Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

net bridge design rule errors

Multisim 10.1.197 and Ultiboard 10.1.197

 

I could not get a net bridge to work in a Ultiboard layout, so I tried in a simplified circuit:  

 

In Multisim, place a connector with several pins, for example HDR1X10.

Place a DGND and GROUND. Connect the first to pin 1. Connect the second to pin 5.

Transfer to Ultiboard

Rotate HDR1X10 so the pins numbers increment left to right  

Place traces on the top layer so the pads of a net bridge connects one trace to another 

Place a net bridge, picking GND and 0 (also tried 0 and GND)

This gives Design Rule Errors:

   Unused pin is connected to NET = GND

   Unused pin is connected to NET = 0  

 

Is there a work around?  

 

 Ray

0 Kudos
Message 1 of 17
(6,640 Views)

What I see happening here is that it will not allow you to connect a net bridge or a trace between 2 separate grounds. I tried to get this to connect and the traces avoid the bridges like the plague. When I run a trace from the bridge and try to connect to the other trace I get the same error message because in actuallity the trace does not actually connect. It open ends the trace. Therefore it seems to be considering copper connected to an unused pin since you can't seem to bridge the two grounds like this.

 

The only options that I can see right now that would work is to go into Multisim under OPTIONS>SHEET PROPERTIES>PCB and put a check mark in the box that says "Connect dital ground to analog ground" . This will tie them together before transfer.

 

If you wish to do this after transfer then it is a little more complicated. You would have to use the Net List Editor and delete all pins associated with one of the grounds and re-assign it to the other. Then delete the unused ground.

 

This will work, but it seems to me that the net bridge should've worked unless it is a safety feature to keep analog and digital grounds separate which would make sense.

 

If anyone else has an easier or different idea, please let it be known. 

Kittmaster's Component Database
http://ni.kittmaster.com

Have a Nice Day
0 Kudos
Message 2 of 17
(6,620 Views)

I used the Net List Editor in Ultiboard as you suggested. I deleted all the pins for the analog ground net, and put them in the digital ground net. It does not allow a cut and paste of the list. However, I did several "print screens" of the Net List Editor for the analog ground pins before I started, so I was able to enter all 40, working from the printed list, without too much troble. I did several "print screens" again, to use to check the entries. I went over that pin by pin and then had a co-worker check it.  

 

Thanks for your help!  

0 Kudos
Message 3 of 17
(6,602 Views)
I've used net bridges many times to connect GND and DGND without trouble, so I was curious to try your simple experiment. I followed your instructions and I had no problems getting the net bridge to connect. The only difference might be that I am using EWB Power Pro 9.1.221.
0 Kudos
Message 4 of 17
(6,566 Views)

I think your right, I believe it is either something that has been added to Version 10.1 or possibly an error in how the programs is now handling these. I do not seem to recall having a simular problem in 10.0.1, but I can't be sure since I have removed it from my drive in favor of 10.1. Or both myself and this user are screwing it up somehow.

 

The best method is to tie these together inside Multisim befroe the transfer takes place. That way you can be assured that they will be as you expect when it does go to Ultiboard. This is, of couse, depending on whether you want your grounds to be seperate or tied to a common ground trace.

 

NI needs to read this a reply to it so we will definitely know what is happening here. I am just as curious as anyone else.

 

 

 

 

 

Kittmaster's Component Database
http://ni.kittmaster.com

Have a Nice Day
0 Kudos
Message 5 of 17
(6,557 Views)

I went back and looked in the help file. It said to create the bridge and then place it on top of both traces that you wish to bridge. I tried this with the users circuit he described and it seemed to connect, but I did still receive the DRC errors when doing so. The help file is sparse when it comes to this, although they do show an example.

 

So apparently using the net bridge connects the two traces and nets, but I still do not understand why it is returning the DRC errors. These can be filtered by the user, but I would like to know more before I say I have found an answer to this question.

Kittmaster's Component Database
http://ni.kittmaster.com

Have a Nice Day
0 Kudos
Message 6 of 17
(6,549 Views)

I am having the  same problems.  This is a very important feature that needs to work since there is no proper work around.  This is always the case when there are ananlog and digital grounds that need to be kept separate, but also need to be connected somwhere in a very controlled fashion.  I've followed the instructions exactly but what I get is a net bridge with no nets assigned to it's terminals.  You can connect it up but you get the DRC errors as stated earlier.

 

This can be manually fixed by going into the  netlist editor and selection each of the nets to be connected and adding on pin from the net bridge to each (NB1, pin _).  This removes the DRC error and everything is happy.

 

The only problem is when you forward annotate again you lose the NB pin assignments and you have to edit the netlist again.

 

I tried a part in MS with the net bridge as the footprint, but UB will not impor the net bridge when you do that.  To get around that I have a 'netconnect' part with just two dots and a silkscreen box around it.  This can be placed where you want the bridge and will import each time.  This is just a marker wheer you want the bridge to be.  You still have to place the bridge manually and edit the netlist to fix the DRC error.

 

This is a bug.  I should be able to assign the netbridge as the footprint of an MS symbol and have it come in with the right netlist connections when I forward annotate.   Alternatively, the netbridge assignments should be made to stick when the netlist is imported again.

 

David B

0 Kudos
Message 7 of 17
(6,244 Views)
The problem is your trying to fix something that should be done in design stage, not the layout stage.  You can tell multisim to connect the dgnd and gnd and 0 together by double clicking the part needed, pins tab, and change the power pins to the desired net by typing it in........so a TTL chip that has dgnd can be assigned to net 0 if needed........this has bitten me in the ass more than once (think $$$$) when in layout and the power pins are not connected because they are seperate nets.   In a simple design, its a no brainer......try that mess in an 8 layer design.........NOT!  The net bridge is great, but THERE IS NO REPRESENTATION OF IT IN THE SCHEMATIC!  This leads to major confusion when the boards are reved........did I put the net bridge in? Did I not?  Are the two connected?  Are they not?  Isn't the whole point of the netlist so you DON'T have to deal with that BS?  JMO, hope it helps some.   Chris


Signature: Looking for a footprint, component, model? Might be here > http://ni.kittmaster.com
0 Kudos
Message 8 of 17
(6,228 Views)

I aggree it should be done in the schematic, hence my net bridge component in MS and a footprint for it in UB. 

 

But telling MS to connect digital and analog ground is definitely NOT the way to do it.  This causes the netlist to loose all distinction between the two and negates the whole advantage of having two separate grounds.

 

There must be an MS netbridge part and it must keep the two nets separate in UB except for the bridge component, which allows the nets to be connected where and how it is required by the design.

 

David B

0 Kudos
Message 9 of 17
(6,226 Views)
I agree about the distinction, but still, that comes in the proper placement of the components.  Most people wouldn't autoroute something like that, but some do.  I can see its use and value for those that truely understand what it means, but overall, most do not understand what/why it is used/needed.....but it is a good point.


Signature: Looking for a footprint, component, model? Might be here > http://ni.kittmaster.com
0 Kudos
Message 10 of 17
(6,223 Views)