メインコンテンツへスキップ

Powerplane clearance

コメント

10件のコメント

  • Brad Levy

    Hi Matt,

    I'm using DS PCB 8.1.1, and it seems to be working okay here.

    The spacing between the power plane copper and the board edge is controlled by the Board to Shapes spacing on the on the Spacing tab of the Design Technology. It uses the value at the intersection of the Board row and Shapes column. The width of the gap I'm seeing in the gerber files is the value of the Board to Shapes spacing on both sides of the board outline. It considers the board edge to be the inside edge of the line used for the board outline. So if the style of the line defining the board outline has a width of ten mils, and the Board to Shapes spacing is set to 30 mils, the gap will be 30+10+30 = 70 mils wide, centered on the board outline.

    You may want to check your plot settings on the power plane layers. The power planes can be plotted positive or negative, isolation gap or items or items plus plane copper. You can see those choices in this screen capture:

    You can also see in the window behind the dialog the result with the spacing set to 30 mils (the pink portions) and a board edge line 25 mils wide (the white portion). The powerplane copper is visible in green in the capture.

     

     

    0
  • Boss .

    Hi Brad, interesting summary. However I thought the board outline used for machining was the center of the board outline? But as my board outline is usually very small about 0.03mm from memory it is irrelevant.

    Looking at the Gerbers does not help as it is how the manufacturer uses the board outline that determines the result.

    So just a general question probably of no real relevance as there is no requirement for a thicker board outline!

     

    One point that caught me out at first is my "unplated board outline" was not checked by default, this caused some unusual results, at least in GC-Preview.

     

     

    0
  • Brad Levy

    Hi Boss,

    Looking at the drill file, the board gets routed abutting the center of the board outline from the outside.

    In other words, if the board outline is a 3.000 x 2.000 rectangle, the routing will be on the outside of that rectangle, but come up to the centerline of the board outline, so the thickness of the line used to draw the outline on screen doesn't affect the finished board size. I was a tiny bit surprised that half the width of the board outline was added to the board to shape spacing spec to create the isolation gap.

    I did some experimenting with four positive/negative choices in the plot settings, using DS PCB 8.1.1.

    The Negative (only plot gaps) option is the one I used in my previous post.

    With the other three choices, it looks like there is no gap between the plane and the board edge.

    I don't know for sure, but to me this looks like a bug.

    I'll send a note to support asking them to check out this thread.

    0
  • Boss .

    Hi Brad,

    Thanks, I agree with everything you found.


    The gap between board outline and the shape I actually expected as the gap is between the objects, so although for a board outline only the central line of the board line style is used for the milling, (logically or not) I expected the gap would take into account the board outline line width, but the line width does not need to be anything other than the minimum you can set. 

    I also found the issue of the plane going to the board edge, so confirm you experiences here. I don't recall these other options for Gerber's in previous versions, but I only ever used the default settings without any issue. 

    Thanks for checking this out.

     

    0
  • Matt Strong

    Thanks for all your feedback, however I still don't think my gerbers are looking right when viewed in a viewer.  I've used the Auto Gen. Plots (with everything but Mirror Bottom Side checked) and I'm using X2 Gerber format in the Gerber settings.  It generates two plots per inner layer.  One is Powerplane that is set to Negative (only plot gaps), and the other is Powerplane Positive that is set to Positive (only plot items).  Both images are labeled accordingly and I would assume that if you overlay the two (third image), then the black area inside the purple rectangle (board outline) would be filled with copper.  This would indicate to me that the copper would indeed go all the way to the board edge and not have a gap set by the board-shape spacing rule (mine is set to 0.5mm).  Can you post screenshots verifying the gerbers in a viewer outside of DesignSpark PCB?  Mine also shows correctly within DesignSpark PCB when I show the powerplane layers, but the gerbers seem to tell a different story!

    Powerplane - Negative (only plot gaps)

    Powerplane Positive (only plot items)

    Powerplane positive and negative overlay

    0
  • Brad Levy

    Here is one I tested with, viewed in gerbv.

    (negative, gaps only)

    The actual board outline is centered in the outer rectangular gap.

    I notice you have some large rectangular areas with no copper. Did you use a pour keep-out to achieve those?
    If you look in the built-in help under the topic Pour Copper, you will find the following:

    --------------------------------------------------------
    Pour Copper

    Pouring the Copper

    Press OK to pour the copper into the area.

