Fusion Electronics 16-Layer/64-Layer Issue

[al_walker]

With the latest Fusion updates, newly created Electronics Designs and Libraries use the new 64 layer stackup, so for example a 6-layer board will use layers Top, 2, 3, 62, 63, Bottom instead of Top, 2, 3, 14, 15, Bottom. 

The issue I have is that as Fusion still doesn't have rectangular and square pad holes, I'm using the polygon workaround with a small hole to link them together. I can't modify or add layers to allow PCB footprints in libraries created before the change to 64-layers to be used with the new 64-layer stackup.

Like I suspect the vast majority of users, I don't anticipate ever using more than 16 layers, so perhaps a sensible workaround would be to make the use of the 64-layer stackup a user preference?

[jorge_garcia · Accepted solution]

Hey @al_walker,

There have been several issues discovered and fixed with the new 64 layer limit. The idea of 64 layers is just to future proof so that there's no mention of more layers as a feature request for many years to come.

It so much work and so foundational that I don't think it could be a user preference. However, the next update should solve this for you.

I'm going to share this with our devs just to confirm that this has been resolved.

Let me know if there's anything else I can do for you.

Best Regards,

[al_walker]

Hi @jorge_garcia 

The notes for the latest update state:

Resolved an issue that prevented saving new libraries and caused placement inaccuracies when copying footprints from a legacy library to a new one with extended layers support. New libraries can now be saved correctly, and all signal objects are placed on the appropriate layers.

This doen't really help my situation, the problem that I have is that I don't want to have to migrate all my existing footprints to new libraries with extended layer support. What I would like is to have extended layer support on existing libraries please. Perhaps an option to upgrade a library or indeed a PCB layout to 64-layers could be implemented? Yes it would mean manually changing layer assignments, but that's less work than having to migrate whole libraries and projects.

For example, a fairly complex footprint for a Wurth USB Micro-AB receptacle:

As a workaround to support both 16- and 64-layer stacks given that don't envisage using more than 16 layers, I would want to copy layers 9-15 to 57-63 so that both exist within the same footprint.

Kind regards,

Al

[jorge_garcia]

Hi @al_walker ,

I hope you're doing well. Its not the only fix, with that said you should be able to use the libraries you have as is no updating or modification necessary. I'll bring it up with the developers just to make sure it has been addressed.

Let me know if there's anything else I can do for you.

Best Regards,

[constantin.popescuXD3CL]

Hi @al_walker,

This issue has been addressed in the last Fusion update. Can you please try again ? If you see any other issues please let me know and I will try to help.

Kind Regards,

[al_walker]

Hi @constantin.popescuXD3CL @jorge_garcia 

I confirm that with the latest release I am not presented with all 64 routing layers, only the 16 routing layers that were the maximum when the library was created.

Using the command LAYER c63 Route63, I am able to create a routing layer such that I can copy a polygon shape from another layer, but I note the following:

• Layer c63 appears out of sequence - it is after layer cb Bottom
• When I select All Layers in the Selection Filter, layer c63 is not selected

 

 

When I create a new 4-layer PCB, the layer c63 polygon shapes and pads are correctly displayed.

In this case, the Selection Filter shows:

• Layer c63 appears in sequence
• When I select All Layers in the Selection Filter, layer c63 is selected

So I think the expanded layer implementation in Electronics Projects is ok, but perhaps some work needs to be done in Electronics Libraries.

Kind regards,

Al

[constantin.popescuXD3CL]

Hi @al_walker,

Thanks a lot for this. I am happy that your initial issue is now fixed and you can move ahead with your project. Regarding the issues you have found with the extended layers order:

• Layer c63 appears out of sequence - it is after layer cb Bottom
• When I select All Layers in the Selection Filter, layer c63 is not selected

these look like bugs (oversight) and we will fix them as soon as possible.

Please let me know if there is anythign else I can help you with.

Kind Regards,

[al_walker]

Hi @constantin.popescuXD3CL 

Thanks very much for your prompt attention, but I'm seeing that there are more issues with the transition to 64-layers.

I just had a work-in-progress 6-layer PCB layout spontaneously change from a 16-layer stackup to a 64-layer stackup, resulting in multiple errors which I am still working through. The Schematic-PCB link was broken and I have had to delete affected components, to restore the schematic-PCB link. It appears that polygon shape pads on layers 14, 15 and bottom, were copied over existing polygons on layers 62, 63 and bottom, resulting in duplicates indicated by cross-hatched boxes. I am now looking to fix these components before re-adding them to the design

Whilst I would expect any new PCB layout design to be initiated as 64-layer, having existing PCBs created as 16-layer change to 64-layer without warning is causing significant disruption. Your help in resolving these issues is very much appreciated.

