PCB Voltage clearance
Arunprakaash6 , 02-13-2020, 03:48 AM
Hello Everyone,
I have a doubt in PCB Trace clearance on different voltage levels. I will calculate the minimum clearance using following website:
I also use Saturn PCB Toolkit.
I calculated clearance for 48V and attached the result showing in website.
I am going to route in a External layer. My doubt is which one I need to choose 0.6mm? or Coated - 0.13mm?
I can't understand what is Coated? Is it a soldermask applied PCB? Can any one explain this?
I have a doubt in PCB Trace clearance on different voltage levels. I will calculate the minimum clearance using following website:
I also use Saturn PCB Toolkit.
I calculated clearance for 48V and attached the result showing in website.
I am going to route in a External layer. My doubt is which one I need to choose 0.6mm? or Coated - 0.13mm?
I can't understand what is Coated? Is it a soldermask applied PCB? Can any one explain this?
robertferanec , 02-17-2020, 08:05 AM
I can't understand what is Coated?
Conformal coating material is a thin polymeric film which conforms to the contours of a printed circuit board to protect the board's components. Typically applied at 25-250 μm[1](micrometers) thickness, it is applied to electronic circuitry to protect against moisture, dust, chemicals, and temperature extremes.
Source: https://en.wikipedia.org/wiki/Conformal_coating
k.ifantidis , 04-27-2021, 12:50 AM
I'm posting this [circuitnet discussion about pcb coatings] here because it's interesting. I have been wondering myself if soldermask is an electrical insulator coating or not. As I know from testing it provides electrical insulation but it is not considered an insulation from the IPC standards and safety engineers.
Conformal coating is an other procedure with other materials than soldermask in order to achieve insulation that will let you use smaller track clearances.
But on the other hand, if you have small track clearances + high speed signals you may anticipate cross-talk issues.
Regards, Kostas.
Conformal coating is an other procedure with other materials than soldermask in order to achieve insulation that will let you use smaller track clearances.
But on the other hand, if you have small track clearances + high speed signals you may anticipate cross-talk issues.
Regards, Kostas.
qdrives , 05-03-2021, 07:41 AM
You can simply see three situations:
1) Inner layer traces
2) Outer layer traces with solder mask (IPC 2221 - B4, "permanent polymer coating)
3) Pads/vias ("lead termination")
Conformal coating is generally only for point 3. Keeping clearance rules for 1 the same as 2 will reduce the number of rules (simplify).
So for traces you can use 0.13mm, but for pads and untented via's use 0.6mm unless you use conformal coating.
With the 0.13mm also keep in mind the production tolerance. I once had a notified body complaining about a board I designed exactly to the limits. They looked under a microscope. A square pad did not have enough clearance in one of the corners.
Besides IPC there is also the IEC 60664 for creepage and clearance and perhaps special product standards.
1) Inner layer traces
2) Outer layer traces with solder mask (IPC 2221 - B4, "permanent polymer coating)
3) Pads/vias ("lead termination")
Conformal coating is generally only for point 3. Keeping clearance rules for 1 the same as 2 will reduce the number of rules (simplify).
So for traces you can use 0.13mm, but for pads and untented via's use 0.6mm unless you use conformal coating.
With the 0.13mm also keep in mind the production tolerance. I once had a notified body complaining about a board I designed exactly to the limits. They looked under a microscope. A square pad did not have enough clearance in one of the corners.
Besides IPC there is also the IEC 60664 for creepage and clearance and perhaps special product standards.
Use our interactive Discord forum to reply or ask new questions.