-
How to create a pattern with single-sided through-hole pads?
Posted by HwAoRrDk on 01 Sep, 2017 01:24 -
I have been trying without great success to figure out how I can best create a pattern that contains pads that are through hole, but only have a pad on one side of the board (top, in my case). That is, the hole only has an annular ring on the top layer, the through hole is non-plated, and there is no annular ring on the bottom layer. Basically, as if it were for a single-sided board, but to go on a double-sided board.
The best I could manage was to create a surface-mount pad on the top layer, then place a mounting hole in the middle of it. This appears to produce the desired end result, but I get loads of DRC errors (2-3 per pad) complaining about clearances.
Anyone got any ideas? -
I have been trying without great success to figure out how I can best create a pattern that contains pads that are through hole, but only have a pad on one side of the board (top, in my case). That is, the hole only has an annular ring on the top layer, the through hole is non-plated, and there is no annular ring on the bottom layer. Basically, as if it were for a single-sided board, but to go on a double-sided board.
The best I could manage was to create a surface-mount pad on the top layer, then place a mounting hole in the middle of it. This appears to produce the desired end result, but I get loads of DRC errors (2-3 per pad) complaining about clearances.
Anyone got any ideas?
mounting hole in a pour? use regular hole and run a drill through it?
gotta ask why you want to do it?
-
mounting hole in a pour? use regular hole and run a drill through it?
I don't fully understand what you mean.
You can't place pours on a pattern with DipTrace's Pattern Editor.gotta ask why you want to do it?
Because I have components where I only want the solder joint to be on one side of the board. Like I said before, as if it were a single-sided PCB, but on a double-sided board.
I have also tried, instead of a mounting hole, putting a circle on the Board Outline layer of the pattern. But that doesn't work at all, because it doesn't come out in the NC Drill export.
-
but I get loads of DRC errors (2-3 per pad) complaining about clearances.
Anyone got any ideas?
Adjust the hole size of the pad to be larger than the bottom pad. The drill bit will then drill away all of the copper on the bottom side.
You can individually adjust the pad's top & bottom paste mask & solder mask swell/shrink properties by:
RIGHT CLICKING ON THE PAD
selecting MASK / PASTE SETTINGS
Note you are given the choice of modifying the Mask & Paste diameters for each layer independently.
Increase the top side annular copper ring by using the "Drawing Menu" (locate by selecting VIEW, TOOLBARS, DRAWING)
Make sure you are on the top side of the board
Select SIGNAL/PLANE from the Drawing Menu
Select "PLACE SHAPE" (which is 3 icons to the left of the SIGNAL/PLANE drop down menu)
Select "FILLED ELLIPSE" from the drop down menu (you can drag the ellipse to a circle)
You can now place an annular copper ring on the board. I suggest you just place it in an empty space on the top layer, adjust its diameter, then drag it (& centre it) over your existing pad.
If you get a design rule error, simply add that copper annular ring to the same net as the pad. -
Adjust the hole size of the pad to be larger than the bottom pad. The drill bit will then drill away all of the copper on the bottom side.
You can individually adjust the pad's top & bottom paste mask & solder mask swell/shrink properties by:
RIGHT CLICKING ON THE PAD
selecting MASK / PASTE SETTINGS
Note you are given the choice of modifying the Mask & Paste diameters for each layer independently.
Increase the top side annular copper ring by using the "Drawing Menu" (locate by selecting VIEW, TOOLBARS, DRAWING)
Make sure you are on the top side of the board
Select SIGNAL/PLANE from the Drawing Menu
Select "PLACE SHAPE" (which is 3 icons to the left of the SIGNAL/PLANE drop down menu)
Select "FILLED ELLIPSE" from the drop down menu (you can drag the ellipse to a circle)
You can now place an annular copper ring on the board. I suggest you just place it in an empty space on the top layer, adjust its diameter, then drag it (& centre it) over your existing pad.
If you get a design rule error, simply add that copper annular ring to the same net as the pad.
Thanks for the advice.
Doing it that way doesn't seem to work though, primarily for the reason that DipTrace still thinks the through-hole pad is plated, and so will not appear in an N/C Drill export for non-plated through-holes. Plus, I couldn't figure out how to add the manually-drawn annular ring to the same net as the pad; the options don't seem to be presenting themselves to me for doing that with the object selected. I can only seem to be able to assign the actual pad to a net, so I still get DRC errors. I did manage to avoid needing to edit the mask swell setting, though - just make a copy of the shape and put it on the Top Mask layer.
I also tried taking the Signal layer shape and converting it to a pad, then assigning it with the same pin number. DipTrace gave me a warning about two pads having the same number, but I thought I'd try it anyway. Didn't work. I just get unconnected ratlines on my PCB layout.
During all this poking around, I did find one thing that seemed potentially exactly the feature I was looking for - with the exception that it's in the PCB Layout app, and not Pattern Editor - was if you right-click on a pad of a relevant component, and select 'Pad Layers', you get the option to turn off the pad for top or bottom layers! And, it does so. Problem solved? No, not quite... This feature behaves weirdly, to the extent that I'm not sure what it's actually for. If I turn off bottom layer for a pad, it removes the hole entirely from that side of the copper - i.e. any ground plane just 'paves over' the hole! It shows the same in 3D view too - just a blind hole from the top, covered on the bottom. Worse still, in the N/C Drill export, you have to specifically export Top only (i.e. not both Top & Bottom) for the holes to appear in the output, and even then they're still considered plated.
