer (layer4) is the dedicated output live conductor. Needless to say, a custom ultra-low-impedance (or on this case it is actually the ultra-low-inductance that matters) "cable" consisting of a pair of 25mm wide flat conductors spaced 0.1mm apart is used to connect from the amplifier output to the "load".  

    0
  • Brad Levy

    You are in interesting design territory. I say this having worked on a high-power low inductance load board that had to handle switching at high frequency. It took a bit of taming. ;-)

    0
  • Col Dedman

    Next (PCB) problem. As mentioned, the bottom layer is a copper-poured plane, dedicated to the live conductor of the output. I need to make connection to this output plane, along one edge of the board. That's fine, except this plane on the bottom layer will be coated with a green solder-resist layer. So how do I arrange for a strip along the edge of the board to be free of solder resist? I could scrape off the resist layer with a razor blade, but must be a better way.

     

    Agreed this is interesting design territory. The design requirement is 14 amps (10 A rms) of output current  with a flat power bandwidth from DC to 10 MHz, into a load that is a "short circuit", though it is all but impossible to construct a "short circuit" at 14A and 10 MHz.  Normally one designs an RF amplifier to connect to a 50 ohm coax cable, terminated with a 50 ohm load. When the required RF current is 14A, that approach is not practical, as the peak power in the load would be 14 x 14 x 50 = 9800W, with a peak drive voltage of 14 x 50 = 700 volts. That is not going to happen, so instead the load resistance will be 0.7 ohms, and at best I might be able to keep the total inductance in the load circuit down to 11 nH, which equals 0.7 ohms reactive at 10 MHz, for a total load impedance of 1.0 ohms. Thus the required peak drive power (VA) is 14 x 14 x 1 = 196W with a peak drive voltage of 14 volts, and this is achievable with x16 paralleled op-amps as previously described. Now calculate what loop diameter an inductance of 11 nH corresponds to, and you will see the extreme challenge in getting the 14A of RF current from the amplifier output to the load. Calculation shows it can be done, but not easily, and not by using 50 ohm cable. Indeed, the inductance of a mere 50 mm of 50 ohm coax will exceed my inductance budget of 11 nH. Thus the custom built connecting cable using 25mm wide flat conductors spaced 0.1 mm apart. Lots of fun. Sounds like you have been in similar territory before.    

    0
  • DesignSpark PCB

    You may add an area to exclude resist by adding a closed shape from the tool bar.

    Select the outline to highlight and from a right click select properties, change the layer to solder mask and ensure 'filled' is checked.

    A FAQ illustrating a more complicated requirement of excluding resist from a track path is illustrated here:

    https://designspark.zendesk.com/hc/en-us/articles/360002572573-How-can-I-remove-an-area-of-solder-resist-

    0
  • Col Dedman

    Thanks for that. Very cool, but I am puzzled. By default it appears that there are no solder mask layer(s), for previous boards I have made have apparently not explicitly had solder mask layers defined, and yet the completed boards certainly had green solder mask layers on top and bottom, except of course for on pads. Is that correct?

    Anyway, I have added user-named solder layer masks top and bottom because there were apparently none by default, and can now define shapes on these layers at will to control where will and will not have solder mask.

    0
  • DesignSpark PCB

    Hello Col, DesignSpark PCB attempts to make the process of generating Gerbers and hence your PCB's as simple as possible and has a set of standard rules it applies to create the solder mask and solder resist layers as you experienced.

    Advanced users may wish to customise layers and the layers can be enabled when the PCB wizard is first launched. The layers can be enabled later as detailed here (for other users viewing this post)

    https://designspark.zendesk.com/hc/en-us/articles/115000394745-How-do-I-add-a-solder-mask- which you have done.

    My advice for advanced users is always enable these layers at the start of the design as it helps if you later require them.

    Also you can check your Gerber's visually with a free Gerber viewer and Ucamco provides a simple visual tool for this purpose. https://gerber.ucamco.com/

     

    0
  • Brad Levy

    It looks like there are problems with the article on How-do-I-add-a-solder-mask-. The first picture is using the paste mask layer type when it should be using the solder mask layer type. The other pictures appear to be broken (don't display).

    Here is another set of instructions, specifying the correct layer type:

    In Settings > Design Technology, go to the Layers tab. To add a Top or Bottom solder mask layer if you don't already have one defined, click the Add button and define one as follows:

    You can set the Name and Color to whatever you prefer. Just make sure the Type is Solder Mask.
    Set the Side: to Top for a top solder mask, or Bottom for a bottom solder mask.

    Click OK to finish defining the new layer. Then click on the layer name in the list of layers on the layer tab. Use the Up and Down buttons to move the layer within the layer order. Move the Top Solder Mask to be above the Top Copper layer, and the Bottom Solder Mask to be below the Bottom Copper layer.

    Click OK when done to close the Design Technology dialog.

     

    0
  • Brad Levy

    Also, in Col's case, where it is very important that the opening in the solder mask extend all the way to the edge of the board, I'd probably use a filled rectangular shape on the solder mask layer, placed to slightly overlap the edge of the board, rather than just abut the edge. The solder mask layer type has parameters that make openings enough oversize for ordinary purposes. But I'd just feel more comfortable with with extra margin on this opening - maybe 0.3mm (12 mil) overlap with the edge of the board.

    0
  • DesignSpark PCB

    @Brad, thank you for pointing out the wrong image I have requested this be updated.

    As for the broken image it works on all our systems including some remote workers, so cannot explain your experience. That second image is also incorrect so will be replaced.

    0
  • Brad Levy

    It is actually the third image in that article (How-do-I-add-a-solder-mask-) that is broken.
    I checked in both firefox and Microsoft Edge.
    Here is the html source for that part of the page, so you can see the two lines it sits between:

    <p>Using the interaction bar you will see your new layer as shown.</p>
    <p> <img src="/hc/article_attachments/115004906453/blobid2.png" width="650" /></p>
    <p>Repeating the above selecting the appropriate details you can created a bottom solder mask.</p>

    As viewed in firefox:

    As viewed in Edge:
    By comparison, here is the html for the first two pictures:

    <p><img src="/hc/article_attachments/360005201393/1._Top_solder_mask.png" alt="1._Top_solder_mask.png" width="650" height="516" /> </p>
    <p>Move layers in the stack for the correct order they physically appear in.</p>
    <p><img src="/hc/article_attachments/360005169894/2._Solder_Mask.png" alt="2._Solder_Mask.png" width="683" height="255" /></p>

    -Brad

    0
  • DesignSpark PCB

    The FAQ has now been updated.
    It would appear the source images were correct but missing when published. As when we review posts we are logged in we see the source material, so we will in future check the published material as a normal user.
    Thank you for bringing this to our attention.

    0

サインインしてコメントを残してください。