On 8/7/2006, Grace Lin wrote:
What is required for creepage and clearance of 230VAC hot, neutral and earth ground that is on internal layers of a PCB per Section 2.10.5.3 of UL 60950? The PCB is a multilayer PCB. Hi Grace: There is no creepage or clearance distance when the separation involved is on inner layers of a multi-layer board. The only requirement is for distance through solid insulation. For isolation between two traces on the same layer, EN 60950 allows you to go as low as 0.4 mm, although I have never been comfortable going that low. For isolation between traces that cross on different layers, the Table 2M in section 2.10.5.3 describes the circumstances under which you are allowed to have less than 0.4 mm insulation thickness. Again, I usually avoid using these exemptions if at all possible. When you use inner layers for circuits that require solid insulation, you typically have to get very involved with the specification of the board stack-up that will be used to fabricate the board. The actual thickness of the layer-to-layer insulation in a multi-layer board can be anywhere from 3 mils to 30 mils, and the exact thickness that will be used is often left to the discretion of the board fabricator. Your EMC engineers will also have a say in the stack-up that is used, so you will have to coordinate with them. It can be difficult to ensure that your board manufacturer has complied with all of your stack-up specifications. The easiest approach for isolation is to use the top and bottom surface layers and void the inner layers, so that you are guaranteed the full board thickness (typically 62.5 mils) for insulation thickness. Of course, this approach forces you to use the full creepage and clearance distances that apply to surface layers. If this approach can't be used and the circuits have to go on inner layers, you will be forced to get involved with the construction of the board stack-up. Typically, the area with the isolation requirement is just one portion of a larger board that has to be 8 layers or more for other reasons. On such boards where I have to use inner layers for isolation, one thing I usually do for added insurance is to put as many voided layers as possible between the circuits I am trying to isolate. For example, if it is an 8-layer board I might put the circuits being separated on layers 3 and 5, with layers 2, 4, and 6 voided. This way, even if the board shop makes a mistake with the specified insulation thickness, you have at least two sets of layer-to-layer insulation separating your circuits. Joe Randolph Telecom Design Consultant Randolph Telecom, Inc. 781-721-2848 (USA) [email protected] http://www.randolph-telecom.com <http://www.randolph-telecom.com/> ______________________________________________________________________ This email has been scanned by the MessageLabs Email Security System. For more information please visit http://www.messagelabs.com/email ______________________________________________________________________ - ---------------------------------------------------------------- This message is from the IEEE Product Safety Engineering Society emc-pstc discussion list. Website: http://www.ieee-pses.org/ To post a message to the list, send your e-mail to [email protected] Instructions: http://listserv.ieee.org/request/user-guide.html List rules: http://www.ieee-pses.org/listrules.html For help, send mail to the list administrators: Scott Douglas [email protected] Mike Cantwell [email protected] For policy questions, send mail to: Jim Bacher: [email protected] David Heald: [email protected] All emc-pstc postings are archived and searchable on the web at: http://www.ieeecommunities.org/emc-pstc
