Schematic/PCB sync deactivated - Nets from Module has different net class in schematic and boad

[oleksandr_velihorskyi]

Dear community, every time when I close the Fusion and then start it with my project again, I see the following error: "Schematic/PCB sync deactivated". The errors after the ERC are looks like "Net DRV1:G+ has different class in schematic and board (0/2)". I have 4 of the same modules (with the names DRV1, DRV2, DRV3 and DRV4) in the schematic that are gate drivers for MOSFET in inverter circuit. The gate driver circuit itself is on another sheet, named "Gate_Drv". Taking into account that electrical potential on source pins of MOSFETs changed in wide range, I need to use rules with clearance for each gate driver circuit.

So, in PCB editor I organized 4 net classes (M+, M-, AC, DC-), and included to these classes nets from the modules.  For example, net class M+ consists of nets DRV1:G+, DRV1:G-, DRV1:+15V, DRV1:-5V, net class AC consists of nets DRV2:G+, DRV2:G-, DRV2:+15V, DRV2:-5V, etc. In the schematic diagram, I can see these nets from sheet Gate_Drv (but with names G+, G-, +15V) in "Design Manager" panel only in the class "default". But in fact, it is another net class, not the same as for main sheet (you can see below that there are two classes default there)... When I tried to assign these nets from modules to net classes in "Net classes" window, I see there is only one class default - see image below: 

During the work, when I just created these net classes in PCB editor and assigned net from modules to their classes, everything is ok, no errors. But, after restarting the Fusion I always see the mentioned error. The solution is removing all nets DRV1:G+, DRV1:G, ... from Net Classes in PCB editor, then error disappears, and I can add these nets to their classes one more time. But it is not a long-term solution, as for me...

What can I do in such case, and why net names from additional sheet, inserted on main sheet as module, disappeared from Net Classes window in Schematic editor?

[oleksandr_velihorskyi]

Dear Autodesk representatives, are there any suggestions or solutions for this issue? In general, how can users use rules for multi-sheet designs, when modules on schematic are used? 

[jorge_garcia]

Hi @oleksandr_velihorskyi,

I hope you're doing well. So the netclasses are really best controlled from the schematic and not from the board, especially when dealing with modules. So for now, restore consistency as you have been doing by removing the special netclass from the board side.

In the schematic go into the module sheet and set the netclass within the module. When you do that then the 4 instances of the module will inherit those rules and follow them on the board.

Let me know if this is clear or if you have any questions.

Best Regards,

[oleksandr_velihorskyi]

Dear @jorge_garcia , thank you for your reply. So, in this case... Am I right that Modules should have the same voltage level because they share the same class and => share the same clearance rules? In this case, this approach doesn't fit the requirement for the design of power electronic devices, where the same gate drivers are tied with the nodes, that have different voltages.

Please see the example below. Isolated parts 1, 2, 3, and 4 are tied to the source node of MOSFETs. I need to specify clearance between 1 and 2-3-4, between 2 and 1-3-4, etc. From the schematic point of view, Gate driver circuits (isolated DC-DC converters and gate drivers with supplemented passives) - are modules. They have the same components and connections. Fusion allows me to specify only clearance between module nets, and other nets outside the module but doesn't allow specifying the clearance between different instances of modules...

The only way in this case - is not to use the modules at all, but it will be a totally flat design... Very-very limited solution.

 

[jorge_garcia]

Hi @oleksandr_velihorskyi,

Every instance of the module would share the same clearance rules, there's no provision for different instances having different clearance rules or being assigned to different net classes.

I figure the concern here is with having proper creepage clearance to avoid arcing from high DC voltages? The best you could do is use the largest clearance for the netclass that all 4 instances use. It may not be as granular as you would like but you could still get a compliant design.

What type of driver arrangement is this? I initially thought it was some form of H-bridge but the topology doesn't line up with what I was expecting. I used to work in power electronics for LED lighting, so I know a little but always curious to learn more.

Best Regards,

[oleksandr_velihorskyi]

The presented circuit is Neutral-Point-diode Clamped (NPC) inverter (https://imperix.com/doc/implementation/neutral-point-clamped-inverter).

The problem is that proper (I mean wider) clearance should not be between nets INSIDE gate driver instances, but between nets in different gate drivers:

• Clearance between nets inside isolated parts of G1 OR G2 OR G3 OR G4 driver circuits - 0.2 mm.
• Clearance between nets in isolated parts of G1 versus isolated parts of G2 OR G3 OR G4 driver circuits - 3 mm.
• Clearance between nets in isolated parts of G2 versus isolated parts of G1 OR G3 OR G4 driver circuits - 3 mm.
• ...