Kind regards,

Al

[constantin.popescuXD3CL]

Hi @al_walker,

"I just had a work-in-progress 6-layer PCB layout spontaneously change from a 16-layer stackup to a 64-layer stackup, resulting in multiple errors which I am still working through. The Schematic-PCB link was broken and I have had to delete affected components, to restore the schematic-PCB link. It appears that polygon shape pads on layers 14, 15 and bottom, were copied over existing polygons on layers 62, 63 and bottom, resulting in duplicates indicated by cross-hatched boxes. I am now looking to fix these components before re-adding them to the design" - Any 16 signal layers design is automatically upgraded when placing components from a newly created library (that has extended layers support). We opted for the automatic upgrade because we thought that the process needs to be seamless and I didn't think there should be any issues because the upgrade only happens once. I am not sure why the polygon shape pads will overlap existing polygons on layers 62 / 63 because when the upgrade happens there should be no layers 62, 63 in the design. There is something in the workflow that I don't fully understand so I will appreciate if you could detail the steps that lead to this situation so I can replicate them here and make a fix.

I know that this might be extra work for you but if you could create a simple example showing this issue that would be greatly appreciated. This would help me fix the issue as soon as possisble.

Thanks a lot for your help.

Kind Regards,

[al_walker]

Hi @constantin.popescuXD3CL 

Replicating the issue requires a pre-existing PCB layout created using the 16-layer limit, which isn't possible to do now. I have another in-progress PCB layout which was only set as a two-layer design, just now changing to 6-layer stayed within the 16-layer limit. I would have expected this action to use the new 64-layer limit.

I need to finish my other PCB first, but will see how I get on with this layout and will communicate my experience. As an observation, it would have been better to fully implement a square/rectangular pad option (to remove the need for the workaround of using polygon shapes as pads on each applicable layer in library footprints) before implementing the 64-layer change.  To take a positive example, the migration to Fusion Hubs was very well communicated and executed, but I don't feel that the migration to 64-layers was similarly as well done.

Kind regards,

Al

[constantin.popescuXD3CL]

Hi @al_walker,

To make it a bit more clear I hope, regarding your 1st question: "Replicating the issue requires a pre-existing PCB layout created using the 16-layer limit, which isn't possible to do now. I have another in-progress PCB layout which was only set as a two-layer design, just now changing to 6-layer stayed within the 16-layer limit. I would have expected this action to use the new 64-layer limit." - any legacy design is upgraded to extended layers in one of the following ways:

1. Through the Board Layer Stack Manager by increasing the number of signal layers to 18+;
2. By running the following CLI command: upgradelayers;
3. When placing components from a library (either from Schematic or from PCB when there is no Schematic) that has extended layers support (this happens automatically because a legacy design can't use footprints that have extended layers);
4. Any new board design or new library is created with extended layers support ON. This is needed because the default maximum number of layers has been extended from the legacy 255 to 16383.

If you only work on existing designs and with existing libraries then no upgrade will ever happen. 

"I need to finish my other PCB first, but will see how I get on with this layout and will communicate my experience." - I understand and I very much appreciate your help and any clues that would help us get to the bottom of this problem. I hope that this only happened for your 1st design that was impacted by the bug that you have reported and already has been fixed.

"As an observation, it would have been better to fully implement a square/rectangular pad option (to remove the need for the workaround of using polygon shapes as pads on each applicable layer in library footprints) before implementing the 64-layer change." - unfortunately I can't comment on this one because I am not in charge of feature scheduling. I apologise for not communicating better about this feature and it's impact on legacy designs.

Thanks a lot for your help and please don't hesitate to reach out if you have any issues.

Kind Regards, 

[al_walker]

 @constantin.popescuXD3CL

Thank you for the information on how to upgrade to extended layers. This should give me the control I need to manage the transition from 16 to 64 layers on work-in-progress designs. What I plan to do is temporarily delete any components that use the square/rectangular hole workaround using polygon shapes, then use the command line to upgrade the layer count and then reintroduce updated versions of these components with the polygon shapes on layers 57-63 rather than 9-15. I will report my experience of using this workflow.

