Diptrace Best Practices?

slacjs

Member
I'm trying to get into diptrace and I'm wondering about best practices for routing. I'm starting off by trying to make a test board. I've laid out my components. I did my ratlines next.
  • How bad is using the auto tracer? I tried it and it seemed fine but to be honest, I'm not sure what is good practice.
  • Ground. I was just using normal routes though I know some people use the rest of the PCB (ground plane?) to act as a ground. Would it be an issue if I just used normal routes?
  • What size should routes be? Can they be too small? Is default okay?
I've attached it if it's of any use. Thanks for any help.
 

Attachments

  • testboard.zip
    10.6 KB · Views: 8

Big Monk

Well-known member
I'm trying to get into diptrace and I'm wondering about best practices for routing. I'm starting off by trying to make a test board. I've laid out my components. I did my ratlines next.
  • How bad is using the auto tracer? I tried it and it seemed fine but to be honest, I'm not sure what is good practice.
  • Ground. I was just using normal routes though I know some people use the rest of the PCB (ground plane?) to act as a ground. Would it be an issue if I just used normal routes?
  • What size should routes be? Can they be too small? Is default okay?
I've attached it if it's of any use. Thanks for any help.

I hand route the whole board. I know that makes me a bit of a luddite but I'm only doing one sided boards. I fou8nd the auto-tracer odd and cumbersome.

I use a ground normal ground trace.

Here is a shot of my latest revision to my Universal Fuzz board done in DipTrace:

Capture.PNG
 

phi1

Well-known member
In my opinion, best practice is to draw the schematic first, and then import to a pcb design. That way all the ratlines are connected automatically. It’s way easier for me to check that the schematic is correct than checking all the rat lines. Of course drawing the schem takes time, but that’s my preference.

on the flip side if you draw the ratlines, you’re probably more aware of layout placing of components for easy tracing. When I layout components I’m always looking at the ratlines to make it as sensible as possible.



i use auto router, it seems to work fine for me. I study the result to look for funky traces, lots of vias, high traffic areas, etc, and adjust the component placement to improve and re-run the auto router looks reasonable.
 

benny_profane

Well-known member
been trying to figure it out too. At first I thought it was eliminating right angles in traces but some of the red lines are right angles as well
Right angles aren’t as big a deal with low-speed signaling with audio, but eliminating inefficiencies is generally best practice. Most of the above edits remove serpentine paths and make shorter connections. Since excesses can potentially introduce parasitic capacitance or points of noise ingress, it’s a good idea to make things short if possible. Also, it looks neater.
 

temol

Well-known member
Some of the red lines to make tracks shorter. Other to make the desing neater (in my opinion). And also to avoid things like below (why not route track through the solder pad?)

1631859946072.png

I know that short tracks, right angles, and so on, are mainly issues with high-speed designs but whty not to incorporate good practices into a pedal stuff?
 

Big Monk

Well-known member
Some of the red lines to make tracks shorter. Other to make the desing neater (in my opinion). And also to avoid things like below (why not route track through the solder pad?)

View attachment 16111

I know that short tracks, right angles, and so on, are mainly issues with high-speed designs but whty not to incorporate good practices into a pedal stuff?

I hear you. I have to put an order in sometime soon for more of these and I’ll take some of your edits into consideration.

Some of it is simply down to component size. For instance in the picture from your quote of me, the bottom red circle trace goes to the interstage coupling cap. Moving it over the trace would mean I’d have to expose the leads of the cap. That wouldn’t look good visually when the cap was installed. The 2 small pads you circled are collector test points for Q1 and Q2. Per your suggestions, the Q2 test point could be moved over the trace to the trim pot but the Q1 test point pad can’t, as it would likely be too close to the Q1 trimpot.
 

Grubb

Well-known member
Not sure if these are best practice, but my workflow is something like this:

1. Draw the schematic.

2. Draw a board template. I find it easier to do this with a rectangle, in case i want to alter the dimensions of the board easily during the layout process. Then I place the proper board over it at the end.

2. Place the template so that the origin is in the centre, which helps me line things up perfectly with my Illustrator designs.

3. Lay out hardware that must correspond to an external drill hole or component (e.g. pots, switches, DC input, 3PDT breakout pads etc). I always specify an exact location for these rather than dragging or using the dimension tool, which I find inaccurate and messy. I also place things like ICs centrally and evenly spaced from each other too. Pads for 3PDT, DC and jack ground are on 2.54 mm centre spacing so that screw terminal blocks can be used if desired.

4. Go through the schematic and firstly complete the LED path and the power paths. Some people use thicker traces here (0.33 mm) for heat dissipation on the power path and thinner ones (0.2 mm) for the audio paths.

5. I then highlight each net, lay the compnents from it out on the board and add the traces. I dont care much about the schematic or ratlines at this stage, just the nets. I ignore the ground net, as I use copper pours as ground planes. I usually get better results if I do traces as I lay out the components, although there is still a lot of stuffing around re-working traces if you do it that way. I used to do layout and tracing as distinct steps but I found it worked less well and I have a bunch of aborted layouts from that time. I always hand-route, although i will sometimes run the autotracer to get ideas about tricky parts. I try and route horizontal traces on the top layer and vertical traces on the back and connect these by vias if necessary for tricky sections (I think I read it's called Manhattan routing?)

6. When I'm laying out components I try to take many leaves from our good proprietor's book and attempt to put runs of resistors in an inner column along either side of the ICs with caps in outer columns, at least where possible. I aim for some degree of symmetry where possible but do not possess Mr. PCB's grandmaster skills. I use DipTrace's alignment and spacing options a lot to get things nice and balanced in each column.

7. After layout and routing, when I'm happpy where everything is, I rotate or move the component labels for the silkscreen.

8. Set up copper pours on top and bottom and connect to ground plane (although sometimes I'll have a power plane on top if I have multiple positive voltages)

9. Place board outlines leaving the required space around the edge of the copper pour. Add vector artwork labels. Remove the board template shape.

10. Important! Check 3D rendering! I have caught so many mistskes by checking the 3D model of the PCB.

Would love to hear any tips others have. Here are 3 boards I've made recently for a custom bass effect I'm building for a work colleague (resonant lowpass filter, fuzz and boost).
 

Attachments

  • 20210918_020430.jpg
    20210918_020430.jpg
    219.7 KB · Views: 24
Top