Author Message
 Post subject: different width traces from same net (or divide a net in 2)
PostPosted: 06 Apr 2015, 03:25 
Offline

Joined: 06 Apr 2015, 03:09
Posts: 2
I did couple of searches but i could not find anything,

i have a T kind of connection in Schematics that goes to 3 pins. pin1 and 2 are the power rail and require a pretty thick trace , pin 3 is just a sense trace and should be a normal trace.
the problem is that this is seen as 1 net connecting 3 pins and i cannot set 2 different thicknesses (via net class, i'm looking for something like net class per line or per segment)

this is even a bigger problem with the ground only 1 ground trace must be really thick the rest must have normal thickness, but if i associate the net class with 1 gnd line it associates it with all of them

is there any way in schematics to configure 2 different trace widths on such a T connection like in the picture ?

also it will be possible to associate with a net class a color or even a line width ?


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


Top
 Profile  
 
 Post subject: Re: different width traces from same net (or divide a net in
PostPosted: 07 Apr 2015, 03:08 
Offline
Expert

Joined: 20 Jan 2012, 10:50
Posts: 116
I believe, unfortunately, the short answer is no, not with separate classes but...

After you have placed the traces you can right click on a trace and select Trace Width to change the width of the entire trace. Or if you just want to change a portion of the trace you can select Segment width. This is, of course, an edit after you have placed the trace with the current class width.

And of course, you will need to do this in the PCB editor not the Schematic editor

If I understand you correctly, what you are asking is definitely a valid request and I've tried to raise awareness of this issue. You can't predefine these differing trace widths and clearances and that is a problem. It's one of those things that don't seem to be a big issue until you run headlong into it. The action that you desire is just another example of the need to have the ability to route different segments of the same net with different attributes. If you try to run separate traces using separate nets and then connect them they will loose their unique attributes when they combine and you will end up with one net. You will likely run into this issue if you are doing mixed signal or audio layouts that require star grounding and power connections. I've seen situations that have as many as 5 different ground paths in one small section of a high gain preamp.

Unfortunately, maintaining multiple separate power and ground paths attributes in Diptrace is not supported and I really don't think most users fully understand the scope of the issue until they are faced with it and then have to try to figure out a way around it. Hopefully, with enough encouragement from users this will change.


Top
 Profile  
 
 Post subject: Re: different width traces from same net (or divide a net in
PostPosted: 08 Apr 2015, 01:23 
Offline

Joined: 06 Apr 2015, 03:09
Posts: 2
thanks very much you explained the problem better than me.

this is what i did i adjusted the width per segment manually later in PCB Layout,
clear example 4 pin resistor (like WSK25125L000FEA)

there are 2 thick traces for the main flow path and 2 thin sensing traces.
and besides the extra clicks needed is also the fact that when you draw those traces that should be thin but are very thick, they are drowed initialy thick and is very hard to place them corectly and start steeping all over other things, anyway is a mess.

ability to configure a net segment thickness in schematics will be very nice.


Top
 Profile  
 
 Post subject: Re: different width traces from same net (or divide a net in
PostPosted: 08 Apr 2015, 03:41 
Offline
Technical Support

Joined: 14 Jun 2010, 06:43
Posts: 2762
At the moment, it is not possible to define in Schematic different width for different traces of the same net. User should keep it in mind and create traces with different widths in PCB Layout.


Top
 Profile  
 
 Post subject: Re: different width traces from same net (or divide a net in
PostPosted: 30 Jul 2015, 11:34 
Offline

Joined: 29 Jul 2015, 22:47
Posts: 2
This has been a BIG problem for me on every design I've done in the past. It is very frustrating to have to spend time re-assigning trace widths to lots of segments of traces because there seems to be no way of defining it up front in the schematic. It means that the schematic design and PCB are not compliant, and it wastes a lot of time. A simple update from schematic at a revision stage of the pcb can mean going through the whole process again.

The best solution I have come up with is still not a perfect way around it, but it does work.....

I have done this in the schematic by creating a two pin component that looks like a link.
In the component definition (I called "TraceLink"), I placed two pins that look like they are connected. You can do this by making the pins touch or by adding a shape between them (could be a shape line). I also used a reference name that makes it easily identifiable when you layout pcb.
Place it in the schematic between the place where you will need the two different net classes and connect them. (Hide pin numbers, ref name etc. unless you want to see them in the schematic).
Now you have two nets apparently directly connected in the schematic.
Design a pattern attached to the TraceLink component that has two small SMT pads partially overlapping each other - So they are shorted. Using this, it is easy to connect the two nets by connecting each net to its own pattern pad. Do not place the pads on top of one another.
DRAWBACKS: The only drawbacks are with auto-routing and verification.
1. The auto-router will not route to the pattern because the DRC rule for clearance is violated by the two pads in the pattern being connected together, so it has to be manually routed. I usually manually route in any case.
2. The DRC will always fail because of the pad clearance violation -- GRRRR. It's easy however, to see and live with.
This gets me net class compliance between schematic and the PCB design.

Maybe DipTrace could include this kind of approach and automatically ignored DRC checks for it? - I would love it.


Top
 Profile  
 
 Post subject: Re: different width traces from same net (or divide a net in
PostPosted: 30 Jul 2015, 12:08 
Offline

Joined: 29 Jul 2015, 22:47
Posts: 2
I forgot to post an image of how my schematic part looks in the schematic when it (apparently) splits nets.
Here it is selected with the nets colored differently.
I also added a pic of the split net part on the pcb with all the annoying DRC errors that result. It's shown attached to the trace, but I often bury it inside the larger trace. This is the biggest problem with the approach - It's not elegant.
If anyone has any suggestions, I'd love to hear them.


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


Top
 Profile  
 
Display posts from previous:  Sort by  
Post new topic Reply to topic  [ 6 posts ] 

All times are UTC - 5 hours [ DST ]


Who is online

Users browsing this forum: Google [Bot] 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