Controlled impedance routing in Altium Designer

[smuel]

controlled impedance calculator no ground plane

Hi,

I'm wanting to tune the impedance of some tracks in a layout that is already complete. I have tried turning on 'characteristic impedance driven width' in routing rules, but no matter which parameters I change here or in the layer stack formulas, it doesn't seem to automatically adjust the track width when I re-route the tracks.

Has anyone had success with this feature in Altium Designer 6?

Also, just another quick question, has anyone ever been able to route with rounded corners in this version of protel? It doesn't seem to work at all...

Thanks

Sam

 

[House_Cat]

impedance controlled routing

The impedance driven rules in AD work only for new tracks being placed after the rule is made. AD does not automatically go back and correct previously routed tracks. You must ensure that the box is checked in the width rule for "Characteristic Impedance Driven Width".

In order for the impedance driven rule to work when rerouting or routing a new track, you MUST have a reference plane adjacent to the signal layer upon which you are routing. The rule will not work without a reference plane, it does not work for differential pairs, and it does not work if your reference plane is a track or copper pour.

AD does not autoroute with rounded corners. If you are interactively routing, you hit Shift+Spacebar to toggle through the routing corner styles. There are two rounded corner styles 90deg and 45deg. The radius of the corner can be dynamically set while routing by using the "," and "." keys. In order for this to work properly, you must be sure that the routing corners rule is set to different values for max and min setback.

 

[smuel]

routing corners

Thanks for the reply. I still cant seem to get this rule working though... Here's a more detailed description of the steps Ive taken.

I have placed a ground plane on the bottom layer, and an adjacent plane on the top layer. I used place>polygon pour, and connected them both to AGND.

I select 'characteristic impedance driven width' in the width rule field, with a min 1ohms, preferred 50ohms, and max of 500ohms.

If i place a new track it shows up as about 1mm thick, then I hit 'TAB' to check the routing preferences, and under the 'calculated impedance' field it says -1.000ohms with an error saying this is out of range. If I change the impedance in this field, then return to routing, the track assumes the preferred width from the previous rule (normal width rule before selecting char imp driven width). Quite strange....

It is definetely set up for 'characteristic impedance driven width' but it seems to default to -1.000ohms and generate an error instead of going with the actual preferred impedance I set up.

I'm guessing this probably has something to do with my reference planes... Is placing a polygon pour the correct method for setting up the reference plane? By adjacent plane, do you mean on the same layer, or underneath on the bottom layer?

Thanks for your help, it's much appreciated.

Sam

 

[House_Cat]

What you are calling a "Plane" is really a polygon pour. That does not work for controlled impedance calculations.

The controlled impedance calculations done by the software expect you to use an actual continuous "Plane Layer" as the next layer under the signal layer. The traces on the signal layer are then referenced to that continuous plane.

There is a six page help document in the "Help" subdirectory titled "AP0107 Impedance-Controlled Routing.pdf". I suggest you read it and look at the examples.

There is no EDA package on the market that will automatically calculate controlled impedance using polygon pours as you are trying to do. You would have to use a 2 or three dimensional field solver to compute the impedance, and then manually adjust the width and spacing.