CircuitStudio tricks and stupid questions

[plazma]

I'm learning CircuitStudio. Some things are hard to find. I'll keep posting them here.
If I can't find the thing I'll ask here.

1. Overscore, overbar, overline: add \ after every letter needing the overbar.

2. Port changed shape automatically when you connect a wire to it. No need to rotate/mirror it unless you want it vertical

[Fire Doger]

Same tricks exist on AD.
I haven't tried CS but I am guessing the schematic engine will be a copy of AD. It makes sense, otherwise Altium developing for 2 different engines? I don't want to see the result....
If you can't find something on CS look how its done on AD, I pretty sure that it will be the same if the feature exists on CS

[JamesH-AltiumOfficial]

Hi plazma,
Good tips!

1. Works with things like Net Labels, Ports, and Pins as you showed.
2. Great tip, always connect a port to a wire in the circuit so it knows what it's connected to, before worrying about what it looks like. Depending on what you connect it to, it may change its look, for example, to show direction for input or output.

Best regards,

James Harriman
Altium

[plazma]

Is there any way to change top layer opacity?
I need to stitch top and bottom gnd pours but can't see through the top layer where the bottom tracks are.

[trophosphere]

Is there any way to change top layer opacity?
I need to stitch top and bottom gnd pours but can't see through the top layer where the bottom tracks are.

I haven't found a way to change a layer opacity but usually if I need to look through a pour I will either unpour it so that only the outline remains, change the layer drawing order, or temporarily hide the layer. I like unpouring it as it also prevents CircuitStudio from having to re-pour the layer every time something like a via is added.

[plazma]

How do you unpour?

[trophosphere]

How do you unpour?

Right click on the pour you want to modify and a menu should pop up with an item called "Polygon Actions". Mouse over to it and a second menu should pop up which has the entry called "Set Selected To Unpoured". You can select that and the pour will disappear except for an outline. To repour, you can right click on the outline and then go through the same menu with exception that the entry you select will be "Set Selected to Poured".

Another way of doing it is double-clicking on the pour and a dialog box will appear with a section called "Properties". Within that section, there should be check box with the label "Is Poured". Uncheck it to unpour and select it to pour.

Menu:


Dialog Box:

[plazma]

Thanks. It is difficult to get the polygon pour selected. It's easier to select it from PCB filer object box.

The overlay designator font was way too big. It took a while to find how to edit all designators at once.
In PCB filter: Select Components in Groups box. Select Text in Objects box. Select Top Overlay and/or Bottom overlay in Layers box. Highlight all rows in Highlighted Objects box.
Select Object Inspector from the View ribbon. Change text height & width.

[plazma]

How do you add the same supplier link to all same components?
I have 30pcs of 0603 100nF capacitors (generic model from Vault). How can I add the same supplier link to all of them without doing it individually?

[voltsandjolts]

Capture the component from the vault to a local library like this:

https://youtu.be/-TBinZRimE4

Then edit the component in the local library, then uodate your schematic sheets with that component.

[voltsandjolts]

Ah, I just discovered you can alter parameters for multiple components in SCH Inspector - didn't realise that worked for parameters til now....live and learn...

[plazma]

How do you add the same supplier link to all same components?
I have 30pcs of 0603 100nF capacitors (generic model from Vault). How can I add the same supplier link to all of them without doing it individually?

Had to do it manually for all 0603 100nF components before BOM showed the correct supplier and price.

This had to be done for two different componets only. All other components were fine in the BOM if I selected supplier link for one component only.

BTW BOM exel file was messed up until I changed decimal separator to "." in Windows settings. It did not work correctly with ",".

[plazma]

What is the correct way to make modifications to a component footprint which is in an integrated library file?
I could not find a way to open the footprint for the component.

This is what I did:
I copied the footprint to a new .PcbLib file.
Then I made the modifications in the .PcbLib file and linked that footprint in the component properties (right click component in the schematic, select properties and add the new footprint to the model).

[voltsandjolts]

I think you are making it more complicated than it is.

File > Open Library > Extract Sources

Open the PCBLib / SCHlib and make your edits

Right click on project > Recompile

Save

[FrankT]

Capture the component from the vault to a local library like this:

When I do that, the schematic also seems to bring across a hidden part identifier, so when I hover over the part, the screen locks while the "Supply chain insight" pops up.  (although that doesn't happen on all parts).  Does anyone know if I can remove the link, or turn off "supply chain insight"?

[plazma]

I think you are making it more complicated than it is.

File > Open Library > Extract Sources

Open the PCBLib / SCHlib and make your edits

Right click on project > Recompile

Save

Thanks. I did not find how to edit the files. I'll try this the next time.

[plazma]

I tried to generate the gerbers. Board outline was a small square which was in fact a bug and was a component top dimension. Some how board outline gerber was generated with it.
After recompile and PCB update the outline gerber become empty.
I had to use the "Board Shape" -> "Create Primitives from Board shape" to get the correct outline.

[tarribred61]

AD has a way to control layer opacity but it seems to be crippled in CS.  There is a hint of it in the menus.  If you right click on a layer tab there is a context menu selection for Layer Transparency but it only brings up the layer configuration menu.  From there the only option for opacity is with the solder masks.

Another way to improve visibility is to use the Show/Hide tab of the View Configurations menu and set polygons to draft mode or even to hide them.

[plazma]

My one month long summer vacation started today. I also got my first CS designed PCB from the university lab


The solder mask is a little bit wrinkled at some places. 0.2mm track width and space. 0.3mm drill for vias. Ground pour vias are all tented.