Community
Fusion Electronics
Working an electronics project and need help with the schematic, the PCB, or making your components? Join the discussion as our community of electronic design specialists and industry experts provide you their insight and best practices.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

How to place via with specific net

16 REPLIES 16
SOLVED
Reply
Message 1 of 17
wleismer
2095 Views, 16 Replies

How to place via with specific net

Hello,

 

I am currently placing many ground stitching vias, and I cannot seem to directly place vias that are tied to a specific net.  For example, when I press Alt+V, I have no option to specify which net that via should default to. Instead, that via is assigned the default N$# net name, so I must manually change the net for each via, which drastically increases the time required.

 

I think the steps should be:

 

1. Alt+V

2. Specify net

3. Place as many vias as needed

 

Instead, the workflow I have been following is:

 

1. Alt+V

2. Place a few vias (so I don't lose track of them)

3. ESC out of via placement mode

4. Click each via I just placed

5. Rename the net for each via to GND

6. Press enter twice to accept

 

Repeat 1-6

 

I also tried copying and pasting ground vias, however they just get renamed to GND2, GND3, etc.

 

Am I missing some step to specify what net the via should be assigned to before placing it on the board?

Tags (3)
Labels (3)
16 REPLIES 16
Message 2 of 17
yiqiu.han
in reply to: wleismer

Hi, @wleismer 

 

What about have a try with below two ways?

1. Place one via and rename it at first, then copy and paste for several times to place them to the appropriate location.

2. Place one via and rename it, then do pattern and move them to the desired location.

 

Thanks,

Yiqiu

Message 3 of 17
wleismer
in reply to: yiqiu.han

Hi Yiqiu,

Thanks for your response. For suggestion #1, I have tried that, but whenever I paste the GND net, it is renamed to GND1, then GND2, etc. So, I must manually go back and rename each one to GND in order to connect them all.

For suggestion #2, that does appear to be much better. When the pattern is "pasted" onto the board, they are all renamed to GND1 or something, but if I rename one, it appears all will get renamed to GND. I will use this method for now, thank you!

Message 4 of 17
ritste20
in reply to: wleismer

Yes, I believe the pattern is your best bet especially for stitching vias since there is no real option to mass edit the signal properties with multiple items (at least with vias) selected.

 

Regards,

 

Steve Ritter
Manufacturing Engineer

AutoCAD/Draftsight
Inventor/Solidworks
Fusion 360
Message 5 of 17
jorge_garcia2
in reply to: wleismer

Hi @wleismer ,

 

I hope you're doing well. Built into the via command is a special function just for stitching. Here's the procedure:

 

1. Click the VIA command

2. In the command line type the name of the signal you want the via to connect to in single quotes. So for GND type 'GND' and press enter. 

3. Now every via you place will be automatically connected to GND. 

 

This avoids any copy or renaming workflows and is very efficient. Let me know if there's anything else I can do for you.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 6 of 17
wleismer
in reply to: jorge_garcia2

Fantastic, just what I was looking for!

Message 7 of 17

Using the via command is not well suited for fanouts of larger boards with many nets.

 

One feature you should consider is setting the via net by whatever it is placed over. If you paste a via or shape on a pad, then the net should update to the underlying. If you past a via on a shape then the via should inherit the net of the shape on the current layer. This is expected behavior for anyone coming from other professional tools. Me at least.

Message 8 of 17
ritste20
in reply to: jorge_garcia2

I always figured there was a way to name the signal prior to placing the via but didn't know how it worked... Is that something that could be included in the dialog in future releases so it is a much more visible feature?

 

Regards,

 

Steve Ritter
Manufacturing Engineer

AutoCAD/Draftsight
Inventor/Solidworks
Fusion 360
Message 9 of 17
jorge_garcia2
in reply to: wleismer

Hi @ritste20 ,

 

I hope you're doing well. That's a good suggestion, I would like to see a value field in the Via dialog where it shows the name of the via that's about to be placed. Typing in a name would overwrite the field and it would stick untill you change it or stop the command. 

 

@erik.buerV95QJ That's on the roadmap but it will likely be some time before it's available. Glad to hear you mention it.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 10 of 17
benjamin.jordan
in reply to: wleismer

YES YES YES. This is something that will be added to the roadmap. Along with a few more advanced via-related features. Thanks for offering this feedback to us. 



Ben Jordan

Senior Product Manager, Fusion 360 Electronics

LinkedIn | YouTube | Personal Blog | Fusion 360 Electronics Series
Message 11 of 17
shawn3WMTV
in reply to: jorge_garcia2

Has this functinlaity changed? When I type the net name in the coammnd line I get an error saying "Invalid Size ...

 

Its thinking what I type is the via size not net name.

Message 12 of 17
TravisJoe
in reply to: wleismer

I was getting angry at this since I do a lot of via stitching of power planes. It is worse when trying to stitch traces. 

I found that maybe there was a change in the VIA command where single quotes are needed for the signal name to work without giving the error. @shawn3WMTV this should resolve your issue if you have not already figured it out. 

For more reference
https://web.mit.edu/xavid/arch/i386_rhel4/help/98.htm

Message 13 of 17
AlexandrGUR2M7
in reply to: wleismer

Future request: Would be nice if via would pick net name from a polygon pour on which it placed, same as when placing on traces. And automatic placement of stiching vias... It`s ridiculous that we still don`t have that basic functionality, that Kicad and any other eCADs have.

Message 14 of 17
TravisJoe
in reply to: wleismer

I have definitely complained on the expert elite discussions on this, and I am being told that some of these updates to vias are finally in process. I believe that automatically connecting to a polygon when placed is one thing that has been discussed before. 

Message 15 of 17
aske.carstensen
in reply to: wleismer

Hi.

I just created a Via with GND just as @jorge_garcia2 described. Then I created a patteren, but then all next vias are called. GND1, GND2... 

 

Is there I way to avoid this, or do I need to rename a crazy about of vias? 

 

Message 16 of 17
wleismer
in reply to: aske.carstensen

EDIT: Sorry, I misunderstood your post...after reading again I think I understand your point.  I tried creating a pattern from a single 'GND' via, and was able to successfully do so.  Did you select "Use Source Signal" in the Pattern dialog box?  When I do that and generate a pattern, the resulting vias are all the same 'GND' net.

 

Fusion 360 GND Net Pattern.png


The via net naming functionality has improved since my previous post, as the development team has added a much easier way to do this than before.

If you are in your PCB file and look in your "Design" banner, select the "Via" option within the "Route" subsection.  The Via placement dialog will pop up, and the first field is "Signal Name".  If you enter "GND", then every via that you place afterward will have that net name.  I believe this is just the GUI version of what Jorge originally provided as the solution.

 

If I follow Jorge's original instructions on v2.0.16265, the solution still works just the same as using the new "Signal Name" field in the via placement dialog. 

 

If you do choose to use Jorge's original solution, be sure to type in 'GND' with the single quotes if you want to use the command line to define the via net name.

Message 17 of 17
aske.carstensen
in reply to: wleismer

Ahh awesome!

Thanks for the fast responds @wleismer 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report