This is due to voltage Vdc between D and S of MOSFETS, caused by the driving sequences:

T1   T2   T3   T4

ON ON OFF OFF

OFF ON ON OFF

OFF OFF ON ON

In addition, clearance can be lower on internal layers, but here in Fusion rules on layer level are not allowed, only on Net level...

My verdict - Fusion should add more elaborated design rules (rules, including external/internal layers, rules, including module instances itself, etc.) if the software is aimed to be competitive for complex power electronics (such as inverters, energy management systems, etc.). As for now, the possibilities for designing such PCBs are quite limited.

[jorge_garcia]

Hi @oleksandr_velihorskyi,

Thank you for the reference, I've got some reading to do.

We are working on improving the DRC, so layer rules are on the road map. The issue with the isolated GATE drivers is trickier. Would it be possible to surface the nets that require these special isolation values so that they are outside of the module? If they are outside of the module then you could use the netclasses to give them different rules. The module would then only contain the nets that can have consistent rules between classes.

Another option would be to create the gate driver design, as it's own electronic design with it's own layout. You can then use the insert Electronic design to bring in the gate drivers multiple times. They will be flat but their layouts will be preserved and then you could use whatever combination of netclasses would get you the correct clearances.

That may or may not be feasible in this case but I thought I would mention it.

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

Best Regards,

[oleksandr_velihorskyi]

Dear @jorge_garcia , thanks for the ideas. 

I tried to simplify net classes but found one more bottleneck. As I have shown in the images above in my first message on the topic, I'm using two sheets. Main and gate driver (module). The issue is, I can't find nets from Gate driver sheet in the list of nets in the "Net class" dialog (Schematic editor). I can only see there nets from the main sheet.  In the same time, in Design Manager (Schematic editor) I can see two Net Classes with the name "default". But for the PCB editor, in Design Manager I see one Net class "default" with nets from the main sheet and Gate driver sheet. 

It looks like I can't assign nets from the module sheet to my Net Classes at all, they are associated automatically with the "Default" net class. Am I right? I have tried to add all nets from module sheets to the additional class "Test" (from PCB Editor), and it leads to the error "Schematic/PCB sync deactivated". 

 

 

 

[jorge_garcia]

Hi @oleksandr_velihorskyi,

For now don't adjust netclasses on the PCB editor, because when you interact with the modules you'll break consistency. All of the assignment to netclasses should be done on the schematic.

Try it this way. Go into the Gate Driver sheet click on the net whose netclass you want to change and then go into the inspector to change the netclass of the net. Let me know how this works.

Best Regards,

[oleksandr_velihorskyi]

Dear @jorge_garcia ,

thank you, it works, but Fusion developers should improve the usability and functionality of net classes and rules for them. Yes, I have tried it, but it does not help for the main task with different net classes for module instances. But yes, it is possible to add nets from the module sheet to the desired net class only from the inspector panel. The window "Net Classes" in Schematic Editor does not contain any nets from modules and from a usability point of view it looks strange. The user needs to use different approaches for nets from the module sheet and for all other nets. 

[jorge_garcia]

Hi @oleksandr_velihorskyi,

I hope you're doing well. I get a feeling that Netclasses dialog isn't handling the modules correctly. I'll bring it up with the developers. Let me know if there's anything else I can do for you. The improvements for modules I've already documented.

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

Best Regards,

Best Regards,

[oleksandr_velihorskyi]

One more issue with the net classes and modules. I have created schematic with modules, and associalted nets to 4 net classes - deafault (shown red), HV_1 (pink), HV_2 (violet) and HV_3 (green). All assignment of Nets to Net classes was done from Schematic. As you can see, Some nets in classes are from the main sheet, and some are from the Module sheet. I have set a clearance 4 mm between all classes - default to HV_1, HV_1 to HV_2, etc. I hae used "Rules DRC/ERC - Class - Rules" window with triangle table for it. The issue - clearance, described in mentioned window, is applied ONLY between nets from module to module sheet, or from main to main sheet. The clearance between nets from different classes, if they are located in different sheets - are not used! You can see it on pink and violet nets - on the bottom side of the image the clearance is applied, and we can see error marks, but on the top side of the image - there are not any error signs, and trace from PH_C are so close from polygon Z6:OUT! How can I set the clearance rules between different sheets???

[jorge_garcia]

Hello @oleksandr_velihorskyi,

I hope you're doing well. It's not possible to scope rules based on a sheet. The best you could do is use a netclass for each sheet and then define rules based on that.

With more insight into what you are trying to do I'm sure we could find a solution.

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

Best Regards,