Username:
Password:
Save Password
Forgot your Password?

 All Forums
 Help For Easy-PC Users
 PCB Layout
 Copper pour workflow - 2 layer board
Author Previous Topic Topic Next Topic  

DB17

25 Posts

Posted - 23 Aug 2018 :  14:51:52  Show Profile  Reply with Quote
Hi. I used EasyPC (for DOS!) back in the 90s and now returning to it after a long break. I am currently trying to get to grips with Easy-PC 1000 version 21.0.5

For my current work, I would like lay out a p.c.b. without creating a .sch schematic first. (That is, my schematic is on paper and I want to go straight to .pcb file design.)

My p.c.b. has a top layer and bottom layer only. 95% of the tracks will be on the top layer. When I've finished organising components on the top layer and connecting them with tracks, I wish to pour copper on the bottom layer to create a GND plane.

Some of the component pads will be connected to GND. How can I identify which component GND pads are not to be avoided when I carry out a copper pour? Is there a workflow method I can apply to carry out my .pcb file creation efficiently?

Users Guide V21.0 has a section on copper pouring (pp218-224) but I can't pick a bit that can answers the above question.

Thank you!

Iain Wilkie

United Kingdom
897 Posts

Posted - 23 Aug 2018 :  15:03:34  Show Profile  Visit Iain Wilkie's Homepage  Reply with Quote
Your GND pads will be on presumably a named net ... eg GND .... the copper pour will ask what net you wish the pour to be ... obviously you give it the same net name "GND" then all GND nets will be connected in the pour, all others (different nets) will be avoided.

Iain
Go to Top of Page

DB17

25 Posts

Posted - 23 Aug 2018 :  15:51:34  Show Profile  Reply with Quote
Thanks for your quick reply, Ian.

So the net name is something I can set for each pad in the .pcb file? I assumed that it would be set only if you did a .sch file first.

I will give it a try and come back if there's a problem. Thanks again.
Go to Top of Page

Iain Wilkie

United Kingdom
897 Posts

Posted - 23 Aug 2018 :  15:56:48  Show Profile  Visit Iain Wilkie's Homepage  Reply with Quote
Nets will be autonamed as you add your connections. You can then edit these names if you need to i.e. in this case

Iain
Go to Top of Page

DB17

25 Posts

Posted - 23 Aug 2018 :  16:08:59  Show Profile  Reply with Quote
OK. Just to clarify, the GND pads won't be connected to anything on the top layer. By the time I've finished laying out the top layer, all pads will be connected apart from the GND pads (because they will be connected by the copper pour on the bottom layer). How will a net name be assigned to the unconnected GND pads when the top layer is complete?

I must be missing something simple, so thanks for your patience.
Go to Top of Page

edrees

United Kingdom
575 Posts

Posted - 23 Aug 2018 :  16:23:45  Show Profile  Visit edrees's Homepage  Reply with Quote
Use the "Add Unrouted Connection" tool (3rd down from top) to join up all the dots (pads) that you want to connect to 0V. It will elastic band them together for you. It will automatically give this a net name like N0000xyz. Then rename this net to GND. Then pour GND either with/without thermal spokes (set in Design Tech).
Go to Top of Page

DB17

25 Posts

Posted - 23 Aug 2018 :  17:05:42  Show Profile  Reply with Quote
Thanks for your explanation - much appreciated.
Go to Top of Page

DB17

25 Posts

Posted - 31 Aug 2018 :  16:49:31  Show Profile  Reply with Quote
quote:
Originally posted by edrees

Use the "Add Unrouted Connection" tool (3rd down from top) to join up all the dots (pads) that you want to connect to 0V. It will elastic band them together for you. It will automatically give this a net name like N0000xyz. Then rename this net to GND. Then pour GND either with/without thermal spokes (set in Design Tech).



I've actually joined all the GND pads with a track on the bottom (ground plane) side. I'm hoping this works just as well as "add unrouted connection"? It seems to. Or should I remove the GND track and replace it with unrouted connection?

I'm getting to grips with 'copper pour', which has an intuitive interface and good user manual section. Two questions:
(a) When I drew a 'test' copper pour rectangle on the top side, the copper only poured into the bit of the rectangle that had a GND pad. Should I put GND vias in the unpoured areas first (I guess that the software doesn't want to create floating islands)?
(b) On one of my trial pours, the software reported an error that less than minimum number of spokes on two pads were present and so the pour could not proceed. I adjusted the pour shape a bit and the error disappeared. I can't reproduce the error now. Was it because my pour area bisected a GND pad perhaps?
Go to Top of Page

DB17

25 Posts

Posted - 31 Aug 2018 :  17:00:09  Show Profile  Reply with Quote
quote:
Originally posted by DB17

quote:
Originally posted by edrees

Use the "Add Unrouted Connection" tool (3rd down from top) to join up all the dots (pads) that you want to connect to 0V. It will elastic band them together for you. It will automatically give this a net name like N0000xyz. Then rename this net to GND. Then pour GND either with/without thermal spokes (set in Design Tech).



I've actually joined all the GND pads with a track on the bottom (ground plane) side. I'm hoping this works just as well as "add unrouted connection"? It seems to. Or should I remove the GND track and replace it with unrouted connection?



Ah. My GND tracks appear as "large spokes". It will function correctly but doesn't look great.

However, some of the GND tracks do need a solid track connection as the carry relatively high currents.
Go to Top of Page

edrees

United Kingdom
575 Posts

Posted - 31 Aug 2018 :  17:09:00  Show Profile  Visit edrees's Homepage  Reply with Quote
1) This does the same add joining up all the dots with the "Add Unrouted Connection" tool. Its has auto named the net something other than GND, so you should re-name it.

2a)You were asked to specify a net name for the pour, so if you answered GND and there wasn't a pad connected to GND within your copper pour area it can't pour it. (Unless you allowed "Isolated Islands" in the Pour Copper dialogue).

2b)The physical spoke size is set up in the Design Tech=> Rules dialogue. You've defined a spoke size such that can't fit (all 4) in the space available on your design.

quote:
Ah. My GND tracks appear as "large spokes". It will function correctly but doesn't look great.

However, some of the GND tracks do need a solid track connection as the carry relatively high currents.

If you still want thermal spokes for the other tracks then make exceptions for the GND pads( Properties =>Plane Connection) used in conjunction with Design Tech=>Rules=>Powerplanes






Edited by - edrees on 31 Aug 2018 17:46:10
Go to Top of Page
  Previous Topic Topic Next Topic  
Jump To: