Power and Gnd

RS · Post by RS » Thu 2006-07-13 15:39

Hello , I have a question for you , can I build the new power and ground , in library there is Power ( 5Vdc ) and Ground (0 Vdc) , I have to have the Power 12Vdc and the second ground ( Ground ext ).
Why if I decompose the symbol power and after create with Make Symbol the new power it isn't connect to net VCC.

Thank you.

dickperin · Post by **dickperin** » Thu 2006-07-13 17:37

Hi,

First a note of explanation. If you grab a POWER symbol and place it in a schematic, by default it connects to every other POWER symbol on the schematic. If you tag it (click right on it) and then click left on it, it brings up a properties window. Put a name such as +5V on it and it no longer connects to the other POWER symbols-- but it connects to every other power symbol labeled +5V. This works the same for grounds. A default GROUND connects to every other GROUND. Tag it, left click it and change it to EARTH and it will then connect to every other ground labeled EARTH. So for purposes of building a netlist, use this method to designate what connects where. If you are placing a chip where the POWER and GROUND pins are hidden, tag the chip (right click) and then left click to bring up a properties window. Click on HIDDEN PINS. Change these to +5V or -8V or whatever. It will now connect to the appropriate net and a text box will be added to your drawing stating this.

On a second point, the COMPOSE SYMBOL is for creating parts. A part is connected discretely to the circuit via its pins. GROUNDS and POWER rails are designed to create unofficial busses, if you will, and therefore do not behave like parts. So you can not decompose a POWER symbol and still expect it to behave like a POWER rail.

If you would like different symbols (for example, I created different GROUND symbols) to use on your schematic, you can create them. Draw a symbol and attach a pin. Label and number the pin (and hide the label and pin) and save them to the user library. If your goal is to create a PC board, use the above method first and generate your netlist for ARES. After that, you can merely drop your newly created symbols on top of the old ones to create a very descriptive schematic. Which is, by the way, another area where Proteus is way ahead of other schematic capture programs-- it's output from a color printer is outstanding. But if you have to go back and change something and regenerate your netlist, you will need to change the symbols back in order to generate a correct netlist. By the way, the "SAVE AS" command is great for having two versions of your schematic. An easy way to have your cake and eat it to. Hope this helps.

RS · Post by RS » Fri 2006-07-14 6:14

Sorry but I don't be able to create the symbol for example 12Vdc , please you can make sense of footstep for footstep as to create the component.

Thankyou

Richard_Reeves · Post by **Richard_Reeves** » Fri 2006-07-14 8:20

To just create a +12V power-rail, do the following:
Click on the Inter-Sheet Terminals icon,
Select a Power terminal,
Place it on your design,
Right-click to tag it, then left click to bring up its properties,
In the String field, add +12V.

You now have a power net that is called +12V, and that is actually connected to +12V. If you don't put a + or - before the value, it will not assign a voltage to the net - see the picture below:

Hope that helps!

Richard

RS · Post by RS » Fri 2006-07-14 10:07

thankyou for help , I have another question , in library there is 5Vdc , it is the default power and your symbol is triangle , I have to build my personal symbol , it have to have a circle of symbol and your default power is 3.3Vdc , I can create it and save in library system??

Hello

dickperin · Post by **dickperin** » Fri 2006-07-14 11:54

Under the Inter-Sheet Terminals, there is a circle already (called default). If you want to make your own, you can create it as a part, save it in your USER LIBRARY, and set its PACKAGE property to NULL (so ARES knows there is no footprint for a part). Place it on the schematic and connect them together via using a WIRE LABEL (see WIRE LABEL in the on-line help). Another way to do it.

RS · Post by RS » Fri 2006-07-14 15:24

Dear Richard , I have a problem with my power 12Vdc , when I build the power I do this:
1 I create a graphich ( line+ circle)
2 I place a node
3 I place a Label
4 I select all
5 I create a terminal with Make Symbol

The terminal isn't the power terminal , I don't enable the type power in my terminal .

Hello

Post by **Ettore** » Fri 2006-07-14 22:24

Such of terminal objects and related properties are well described to the OBJECT SPECIFICS section in the ISIS help file. You'll want to have a look at.

However, the power terminals are very similar to the default one, except for the TYPE=POWER. This special assignment allows the object to be included into the Power Rail Configurator list.

So, as a final step - but the most important one - to add in the list of the operations that you have mentioned above, you must include those followings:

1) press the 'A key of your PC keyboard. This opens the 'Property Assignment Tool' dialogue.

2) Type in the field 'String' : TYPE=POWER and click on OK button.

3) Using the mouse, click left on the pin of the terminal you have created just now.

If now you connect a voltage probe to the new power terminal then it shows the same voltage that you have set as a label. Remember the Richard's recommandations about the correct label format.

RS · Post by RS » Mon 2006-07-17 8:54

Dear Ettore , I have do the Property Assignment Tool and the Terminal now is Power but I have a question for you , why I can't do the Property Assignment Tool when my component is Decompose , the program say "This graphic object cannot be edited" , I can assign the ownerships in definitive way.

Thankyou.

janneman · Post by **janneman** » Mon 2006-07-17 11:19

If decomposed it is no longer a component, its just a bunch of graphics. You have to make it a component before you can assing any properties'to the component.

Jan Didden