Altium designer 6.6 routing problem

Hello, I'm using altium designer 6.6 for auto-routing. sometimes I define some rules that are pretty hard to satisfy so after a great percentage of routing had completed I have to stop the autorouter, redefine rules with more relax restrictions, lock previous tracks and run the autoroter again to route the remaining nets. for example I want my power track all be in bottom layer and all be 50 mils as long as it is possible. Obviously it is impossible for a very complex board with many hundreds of nets, so somewhere I have to give in and allow routing to be done also in another layer.
the problem is, when I want to re-run the autoroter some tracks that had been partially routed in previous routing session inhibit new routing success. I want to un-route them but it is impractical to do this by hand(it takes hours) and even so, small parts of some tracks may remain unseen under pads or other tracks. I usually select 'rip-up violation after routing' check box but it seems because DRC dose not regard them as violation they do remain. how can I select partially routed connections and un-route them??

one thing else How can I create a net class in PCB. I want to group some neighbour components and define some rules for their width and other properties. I tried TouchesRoom and WithinRoom but they return components and pads and tracks not nets and in rules for defining width I need to have a net class. Is it possible that I Have a special width rule for some parts of PCB e.g within a room?
Thanks a lot

The only way to unroute partially routed nets is manually.

Net classes are supposed to be defined in the schematic. However, you can define a class from the PCB editor by going to Design>Netlist>Edit Nets. The left box in the resulting dialog lets you add, edit, or delete net classes. Note that if you import the data from the schematic after manually defining a net class in the PCB, the software will try to remove the manually created PCB net class.

Yes, you can define a width rule for tracks in a room. You would use something like "IsTrack AND TouchesRoom(xxxx)" or "IsTrack AND WithinRoom(xxxx)". You can even use "OnLayer('TopLayer')" to further qualify the rule.

@ltium designer 6.6 routing problem

Hello House_Cat, Thank you for your help. I tried IsTrack AND TouchesRoom('xxx') but autorouter dose not listen. I defined different width definitions for different rooms and set their priorities but it seems autorouter always love to route with the least priority rule and ignore higher priority rules(except when I define rules using NetClass). when I check the query sentence in PCB Filter it correctly selects the tracks that I want but it seems in autorouter because I still has no track(they are all rat nests) these rules have no effect. Are you completely sure that IsTrack AND TouchesRoom('xxx') work in autorouter?
As I said my problem is to set width for different rooms that I define within PCB.
Thanks.

I was wrong. You are correct that an "IsTrack" rule won't have any effect for autorouting.

A way of handling your problem would be to use a width rule that says something like "InNet('xxx') AND TouchesRoom". Aside from net classes, that looks to be your only option.