Trace Clearance for 500V DC Insulation Resistance Measurements - Page 1
Forum section: electronics / projects

author: koffiend
author_rank: Newbie
timestamp: September 08, 2020, 05:01:20 pm
content: Hi all,I am designing a tool for work that allows us to speed up our insulation testing of harnesses. Some of our cables have 55 pins plus the shield, which leads to 1540 pin to pin test combinations. We have made a couple of boxes soldering wire to daisy chaining switches, but they require a lot of labor to produce and the solder joints have broken many times due to rough handling during shipping and use. We currently use Fluke 1587's to measure insulation resistance at 500VDC. In order for a cable to pass it must measure at least 100Mohms.I have been looking around for guidance regarding high voltages and PCB trace clearance. Mostly what I have come across are IPC standard recommendations. The problem though is that it would require 100 mil trace clearance at those voltages. I came across this article that talks about a difference between functional and operational insulation.https://www.smps.us/pcbtracespacing.htmlIn my application equipment and personnel safety is not a concern. The harness is disconnected from all electronic components and the meter produces the equivalent to a static shock if the probes are touched. The highest operating voltage in the harness is 28V DC if we were to use it as an inline breakout box to scope signals. This is a tool for in-house use only. I am looking for some guidance regarding the minimum required trace clearance for such an application. My only concern is ensuring that the PCB does not affect our measurements and gives false failures in our readings. I have seen that using internal traces significantly reduce the IPC requirement and I have also received the suggestion of conformal coating. I am trying to keep cost down as much as possible, but if needed conformal coating could be an option if it would help.Below are screenshots of the schematic, layout, and model of the concept. The schematic is cut off, but the portion not seen is just more switches and test points connected in the same fashion as those shown. The maximum trace clearance I could achieve while still being able to route between the pins of the connector is 11 mils.

author: Laszlo
author_rank: Contributor
timestamp: September 08, 2020, 06:11:48 pm
content: Hi,I'm not sure if you have seen this article, linked down below. Apparently UL has done an experiment to test PCB tracks for purely insulation purposes. It specifies 44V/mil for adequate clearance in between parallel tracks.https://www.smps.us/pcbtracespacing.htmlI think 11 mils are not adequate without coating the PCB's. If your test box is going to be used in dusty environment surface contamination will have an adverse affect on your readings.Hope that helps a little.

author: jkostb
author_rank: Regular Contributor
timestamp: September 08, 2020, 06:41:33 pm
content: You need to consult relevant safety standards. For measurement equipment you can consult IEC61010-1. These standards specify clearance, creepage distance, and insulation through solid. The insulation distance will also depend on pollution degree, overvoltage category and comparative tracking index.

author: koffiend
author_rank: Newbie
timestamp: September 08, 2020, 07:39:31 pm
content: Hi Lazlo,Thanks for the information.I did read that article, but I don't have access to that UL standard, so I couldn't reference the table for findiing the withstand voltage. However, just using the 500V the insulation resistance tester puts out and the 40V/mil isolation provided by clearance alone, I would need just under 13 mils clearance. Looking into conformal coatings a little bit, i found Acrylic coatings providing at least 300V/mil(https://blog.paryleneconformalcoating.com/comparing-ar-to-ur-conformal-coating). With that information, it sounds like I can keep my current trace separation and put on a 2 mil thick Acrylic coating and not affect my measurements. I'll keep looking into it, but thanks for the confirmation of my suspicions.

author: bjbb
author_rank: Contributor
timestamp: September 08, 2020, 07:55:25 pm
content: Insulation Resistance and Dielectric Withstand tests are not the same, and do not typically use the same test equipment, and are intended for different reasons, and have different test conditions. You must understand that environmental conditions and the surrounding material properties can have a significant affect for the IR test.'Functional' insulation has no meaning per the dielectric withstand Type Test referenced in product safety standards; so comments where the reference is solely a safety standard should be disallowed. Also note that IPC manufacturing and construction standards, and the nationally harmonized references based on IEC standards have somewhat similar spacing recommendations or requirements.For 500V, where correct materials are used and environmental conditions controlled, 0.28mm of air will provide approximately 800V of withstand.

author: trobbins
author_rank: Frequent Contributor
timestamp: September 08, 2020, 11:29:37 pm
content: Have you costed up a multilayer pcb with internal traces to achieve solid insulation isolation. Once a pcb is accepted as ok, then there would be very low risk of the insulation degrading over time, and periodic testing of the pcb could maintain confidence.Is there a way to divide the test voltage in two in some manner as a +/- V to ease your equipment/part/pcb voltage stresses?Are you able to use optomos devices for controlled switching of test voltages? A quick look at 1500V device indicates its off-state resistance exceeds the 100Meg requirement.

