Note: You must be registered in order to post a reply. To register, click here. Registration is FREE!
T O P I C R E V I E W
kda406
Posted - 05 Feb 2020 : 22:57:05 Can someone tell me how to properly make non-plated mounting holes in Pulsonix V10.5?
Help doesn't tell me. The pad definitions in Technology Parameters do not seem to cover holes with no pads (mounting holes). I translated non-plated holes from another CAD system and they are not correct in Pulsonix. They translated as holes that are non-plated, but have pads.
What I am experimenting with is a mount for a standard 8-32 screw hole with a keep away large enough to prevent industry standard nut drivers from hitting the surrounding components. In the other CAD system this was a 178mil diameter hole with a 520mil diameter keep away.
I have many hours in on this, so if someone could please tell me the proper way to create this hole, I would very much appreciate it.
-Kyle
4 L A T E S T R E P L I E S (Newest First)
Olaf
Posted - 08 Feb 2020 : 20:28:07 Well, I think you can do this. Edit your pad style in the technology menu, use the 'By Layer' button, and add exception type 'Spacing Shape' with exception layer <Through Board'> and your required diameter. You do not need to create a footprint.
kda406
Posted - 06 Feb 2020 : 15:32:52 Thanks, that helped. Since this is such a common requirement, I'm surprised Pulsonix doesn't already have a built-in mounting hole definition (non plated hole with built-in keep out) in the Pad Styles. Having to put the area in as a secondary operation leaves a lot of places for mistakes to be made. Other CAD systems had this figured out and built this in 35 years ago.
Still, at least there is a work around for this. Thanks very much for your help!
-Kyle
jameshead
Posted - 06 Feb 2020 : 07:21:09 If this is a standard mounting hole that's going to be used time and time again then I suggest adding the mounting hole to your library either as a part to the parts library or a PCB documentation symbol.
Creating a footprint for your mounting pad is broadly the same process whether it is a part or a PCB documentation symbol.
The advantage of the Part approach is that you can show the mounting pad on your circuit diagram, show a connection to a 0V return reference (though not in your case as you are not using a copper land), and bring up part numbers for screw, washer, nut etc. in a BOM.
Create a blank PCB documentation symbol or a footprint and insert your pad.
In your example you suggest a pad size of 0 for the copper land and a hole size of 178 thou [4.52 mm]. As Ben says, unselect the box for non-plated holes. Next though I'd use the BY LAYER button in the Pad Styles Technology dialogue and enter values for Solder Mask Top and Solder Mask Bottom of 185 thou [4.70 mm].
Next use the menu Insert > Area > Circle and add a circular area from the pad and whilst you are drawing it out, right click and select Enter Diameter then enter 520 thou [13.20 mm].
Select this area, click the right mouse button, select Properties then the Area tab, then make the appropriate Keep Out selections. Change "Tracks" from "Unrestricted" to "Keep Out" etc.
If you have a STEP file for a screw/washer assembly then you can for completeness use Tools > Position STEP model to add this.
I mentioned you are not using a copper land. Personally I use a copper land on non-plated holes to provide mechanical strength to the PCB whilst a screw/nut is being tightened onto the board.
bkamen
Posted - 06 Feb 2020 : 01:49:04 Hey there!
In Technology settings for pad styles, there's a check-box for plated hole or not.
That's step one.
Step two -- is that you'll want to create a plot for plated holes and non-plated holes.
It's a good idea to make a separate NC drill file for plated and non-plated holes as well as a separate gerber file for plated and non-plated holes.