-
Aha! Just found a different way of turning off a pad on the bottom layer. It was staring me in the face - right next to the aforementioned 'Pad Layers' option. Selecting 'Hide Pad Ring In Layer' from the right-click menu while viewing the bottom layer does the trick; hole is respected, complete with clearance from ground pour, etc.
But... it's still considered a plated through-hole, though.
I suppose I could, post-export, manually hack up the code in the N/C Drill file and cut out the relevant lines for such holes (luckily for my situation, all my single-side holes are using a distinct tool size) and put them in a separate 'non-plated' file.
Edit: Damn, there seems to be a bug with the pad ring hiding functionality. If I hide the bottom pad rings for several components, then use the 3D Preview, it renders as one would expect. However, if you export Gerbers, the solder mask aperture where the bottom pad ring would be is still there in the Gerber! It seems the Gerber export for solder mask layers is ignoring the 'hide' setting.
I could now turn off the bottom solder mask for those pads, but then you get no aperture in the Gerber for the through hole at all. I don't know whether a board house would be willing to accept a file like that. -
Yep, I'm 99% certain I've found a bug in DipTrace. I tried creating a new PCB layout just in case it was something funny going on with my existing layout, but the bug occurred there too.
Could someone else try these steps and see if they can confirm the bug?
1. Open PCB Layout and create a new file.
2. Draw a small board outline.
3. Place a through-hole component (e.g. Discrete > RES) on top layer in the middle of the board.
4. For one or more of the component's top layer pads, right-click on the pad and select 'Hide Pad Ring in Layer'.
5. Open 3D Preview. Observe the mask is rendered correctly.
6. Open File > Export > Gerber.
7. Select Top Mask layer, then click Preview. Observe the shapes for hidden pad rings are still present when they should not be!
8. Export the Top Mask layer to a file, and load the file in a 3rd-party Gerber viewer (e.g. KiCad Gerbview, ZofZ). Again, mask apertures for hidden pad rings are erroneously present, as per the preview in step 7. -
Yep, I'm 99% certain I've found a bug in DipTrace.
4. For one or more of the component's top layer pads, right-click on the pad and select 'Hide Pad Ring in Layer'.
I believe this works as intended - but only for internal layers when designing multilayer boards.
What you are trying to do is very unusual in that, engineers would not normally want to weaken the integrity of the soldered top pad by doing away with the plate through hole & having no pad on the bottom side.
In your case, you have found a way to do it, so just ignore the design rule errors that are generated. These design rule errors are not pushed through to the Gerbers, so the final design files you send to the board shop represent exactly what you want.
If you feel that the software should have some changes made, please register on the DipTrace Forum & ask the DipTrace engineers to look at your request.
A group of us have been working closely with DipTrace to implement many of the better features of Altium into the DipTrace software. The DipTrace programmers have taken much of this on board, so much so that I now use DipTrace in preference to Altium. -
I believe this works as intended - but only for internal layers when designing multilayer boards.
I beg to differ. If hiding a pad ring is supposed to leave the mask layers as-is, why does the 3D Preview render without the mask aperture? So either the Gerber export is wrong, or the 3D Preview is - which is it? Anyway, if it's only intended for internal layers, why make the 'Hide' option even appear for top and bottom layers?What you are trying to do is very unusual in that, engineers would not normally want to weaken the integrity of the soldered top pad by doing away with the plate through hole & having no pad on the bottom side.
Sorry, what I failed to mention is that the components I want to do this for are to be mounted on the bottom side. Therefore, by hiding the pad ring on the bottom, they are soldered only on their opposite side, as per normal for if it were a single-sided board. Doing so can't be that uncommon, as I have seen several double-sided boards where some through-hole components have pads on a single side only.
I want to do this because it makes the components in question much, much easier to de-solder (without risk of damage to the board) if they need to be replaced. I presume this is why other boards I have seen (in commercial products, no less) like this are done that way too.In your case, you have found a way to do it, so just ignore the design rule errors that are generated. These design rule errors are not pushed through to the Gerbers, so the final design files you send to the board shop represent exactly what you want.
Indeed. But, having a large list of DRC errors makes the signal-to-noise ratio very low, such that it would be too easy to miss a genuine error. I'd rather not take the chance that I may miss some issue due to it hiding in amongst so many false-positives.
It would be nice, actually, if DipTrace had some feature to mark DRC errors as to be ignored. I believe Eagle has something like this.If you feel that the software should have some changes made, please register on the DipTrace Forum & ask the DipTrace engineers to look at your request.
I e-mailed their support address about it, so hopefully they fix the issue or clarify what the intended behaviour is supposed to be.
In the meantime, I managed to work around by taking a quick crash-course in Gerber code, and figuring out where I need to hand-edit the code in the mask's file to change the size in the definition of those apertures.