Understanding Power & GND - Part 2

Drawing Schematics, Hierarchical Design, BOM, Exporting net-lists, etc.
Post Reply
Message
Author
doug12745
Posts: 14
Joined: 10 Sep 2018, 17:24

Understanding Power & GND - Part 2

#1 Post by doug12745 » 01 May 2019, 12:29

Related to a post I made a few minutes ago, I am having difficulty understanding how to specify two voltage sources and to separate them.

In my project, I have a USB powered circuit. Power entering through the USB is +5V known as VBus. VBus is filtered through a ferrite bead and three capacitors the output being the system +5V Vcc. Right now the system voltage is showing up as VBus everywhere +5V is specified. I want to keep these separate as they are unfiltered and filtered voltages. Again I cannot locate where these voltages are specified. Both the settings of power sources and GND seem to be "hidden behind the scenes". Not so in layout programs such as Altium, Eagle, and even the simple ExpressPCB.

I've checked this forum for similar questions but found none. If this is written up somewhere please point me to the source.
Thanks in advance for any info and tips on this subject.

Tomg
Expert
Posts: 1345
Joined: 20 Jun 2015, 14:39

Re: Understanding Power & GND - Part 2

#2 Post by Tomg » 01 May 2019, 13:39

I don't know what your schematic looks like so I can only make a guess that your ferrite bead is not represented by an inductor-type component. Once your two nets are separated by the inductor, you will be able to give them different names. Just right-click on one of the nets and then left-click on the net name at the top of the pop-up menu to rename the net...
VBus.gif
Note: Same-name net ports will connect all nets together (see the "GND" net in the example above).
You do not have the required permissions to view the files attached to this post.
Tom

User avatar
KevinA
Posts: 373
Joined: 18 Dec 2015, 15:35

Re: Understanding Power & GND - Part 2

#3 Post by KevinA » 01 May 2019, 14:01

Add a USB connector or a power port like:
nets.jpg
You do not have the required permissions to view the files attached to this post.

doug12745
Posts: 14
Joined: 10 Sep 2018, 17:24

Re: Understanding Power & GND - Part 2

#4 Post by doug12745 » 01 May 2019, 16:17

TomG,

I tried your suggestion, however, the inductor I have placed evidently does not break the path into two separate nets. I named the power port before the inductor to "VBus" and then renamed the power port on the right to "VCC" (see below). Then I displayed the names of each net and they both show as "VCC". You said in your reply:
I can only make a guess that your ferrite bead is not represented by an inductor-type component. Once your two nets are separated by the inductor,
I guess I do not understand how the ferrite bead breaks the nets as you said. Maybe something is wrong with my schematic part for the ferrite bead. I did pull it from a Diptrace library, so would think that would be OK.

I also noted that I have placed C6 on the wrong side of the inductor. Will correct that by moving it onto the VBus segment before the inductor.
Capture.JPG
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1345
Joined: 20 Jun 2015, 14:39

Re: Understanding Power & GND - Part 2

#5 Post by Tomg » 01 May 2019, 16:42

It looks like you may have unintentionally merged the two nets. Once they are merged, they will stay merged even after being disconnected/separated from each other. The fact that DipTrace will not warn you of an impending net-merge in the schematic editor is an old "gotcha" that hasn't yet been resolved by the developers. In the meantime, make sure the two different nets are not physically connected to each other (no common wire or net ports with identical names), then...

1) Right-click on one of the two nets and select "Properties..." in the pop-up menu to bring up the Net Properties dialog window.
2) In the Net Properties dialog window disable (uncheck) the [ ]Connect Nets by Name option and click on the [OK] button. This should separate the two nets. You may have to rename at least one them to get the net names you are looking for because one of the nets will be automatically renamed with the next available default net name. Also, if there is a pre-existing net label being displayed for the automatically-renamed net, that label might not change to reflect the new net name so you'll have to delete the old/incorrect label and generate a new label.
3) Right-click on one of the affected nets and select "Properties..." in the pop-up menu to bring up the Net Properties dialog window.
4) In the Net Properties dialog window re-enable (check) the [x]Connect Nets by Name option and click on the [OK] button.
5) Repeat steps 3 and 4 above for the other affected net. The two nets should remain separated.

p.s. Don't forget to resave the schematic and use the Renew Layout from Schematic tool with its "By Components..." option in the PCB editor.
Tom

doug12745
Posts: 14
Joined: 10 Sep 2018, 17:24

Re: Understanding Power & GND - Part 2

#6 Post by doug12745 » 02 May 2019, 18:11

Finally got it, Tom. Thanks for your detailed 5-steps above. It was a strange situation. Prior to your last response, I removed inductor L1 completely leaving that circuit section open. The nets on both sides continued to change together even with L1 missing. I then decided to delete the wiring surrounding VBus (VBus power point, wire to pin 1 L1, wire to C6 pin 1, and J2 pin 1). I then rewired L1, C6, and J2. Last I placed a power point and named it VBuss just in case and wired that in.

Applying your net naming examples from above VBuss and VCC now remained separate as we expected. I never did find what caused this but rewiring the VBus portion must have deleted the culprit attached to that wire and nets. Thanks again, Tom.

VBus.JPG
TomG,
You do not have the required permissions to view the files attached to this post.

Post Reply