Breadboard layout to a PCB - a DSPCB approach

Note: to complete this design process, you will need DesignSpark PCB with a Creator or Engineer subscription.

Introduction to the concept.

A common design development route is to sketch a design and test using a breadboard/prototyping board such as this popular product from RS (287-9142) .

Once you have produced and tested your breadboard design, how can you proceed to produce a PCB layout?

The original schematic sketch is often out of date as you made your changes on the breadboard, so the breadboard is often photographed for a record such as this image from the Flood Alert project published by Hey Jude.

For documentation purposes, Jude Pullen translated this into a Fritzing layout as shown, which is visually clearer than the photograph, but this still requires converting into a schematic to reliably produce a PCB within DSPCB.

Producing a breadboard layout in DSPCB.

Why not perform the documentation process as a schematic in DSPCB?

As an example, this is the left part of the above image:

The above schematic is produced with the standard features in DSPCB Creator and Engineer V13.

Initially, you may have automatically considered the schematic design as only conventional schematic symbols. Well, what if you create the schematic symbols to look similar to the component and foot print?

Hmmm, well, we all love or hate the automated schematic symbols that look like blocks, so let’s expand on these and make our schematic symbols look like the actual component!

Here are four example components created as concept models to test the idea.

a Blue LED, b Vertically mounted resistor, c RPi2040 Zero and d Sounder/mic.

These can obviously be edited as required for the visual representation, but for this test these will be used.

Note: All the schematic symbol connections/pads are on a 100thou pitch to match the breadboard.

Creating the breadboard schematic symbol.

But how to handle the breadboard itself? Well, this was created initially as a ‘schematic only’ library symbol representing the breadboard as groups of the same net pads. 
It is required to be schematic only, as it will not form part of your PCB design as a component. It actually just represents an array of nets providing an interconnection between the component pads/pins on the schematic design.

Although nets can be assigned to the symbol pads in the pin mapping, this was not found suitable for the final task. The approach taken was to add this schematic symbol to the schematic design sheet, and then add all the net connections as required between the pads. 
A time-consuming process, but attached is the schematic design (which you will always need as the starting point), to allow you to evaluate the process. 
Make copies of this design for future use, or download again when required.

NOTE. If there is sufficient user interest, we shall discuss with our developers improvements to the tools and features for this process. We have already requestedthe  component colour fill to be individually selected by component rather than the current global fill option.

This is how the schematic design represents the breadboard.

Adding components.

We now have our schematic design with the breadboard and can add our components as required.

A key feature provided in the Creator and Engineer subscriptions that is required to be enabled, is in Settings – Preferences – Schematic Interactions, this is “Weld on Drop”.

This provides the automatic connection between the component pads and the breadboard nets as the component is placed.

Here is the process in action for a few components (it may take some time to load the GIF below):

An important note is that every symbol is created on a 100thou pitch, and the symbol position is defined at the centre of a pad, this makes positioning easy with a 100thou snap to grid setting.

NOTE.  Should you place the component in the wrong position, DO NOT move it to the required position! “Weld on Drop” may have connected the symbol to the nets, and these will be dragged with the component. Simply delete the component and add it again.

We now have a simple example with some components placed on our breadboard.

Adding wires.

Next to consider, is how to add wires?

The wires will be standard net connections, however, we can change their style and colour to be visually appealing and representative of the real situation.

To simulate a wire, we select the segment mode as ‘Free’ and set the snap to grid at one quarter or finer. It is important to note that nets crossing each other will not become connected. Any potentially connected point will be identified by a red dot.

At this point, we have moved to the real example of the Flood Alert project as we wish to show a realistic layout.

Here we show the representation in DSPCB with the wiring to the ‘off board’ display and serial communications connector. As well as illustrating the wires it also shows that you can easily have ‘off board’ components.

The DSPCB implementation has all the normal schematic editor features available, so you can add text, select and highlight nets using the Goto bar, making for an interactive experience.

A summary of the steps to place a wire and set the colour are:

1. Select “Add Net” from the toolbar and set a Style, say 15 or 20 thou.
2. Set the Segment Mode to “Free”.
3. Set the Snap to Grid at a “Quarter Grid” or finer, to allow for routing the wires between the breadboard pins.
4. Click the starting pad and route the ‘wire’ across the breadboard, clicking to position as you route to the destination pad and click on the destination pad to complete.
5. You can now set the colour. Right click on any net segment and from the context options select “Change net colour”. Click “Own colour” and choose the colour. 

The wire is now complete.

NOTE. The colour is assigned to the net, so all wires on this net will be the same colour. This is an advantage for visibility, even though possibly different from the random wire colours used on the ‘real’ breadboard.

Remember at all times that you are documenting your ‘real’ breadboard, not replicating the potentially messy ‘real’ breadboard. Always use your DSPCB schematic to make your routing clear, group wires according to the function such as the RBG routing shown here. Do not just route as you observe how the wires were placed on the real breadboard!

Now produce the PCB.

This step is the same as normal. Translate the schematic to a PCB and all your component footprints as defined for the “breadboard” components, can be placed with the air wires showing where to route your tracks.

The breadboard component was “Schematic Only”, so this is just replaced by any net connections that were used.

Note that single pin nets. i.e. any pin that does not route to another pin are initially identified with a stub track, simply select and delete these before moving the component on to the PCB.

Alternatively, for future design development options, while editing the schematic, place a single pin/pad component and these pads will appear on the PCB.

As shown previously, the components can be positioned on the PCB for routing. 
But you can now add ‘real’ components from your standard libraries i.e. with values and even change through hole to surface mount components as required.

This reinforces a key point, the components used for the Breadboard schematic sheet do not need to have values assigned at that stage. This is completed at the PCB step.
You do not require lots of components for creating your breadboard schematic, just a few with the required pin spacing.

Routing the PCB, we quickly have a completed PCB design.

Please watch this short video giving an overview of the entire process:

Summary.

We hope this introduces you to another way of using DSPCB, “breadboard layout to a PCB”.

Attached are the following files:

1. Breadboard schematic files to start your design or evaluating this method.
   “Reference Breadboard  Creator 400pins.sch”
   and
   “Reference Breadboard  Creator 800pins.sch”.
   Note these mention “Creator” in the filename to indicate the tier used during the design and can be opened with Engineer also.

2. A minimal set of “Breadboard” components to evaluate, and also to examine what is required to create your own. These can also be enhanced as required. 
Supplied as an Export Library, type .elt.  “Breadboard components.elt”
Use “ADD File” to add these to your library. The attachment below is in a ZIP file, please extract the ELT  from it.

3. The completed schematic as used in this article for you to explore.
“Example Breadboard design - Creator.sch”

We would love you to post your feedback on this article. It uses features that are currently available in DesignSpark Creator and Engineer subscriptions. 

If there is an enhancement that you would like to see, let us know and we shall discuss with our developers.