Multisim and Ultiboard

cancel
Showing results for 
Search instead for 
Did you mean: 

Print netlist in Ultiboard

Does anyone know of a way to print out the netlist in Ultiboard?  There has been a lot of forward/backward annotations between Ultiboard and Multisim, and I want to check and make sure everything is connected properly.  I could do it visually using the netlist editor, but I would print it out and have a hardcopy that I could go over.

 

Michael

 

0 Kudos
Message 1 of 9
(3,970 Views)

Hello Michael,

 

 

Thank you very much for your questions. I would like to know if by going to View > Enable Spreadsheet View you will be able to see the view of all different components. If you select the Nets tab, you will be able to view a list of all the nets of the circuit and on top of it, you can see an export dropdown menu. In this menu, you can either select to export it into a file, into the clipboard, or to print it. I would recommend either of this to export and visualize all the information of the nets of the circuit.

 

Please let me know if there is some information that it is not listed here and we can try to find a workaround for it.

 

 

Regards,

Luis

0 Kudos
Message 2 of 9
(3,957 Views)

Thank you very much for your response.  Unfortunately the spreadsheet does not help.  The parts tab does not show me the nets, and the nets tab does not show me the components.  If (in the parts tab) there was a column containing the net that the component was attached to, it would be ideal.  That way I could sort by the net, and see immediately whether or not the parts that should be attached together really are.

 

 

0 Kudos
Message 3 of 9
(3,953 Views)

Hi Michael,

 

Thank you very much for explaining more the request. Ultiboard will not be able to export this type of information together as we were looking at. Let me show you the following article:

  • Exporting Gerber Files from NI Ultiboard

http://www.ni.com/tutorial/6952/en/

 

But we can use Multisim to do this. Multisim will give us greater amount of functionalities that can help us have what you require.  For example, we can use the Netlist Report. Let me show you the following links:

- Multisim Education Edition Help 372062L-01

http://zone.ni.com/reference/en-XX/help/372062L-01/multisim/usingnetlistreport/#wp167575

- Multisim Education Edition Help 372062L-01

http://zone.ni.com/reference/en-XX/help/372062L-01/multisim/netlistreport/#wp69714

 

 

Is there a particular reason why you are using Ultiboard for this instead of Multisim?

 

Regards,

Luis

 

0 Kudos
Message 4 of 9
(3,942 Views)

I'm using Ultiboard as a final check, to make sure all my connections are correct before I have the board made.  Here is a perfect example of why I need to do this (because this was a mistake I found last night):

 

I have a voltage regulator that I created in Multisim.  The component has 3 pins, and I've labeled the symbol pins In, Out and Com.  I selected the correct footprint in Ultiboard but I screwed up the pin mapping - I mixed up pins 2 and 3.  In multisim all the connections are correct - my input voltage goes to pin In, my output voltage to pin Out, etc.

 

I transfer the parts to Ultiboard, place the components and use the Autoroute function.  Since I messed up the pin mapping, Ultiboard routes the input and output voltages to the wrong pins.  I don't see it - it's hard to notice a mistake like that if you're just looking at colored traces on the screen.

 

Last night I opened the Netlist Editor and went through the nets 1 at a time.  For each net, I compared the components that are listed in the text window to the schematic, to make sure all the connections are correct.  When I got to the V15 net (this is the input voltage to the regulator) I saw that the pin number for the regulator was incorrect and I fixed it.

 

I've also had a strange issue where 2 components in Multisim seemed to be connected together, but the wire between them was actually 2 wires with different nets.  That's why I check the Ultiboard netlist against the schematic.  The schematic always looks fine, but that doesn't mean it translates properly to Ultiboard.

 

Going through the netlist editor works ok, but I'd rather just print out a list.  It's the same process, but I can do it anywhere and am not stuck at my computer.  I can do it at home.  In front of the TV.  With beer.  I can't guarantee how accurate I'll be, but I'm willing to take that risk.

 

If the SMT pads / THT pads tabs had a Net column which showed what the pad was connected to, it would be perfect. 

 

Michael

 

0 Kudos
Message 5 of 9
(3,938 Views)

Hi Michael,

 

Looking deeply into your question, I believe we can do something that might help. We can go to Transfer > Backward annotate to Multisim > Backward Annotate to File. This will generate a .ewnet file that we can use with any plaintext reader. We can do the same on Multisim file and then use a text diff tool such as compareit or something similar to compare the information of them. On this files, you should have the information requested.

 

I believe that this might be the only approach we can have on Ultiboard to obtain the information we expect.

 

 

Regards,

Luis

0 Kudos
Message 6 of 9
(3,899 Views)

Thank you very much for your help.  Your suggestion is a good one, but I think it will only get me halfway to what I need.  I can find differences between Multisim and Ultiboard, but that's just forward/backward annotation.  What I really want is a way to scan through all the nets to make sure everything is connected to the correct pins (e.g. I know my op-amps should all have V- on pin 4 and V+ on pin 7, etc).  .

 

That being said, I think I can probably just take the ewnet transfer file and write a small Matlab program to extract the info I need and organize in a spreadsheet.  That's further than I could get before, so thank you.

 

If I could make a suggestion for future versions, it would be great to add a 'net' column to the Ultiboard SMT pads tab to make things easier.

 

Michael

 

0 Kudos
Message 7 of 9
(3,865 Views)

Hi Michael,

 

I agree with you on this one, it would be great for future versions to add the net column on the SMT pad. The idea exchange is a great place to request for new features because this is a webpage that is monitored by our R&D department and they take ideas out from here. I think that it will be very useful for us if you can post over here because it will cause a greater impact that a user is requesting this feature. The link for it is the following:

 NI Idea Exchange - Discussion Forums

https://forums.ni.com/t5/NI-Idea-Exchange/ct-p/ideas

 

Thank you very much for your questions! I will do my best from my end to also document this request.

 

Regards,

Luis

0 Kudos
Message 8 of 9
(3,854 Views)

MS and UB use the same netlist so it doesn't make much sense for UB to re-export the netlist again.  When MS exports a netlist it looks up the footprint pin mapping and that information is embedded with each instance entry in the netlist.  If your footprint print mapping is wrong then you should be able to see it checking in there.  I think if you do a back annotate and compare you are just comparing the same data to itself, unless you have made changes deliberately in UB that effect the netlist.  I tend to avoid that.

 

BTW I think a much easier methodology is just to QA all your MS parts both for the MS symbol pin labels, footprint type and MS symbol to footprint pin mapping.  If you feel more is needed then I think it's best to just do it directly in UB by selecting or zooming in on each pin to see the expected net label in that pin.  You do need to be sitting in front of the UB workstation to do that, but it's probably much more fun than wading through the netlist.

 

I do like the idea of adding the nets to the SMT (and TH and via) pads tabs in the spreadsheet.  Note that this is already done for copper areas tab.

 

Any object that can have a specific net assigned to it should have a net column in the spreadsheet.

0 Kudos
Message 9 of 9
(3,835 Views)