Back on the pcb saddle again

Making PCB Layouts, Manual routing, Auto-routing, Copper pouring, Updating from Schematic, Manufacturing Output
Post Reply
Message
Author
carlmart
Posts: 43
Joined: 22 Jan 2015, 07:11

Back on the pcb saddle again

#1 Post by carlmart » 07 Apr 2020, 08:48

It's been close to five years since I designed my last pcb with DipTrace, and my 72 years old age does not make it better to remind how I did things back then

I do know that I went through the tutorial from beginning to end, designed many components not on the library and mastered all things to make a pro design.

Now I'm back on the saddle with some simpler projects, mostly discrete, nothing digital, little or no SMD parts.

Due to the present situation, it's quite likely I will have to build the prototypes myself, so I will quite likely work on a single side of the pcb, with as few as possible wires on the component side, for those situations that can be avoided.

As some of the designs are old and from a time where the industry also built things single sided, thing shouldn't be particularly difficult.

So let's go to the first two questions:

1) How do you split a trace at a specific point? I didn't find an option like "break trace" as I had used on other pcb programs.

2) How do I convert a part I designed, based on an library part transistor, into an active part that I can add to my personal parts library?

3) Is there a way to know which transistors have which pin assignment, even if they name is different, so I can use on my design? How? Going one by one?

Let's hope there's someone around that is finding therapeutic to be active on forums like this. But it seems few or no people is coming around.

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: Back on the pcb saddle again

#2 Post by Tomg » 07 Apr 2020, 13:26

1) How do you split a trace at a specific point? I didn't find an option like "break trace" as I had used on other pcb programs.
If you want to delete a portion of a trace move your mouse cursor over it at the desired point, add a node by pressing hotkey "n", right click on the side of the trace you want to delete and select "Unroute Segment" in the pop-up menu. If there are any segments of the unwanted portion of the trace that remain, right-click on one of them and select "Unroute Trace" in the pop-up menu. This method does not eliminate the net connection.
2) How do I convert a part I designed, based on an library part transistor, into an active part that I can add to my personal parts library?
Pattern or component? Do you want to copy it from the standard DipTrace libraries into your custom library?
3) Is there a way to know which transistors have which pin assignment, even if they name is different, so I can use on my design? How? Going one by one?
Are you referring to accessing datasheets, hovering the mouse cursor over a pin and reading the pop-up hint or using the Pin Manager?
Tom

carlmart
Posts: 43
Joined: 22 Jan 2015, 07:11

Re: Back on the pcb saddle again

#3 Post by carlmart » 08 Apr 2020, 06:41

Thanks, Tomg.

OK, I have tried the add node method and it seems to work. How do I eliminate the remaining net connection now? Can I mark two nodes and delete the part between them? Or how is that done?

I'm not sure if it's pattern or component, I think it's the latter, but I do not think it matters, does it? What I did was to take a 2N listed transistor, probably a 2N2222, and use it on my schematic design, not caring whether it was NPN or PNP, as the KSA and KSC parts I needed were not there. So on the pcb design I took that 2N part and designed a new one, assigning b, c and e to the right pins, corresponding to the KSC and KSA assignment.

Now I wonder how do I do to convert those into real parts that I can add to my library. I completely forgot how it was done.

It would be much easier if there was a way to identify the library parts, in the case of the transistors, by pin assignment. Instead of going one by one and looking into each transistor to identify the ones that have the same pin assignment as the new unlisted parts, I'm using. At least I would just have to change the part name.

