www.eda.co.uk

Within Protel 2004 is it possible to use placement rooms to define design rules to a specific region of a PCB.

For example we will create a height restricted area on a PCB using a placement room.

First of all we need to place our room on the PCB to define our height restricted region.

Use the command Design » Rooms » Place Rectangular Room.  Once placed in your desired location you can double click to edit the rooms Properties and change its name.  In this case we have called it Warning Low Bridge.

You may also wish to lock the room in this position which can also be done in the room properties.

Now that we have our room placed in our height restricted area we can assign a height rule within the design rules.

Open the rules dialog box using the command Design » Rules and locate the height rules under Placement.

Create a new height rule using Right Mouse Button Click » New Rule and give it a new name e.g. Restricted Area.

Open the Query Helper and double click on TouchesRoom under the Membership Checks list.

then add the name of your room to this query, it should auto complete this and you will end up with a query similar to.

TouchesRoom('Warning Low Bridge')

Once you have created your query you can set your Preferred, Minimum and Maximum heights for your area and click OK to accept the changes and close the PCB Rules and Constraints Editor.