Author Message
 Post subject: 3.101 drops connection on PCB
PostPosted: 09 Jul 2017, 02:16 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 167
I drew up a schematic :
Image
But when I use this schematic to create PCB C1 is left floating and C2 connects to D1.
If I delete the +5 buss and add a +5 to each cap I get the same results.


You do not have the required permissions to view the files attached to this post.


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 09 Jul 2017, 08:28 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 946
Looks fine to me. Hover your mouse over D1(1) and watch all same-Net connections highlight. If it will make you feel any better press softkey [F12] to optimize the ratlines. Do you see a specific connection in the schematic (component/pin number to component/pin number) that isn't showing up on the PCB?

p.s. There are component differences between the schematic and the PCB.


You do not have the required permissions to view the files attached to this post.

_________________
Tom


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 10 Jul 2017, 12:27 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 167
I changed the layout to two sided with the connectors and Caps on the bottom BUT: (This is a 1 part test since the whole project blew up)
Image
I can not figure out the DRC errors, GAP? I looked in help, no help.
Basicly I want the smallest board with the ability to stack boards side by side. Moving the connectors was easy since they are Thru Hole devices but the cap turned into a nightmare. I did learn how to stop the pour from making connections enabling me to have the power go from input to cap to the ws2812b since I could not figure out what good the cap would be if it and the ws2812b were both connected to the power plane.

Top Side
Image
Bottom Side
Image

From the 3D it appears to work.
One other observation: The Objects/Update All Copper Pours has to be manually applied at times and other times it happens when you change something that affects it, very confusing since I didn't realize a manual Objects/Update All Copper Pours was required, sometimes.


You do not have the required permissions to view the files attached to this post.


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 10 Jul 2017, 19:55 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 946
Both the bottom copper pour and the Static Via on C1(2) need to be connected to Net 1. This is why the DRC is complaining about these "unrelated" objects colliding. Perhaps a better way would be to...
1) Delete both the Static Via on C1(2) and the top side trace/via between D1(1) and C1(1).
2) Route a new trace between D1(1) and J1(2) on the top side.
3) Connect the bottom pour to Net 1.
4) Update all copper pours.

When you edit a copper pour and the Current State: drop-down list is set to "Poured", it will automatically update only that pour after clicking on the [OK] button. Any changes made to other objects residing within a copper pour will not automatically update that particular pour. If you haven't already, assign a hotkey for updating all copper pours to make things a little easier.

_________________
Tom


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 10 Jul 2017, 21:09 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 167
Now I'm confused
Schematic:Image
Top: Image
Bottom: Image
The top pour is attached to the GND and the bottom pour is +5
The I assigned the left via to GND net so that the via is attached to the top layer (pour) and Pad 3 of D1 is attached to to the top layer, GND, the connector Pin 3 is attached to the top layer, GND. The The top view in PCB editor shows the left via attached to the top layer, pin 3 of D1 attached to GND and Pin 3 of the connector attached to GND but I still see a ratline between the left Via and pin 3 of D1. The Bottom view shows Pin 2 of the connector connected to pin C1 pin 1, C1 pad has a Via (right Via) that is connected to the C1, pin 1 pad. On the Top view C1 pin 1 Via (right Via) has a trace to D1 pin1 VDD (+5) and that Via works without errors. The Via on the right can not be selected on the top layer of bottom, at least I haven't found a means to select it. I noticed the bottom layer was not attached to a net so I attached to to +5 and C1 pin 1 and the connector pin 3 grew thermal reliefs. Running DRC shows no Error but the Ratline will not go away.
Image
and a bottom view:
Image


The hotkey, that clue was/is priceless! :D


You do not have the required permissions to view the files attached to this post.


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 11 Jul 2017, 05:34 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 946
I don't know why that last ratline is still there. Press soft key [F12] (optimize ratlines) to get rid of it. The via on C1(1) is a Trace Via (it is considered to be part of the trace), not a Static Via, and that is why you cannot select it. Deleting a trace will delete all of its Trace Vias. If you should ever want to convert that Trace Via into a Static Via then go to the Top layer, activate the Edit Traces tool, right-click on the Trace Via and select Convert Via to Static in the pop-up menu.

p.s. Another handy hotkey is the [Home] key, which is tied to the Zoom Extents tool by default.

p.p.s. I just found out that the ratline exists because there is no trace connecting the Static Via to the pad. Temporarily move the Static Via off the pad and you will see a hidden ratline. Route a trace between the moved Static Via and the pad (on the bottom layer) and then move the Static Via back to its original location.

_________________
Tom


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 11 Jul 2017, 13:06 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 167
Full board with Ground planes on top and bottom, hand routed, learned how to get the via to connect correctly :shock: and also learned the Auto-Router can't read my mind.
ImageImageImageImage

Now to find out if it will work; OSHPark $5 and yes I do feel guilty sending a sub-square inch PCB to be built but my wallet likes it. FYI: WS2812B $0.10 each now
I did find out the almost all editors zoom extent on the Home key but the Schematic Editor was set to E and the F12 cleared the ratline ... Thanks Tomg


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 11 Jul 2017, 13:39 
Offline
Expert

Joined: 20 Jun 2015, 14:39
Posts: 946
Read the "p.p.s." in my previous post about the ratline being caused by a missing trace. Don't worry, this probably won't affect the functionality of your manufactured PCB.

_________________
Tom


Top
 Profile  
 
 Post subject: Re: 3.101 drops connection on PCB
PostPosted: 11 Jul 2017, 14:41 
Offline

Joined: 18 Dec 2015, 15:35
Posts: 167
Tomg wrote:
Read the "p.p.s." in my previous post about the ratline being caused by a missing trace. Don't worry, this probably won't affect the functionality of your manufactured PCB.

The new layout was from scratch since I could not get the previous layout to 'un-pour'. Every time I selected Unpoured from the Current State: nothing changed, it remained 'Poured'.
FYI: That PCB cost $3.40 and I was feeling so guilty I ordered the 5 day special, $7.40, more guilt


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 9 posts ] 

All times are UTC - 5 hours [ DST ]


Who is online

Users browsing this forum: No registered users and 2 guests


You cannot post new topics in this forum
You cannot reply to topics in this forum
You cannot edit your posts in this forum
You cannot delete your posts in this forum
You cannot post attachments in this forum

Search for:
Jump to:  
Powered by phpBB © 2000, 2002, 2005, 2007 phpBB Group