WTH.....PCB prototype missing nets in hardware......arrrrrrrrrrrrrr

[lacy]

I have some further results to report on this issue. This is not only affecting the grounds but the power side also. What I did was to create a mini circuit just to test the tranfer functions and what I found is that if I have an IC hat uses VCC and one that uses VDD then these pins do not get connected together even though they have the same voltage value. So this indicates to me that if you do a design then you will have select ICs that uses the same power requirements so that all the sources get hooked up together unless your design actually uses multiple voltages that need to be separate.  I will post my test circuits for you to examine. In this one I have DGND and Ground connected together on the PCB through the Multisim option Sheet Properties menu . Notice however that VSS on one IC did not hook up to the negative supply or the other IC ground pin. This circuit was not intended to simulate, but just test this issue

This definitely needs to be addressed by NI. We need to know your thoughts on this.

[kittmaster]

ah.......a very good example, using these two files you can clearly see that the negative terminals never get connected to the ground anywhere.......this is a huge problem. Makes life easy for simulation, but for real world building, its a problem.

What to do what to do.

[nestor-sg]

Chris,

You don't have to rename all GND nets to 0 to connect them. You have two options to do this, whenever you want to connect the grounds together:

1. (Recommended) In Ultiboard, you will have two different nets, 0 and GND. You can trace  both of them with copper, no problem... at some point, either between tracks or between copper areas connected to each ground net (GND, 0) you can place a Net Bridge. This is what Net Bridges are for.  Go to Place > Net Bridge, select a Net Bridge from the database and then select which pin of the net bridge selected connects to each net. Then just place it. This will create a connection between two nets without each one of them loosing their own properties, its commonly used to connect analog ground (0) to digital ground (GND) at the point where the two of them must meet.

2. Follow Lacy's suggestion, from Multisim choose to connect the grounds together.

[lacy]

Thanks Nestor. I knew there had to be another option on this subject. Thanks for that information as Net Bridges never crossed my mind. I was trying to do this as it was being transfered to Ultboard from Multisim.

Also, just so you know. When an IC uses VSS instead of DGND, It doesnt get connect to GND in Ultiboard when using the Multisim option of connecting the ground together before export.

There should be an option that can be selected to use a single power source across components that may use different terminology for their power. This, in my opinion, would solve the problem and you wouldn't have to manually place Net Bridges. This could get tedious on a large design.

[nestor-sg]

Thanks for your suggestion Lacy... I will make sure that we file that suggestion. I would prefer to see a list where you can add which nets are your grounds and if you want to connect them or not... in this way you can add custom ground nets...

[kittmaster]

nestor,

You approach makes sense, but is a complete design flow contradiction.

Creating netbridges in UB is dangerous because now you have to play the game > "did i connect them/did I not?"

Unless your a super pro and can create a perfect master schematic, then every time you forward annotate, you'd have to reconnect the new net bridges. That will not work in any design environment. Unless this setting is retained somewhere.....but i don't see how since a forward annotate removes all netlist data during reimportation

In the design pyramid, these decisions of connecting VCC, VSS or VDD and ground or net 0 MUST be done at the top of the pyramid in MS so this round and round thinking is completely removed from the equation.

I'm using this software and paying hard earned money, many students are now sending their boards to board houses at $85-150 per design. This net bridging may be a bandaid fix but there is no way to expect them to remember to do this step.....who's fault does that become?

I know patrick is doing designing with this as he told me so because I asked him if he realized that is a money intensive process, but when your in small business or even personal, these types of things can not be part of our thought process.


EWB/NI's position should be that ANY TIME power pins are shown/hidden and of variant types that a dialog box is handled during forward annotation to determine by the user and or alert the user to see if the power pins are to be connected or not.

In ASEE training, VCC and VSS are "handled" the same way in a lab environment as a connection to the positive lead of the DC power source and grounds/VSS are also treated the same. MOST people do not deliniate between VCC and VSS as seperate entities since ULTIMATELY they some how some way connect to the +/- terminals of a power source.

There should parsing and checking and user warning before moving ANY of this data to real world designs! Please remember that ultimately its no ones fault but our own, but WE end up paying the price for this oversite

[lacy]

I may have a partial solution that could possibly work when it come to this layout situation. Instead of using net bridges or the Multisim option of connecting grounds you could click on the components properties within Multisim and edit the net assignments for the power pins. Granted this isn't the best solution as things like this need to be automated, but it sure beats guessing with the net bridges at the layout step.

[kittmaster]

that was what I originally found to fix the problem. Now take and place 10 of the same part on the same page, select all the components, and try to change them all at the same time......net zero to gnd or whatever. Say OK, now go back and pick any part.......NET name will be unchanged......but if done chip by chip.....change will be accepted.

to clunky.

I'm thinking of placing a VSS bar and attaching a net direct to the ground symbol to see what that does. Not sure if a DRC flags or not.....

[lacy]

Sorry about that. I forgot that was what you did at the beginning and I can see how this would be a pain to do on a large schematic. Anyway, I thought I had maybe come up with something there.

[Lodin]

Hello,  I am not sure if I understood everything correctly.

But I think, "netbridges" are a good idea. But as a component in Multisim !!

If I need different grounds, I have my reasons for it. So I have to document this, and this documentation should be part of the schematic. There must be a point, were both grounds are connected (power supply or ADC). So this connection point and his position is very important.

When I am using a netbridge as a component, I must think about the placement at the pcb. So the design cycle is OK.

Its just an idea 🙂

regards,

Lodin