Sort patterns in alphabetical order:
Menu Library/Sort Patterns by Name
Package, Temperature Range, material, tolerance, ... All this properties combined gives a myriad of variants of the "same" component. Every one have a unique identifier: the "Manufacturer Part Number", the orderable product in a Bill of Materials (BOM).
How manage this? Do we need to have all of them in Diptrace? When we are in the design stage, do we need to know the exact Manufacturer Part Numeber of a 220 ohm resistor we are going to use?
This is a simplified guide of the workflow of Mechanical CAD, Electrical CAD. Don't limit yourself to make rectangular PCBs. Mechanical constarint is the norm, you can't place all the component where you want. The design of the PCB not starts in an empty space. Test jigs/beds are created at the same time as another PCB or PCBs assembly in the same design enviroment. I recommend an easy CAD software as QCAD as DraftSight could be overkill to learn the basics. Sorry if I omit things in the resume, is a start point to understand the relationship between Mechanical and Electronic PCB design. Also, Diptrace are working in the CAD aspects, and now we have to do too many workarounds to integrate both worlds. Its very important to make the Components Library via a CAD soft and then import the DXF in DIPTRACE. You will learn all the concepts involved and will have an ECAD independent component library.
For starting an unconstrained design:
First, is more practical approach to have a good Schematic library with generic components without pattern assigned. For example: resistor. Later give value, power, material, etc. in property fields (use Additional Fields).
You could concentrate in design and not in the Bill of Materials at first. You could make all the changes you want at this stage.
Second, think about size of the PCB and the type of components (through hole, smd), and replace the symbols in schematic editor (right click in component and "Replace Part"... be aware to apply to this component or to similar components) with a components of a second library with variants of patterns. One part by pattern. in this process, property fields are manteined. Generate a Bill of Materials in CSV. Open with Excel or Open Office and go to Mouser and Digikey in two tabs in your prefered web browser. Find the parts not spending a week or so in this tedious process and assign into the BOM. There are too many parts with different attributes and prices. The next time you will gain a lot of time.
Third: Start with PCB Layout ...
For starting with a constrained design:
2. Specific use of parts
Start at the end? Yes.
Start in a CAD program:
1. To design the components, mechanical determines electrical (pin size/position -> pad size(formula of pin size)/position):
1.1 Mechanical package 2D (body, pins, pin1 region, outline...) and 3D (start with the included in Diptrace or get it from web collections)
1.2 Land pattern (pads)
2. To design the PCB
3. To palce some components by enclosure or form factor constraints. For example, a plastic enclosure has screws in the corners or/and in the center and a delimited space for components in height, and as a form factor, arduino shields have a size, a type of female connector and an area to avoid some components by height. As the component has been designed in an unified CAD enviroment, you could use absolute coordinates in both MCAD and ECAD (Diptrace) "manually" emulating IDF in bigger programs as Altium, Pads, Allegro ...
Well, now a PCB shape (outline), PCB Cutouts, keep-in, keep-out regions, and critical components placed. Ordered in layers and blocks for easy manipulation and modification/replace. Make a X,Y placement table for the components.
Now you can start in Schematic Capture and insert the constrained components (whith the second library of components with pattern).
Convert to PCB, import DXF the PCB shape. Place by coordinates the first components and lock them. As the pattern library has been made from the MCAD-ECAD enviroment, the package outline appears, and the center is the same in both softwares.
Now the free space to place the rest of the future components and the technology usable (size of components and trace and vias Design Rules) could be evaluated.
Back to Schematic Capture, and continue with the "generic" library. Then replace components and go to PCB Layout. Go back and forth making the changes to accomodate the design to the final BOM.
Last edited by konekted on 16 Sep 2012, 16:34, edited 1 time in total.