Managing PCB Text - F360 Best Practices

[joshXL7B3]

Hello!

I'm pretty new to F360 PCB design and PCB design in general, and having a lot of fun (with a moderate dose of frustration). I have found that managing various text elements on the PCB design is confusing from a best practices standpoint, not to mention from a F360 user experience perspective. I have read several other threads of people challenged by various aspects of this and understand that at the time writing, text vs. pcb layers vs. the silkscreen is a work in progress by the development team.

So, I'm hopeful this thread can help others like me who are struggling with how to handle PCB textual elements. Specifically I think some perspective on how to show or hide component attributes (e.g. name, value, etc.) and what layers things should exist on would be helpful.

Examples of things I'm struggling with:

• The value of a component exists on the tValues layer, but never gets rendered to the 3D model or silkscreen for me to review for placement. So, I've moved it to the tNames layer as a hack; this feels fundamentally wrong to me; I'm sure it's wrong...
• Custom text (e.g. "Rev. A") exists on the currently selected layer when you drop it. As a noob user, this makes no sense to me, and I have no idea where it should be placed. Again, as a hack I have been putting it on the tNames layer, though tPlace seems to work to. Both seem wrong...
• Changing the font for components from whatever they were designed with to my own font (for consistency). I can change my own component fonts easily enough, but components from say, the sparkfun libraries use whatever font, and I'd like to change it for consistency on the board. The default font is ugly, I don't like some of the other fonts used by others, and I'd like some control here.
• I've played with some of this in the CAM processor, but I have no idea if this is how we're meant to tweak some of these things.

I think this all really boils down to looking at the problem from the perspective of the following conditions, thought I'm confident these aren't the only to consider:

• A component where we want to display it's name designator but not it's value (e.g. LED1, J12, R1, etc.)
• A component where we want to display it's value but not it's name (e.g. "100k" or "Green" or ".1uf" or "Power Switch")
• A component where we want a human-meaningful label associate with it (e.g. "SWD Connector" or "JTAG" or "on/off" or "Water Level Sensor", etc.)
• A densely populated board where we only want to display custom text and select name designators.
• Free Text (e.g. "keep out" or "high voltage" or "Rev A", etc.)
• Font management, specifically font faces (Arial, Calibri, etc.)

I'm sorry for the long post, but wasn't really sure how to break this down into something that can be somewhat comprehensive guidance for those like myself who are struggling with text.

Thanks for your thoughts and perspectives!

[jorge_garcia]

Hi @joshXL7B3 ,

So to clarify the points you mentioned (very concisely and accurately, thank you for that). Here's are the proper layers for each type of text.

tNames/bNames are for Reference Designators

tValues/bValues are for Component values

tPlace/bPlace is used for any other text you place on the PCB

You can change the fonts on the board but you'll have to do that every time so that can get old. The more permanent way to changes this is to set the fonts in the library. You can copy the sparkfun parts to your personal library and make the changes there. The CAM processor doesn't really change the fonts so it doesn't play much of a role here. One thing I want to note is if you want to make some category of text you could use one of the user layers and then add it to the CAM output to include it on the silkscreen or some other area of the PCB.

By placing texts on different layers by function makes it easier to include or exclude certain types of texts from the board. The 3D PCB is currently limited in user control of what text layers are shown. The view in the 2D PCB is going to be your best bet for now.

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

Best Regards,

[joshXL7B3]

Thanks a ton @jorge_garcia , this is super helpful. I didn't know I could copy components from other libraries into my own for modification; that's awesome!

How do you handle the situation with hiding or showing the component designator and value text that exist on the tNames / bNames (and values) layers? I watched a video of Dave Jones creating a dense board in altium and (I'm sure I'm probably wrong here) I think he hid all the designators in one crack with a keybind. He explained that he was doing that to make the board more readable while he was routing things, and I don't think he ultimately ended up putting many (or any) of them on the actual production board. I also imagine that on small boards with close components, the silkscreen would just turn into a hot mess.

So my attempt to replicate this in F360 looked like the following:

I selected "attribute" from the selection filter, then drag-selected all the attributes on the board, and then finally selected "Off" from the display property in the inspector. Everything disappears like you'd expect, perfect. Here's the problem though... how do you get them back? I tried going to the document "tab" and selecting "autoposition attributes" from the Draw option as another user mentioned. Unfortunately no amount of selecting "name" or "value" or anything had any effect; my designators and values are gone and no amount of anything I could figure out would bring them back.

I think this is summed up with the following use cases:

1. I want to hide designators and values because they are distracting while routing.
2. After I'm done routing I want to show one or more or all designators / values and place them according to how the board was routed.
3. I want the above two use cases to be reflected on my actual PCB.

I can't help but feel I might have uncovered a bug for your development team to investigate. It would seem the ability to do this is there, albeit in a non-intuitive way, it just doesn't seem to actually work (for me).

I also recognize the issue might just exist between seat and keyboard too....

[jorge_garcia · Accepted solution]

Hi @joshXL7B3 ,

I hope you're doing well. That display property probably shouldn't be shown in the inspector since that's an intrinsic library property. I will bring that up to the devs since it can cause confusion.

By putting the text in separate layers all you have to do to control the visibility of the texts is to turn the layers on and off. Do go into the Display command and turn off the appropriate layers. That's all you need to do for routing purposes.

