1
\$\begingroup\$

I'm designing a PCB with allium and after route all the nets, I put allium in 3D view. (My first Double layer PCB)

In 3D, it appears to me that the pads are not plated (connecting both sides of the PCB, through the hole), despite the option to plate the pads being selected in pads properties.

Is this a 3D view bug?

The right ones appears to be plated but the left ones looks like they are not.

enter image description here

Left Pads properties: enter image description here

Right Pad Properties enter image description here

\$\endgroup\$
1
\$\begingroup\$

Look Closely

From the picture, it looks like the holes are actually plated (as your settings indicate).

Rather, it looks like they are missing the pad on the top or bottom, because when you see that darkish almost-transparent core of the PCB, it's like you have no copper or soldermask there.

I've never seen Altium be as buggy with the 3D view as others here claim, even before I had a good graphics card. In fact, I trust 3D view the most to see what's going on sometimes! For example, it will even properly display tented vias.

My guess is either you have some sort of net tracing on and it's dimming layers, so make sure in the bottom right you click "Clear" near "Mask Level"

That, or also possibly you generated the footprint incorrectly at first, using the "top-middle-bottom" or "full stack" options, without really knowing what you're doing. My guess is you made the top or bottom layer 0 sized. Now you're showing us the footprint is fixed in the library, but my guess is you forgot to actually update the instantiated footprint on the PCB from libraries. To do that, from the PCB view, click Tools -> Update from PCB Libraries. Click OK and go through the wizard.

========================================

Sidenote:

An easier way to confirm NPTH (Non Plated Through Holes), which sometimes are desired like for mounting holes or light pipe mounts that get glued, you should read through the board report. To do so, click again from the PCB view: Reports --> Board Information.

Click Report, turn All On (really you only need Non-Plated Hole Size, but they can all be enlightening). Then click Report at the bottom.

You'll get something like this, which you can count what you expect and find the error.

enter image description here

By the way, don't get thrown by the 32 0mil pads. It's how Altium counts a top or bottom layer surface mount pad with no hole. Kinda stupid, probably the way the tool came originally from through-hole days and that legacy code just continued on counting a SMT pad as 0-mil hole.

\$\endgroup\$
  • \$\begingroup\$ Thank you very much for all the tips. It was really a problem with the pads. For some reason when I have used the "Remove Used Pads Shapes" tool Instead of removing the pads as it was supposed to do it did that thing. After run "Update from PCB Libraries" I have deleted used pads by hand an Know it's all ok. \$\endgroup\$ – Sebastião Feb 12 '17 at 13:45
  • \$\begingroup\$ @Sebastiao Glad it's all working for you now. If one of the answers was the solution for you, please select it as the answer. \$\endgroup\$ – Joel Wigton Feb 12 '17 at 21:04
  • \$\begingroup\$ I forgot that part... \$\endgroup\$ – Sebastião Feb 12 '17 at 21:05
0
\$\begingroup\$

Can you show the settings dialog for both of them?

The left ones look like something is wrong with the stackup or you set the pad size inside the pad smaller than the drill hole.

"Plating" in Altium (!) usually means if the barrel/hole is supposed to be plated with copper, not the pad itself. There is a checkbox in the Pad properties dialog for that.

\$\endgroup\$
  • \$\begingroup\$ Have just updated my post. And by plating I mean both sides of the hole are connected so I can solder the component on either side. Thanks for the help. \$\endgroup\$ – Sebastião Feb 11 '17 at 16:04
  • \$\begingroup\$ Pad properties look good. Try restarting Altium, I'd consider it a bug in 3D view; if 2D view looks fine, create your data and check the produced Gerbers for irregularities - but from the current point of view I'd consider it an Altium bug. \$\endgroup\$ – Tom L. Feb 11 '17 at 16:16
0
\$\begingroup\$

If this is twice the same component (left and right) and no differences have been made, it's quite possible it's a bug. Altium's 3D live view is very buggy if you don't have a top-range graphics card.

However, it's smart to still check. In 2D view you can double click a pad, and then it asks you if you want to see the options for the component or for the pad, choose pad.

Then there are options for layer stack (you can define the pad for all layers independently with a special setting) or for "simple", if you chose simple all layers should be the same pad shape, if you have a full-layer-stack option selected, verify that all layers have a pad laid out.

It also has an option for "plated" which means the inside of the hole, not the pads, but if that's what you mean, there should be in the lower to middle left side a check at "Plated". Of course it's best to go back to your library when fixing problems and update the parts on the PCB from there, since then you will never have to fix it again.

Finally, before you have your PCB made, especially your first projects, be sure to inspect the Gerber plots you will send to the manufacturer. Anything that is shown on the Gerber data will be there when they send it back. Unless they make a mistake, but then you have checked the Gerber data and you can prove it's their fault.

I prefer to use a separate program for checking Gerber data, so that I am sure there's no glitches in Altium when generating and viewing that cancel itself out. ViewMate is my go-to application, you need to register to download it (or to use it), but after registration it is free and it has never let me down.

Good luck, and don't be afraid to google some of the above, because a lot of it is a bit fiddly and differs between versions of Altium.

\$\endgroup\$
  • \$\begingroup\$ Have just updated my post, can you please check the properties. And by plating I mean both sides of the hole are connected so I can solder the component on either side. Thanks for the help and for the tips. \$\endgroup\$ – Sebastião Feb 11 '17 at 16:05
  • \$\begingroup\$ Unfortunately I can't download ViewMate, there is some problem with the link they provide, the file does't exist on their FTP Server... \$\endgroup\$ – Sebastião Feb 11 '17 at 16:46
  • \$\begingroup\$ @Sebastiao The settings look fine. You don't have to use ViewMate, there are dozens. You can also see if someone has a "grey" copy of ViewMate somewhere. As for what you seem to look for, you use somewhat confusing language in the industry standard. I think you mean to say "Verify that pads are on both sides of the board" connected, again means plated, which is the inside of the hole, nothing to do with pads. You do want them plated, but it isn't your worry or problem. \$\endgroup\$ – Asmyldof Feb 11 '17 at 18:15
0
\$\begingroup\$

Create a drill file for your board, and look at it with a text editor.

If the drill file has sections for plated and non-plated holes, or there are separate drill files for plated and unplated, your board may be made with some holes not plated. Hole plating information is not included in the Gerber photoplot files.

With only one drill file, all holes will normally be plated, regardless of what may be shown in Altium's 3D viewer.

\$\endgroup\$
  • \$\begingroup\$ Altium have generated 2 drill files .GD1 and .GG1. In the .EXTREP file it says that .GD1 is a Drill Drawing and .GG1 is a Drill Guide. Given that can I assume that all holes are plated? \$\endgroup\$ – Sebastião Feb 11 '17 at 17:48
  • \$\begingroup\$ Neither of those is the drill file I was referring to, but if those drawings don't indicate that the holes you are concerned about are unplated, I'd assume they are plated. (I don't think I ever made drill drawings when I used Altium/Protel.) \$\endgroup\$ – Peter Bennett Feb 11 '17 at 18:04
  • \$\begingroup\$ What is the drill file extension? \$\endgroup\$ – Sebastião Feb 11 '17 at 18:07
  • \$\begingroup\$ @Sebastiao Peter means the Excellon Drill file, it has a .txt extension, but you need to export that separately, it's not Gerber standard. But that will give you plating, not pad presence, for the Pads you need to look at the layer data in the Gerbers. \$\endgroup\$ – Asmyldof Feb 11 '17 at 18:16

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.