Community
Fusion Electronics
Working an electronics project and need help with the schematic, the PCB, or making your components? Join the discussion as our community of electronic design specialists and industry experts provide you their insight and best practices.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

PCB definition

14 REPLIES 14
SOLVED
Reply
Message 1 of 15
mario.brizida
249 Views, 14 Replies

PCB definition

Hello,

 

I'm pleased that you made nice improvments  on pcb stack layer definition.

mariobrizida_0-1653576661437.png

Nonetheless, there's some small issues:

  • I need to draw a single sided pcb (only one layer of copper) and you don't have such option. The minimum you allow is a 2 layer stack. And you don't allow edition for silkscreen (colour definition is important).
  • In the stack you should not (in my opinion) to link the top and bottom layer pair. It's possible to have on side with 2oz and the other with 1oz... when you edit copper you edit the pair, and that's not what the engineer or designer wants
  • The same for the other layers (solder mask and silkscreen). In many cases you have silkscreen on compoments side and no silkscreen on solder side. Many pcb's have components only in one side... and some have also copper on only one side, as the one I'm working right now.
  • In my opinion, you shoud allow the user to decide which layer he wants and if wants layer pairs or not

Thank you,

 

Mário Brízida

  •  
14 REPLIES 14
Message 2 of 15

Hi @mario.brizida ,

 

I hope this message finds you well. Generally, if you only want to do a single layer PCB then you use the 2 layer stack up and only draw on one of the layers. When you generate your gerber files just ignore or delete the unused gerber files.

 

Looking more closely, you mention being able to specify different copper weights for each layer. Is this something you legitimately need to do or you just want the ability to do it? In general, asymmetrical stackups are not desirable because the difference copper distribution causes the boards to warp, that's why they are not supported out of the box.

 

That's the way you can approach it now. I'll add your comments as a feature request for the layer stack manager.

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 3 of 15

Hi Mario,

Thanks a lot for your comments regarding the new Layer Stack Manager. Regarding your points here are my answers that will override Jorge response unfortunately:

"I need to draw a single sided pcb (only one layer of copper) and you don't have such option. The minimum you allow is a 2 layer stack. And you don't allow edition for silkscreen (colour definition is important)." - having a asymmetrical layer stack is already possible (implemented) and it is driven by the property "Maintain Symmetry" that can be found in the "Layer Stack Properties" dialog that can be launched by clicking on the icon next to the Layer Presets combo-box Save icon (please see the attached picture named LSM-Asymmetrical-TopSide.png). To create an asymmetrical layer stack-up you need to select the "Open Form Setup String..." command from the Layer Presets combo-box (left most control in the top side commands toolbar, please see the attached picture named LSM-Asymmetrical-LoadFromLegacySetupString.png). If you hover with the mouse cursor over that combo-box you'll get a tooltip that tells you that loading the old Eagle Legacy Layer Setups is possible and in the subsequent dialog (please see attached picture LSM-Asymmetrical-LoadFromLegacySetupString.png) you can input 1 and you'll get a layer stack that contains Top Layer + Dielectric Below + Tops Silk + Top Solder and Top Surface Finish (you can also specify that you don't want the Silk / Solder and Surface Finish layers to be automatically created see the check-box in the Get Setup String dialog that allows you to input the Legacy Setup). You can manually remove any of the layers apart from the Top Layer. To remove the layer you need to use the Mouse Right Click Context Menu inside the LSM table (please see the attached picture LSM-Asymmetrical-DeleteLayer-ContextMenu.png).

I hope these comments answer all your questions. Please let me know if you see any other issues or require other special features that might not yet be available.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 4 of 15

Hi Mario,

I forgot one more thing regarding the asymmetrical layer stacks creation, you can also start with a 2 layer stack for example (if you want to make a 1 layer stack) then open the Layer Stack Properties dialog and un-check the "Maintain Symmetry" check-box save and then you can start removing any layers that are not required using the Right Mouse Click Context Menu. Doing it this way might require more work then starting with the "Open From Setup String..." command that allows you to enter the old Eagle Legacy Setup String directly.

Hope this helps.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 5 of 15

Hi Constantin,

 

Thanks for your explanation. I tested. It worked perfectly. Good job from Autodesk electronics team.

Good improvments! I think you can even improve a little bit if you allow to edit the silkscreen as all the other layers (I think it's a bug, as I can edit all the other layers).

 

Thank you 

Message 6 of 15

Hi Mario,

Good to hear it worked well for you. Regarding the Silkscreen Color not being available this is by design not a bug but it looks like the design choice we made was not the best. We can add that in a future update. What properties you think are needed for Silkscreen apart from Color?

Thanks a lot.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 7 of 15

Hi Constantin,

In my opinion the colour is the most important. Maybe allow also OEM name to put a special property to the manufacturer, and  also thickness.

As far as I saw, OEM name is only available for dielectric layer, and I think it's important also for all the other layers because some times we need to send to the pcb manufacurer the ink or process reference in order to keep constant the pcb colour in all the batches we order. PCB visual is very important for products where it is visible, like in some lighting applications.

 

Good work and thank you.

 

 

Message 8 of 15

Hi Mario,

Thanks a lot for this. I will create a feature improvement ticket with these requirements and hopefully we'll get to it in the near future. Regarding the Silkscreen Thickness what are the most used values (micron or mil) ?

 

Kind Regards,

Constantin



Constantin Popescu
Principal Software Engineer
Message 9 of 15

Hi Constantin,

I suggest to use both, as in all other layers.

 

Regards,

MB

Message 10 of 15

Just one question.
Does PCB color and thickness impact 3D view?
Message 11 of 15

Hi Silvio,

I think the PCB thickness is taken from the Layer Stack Manager but I am not 100% sure about the color. I will ask my colleagues that worked on that and then update my response.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 12 of 15

Hi Silvio,

I checked our current 3D PCB export and here are my findings:

  1. The board thickness is taken from the Layer Stack Manager and it only contains the copper and dielectric thicknesses. We'll improve this in a future update.
  2. Only the Solder-Mask color is taken from the Layer Stack Manager. There is no support for Dielectric Color or Surface Finish. The copper color is taken from Layer Manager manufacturing colors as was the case before the updates to layer Stack Manager.
  3. The plan is to unify the manufacturing colors in one place ideally the Layer Stack Manager but we didn't have time to get to it in this release. 

I hope this helps.

 

Kind Regards,

Constantin Popescu



Constantin Popescu
Principal Software Engineer
Message 13 of 15

Tha's nice, thanks!
Message 14 of 15

Hi Constantin,

Good news again.

Indeed right now we have information about pcb stack in 2 different places.It's a good idea to concentrate all the information in Layer Stack manager and end with the inputs in Layer Manager manufacturing.

Also important is that ODB++ generator gets all these inputs from Layer Stack Manager in order to have a really automatic production files generator, with all relevant info about pcb caracteristics, including colours, that I'm not sure ODB++ supports.

 

Regards,

 

MB

Message 15 of 15

Hi Mario,

There is no support for color in latest ODB++ standard. Maybe one day. The other issue is that the ODB++ expanded Xml Layer Stackup information has not yet been implemented by any E-CAD vendors (Altium, Cadence or Mentor, Pulsonix) and I haven't seen any example of a database that contains these details (from Valor or someone else).

 

Kind Regards,

Constantin



Constantin Popescu
Principal Software Engineer

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums