How to edit rule scope in Circuit Studio

If you use the rule wizard to create a rule, then you'll have no way of editing it.  Yes this is stupid.

The background. In Altium Designer there is a thing called a custom query.  When you get to the end of the rule wizard and it shows you the query text that it's going to produce, this would normally end up in the custom query box in AD.  In AD, you would then be able to just edit the query text.

Hi Harvie,

Thanks for confirming editing is not possible.

It seems very silly not to allow this as you can effectively 'edit' it by creating a new one and deleting an old one; it just majorly interrupts my workflow in the process.

Is the idea that Altium essentially annoys you into upgrading to AD? I can't imagine it would be a significant code change to allow for that.

Hi Aaron,

Here is a response with a work around, since the functionality isn't in CircuitStudio currently.

CircuitStudio Design Rules don't have the queries exposed so the only inbuilt method is to us the Rule Wizard to replace the query.

However Rules can be exported and edited as a text file, then imported again to replace the rules. This could be useful if the rules are complex and take a long time to re-enter via the wizard.

1. Open the Design Rules dialog. Right click in the tree in the left. It doesn't matter where, but it is best to right click on the rule you're interested in so that you see those rules displayed.

2. Choose Export Rules from the right click menu and save the *.RUL file.

3. Open the *.RUL file in a text editor. If using CircuitStudio, use Open Document and choose All Files (*.*).

4. Carefully edit the rules by following the syntax within the file, such as adding OR InComponent('H6')

Each line is a rule. You may add or remove lines. The NAME= field can be used to overwrite existing rules with the same name or add new rules.

5. Open the Design Rules dialog. Right click in the tree in the left.

6. Choose Export Rules from the right click menu and save the *.RUL file.

Normally choose Yes to clear existing rules prior to import, unless you're deliberately wanting to add extra or replace only some existing rules.

Choosing Yes will delete rules in any rules chosen in the "Choose Design Rule Type", even if your *.RUL file doesn't contain that type of rule.

Notes:

1. You MUST click in the dialog to Choose Design Rule Type, even if the rule is already highlighted blue, otherwise it won't actually be selected.

2. The *.RUL text file may only have one blank line at the bottom of the file, not two, or it will crash when importing. The text editor in CircuitStudio sometimes adds the extra line so if you use the inbuilt text editor, make sure there isn't a red vertical mark on a blank line at the bottom of the file. Use backspace to remove it.

I hope this helps!

Tony

Hi Tony,

This work around is a massive help. Will go and try it now.

Thanks!

Aaron,

Anytime...please reach out if you need additional assistance.

Tony

Hi Guys,

I'm trying to create a component class for components that need to be directly connected to ground (i.e. bypass capacitors).

I created a "ClassName" parameter in my components schematic, but I can't seem to find it when I'm running through the Advanced Rule Wizard.

Is CS missing "Generate Component Classes"? Or user-defined component classes?

I also tried editing the .RUL file but when I import it back it doesn't seem to register the rule properly or it doesn't see the ClassName I created.

Any ideas would be greatly appreciated.

- Sujit

Bump

Hi Sujit

There is a setting in AD which allows switches on and off manual component classes (which is what you're trying to do), they obviously have this switched off in CS by default and have removed the options page where you would normally switch it back on.

However, as usual there's a file hacking workaround.  Close your project or exit CS, open your .PrjPcb file in a text editor and find the section that looks like:

[PrjClassGen]

CompClassManualEnabled=0

CompClassManualRoomEnabled=0

NetClassAutoBusEnabled=1

NetClassAutoCompEnabled=0

NetClassAutoNamedHarnessEnabled=0

NetClassManualEnabled=1

the line

CompClassManualEnabled=0

is the one of interest, if you change it to a 1 and save then reopen, I think you will find it will now work as you expected it to.

Regards

Hi Harvey,

Yes!!, that did the trick.

Is there anything similar to isVia , I'm trying to get ground vias to connect to ground polygons, without connecting all other component grounds to the same polygon.

- Thanks for your support

Yes you can match on more than one thing (you can use logical AND / OR expressions.)  So I believe this is what you're after, matching on both IsVia and InNet('GND'):

SELECTION=FALSE|LAYER=TOP|LOCKED=FALSE|POLYGONOUTLINE=FALSE|USERROUTED=TRUE|UNIONINDEX=0|RULEKIND=PolygonConnect|NETSCOPE=AnyNet|LAYERKIND=SameLayer|SCOPE1EXPRESSION=InNet('GND') AND IsVia|SCOPE2EXPRESSION=All|NAME=GroundViaConnect|ENABLED=TRUE|PRIORITY=1|COMMENT= |UNIQUEID=XACHTJSP|DEFINEDBYLOGICALDOCUMENT=FALSE|CONNECTSTYLE=Direct|RELIEFCONDUCTORWIDTH=10mil|RELIEFENTRIES=4|POLYGONRELIEFANGLE=90 Angle|AIRGAPWIDTH=10mil¶