How do you change the default via dimensions in Altium?

Question

When I place a via, it always has a diameter of 1.27mm and a hole size of 0.711mm. I want all of my vias to be smaller and it's really annoying to have to change them manually EVERY time. I tried going to Design > Rules and changed the "RoutingVias" rule so that the "Preferred" dimensions would be the ones that I want, but they still come out with the larger default dimensions.

I've googled this but haven't found what I'm looking for. I also tried changing the maximum hole dimensions to be the ones that I want, but the vias are still coming out way larger.

Anybody know how to get my vias to default to particular dimensions when I place them?

Thanks!

Answer 1

You can set the default via through DXP->Preferences->PCB Editor->Defaults->Via

For placing vias in interactive routing, you can press 4 and cycle through sizes of via- minimum, maximum, preferred or user choice (favorite).

Shift-V during interactive routing allows you to select a favorite from a list- and you can customize the list through DXP->Preferences->PCB Editor->Interactive Routing->Favorite via sizes

Answer 2

@markt answer is correct.

This is more of a side answer since it doesn't address your question directly, but it does help if you have made a mistake of choosing the wrong via size in the first place and need to change it.

If you have a bunch of vias (this method actually applies to any object within Altium) like in the image below

If you right click one of the vias, and select Select Similar Objects.. You'll get a window like this

These are basically search critera for you to find similiar objects.

If I'm looking for any via, I would change the Object Kind - Via to Same

If I'm looking for vias that have a certain hole size or via diameter, I would change those parameters to Same

Check the Selected Matched check box at the bottom of the window and it will create find and select all those objects that meet your criteria.

Now the awesome part.

In your PCB Inspector Panel (it would have opened up if you have checked the Run Inspector at the bottom of the previous window). If not, then just open up your PCB Inspector Panel.

You would see something like this

If I were to change anything here, it would apply to all the selected objects. I can change its hole size and via diameter and it will change it for every via I have selected.

It helped me a few times when I made a via too small and my fab house said it cant do it. To go through the entire PCB and find every single via and manually change it would have been a nightmare. But in a few short clicks, I changed all of them.

Answer 3

After you select the "place via" tool, hit tab and the "via options" dialog will come up. Any modifications you make in the dialog will be replicated for every via you place, until the next time you change it the same way.

Answer 4

Adding to this because I have spent time attempting the previous solutions for Interactive Routing and failed to alter the via size from the default 1.27mm. Maybe I did wrong, I dunno.

What worked for me was to go into Design> Rules> Routing> Routing Via Style and select the template to use. However initially this also did not work as the 'Enabled' check box was not selected. Once ticked, it works as desired.

Answer 5

Also adding to this thread. With no regards to Design Rules; The default dimensions of Via in Altium can be found here:

Tools->Preferences->PCB Editor->Defaults Under "Primitive List" there is a Via item where the defaults are set.