How to make more voltage sources in multisim

[haklesup]

I am using MultiSim (power pro version 10) for schematic entry on a moderately complex design.  It has 5 different voltage sources and 3 different grounds.  The component library only has 4 DC sources (VCC, VDD, VEE, VSS) and 2 grounds (GROUND and DGND).  How do I make more?  I am not simulating but I will be using this to make a board with UltiBoard.

I've tried renaming the Label and value on a VCC (to VC1 for example) and if I say no to the question that follows I get a new source (without editing all VCC on the page).  Sounds good but when I copy and paste that object, I always get the unedited original VCC again (that seems like a bug).  I also tried copying that new component to the user library but was denied because it is virtual.  What is the best practice method intended by the program to deal with additional supplies?

On a similar note, How do I label a node so I can use it on the same page.  I tried an offpage connector and HB/SB connector but you can only use it once per page.  What if I have a several subcircuits using ther same signal on the same page and I do not want to draw a wire between them.  I would rather have the label name showing (similar to how an offpage connector looks). 

I tried placing a junction then drawing a wire to that spot then naming the node but if I turn off node names, the label disappears from the page.  Is there a more universal way than doing this.  Furthermore, if I try to copy/paste the node, all I get is the junction which assumes the node name of whatever I connect it to (just like a normal junction) the node is not copied.

If there is no way of copying a node or edited DC source around a page or to other pages than I quess I would be stuck editing each node's properties individually which is inefficient.  I am mainly looking for someone a little more experienced to tell me I am not wasting time.

[lacy]

I can answer one of your questions about node labeling. If you put a wire from your component to a junction connector then you can label that node to what you want. If you want more component pins tied to the same node, just do the same thing to each one and label it to the first node. I will post a simple circuit showing this for you to look at. It is called Virtual Wiring and the circuit will simulate with it.

Hears the Example circuit. Notice that all the nodes that are supposed to be connected together have the same name.

Edit: Sorry, it seems like you have already tried this. If you leave them on it does show up in the print Preview. So I would assume it would print them if that is what you are wanting.

Message Edited by lacy on 09-10-2007 06:33 PM

[lacy]

You can turn on just the Nets you want to see by setting the sheet properties to Net-Specific Setting and then clicking on the Net and where it says "When using Net Specific hide/show setting" put a check in the box that says "show" This way you can leave all the rest off and just select which ones that you want to be visible. You can also change the Net Specific setting from the spreadsheet view if you have the Power Pro Edition.

 As far as the copy and paste, you are correct that it only copies the junction and not the net. I have no idea on a solution to that problem.

I hope I was of some use to you on this subject

Have a Nice Day

[nestor-sg]

We are currently working on having that feature, that users would be able to create custom supplies and ground references and save them into the database.

As of now, like you said, Multisim has only 4 sources and 2 grounds. If you need an extra one you need to rename the RefDes, say GND3, if you copy it, it will default to the original one and you'll need to rename it back to GND3 to make a virtual connection between them. This is what we are working on, to facilitate to users the use of custom made sources and grounds.

For the junctions question, junctions are a representation of an intersection, it becomes part of a net when you wire a net to it, but the junction by itself has no 'net properties'. So when you copy it, it is not inheriting the net it was connected to. On this case, when you want to place a net somewhere else, use the virtual wiring process described by Lacy (see above), you need to create a new wire and then change the Net Name to match the Net Name of the net you want to create a virtual connection to. Off Page connectors are only used for Multi-page designs, for single page designs use virtual wiring.

As Lacy suggested, you can turn on the net names of that specific net that you wish to see its label (net name) or, use the graphic annotation tools to place a text label instead.

[haklesup]

Sounds like you're telling me I already figured it out myself, score one for intuitiveness of the program.

After reading your replies and reflecting on my own experience, for the puropses of PCB design (not simulating), it now seems to me that there is not much of a difference between a net and a net with a source connected to it.  The source is a nice little symbol but just naming a bunch of nets the same will get you to the same place when you go to UltiBoard.

I suppose I will use a combination of Offpage connectors for output nets which are used on and off the same page and virtual wiring on input nets.  For sources I will rename the sources but rather than one by one, I think I can save some time doing it in the spreadsheet view.  It all comes down to me needing to adjust my schematic drawing style a bit to match this GUI and project.

In addition to being able to copy an edited DC source while maintaining its new attributes, I would also like to be able to save it to my user library just like any other component.  I'm Looking forward to the next version.

[lacy]

"The source is a nice little symbol but just naming a bunch of nets the same will get you to the same place when you go to UltiBoard."

You are absolutely correct in your statement. Even if you have the source on the schematic {i.e the DC Power Symbol} it does not get transfered to Ultibooard because it is considered a Virtual Component. I have never actually tried what you have said, but I would think that it would work just fine.

You sound like you are understanding Multisim pretty well. I wish you continued success with it and maybe one day you will get into simulating the circuits that you draw.

Have a Nice Day

[nestor-sg]

That is correct, sources are virtual components that act as reference for the net, however, they are required when simulating a circuit for obvious reasons (generating the source voltage or referencing ground), in schematic capture they should still be present since its a very good practice to use those symbols to represent voltage sources or grounds for easy reading and understanding of the schematic itself.

In Multisim, the nets that are assigned to a source or a ground reference are transferred to UItiboard just like any other net of the netlist, if at some point in Ultiboard you wish to connect your net GND, to net 0 and to net AGND and to net GND1 (I'm just giving examples) you should use Net Bridges in order not to trigger DRC errors.

[GarretF]

Nestor is correct that you can use Netbridges in Ultiboard to connect different nets without generating DRC errors. I'd like to point out you can also automatically connect all ground nets (Analog and Digital) together when you transfer to Ultiboard.

In Multisim, go to Options > Sheet Properties. Select the PCB tab, then check the Connect digital ground to analog ground setting.