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: Back on the pcb saddle again

#4 Post by Tomg » 08 Apr 2020, 09:47

How do I eliminate the remaining net connection now?
After separating the two sides of the trace, right-click on the destination pad to which the unwanted portion is/was connected and select "Delete from Net" in the pop-up menu. The destination pad will be disconnected from the net and any remnants of the unwanted portion of the trace will also be deleted. The other side of the trace should remain in place and still be assigned to the net.
Can I mark two nodes and delete the part between them?
Yes. Right-click on the newly-formed segment and select "Unroute Segment" in the pop-up menu.
I'm not sure if it's pattern or component, I think it's the latter, but I do not think it matters, does it?
In DipTrace a component is made up of a pattern with pads (created using the Pattern Editor) attached to a schematic symbol with pins (created using the Component Editor). You must approach component creation in the manner outlined in the DipTrace tutorial. Try watching all of the DipTrace videos and going through the DipTrace tutorial to help refresh your memory.
What I did was to take a 2N listed transistor, probably a 2N2222, and use it on my schematic design, not caring whether it was NPN or PNP, as the KSA and KSC parts I needed were not there. So on the pcb design I took that 2N part and designed a new one, assigning b, c and e to the right pins, corresponding to the KSC and KSA assignment.
If you used the "Group into Component" option on the PCB, the pattern can be saved to a custom library. Before doing so, give the component the desired name and then...
1) If an editor other than the PCB Layout editor is open with the destination library currently selected/highlighted, either temporarily select/highlight a different library in it or close that editor.
2) Open the PCB and select User Patterns in the Current Library Group panel on the left side of the screen.
3) In the libraries list located just below the Current Library Group selection box, select a destination library.
4) In the Design Area first select/highlight the component pattern you wish to copy, then right-click on it, select Save to Library in the pop-up menu and choose Add to "[destination library's name]" in the fly-out menu.
5) In the Confirm dialog window, click on the [Yes] button. A copy of the pattern of the selected/highlighted component should now be displayed at the bottom of the destination library's patterns list.

The new pattern that was just added to the pattern library should be sporting the name you gave it when you created it in the PCB Layout editor. Make sure the reference designator has only the prefix without the appended number (e.g. "Q" instead of "Q23"). Resave the pattern library after making any changes.
Tom

carlmart
Posts: 43
Joined: 22 Jan 2015, 07:11

Re: Back on the pcb saddle again

#5 Post by carlmart » 08 Apr 2020, 11:48

I can't seem to be able to disconnect the net without eliminating the threads.

What am I doing wrong?
You do not have the required permissions to view the files attached to this post.

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: Back on the pcb saddle again

#6 Post by Tomg » 08 Apr 2020, 12:23

You need to split the trace first.
Tom

carlmart
Posts: 43
Joined: 22 Jan 2015, 07:11

Re: Back on the pcb saddle again

#7 Post by carlmart » 08 Apr 2020, 15:22

Which trace, the thick one or the thin one? Just adding a node over it?

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: Back on the pcb saddle again

#8 Post by Tomg » 08 Apr 2020, 15:43

There's a thin one? If by "thin one" you are trying to indicate a ratline (thin blue line) then you should realize that a ratline is not a trace. What is your goal? Do you wish to completely delete a trace without deleting the net connection (indicated by a ratline), or do you want to delete the net connection, too?
Last edited by Tomg on 08 Apr 2020, 16:03, edited 2 times in total.
Tom

carlmart
Posts: 43
Joined: 22 Jan 2015, 07:11

Re: Back on the pcb saddle again

#9 Post by carlmart » 08 Apr 2020, 16:01

No, sorry for the confusion. What I'm trying to eliminate is the ratline. The thread only when necessary,

Tomg
Expert
Posts: 1523
Joined: 20 Jun 2015, 14:39

Re: Back on the pcb saddle again

#10 Post by Tomg » 08 Apr 2020, 16:03

Assuming you want to remove the net connection between the two pads of C502, and everything is still in the state shown in your screen shot...
1) Right-click on C502 (not its pads) and select "Disconnect Traces" in the pop-up menu.
2) Right-click on one of the pads of C502 and select "Delete from Net" in the pop-up menu.
3) Right-click on C502 (not its pads) and select "Connect Traces" in the pop-up menu.
Tom

Post Reply