author: koffiend
author_rank: Newbie
timestamp: September 09, 2020, 04:13:44 pm
content: bjbb,I was under the impression that Dielectric Withstand and Insulation Resistance are very similar in terms of testing procedure, the difference being that withstand is done at much higher voltages and measures leakage current, where as IR is done at lower voltages and measures resistance (which would basically the same test since it uses Ohms law to measure the resistance).trobbins,I have not run the cost of the PCB yet. I am still in the beginning phases. I wanted to get some input on trace clearance before I do the layout on the entire board. There a lot traces and I would hate to complete layout, only to have to redo it. I will look for an estimate, it may just be worth it to move the traces internally and not have to worry about it.As for dividing voltage, I am not sure what you mean. The cables we are testing have to be exposed to 500VDC as part of the check out, and our source comes from a handheld tester. Also, I need to keep the components in the test box passive. We don't always have access to power and I do not want to rely on batteries. We never have them when we need them and depending on where we are working, sometimes they're not readily accessible.I am not sure I have explained my application clear enough. I have drawn a quick diagram of my application. Our high voltage "source" is a handheld insulation resistance meter, model Fluke 1587. The box is basically a breakout box for the cable, giving us ease of access to each wire in the cable. The cable is the component which must pass the insulation resistance test. I have to design the box in such a way that it will have no to minimal effect on the insulation resistance reading of the cable. This is why I have no worries about safety. We run no risk of damaging any electronics (none are connected) nor injury to personnel (the meter cannot produce enough current to harm anyone, I have touched the probes accidentally a few times and while it stings, it is no worse than the static shock you get from rubbing your feet on the carpet and touching a door knob). The actual signals on the cable lines never exceed 28V, the insulation resistance test we run is solely to check the integrity of the cable. The sole purpose of the box is to significantly reduce the time it takes us to run pin to pin insulation resistance measurements on high pin count cables. I hope this clears this up some if there was any confusion.I am grateful for all the advice and taking them into consideration like looking into coatings, growing the board to use larger connectors, internal vs external traces, etc. The good news is that this is not a critical item, just something that would be nice to have, so I have the time I need to look into these things. Thanks for all the help so far.

author: trobbins
author_rank: Frequent Contributor
timestamp: September 10, 2020, 12:12:45 am
content: Can you clarify that your issue relates mainly to how to work with a 62 pin D-Sub socket (where your DUT is a harness with a 62-pin plug)?If so, then is it that you want to mount a socket on a pcb, and use pcb traces to connect to the socket pins, and that is where you have trace routing concerns?If so, and given it is a custom test jig, then could you free wire directly from each socket pin terminal to individual points on the pcb, such that all pcb traces have sufficient creepage (ie. don't even provide socket pin pads)?

author: TimNJ
author_rank: Super Contributor
timestamp: September 10, 2020, 02:14:22 am
content: For no contamination/very light contamination, you can use 1KV/mm as a starting point. By this "rule", I would shoot for about 0.5mm for 500V.

author: koffiend
author_rank: Newbie
timestamp: September 14, 2020, 01:12:26 pm
content: Hi Trobbins,My main concern was trace separation on the external layers. When I started layout, I quickly realized how crowded it would be. I have decided to use a multi layer board, just so that it is not a concern anymore. I have a 10 mil trace separation on the internal layers, which would be up to IPC 2221 standards, which probably exceeds my need for just insulation resistance testing.The secondary concern would be the connector not having 100 mils of separation between the pads, per IPC 2221. I currently have just over 34 mils of pad to pad clearance, and set my rules for 25 mil clearance on external layers. Following the guidance on this link,https://www.smps.us/pcbtracespacing.html,for HiPot testing a 40V/mil separation would provide sufficient clearance.I could use an in-line panel mount D-sub connector, but it would make building the kit a bit more labor intensive and drive up the cost to manufacture, but may be worth it in the long run. I will have to get some estimates. I was also considering conformal coating the board and just masking the mating face of the connector and allow the conformal coating to provide some insulation on the PCB pins.TimNJ,Thanks for the input, the routing rules I have in place are set to a minimum clearance of 25 mils (.635 mm), which is just a little more than you are recommending. So, that provides some sense of assurance.