The problems that I experienced was due to adding components with polygon shapes both on layers 9-15 and 57-63 on a PCB layout that hadn't yet been upgraded to support extended layers. I would suggest that based on this experience that this automatic method of upgrading a PCB is not recommended.

Kind regards,

Al

[constantin.popescuXD3CL]

Hi @al_walker Al,

Yes, please let me know how you go when upgrading the design before hand and then use components from a new library.

Regarding your statement:

"The problems that I experienced was due to adding components with polygon shapes both on layers 9-15 and 57-63 on a PCB layout that hadn't yet been upgraded to support extended layers. I would suggest that based on this experience that this automatic method of upgrading a PCB is not recommended." - I agree. The assumption is that a legacy design can only contain objects on layer 1 - 16 so there should be no issue upgrading to extended layers in this case. I understand your apprehension regarding the automatic upgrade workflow and unfortunately it was caused by us not finding all the bugs before we released. Our thinking was to create a seamless user experience when using both Legacy / New libraries with new designs. The idea was that the user shouldn't have to touch any of the existing libraries.

I have a question regarding your footprints that use custom pads with polygon shapes: are the pads SMD pads, through hole pads or both? Regarding the SMD pads are any of them placed on Bottom signal layer? Currently, these complex SMD pads will not upgrade correctly when placed on Bottom signal layer because the polygon shapes, wires used to make the complex pads will be left on the original legacy bottom layer 16. If possible avoid placing them on Bottom layer and you'll be okay. I will fix this issue ASAP.

Kind Regards,  

[al_walker]

Hi @constantin.popescuXD3CL 

The workaround to create square and rectangular hole pads goes back to EAGLE, a small through-hole pad is used to connect polygon shapes on each layer to join them electrically. I then use the Milling layer to define the square or rectangular hole cutout. I also use a couple of user defined layers for Milling_PTH and Milling_NPTH and put polygons on those layers the same size as the cutout on the Milling layer, as that layer alone doesn't define whether a hole should be plated-through or not. These two user defined layers are included as part of the CAD release as Gerber files.

I use a deliberately small sized through-hole pad (0.09 mm drill on a 0.2 mm pad) that can't be achieved by conventional PCB drilling within the area defined in the Milling layer, but still get it queried every time I do a PCB release, despite the explanation in the release documentation! So the provision of a rectangular through-hole pad (in addition to the obround one) would be greatly appreciated. 

Your point about the bottom layer explains one of the issues that I encountered that I didn't appreciate the significance of at the time. The polygon shapes on the bottom layer weren't being recognised as such. Just out of thoroughness, I had deleted the existing bottom layer polygons on the library parts that I updated for use with the extended layers and added new ones, this worked ok in that they were recognised as such.

Kind regards,

Al

[constantin.popescuXD3CL]

Hi @al_walker Al,

Thanks a lot for your thorough explination of what you need to do to be able to have a rectangular through-hole pad. This process is very complex indeed and I don't fully understand why a rectangular / square through-hole pad was never made available in Eagle. I will ask my colleagues and see what can be done.

Kind Regards,

[al_walker]

Hi @constantin.popescuXD3CL 

Thanks very much, please see this thread on the benefits of using a hole that matches the pin cross-section to eliminate defects when wave-soldering:

https://forums.autodesk.com/t5/fusion-electronics-forum/holes-drills-defined-in-package-to-not-trans...

Kind regards,

Al

[Closed-Loop-Bot]

We're happy to report this issue has been resolved. Update Fusion to the most recent version to apply the fix. If this update resolved your issue, feel free to click the "Accept Solution" button to help other community members find the answer more easily. If the issue persists after updating, don't hesitate to reach out to us by replying to this thread. We're here to help! Let us know if you need any further assistance!

[al_walker]

The issue is not resolved, the latest release does not feature a rectangular pad option and numerous new issues have been introduced that prevent me from using Fusion Electronics until a remedial update is available. Indeed, given the severity of the newly introduced issues, I consider the above message highly inappropriate.

Please see here:

https://forums.autodesk.com/t5/fusion-electronics-forum/new-layer-color-descrepancy-in-latest-releas...

[jorge_garcia]

Hi @al_walker ,

I hope you're doing well. The above response was by a bot that saw that the original issue of the layers was reported as a ticket and that ticket was "supposedly" solved for this release. That's where the response comes from. 

I'm already triaging your other post with the devs to see what's going on. If you are able to share files that will help.

Best Regards,