_Altium Designer Autorote Preferred width

Hello board, is there anyway that we can tell autorouter to use preferred wdth for routing but if it failed to find a way it can use narrower widths still within the range defined by the width rule?
Thanks

No - Situs isn't smart enough to automatically switch to a smaller width when it can't route with the default width. The router works from the design rules you have established. You should have a default rule for the routing width which covers the most common routing width used on the board, then add subsequent rules to selectively target other nets, classes of nets and so on.

Thanks a lot House_Cat,
I have two more questions, please
1- What is the most efficient way of using autorouter,
a) to group Nets in schematics and then after pre-routing sensitive/difficult nets use Auto-Route All
b) After placement and pre-routing use Auto-Route Component/Net lock good routes and again Auto-Route Net/Component...
if 'a' is most efficient when is most useful to use Auto-Route Component/Net/Area/Room
I feel this is not a good question because situation may vary from board to board but if you give me a basic theme that can be applied to many(if not most) boards of what is the most efficient way of using Situs Auto-Router (beginning from schematics) I really appreciate it.

2- In some months ago I remember I asked you a question about guard rings and you showed me a link that had some experimental graphs that showed guard rings are not much better than just increasing clearance. Since then I encountered many datasheets from different manufacturers Analog Devices/ Burr-Brown,.. that strictly recommended using guard rings for some sensitive ICs. e.g. very high impedance Opamp electrometers,..., why they are so commonly recommended? are they useful if you can't increase clearance enough but instead you can inset a very narrow, low clearance guard between aggressive track and victim track?

Thanks again,

The most common way of using the autorouter is to manually route the sensitive/critical traces and circuitry. You then lock all of those tracks, and use the autorouter to finish the non-critical routing. This technique generally requires fanning out the large chips first, then critical routing, locking, then autorouting. Using this technique, you would define special net requirements using directives and classes at the schematic level to establish the design rules for the board.

There are two different issues with guard rings and guard traces. One is their use to separate tracks to prevent cross-coupling. That is the one that is unnecessary. You can accomplish the same goal with careful layout and separation. The second use of guard rings/traces is to isolate sensitive circuitry from leakage currents. This is what Burr Brown is concerned with in their application notes. The high gain, high impedance, amplifiers are working with extremely small input signals (both voltage and current). They are recommending that you use grounded guard rings/tracks to ensure that no current leakage across the insulation of the board material gets into the sensitive input circuitry. From my experience, such a thing is only a problem in extreme enviroments when the traces are run in close proximity on the surface layers of the PCB.