    During the pour of an area, all spacings are used as defined in the Spacings dialog.

    Warning: Do not pour copper onto layers which have been defined in the Layers dialog as Power plane. When plotted this can cause strange and unrequired results. See Split Power Planes if this is what you are trying to do.

    To edit a copper area shape, it is recommended that the poured copper be unpoured first using Clear Copper. The Copper Pour Area outline can then be edited and re-poured.

    --------------------------------------------------------------

    Also, take a look at (as the warning suggests) the Split Copper Planes topic in help.

    The uptake of it all? If you are doing anything special with your power plane (like defining keep-out areas), define it as a regular inner layer instead of a power plane layer, Then use a regular copper pour with a desire clearance inside of the board boundary to form the fill of the plane. That method will respect but not get confused by your keep-outs.

    -Brad

     

    0
  • Boss .

    I think you can blame this on history....
    I may be wrong but in the good old days of tape artwork and photo reproduction it seems that if you wanted powerplanes you sent your top and bottom artwork and the PCB manufacturer (somehow) produced the powerplanes from the copper layer artwork. I presume this process resulted in a negative powerplane image, so that became the standard.

    Along came CAD which did not need to follow that "standard" but it did for a very different reason (I only found this out on the web yesterday) it was the file size! In days of 180kB floppy discs (anyone remember those?) and very slow modems for file transfer, the powerplane negative format was amazing small compared to a positive as it only had to generate the missing bits of copper!

    So we have inherited this format. To add complications to this some unruly designers in the distance past wanted some copper tracks on their powerplanes! It appears that process required these as positves, just like the outer copper layers.

    Today we still have many of these traditions embedded in the CAD programs and many PCB houses require these to be followed. However the cheap PCB manufacturers through some of the history away as they wanted their own simple process that can easily be automated, so positive powerplanes became more common. They are easy to visualise and file size is not an issue. Many others followed suit.

    So this is why the options become confusing and PCB manufacturers appear to have different requirements... Correct me if I'm wrong!

    Back to reality and the real question. I find the Gerber's for powerplanes are correct in negative form regarding the board edge spacing as Brad pointed out. The positives appear to ignore this spacing and copper goes to the edge of the PCB. I have only explored those to options and reported this to the developers and will pass on the outcome.

    Back to the history... The bits I read seem to imply manufacturers convert any positive powerplanes to negative for production, so does anyone have inhouse experience and can clarify the actual (typical) process? 

    I'm very interested as it appears that although Gerber file are the norm, the manufacturer has to do a lot of work on these before they can be used internally.

    All my recent designs have used signal layers and copper pours, seems the most simple and flexible solution.

     

    0
  • Matt Strong

    Thanks Brad for pointing me in the right direction with my copper keep outs.  I do indeed have 3 areas of copper keep out on all layers.  I ended up just switching the inner layers to signal layers and using copper pours.  I actually had this at first but changed it because I thought the maybe the software had some unique powerplane features that would help me out later on in the design.  I guess the lesson learned is to stick with what you know!

    I will say that in my 15 years of experience designing boards, I've never seen the positive and negative powerplanes.  Probably because I've been able to use the internet where we could e-mail or upload gerbers and file size didn't matter.  Also, since I've never seen positive and negative, I've never asked our manufacturers if they have a preference, but I do know that they never complained about the gerbers we sent them.  I was even on a team to standardize our design practices and we reached out to them directly to see if they had any issues processing gerbers or if we could do anything to help them read them easier.  The only thing they came back with was to put any notes and dimensions on a separate Gerber file instead of a separate text file as the viewer programs didn't open the text files so the operators just ignored them if they could.

    I'm still learning the nuances of DesignSpark, but it is very impressive software and you can't beat free!  Now if only it would let me remove solder mask on the opposite layer from only the vias in my thermal pads! I might open a separate topic for that!

    0
  • Brad Levy

    While DS PCB can generate solder masks plots automatically from the other layers, you can also include explicit solder mask layers in DesignSpark PCB designs. If you include these in the design technology for your components where you use vias in thermal pads, you can add openings on the opposite side solder mask layer in the component definition. Then as long as you include explicit solder mask layers in the design technology of the PCBs you use the components on, it will include the mask openings you defined in the component footprint.

    -Brad

    0
  • DesignSpark PCB

    Thank you for pointing problem with powerplanes we are working on fixing this bug already.

    0

サインインしてコメントを残してください。