Getting Started in Altium Designer | Changing the Rules!

The Altium Designer environment is controlled by rules, which are created using a powerful tool called the “PCB Rules and Constraints Editor”.

By creating rules before component placement and routing starts, Altium can warn you or prevent you from making mistakes, depending on how your preferences are set. If rules are changed midstream, Altium’s sophisticated Design Rule Checker can highlight violations based on the revised rules, and report them in an organized format for review and editing.

The PCB Rules and Constraints Editor

If you create a New Project using the “<Default> template, and then Add New PCB to the project, a blank PCB will be created with some default settings already assigned. We are going to review some of those settings and suggest a few changes to them.

From the Main Menu, choose Design > Rules, or from the keyboard type “DR”

You should see a new window appear with a column on the left side sorted into categories.
Categories with a white triangle next to them mean there is more info inside them.
In the example below, I clicked the white triangle next to the first category called “Electrical”. It then expanded it to show sub-categories, and clicked “Clearance” to show the Clearance Rule.

In the Clearance rules shown above, the units are set to mils and the default clearance is set at 10mils (except for Holes). Old-timers like me still “think in mils”, and some bare board fabricators use mils in their DFM documents, but most people are using the Metric system now (in case you are metric-only, a mil is one thousandth of an inch).

You can use either system in the editor, and you can switch back and forth between mils and mm easily by using “Ctrl-Q” (hold down the Control key and hit Q). Entering values in the units that are provided is much easier than using a unit conversion tool.

In several of these categories, there is an “Advanced” mode that will open even more possibilities. In the picture above, it is next to the “Simple” button.

Also, notice that this Clearance rule applies to All nets. If you want to create another rule with different clearances for specific nets, right-click on “Clearance” in the left column and select “New Rule”. In the new rule, change the scope to your specific nets, like a High Voltage Net Class, for example, and then in that rule you can increase the clearance for your High Voltage nets. Move the most specific rules higher in the priority list, and make sure the “All-to-All” rule is the last rule in the list.

Now that we’ve briefly seen the structure of the PCB Rule Editor, the rest of this article will discuss the individual settings in some of the editor’s rule categories.

For example, in the picture of the “Clearance” settings above, all of the clearances are set for 10mils, except for holes. Most modern circuit board designs are using smaller clearances than that. For many years I routed 8 mil traces with 7 mil clearances, and I still use that today if I have room on the board, but smaller widths and clearances are more common. If you can find out where your bare board fabricator starts adding cost for smaller features, you may be able to save money by staying above their limits.
For the Clearance Setting for Holes, the default is set to zero. The example in the Altium documentation (under the paragraph called “Hole-to-Object Clearance Checking”) has it set for 0.381 mm, which is 15 mils. 15 is a good minimum, but I use at least 20.https://www.altium.com/documentation/altium-designer/pcb-dlg-clearancerule-frameclearance-ad

Modifying the Default Rule Settings

Here are some of the default settings you might want to review:

Electrical > Un-Routed Net
This setting is disabled by default, because the latest versions of Altium consider a net as fully routed if the copper features touch each other (e.g., stopping a route at the edge of a pad instead of routing fully to the center of the pin). While I can’t argue that “routed is routed”, I am more comfortable having the system check for loose ends.
Consider marking the checkbox “Check for incomplete connections”

Routing > Width
Revise the default routing width to match the Clearance settings (5/5 6/6 8/7, etc.)

Routing > Routing Via Style

The default via is a 28mil hole in a 50mil pad. This setting is much larger than it needs to be for all but the easiest designs. The older standard In-Circuit Test Point size was a 40 mil pad diameter, and that should be more than sufficient for everything except High-Power circuitry. Test Fixtures are reliable with 32-36 mil pads, and some advertise 25 mil pads as the lower limit for ICT these days.

For hole sizes, you should never go below an 8 mil diameter without checking with your fabricator. Try to use 10 mil or more if possible

(You can always make smaller laser-drilled via types, blind and buried vias, etc. These recommendations are for the default typical point-to-point routing)

Mask>Solder Mask Expansion
This setting clears the solder mask away from exposed copper and is set for 4 mils. This should probably be changed to not more than 3, we use 2. If you make a separate rule for vias, it can be less. Altium supports via mask tenting and mask encroachment, with a checkbox to add the expansion from the hole edge instead of the pad edge (if you aren’t using vias for ICT test points).

Plane > Polygon Connect Style
Make sure you look at the “Advanced” settings for this one. You probably want your vias to be directly connected to planes and polygons instead of using Thermal Relief.

Sometimes Through Holes are placed in rows, so it is better to have 45 degree spokes (so they don’t overlap each other), but you don’t want spokes coming out of the corners of Surface mount pads, so set these to 90 degrees.

To limit self-heating in power circuits, the spoke width should be wider than the length. In high current applications, it is better to use two wide spokes than four thin ones.

Testpoint > Assembly Testpoint Style

Check with your assembly partner, but the default test point size probably doesn’t have to be 40 mils anymore; some fabricators are setting the minimum at 25. A diameter of 32 mils is reasonable if Tooling Holes are provided in your design, otherwise a diameter of 35 will be safer. Reducing this diameter (and corresponding via sizes) can make a significant improvement in the routability of your design, and sometimes even the layer count.

Testpoint > Assembly Testpoint Usage
You would ideally want a lot of GND test points available to the tester, and several each for power nets, and sometimes two on each side of low impedance Kelvin 4-wire circuits. For these reasons, you should fill the checkbox to “Allow More Testpoints (Manually Assigned)”.

Manufacturing > Hole Size
Currently, you would never want to Mechanically Drill a hole that is less than 8 mils in diameter, so change the Minimum setting here to something more reasonable.

At the other end of the spectrum, the default is set for a maximum drilled hole size of 100 mils.
I would consider doubling this diameter, or at least raising it enough to include any 0.125” unplated Tooling Holes.

Manufacturing > Silk To Solder Mask Clearance
The default setting is to check the distance from silkscreen ink to exposed copper, but sometimes we are asked to remove solder mask from specific areas of the board, and in cases like that I want to be warned if there is silkscreen in those areas. I also don’t want silkscreen to drip over the edge of the mask material, so I change this rule to “Check Clearance to Solder Mask Openings”.
For this check the clearance can be set to zero.

Manufacturing > Minimum Solder Mask Sliver
The picture shown for this rule does not make it easy to understand what a solder mask sliver is, but look at the previous picture above, with rectangular pads. If these pads were close together, the green mask material between them would become a very thin strip. If the strip is too thin, it can break off and cause problems during soldering operations. I would set this “sliver width” to be 4-5 mils. A larger setting could generate many false warnings.

Summary

This article introduced the “PCB Rules and Constraints Editor” in Altium, which gives designers the ability to create and edit custom rules to suit the needs of their circuit board layouts. Creating design rules for a project can be tedious, so as you become more familiar with Altium Designer, you will want to create one or more templates to store your default settings.
Starting a new board design from a template can save time and reduce the chance of error.
Learn more about Project Templates

For More Information

Altium Designer Documentation: PCB Design Rules Reference

Would you like to find out more about how Altium can help you with your next PCB design? Talk to an expert at Altium or continue reading and learning more about utilizing rules to their full potential.