Power symbols schematic

[christopher2KLSVU]

Perhaps I do not know how to use it.

I want to have power symbol +15V. In power symbols Lib there is no such one, but I take 12V one( or +V) I change its value to 15 V, now problems are coming.

When you connect a net to this symbol, the track/net name becomes 12v not 15V. It is very bad.

When you take 12V ready symbol from lib, all the nets connected with it have automatically name +12V. Fine and logically but how about my 15V symbol.

Every time I copy my 15V symbol the net connected became +12V or V+.

What a shame, why is this so poor and not user friendly?

If I have 10 sheets of schematics, or just want use 15V symbol 6 times within one sheet, then every time I put my 15V symbol I must rename its net by hand. Man we have XXI century now. If you do not rename the net or just forget on the 7th or 8th sheet  it can happen that you left net unconnected or wrong connected  to the supply!. Then it is better to not use such power symbols besides those predefined...But symbols are to speed up the work..to not make spaghetti schematic..

What I do wrong or why is the software not friendly???

------

When I try to change name to 15V then Warning: You can not rename Power symbols.

[rlweinberg]

I have also run into this, and found I needed to create a similar new symbol for what I needed.

[RichardHammerl]

Hi @christopher2KLSVU 

the supply symbols are created with a pin with direction Supply. And the name of the pin given in the symbol editor determines about the net name. 

Renaming the symbol in the schematic does not help. Best is to create a new supply symbol with the pin named +15V.

Hope this helps.

Regards,

[christopher2KLSVU]

General concept of power symbols here is wrong.

Buying F360 is like buying fancy Makita drill machine with original suitcase and set of drills. You are happy until you want to hang on an image on the wall and then you realize that there is no 10 or 8mm drill in your fancy set!

Proposed solution, Creating symbol for every power line  is time consuming and risky as f360 does not keep added libraries to the project. There are dozens of doubled libraries in F360, no any order.

Look how it is done in Orcad or Mentor. In Pads you do not have dozens power symbols like you proposed me! Let imagine 12V 15V 24 and 48V in one project?

You take a power symbol ; circle, bar or ground , earth and after you drop it on schematic, it ask you immediately for a net name!
It automatically /creates assign  a net property for a symbol, even the net is not connected yet. You can easy and quickly create as much power lines as you want!

The Value is displayed next to the symbol if confusing.

If you are on the second sheet you can copy paste such symbol with assigned net name or when you take from library new one, it ask you about the net name and automatically display in small drop down list of all previous defined power nets. Just use a net list data ! You take for example bar symbol and from the llib you just select 15V, or you copy paste it from another place.

Just give users ability to assign a net name in the power symbol! Making of 20 power symbols it misunderstanding.

[RichardHammerl · Accepted solution]

Hi @christopher2KLSVU 

thank you for you reply. 
I fully agree that the way how supply symbols are handled in Fusion Electronics could be easier and more user friendly. 

The reason for the way the supply symbols are handled has historical background. The libraries that are available via the library.io platform date back to EAGLE times. A long time ago in EAGLE it was defined  that there are supply pins which determine the net name and are used as power supply. The definition has to be made in the library already.

The concept has never been changed, because it has been used and worked with for many years and could not be changed easily without requiring a radical change in the user's usual way of working.
Now with Fusion, the opportunity has come to rethink and modernize the library concept. We will see a thorough revision and modernization in the near future.

Thank you and best regards,

[christopher2KLSVU]

Hello @RichardHammerl I suspect there are some reasons, like historical or comapbility issues thus it is not easy to change one thing without rebuliding complete house from ground.

The simplest way now perhaps could be add user a right to modify the Net name in Power symbols.

Then you must only introduce some kind of Warning when user is trying connect  Power symbol to the already existing net, to avoid shorting two nets in one if not needed. Such warning actually exists already.

Thank you for the interest.

The power symbols I use often as kind of ( Orcad way Of-Page connectors) I  know I can use just a net name and all the pages are connected via Net name, however drawing is looking more nice when there are some symbols attached. And it is Faster than adding and clicking label.

Such symbols make schematic nicer and more clear ( not spaghetti). Nn mentioned by me previous list I forgotten to list in Vref -s which we have had 2 or 3 in the past. Now lets imagine you must create each one symbol.., yes it is doable but not user friendly.

[silvio3105]

Hi,
I don't want to open a new topic - but is there any news about solving this issue? Why Power pin's does not use eg. value from component to create net name?

It's important for me since I have three symbols for VCC(point, flat and arrow) and three GNDs(signal, earth and chassis). Not sure how to make multiple GNDs/VCCs. Thanks!

[RichardHammerl]

Good morning @silvio3105 ,

thank you for the follow-up post in this thread. 

I am sorry, but have to say that there is no change in handling supply symbols yet. The library concept is still being worked on. 

About you question with having different GND symbols:

For each supply symbol you must create a device with the symbol assigned. The pin in the symbol has the name of your power signal (GND) and it has the pin direction supply (SUP). 

Best regards,

[rhdfmail]

The power-pins can also give a "intresting" experience when you add a MCU (from libraryIO i think) where the power-pins are named VDD, VDD1 VDD2 etc

Try to connect all those to your 3.3V net (or even to VDD and ERC-chaos emerges)
Solution is to edit your part so all vdd-pins on footprint is connected to 1 pin on symbol (not optimal)

last week i spent more time editing parts and create new ones than creating circuits in my project.

[silvio3105]

Thanks for anwser.
I've created my own power supply symbols.
GND symbol has direction "Supply" and name GND.
VCC symbol also has direction "Supply" and name VCC.

As far as I know, I can rename names while working on schematic(not by editing symbol). Since I mostly work with voltages up to 12V, I guess I can place VCC symbol and rename supply pin to eg. 1.8V.
Later I copy(CTRL+C - CTRL+V) symbols.
All other pins in symbols have direction "IO" since I don't use ERC.

[zdenekZzz]

Hello,

I have created an own power supply symbol "PE_GRID_EARTH" and a new device contains this symbol.
But the Fusion refuses placing this device into a schematic, because this device does not have a footprint.
What is the trick in library, enabling place into schematic possible?
Thanks.

[jorge_garcia]

Hello @zdenekZzz,

I hope you're doing well. Make sure that your power supply symbol only has 1 pin and that it's direction is set to sup. This lets Fusion Electronics know that you are making a supply symbol and it won't require the footprint.

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

Best Regards,

[zdenekZzz]

Thank you, Jorge, it works now.

Explanation for next visitors:

pin direction was "pwr" (power), instead of correct "sup" (supply).

[pblase]

Any luck in changing this? For most CAD packages, if I change the value of the supply or ground symbol everything else changes properly. Do I really have to create an entire new library just to add -12V to "Power Symbols"? 

[jorge_garcia · Accepted solution]

Hi @pblase,

I hope you're doing well. This has been changed, you can now use the NAME command and change supply symbol name to alter the net that it connects to.

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

Best Regards,

[pblase]

I second the motion!