Community
Fusion Electronics
Working an electronics project and need help with the schematic, the PCB, or making your components? Join the discussion as our community of electronic design specialists and industry experts provide you their insight and best practices.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

npth that will have pads on both sides for a pressfit nut to form a switch thru the board

18 REPLIES 18
SOLVED
Reply
Message 1 of 19
pstamand
592 Views, 18 Replies

npth that will have pads on both sides for a pressfit nut to form a switch thru the board

How do i place a via 400 mils with a 250 mil hole that's not platted with a pad on both sides of the board?

 

Is there a way to suppress the platted thru of a viaor make the via hole smaller and then drill out to the desires 250 mil?

 

I'm putting a press fit nut that will be a switch and I cant find a way to do this.

 

pstamand_0-1669584479505.png

 

18 REPLIES 18
Message 2 of 19
jorge_garcia2
in reply to: pstamand

Hi @pstamand,

 

I hope you're doing well. This is a tricky one. I would recommend two things

 

1) Have good communication with your board house, they may be able to take care of it for you as long as you provide specific info to them.
2) You could also do a more hacky option where you draw a polygon on the top and bottom layers and then stick a hole in the middle of them. When you go to generate your gerbers you have to generate two drill files, one with the plated through holes (drills layer) and one with the non-plated through holes (holes layer).

 

Let me know if there's anything else I can do for you.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 3 of 19
pstamand
in reply to: pstamand

Hi,

I've made progress.

I'll have to ensure the board manufacturing can handle this and ensure the second surface component on the other side of the board works. I didn't like the polygon as it was being difficult to manage the desired shape.

I created a surface mount pad with a single pin and a npth place at the center on one new custom library component...

I've attached the top and bottom 3d view the top side component.

I'm thinking if I create another separate component that is simply a surface pad and pin without the hole... Will this work, no idea yet, but as a surface mount there should hopefully be no constraints and I'll have the desired outcome.

Being able to deselect the pth and change it to a npth should would be helpful as a via or something else directly and not have to go through all this trickery or allow a drill at a via and not block it.

Message 4 of 19
jorge_garcia2
in reply to: pstamand

Hi @pstamand,

 

I hope you're doing well. Could you post a picture of what you are seeing in the 2D PCB? At the end of the day the source of truth is the 2D PCB so if everything looks good there it is good.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 5 of 19
pstamand
in reply to: jorge_garcia2

I did its attached as 2 png files.
Message 6 of 19
pstamand
in reply to: pstamand

Ah, I posted 3d, here also the 2d top and bottom

pstamand_0-1669935428992.png

 

 

pstamand_1-1669935462263.png

 

 

I  still need to add the surface component to the bottom side, but as surface the pads shouldnt matter.  I have no idea what the hole in the top side custom component will do on the bottom side, my desire is as  surface the bottom wont care about the top side hole.  for manufacturing as long as the hole happens last, I'll achieve the desired outcome.

Message 7 of 19
jorge_garcia2
in reply to: pstamand

Hi @pstamand,

 

I hope you're doing well. Unfortunately, I don't think this will work. One of the last steps in PCB assembly is plating if it's not specified that the hole shouldn't be plated then I think it's still going to plate through.

 

Here's another idea. In the library put a single hole then at the north-south-east-west positions and at the device level make sure they all connect to the same pin. Do this on top and bottom. When you press fit the nut it will make contact with at a least one of those 4 pads. If you really want to guarantee the connection you can add more pads (6 or 8). This might be the easiest way to proceed.

 

Best Regards,

 



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 8 of 19
pstamand
in reply to: jorge_garcia2

ignore the trace widths,  I took another approach to separate the hole and place a large pad with a single pin in it...

 

pstamand_0-1670265615396.png

Is the hash in the VCC pin indicating a concern or normal...

 

Fusion wont let me put a wide trace into the pad and it goes beyond a tangent to the pin, which is understandable.  I can certainly add addition common pins to create more connection points if that's an option.

Message 9 of 19
jorge_garcia2
in reply to: pstamand

Hi @pstamand,

 

I hope you're doing well. I think this will work, the DRC is reporting violations but from a manufacturing standpoint this will work. If you want the bolt to be able to connect, make sure to expose the copper by covering the copper in tStop and bStop.