If on the finished board you don't want the silkscreen(tiny boards are a good example of this, but if you have the room it can make it easier to populate boards).

The Fusion 360 Electronics environment still doesn't have the appropriate shortcut system for binding the layer switching operation but it's not too bad manually.

The CAM processor controls what will end up on your manufactured PCB. If you exclude silkscreen layers from the silkscreen they won't be on your finished board.

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

Best Regards,

[joshXL7B3]

Thank you so much @jorge_garcia, this is incredibly helpful for me.

[yaqoubdesign]

That's good information. 

I haven't tried yet but I am wondering the following:

1) how the tNames etc,  goes to the silkscreen layer?  How does it know top of board or bottom?

2) For a footprint, like the outline of a capacitor or a dot to indicate pin 1,  is that completely handled in the footprint editor?   I see for example, one of my components has a circle on layer 21 tPlace (what does that mean?)  to indicate pin 1 of the device.

3) On the same device the outline is on 51 tdoc (What does that mean?) .   How to put this in the top silkscreen?

Thanks for clarifying 

[yaqoubdesign]

ok i found this link https://www.autodesk.com/products/eagle/blog/every-layer-explained-autodesk-eagle/   

I will go through it and try to figure it out

[yaqoubdesign]

After going through the naming convention of different layers I have some confusion.

Below is a footprint of a sliding switch that I downloaded.  The outline is in layer 21 tPlace.   

Here's my questions 

1) the vertical hash lines inside the yellow box -  if that's supposed to be silkscreen,  then isn't that directly over some pads?  Same with the inner rectangular outline which is on 25 tNames.  Is this a mistake?

2)  Is it the 3D view that gives the final view of what the silkscreen will look like?

3)  Just looking at the top side of board,  I understand that 25 tNames, 25 tValues, 27 tValues, 21 tPlace and 51 tDoc are the silkscreen layers correct?

[yaqoubdesign]

sorry I meant to reply to Jorge

[RichardHammerl]

Hi @yaqoubdesign ,

the 2D PCB gives the silkscreen on the 3D PCB and finally on the real PCB.

For you first question. I think the drawing is not made properly. Usually you have silkscreen dran in layer 21 tPlace. This is what you will see printed on the PCB. It should not cover soldering areas. On the other hand, the board manufacturer would automatically clip all that is inside the soldering area. 
Additionally you can use layer 25 tNames for the designator and layer 27, tValues. This one is optional. The vertical lines should be drawn in layer 51 tDocu. This is used for documentation prints, for example. It is not used for the PCB itself. 

In case you are working with components on both sides, you have to mirror the components and layers 22 bPlace, 26 bNames, 28 bValues and 52 bDocu will be used.

I hope this info helps.

Regards,

[yaqoubdesign]

Thanks for the information 

On the schematic there is a layer 95 Names.  For this switch it is s0.  So when I go to 2D view, does it automatically translate this to layer 25 tNames ?   Is there some sort of mapping from schematic to 2D view that I should know about?

[RichardHammerl]

Hi @yaqoubdesign 

the schematic layers are independent from the PCB. The used layers are set in the component's library. In the Symbol  editor there is a text variable >NAME which is placed in layer 95, Names. For the value you have to place a text variable >VALUE in  layer 96, Values. 

For the 2D PCB footprint you want to use text variables >NAME in layer 25, tNames, and >VALUE in  layer 27, tValues. 

If you start with the 3D package creator, these two placeholders will be created automatically. 

Regards,

[kb9ydn]

---

@joshXL7B3 wrote:

• A component where we want to display it's name designator but not it's value (e.g. LED1, J12, R1, etc.)
• A component where we want to display it's value but not it's name (e.g. "100k" or "Green" or ".1uf" or "Power Switch")
• A component where we want a human-meaningful label associate with it (e.g. "SWD Connector" or "JTAG" or "on/off" or "Water Level Sensor", etc.)

---

It doesn't seem like these items were fully addressed here.  How do we go about hiding/showing the name and/or value of specific components on a PCB?  I don't want to change the component library; I just want to manually override these in some situations.

And how to add custom text to the silkscreen layer?

C|

[RichardHammerl]

Hi @kb9ydn ,

each component usually has a text for designator and for value. They are defined in layer 25 tNames and 27 tValues for components on top and 26 bNames and 28 bValues for components in bottom side. 

For single components in the layout (or also schematic) simply delete the text you want to hide. 

In case you want to bring it back and make it visible again just use "Reposition Attributes" for the component.

For text in the solder stop layers use the Text tool, choose layer tStop or bStop and place your text. 

I hope this helps.

[kb9ydn]

---

@RichardHammerl wrote:

Hi @kb9ydn ,

each component usually has a text for designator and for value. They are defined in layer 25 tNames and 27 tValues for components on top and 26 bNames and 28 bValues for components in bottom side. 

For single components in the layout (or also schematic) simply delete the text you want to hide. 

In case you want to bring it back and make it visible again just use "Reposition Attributes" for the component.

For text in the solder stop layers use the Text tool, choose layer tStop or bStop and place your text. 

I hope this helps.

---

Yep, exactly what I was looking for.  Thanks!

Just as an aside, having this function buried in the "Draw" menu seems rather unintuitive.  It really ought to be accessible from the Inspector window, or even a right click menu option.

C|