Huge problems exporting Gerber X2 for a panel with blind vias

[Electr0nicus]

Hi all.

I have a project in Altium which consists of 3 individual PCB- projects.
For manufacturing I wanted to combine those 3 child-PCB projects on a production Panel with 220x270mm.

Other specs of the PCBs (production panel and individual PCBs):

• 4 Layers, all signal layers
• Blind vias from 1st to 2nd and from 3rd to 4th
• Vias from 1st to 4th

So I designed the production panel with all the cutouts, fiducials etc. and wanted to generate Gerber X2 files (via File->fabrication outputs -> Gerber X2 files) to send them over to our PCB- manufacturer. When I checked the Gerber outputs I noticed that on the Panel_Plated_Drill_1_2.gbr and Panel_Plated_Drill_3_4.gbr files are completly empty. If it had worked properly, in these Gerber files there should be at least a few thousand blind via holes. It seems Altium behaves like there are no blind-vias present.

Then I spent the whole workday yesterday figuring out that problem. Here is what I've tried:

• Checked the Layer Stackup of the panel- PCB and each individual child-PCB which is placed on the panel. Result: The layer setup is exactly the same for all of them.
  
  • Layer order matches
  • Layer type matches
  • Layer name matches
• Exported a Gerber File from one child-PCB alone (without placing it on a panel). Result: Everything is there where it should be. All blind vias got exported correctly
  
• Created a completly new PCB-panel project and added only one child-PCB. Result: The same, blind vias don't get exported at all.
• Placed a set of vias from 1st-2nd, from 3rd-4th and from 1st to 4th on the panel PCB directly. Result: Only the blind vias on the Panel- PCB itself get exported. All blind vias in the child-PCBs are still missing.
• To rule out a problem with the child-PCBs themselves, i created a simple new child-PCB with 3 via holes from 1st-2nd, 3rd-4th and 1st to 4th and also a new panel PCB. I placed the simple child-PCBs with the vias on the panel and generated the Gerbers. Result: No blind vias get exported.
• I've tried the same with a old Altium Designer 17 version, Altium 18.0.9 and 18.0.11. Result: Makes no difference at all, problem still persists.

So what I've learned from my endless trial and error yesterday, is that the problem is only there if the blind vias are on the child-PCB of a panel. They are obviously completely ignored by the Gerber-X2 exporter. Placing vias on the panel itself is no problem, and they are properly exported. Also vias going though the full stack (1st to 4th) are exported without a issue.

So i have no ideas left, what the deal is here, and what i can try or what I'm doing wrong. I'm literally completely stuck on this issue. So maybe one of you can help or knows what I'm doing wrong, that would be highly appreciated.

[Gribo]

Did you try exporting to another format? ODB++ or standard Gerber (not X2)? 

[Electr0nicus]

Did you try exporting to another format? ODB++ or standard Gerber (not X2)? 

I'm not familiar with ODB++. But I gave it a try, and obviously only the first of the 5 child-PCBs on my panel gets exported.
Standard Gerber works (all which should be exported, gets actually exported), but the PCB manufacturer does only accept Gerber X2.

[Electr0nicus]

What really puzzles me is, that my PCB is not something out of the ordinary. Just a classic 4 Layer PCB with blind vias. I think hundreds of them are made everyday in Altium Designer. If it is a bug, then it should have been reported long ago and fixed, because then it would be a very severe one.

And btw, I've tried the same thing on different computers as well, with no difference. So it can't be a corrupted Altium installation on my machine.

[ddavidebor]

Can you post a screenshot of your altium "project" panel ? there may be issues with how your files are set up.

[Electr0nicus]

As this is a company project, i can't post any files here. But I've created a simple demo project, which repoduces the error exactly the same way as in the original project.
Maybe one of you can open the project, and export X2 Gerbers and see if the same problem occurs.

Here is the link:
https://drive.google.com/open?id=1VzLTwCvwzGIxY0RomkdVLR4HFBW8OjlS

There is a simple 4 Layer PCB, which has holes from 1st to 2nd, 3rd to 4th and 1st to 4th. This simple PCB is panelized 5 times. On the panel itself there are also some vias from 1st to 2nd, 3rd to 4th and 1st to 4th. When you go to File->Fabrication Outputs -> Gerber X2 files and generate the Gerbers you should see on the "test_panel_plated_drill_1_2.gbr" and "test_panel_plated_drill_3_4.gbr" that only the blind vias on the panel itself are there, and none of the blind vias on the child PCBs themselves.

Kind regards,
Gregor

[Flammert]

Hi Electr0nicus,

I am having similar problems, did you manage to resolve this issue?

Kind regards,
Ruben

[Electr0nicus]

Hi Electr0nicus,

I am having similar problems, did you manage to resolve this issue?

Kind regards,
Ruben

Hi Flammert.

Sorry for the late reply, i had much work to do and actually forgot about the thread after I found a workaround.
To your question: No I did not solve the issue itself, but I found a workaround for it. It's tedious, but at least it works. I can say that, because up to now, I have received the fabricated boards, and they work as intended.
The workaround is as following:

Export the Gerber X2 Files from each of your child PCBs, which you want on your panel
Then export the Gerbers for you panel, here the bild vias are missing. So you can guess what's coming next 
Navigate to the Camtastic Files of your child PCBs and make sure you have selected the CAMtastic Menu panel
In this panel you can see the individual layers of your PCB like this

Right Click on the layers and select "all OFF" and then activate the layer witch ends linke: **plated_drill_1_2.gbr . You should see the blind vias of your PCB. Do this for all your blind via Layers. This is only to ensure that they are exported. 

Now open the panels CAMtastic file again.
Navigate to File->Import->Gerber and select the gerber file **plated_drill_1_2.gbr from your child PCB
After selecting the file, a window pops up where you can configure how the Gerber should be imported. Click on settings and make sure everything is according to you specifications

Now you have the Child PCBs Gerber imported to your panel PCB. By selecting ony the imported layer you can easily select, rotate and move your imported Gerber.
The user interface is different in the Gerber editor. If you select something you click with your left mouse and a selection rectangle pops up. If you want to finish the selection you have to click the right mouse button. Then to move the selection you have to left click and you define a start point. Then when you move the mouse a line is drawn from the startpoint. If you click the left mouse button again, the selection will be moved by the vector defined by the start and endpoint. The same thing is with rotating the selection. Here you will get a promt to enter the rotation which is counter clockwise.
To align the via holes with the actual PCB, you have to make a change in the preferences. Therefore navigate to Tools->Preferences and then select in the "Object Snap" Dropdown field "Center"

Select the all the imported blind vias again using the move command Edit->Move. Then when you are selecting the start- point and hover with the mouse over a blind via drill hole the mouse sort of snaps the the center of the hole. Select a hole which you can easily relate to a feature on the PCBs copper layer. Then activate the Top or Bottom Layer depending which blind vias you are dealing with. Move to the corresponding position on the copper layer where the via hole should go and snap and click. Then the holes should be perfectly aligned in the center.



This you've to do for every child PCB and every blind via layer
In the end you have many imported blind via Layers which you wand to merge to one single layer to send to the PCB manufacturer. This can be done by using Edit->Layers->Merge and then selecting the layers to merge out of the list. Also don't forget to give the merged layer a new name in the name field in the upper part of the window, otherwise you can't merge them

I know this is a extremly tedious process but you will get used to it. And hey you have to do what needs to be done to get those CAM files to the PCB manufacturer 

[Flammert]

Hi Electr0nicus,

Thanks for your explanation!