 

Let me know if there's anything else I can do for you.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 10 of 19
pstamand
in reply to: jorge_garcia2

Hi,

Wouldn't the tstop and bstop automatically and already be slightly large
than the footprint pad/ring that is the trace around the hole?
Message 11 of 19
pstamand
in reply to: pstamand

I've updated the custom component to have numerous pads connected to the same pin to help make routing easier.  Block I'm blocked when I try to connect to any even though the NET has the same name and is connected to the schematic to that net.

 

Yet the airwire wants to go to any of those pads and the pads all share the same pin.

pstamand_0-1670339591456.png

 

Message 12 of 19
pstamand
in reply to: pstamand

OK, larger pad that extends outside the round hole copper is reachable.  I dont like the protections that prevent from achieving a nice straight trace into this ring.

pstamand_0-1670342849842.png

 

Message 13 of 19
jorge_garcia2
in reply to: pstamand

If you want to make the connections easier, just switch to ignore violators mode. That way you can route however you want, that will allow it to route cleaner.

 

Let me know if there's anything else I can do for you.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 14 of 19
pstamand
in reply to: jorge_garcia2

ok, if I ignore the violators I get to the desired state.

 

pstamand_0-1670362959692.png

Then I can likely also shrink the footprint so its doesnt have to bump out in the pattern as well and have a clean copper ring and pads contained completely within the ring.

Message 15 of 19
pstamand
in reply to: jorge_garcia2

Hi Jorge,

 

Thank You!

 

This is the outcome I was looking to achieve.  surface copper around a not plated thru hole, copper pad encircling the hole, and a pad that could be connected to.  For conveience in the routing I've patterns 8 connection pads to the one pin.

Now I need to get all the dimensions correct so everything is the proper size for the hole and copper, and as Jorge comments earlier get the tstop and bstop proper so the copper as intended is exposed so I can solder the pressfit nut so there's a good electrical bond.

 

Now I need to get the

pstamand_0-1670363547419.png

 

Message 16 of 19
pstamand
in reply to: pstamand

I do think I'm close, I create a second component that has the same details without the hole.

 

I struggled to get the component to the other side, finally google provided use mirror to get the component to the other side of the board.

 

Last piece to work out is to get the top and bottom component at the same location on the board???

 

pstamand_0-1670514885572.pngpstamand_1-1670514906377.png

pstamand_2-1670514944943.pngpstamand_3-1670514967931.png

Jorge, you indicated I need to expose the copper, how do I ensure the big round pad has its copper exposed,  where to I ensure the tstop and bstop remove larger than the large trace around the hole?   The pressfit nut can then electrically connect, bottom side soldered and top side the bolt that completes the connection through the board from battery to the rest of the board from the bottom side BATT to the top side VCC powering the rest of the board.

Message 17 of 19
jorge_garcia2
in reply to: pstamand

Hi @pstamand,

 

You are super close now. What you do now, is within the library you draw both top and bottom in the same footprint. Now to expose the whole ring all you have to do is use the drawing tools and go over the copper ring. Any thing tStop and bStop touch is exposed copper. The easiest thing to do is to draw a filled circle using the CIRCLE command with a width of 0 on tStop (for the top) and bStop for the bottom.

 

All the pads on the top connect to one pin in the device and then the pads on the bottom connect to another pin that way in the schematic you can connect the top to one signal and then the bottom to another.

 

Let me know if you continue to run into problems.

 

Best Regards,



Jorge Garcia
​Product Support Specialist for Fusion 360 and EAGLE

Kudos are much appreciated if the information I have shared is helpful to you and/or others.

Did this resolve your issue? Please accept it "As a Solution" so others may benefit from it.
Message 18 of 19
pstamand
in reply to: jorge_garcia2

I do think I'm finally there!

top

pstamand_0-1670538562691.png

bottom

pstamand_0-1670538972951.png

schematic

pstamand_1-1670538579162.png

top trace

pstamand_2-1670538607019.png

bottom trace

pstamand_3-1670538626725.png

Thanks Jorge!

Message 19 of 19
bryanjkoop
in reply to: pstamand

Are you willing to share your completed component? I'm struggling to create a similar switch and am a complete beginner. PCBWay is struggling with my files, even though Fusion renders them as intended. 

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report