[Tutorial] Creating Part Devices using technologies

If you have a part symbol and package set up properly you can go on with setting up a new device and the devices technologies.

In the Device Editor you have to create a new Device and add a Symbol (by simply). To have an easy example we will start with an simple 2 terminal resistor, and call the device R. Then you add your Package Variants, as i did here. I’ve added some Packages i have drawn before, and connect Symbol Pins with the Package Pins.

The Package Variant Name will be directly shown in the Technology Name, therefore i named the Variants in my example 0603, 0805 and so on.Library_Device_Variants

The Prefix of the Device will be Name of the Part in the Schematic trailed by a ongoing unique Number. Here it will be starting with R1, R2 etc.Library_Device_DevicePrefix

The Description can contain html formatted Information, and is useful for containing links to Datasheets of used Parts in the technologies.Library_Device_Description

And at last the most important, creating technologies.
Every Package Variant can have several Technologies.

For example think of a 0603 Resistor, in values 1kOhm and 100kOhm. These would be the Technologies (i created here some more technologies for later use) in the Package Variant 0603. After adding these technologies you can easily add attributes and fill in the Information for every technology and every attribute. If you include an attribute called Value, the placed technology would automatically set this value for the part in schematic and layout editor.Library_Device_Technology

Some Attributes which should always be added for a complete BOM export:
MF (Manufacturer)
MPN (Manufacturer Part Number)
OC (Order Code)
OTHER (for some additional Information)
VALUE (for the displayed Value)


additional Attributes for faster part choice which i use in some other devices could be:

POWER (rated Power)
TOLERANCE (Tolerance in Value)
COST-100 (cost of 100Parts@supplier)
I-SAT (saturation current of a coil)
RDC (DC Resistance of e.g. a coil)
IDC_MAX (maximum DC Current)
VOLTAGE (rated Voltage e.g. of a Capacitor)

If you keep all that in mind when creating a new Device you will get a sweet Bill of Materials with every Information you need with one easy click. To see such a sample BOM only created by filling in all listed attributes in every device you will get something like this:

BOM AnalogZ V2 0 Rev A
BOM_AnalogZ_V2_0_Rev_A.html
12.7 KiB
1505 Downloads
Details...

Where PCB Perfection starts – Part3

The Component Library

The E.A.G.L.E library is devided into 3 parts:

The Symbol, displaed in the Schematic Editor
The Package, displayed in the Layout Editor
The Device, connects Symbol- with Package pins

What you really should consider is to use device technologies. This will enable you the power of one-click generation of your Bill of Materials (BOM), with all Part Numbers and Distributor Order Codes, of every Part you used in your Design. To benefit of this BOM Generation, since Ealge6 its directly located under
file->export, it is recommended to use device technologies, for every single Part!

At the first look it seems that this might be some horrible work, but its only the very first time. Once you have device technologies, for every part (resistors, capacitors etc.) schematic design with choosing all parts, will be very very easy, because you wont have to look up order codes never ever again.

Ordering Parts at your Distributor for a whole Project will be done in one minute with a simple copy paste of your BOM.

In the next Tutorial i will show you how to set up a Device and the technologies in a professional way.

[Tutorial] Generating 3D PCB Data in seconds

In this Tutorial i will show you the few steps needed to generate 3D PCB Information easily.
First of all you will have to use this tools:

  • EAGLE Layout Editor (generate-3d-idf-data.ulp) – for generating idf Information.
  • IDFStepper – for generating STEP Data.
  • FreeCAD – for viewing generated 3D Data and assembly with housing models.

If you are using EAGLE, you know how libraries are organized in Symbols, Packages and Devices.
In some other tutorials i will show how to set up all library Informations properly, this tutorial will focus only on the library parts concerning 3D Data, which is the Package Information. This additional Infomation to generate step-files will cost you maybe one additional minute when creating a new Package but the 3D Information you get is completely amazing.

First of all you will have to generate some new layers in the Package of a Device:

  • Package Layer 57: for top placed parts
  • Package Layer 58: for bottom placed parts

(just copy paste into the command line of eagle-Package Editor: layer ’57’ tCAD or layer ’58’ bCAD)

By only drawing the outlines of your part in this layers, shapes will later be extruded with the height of your line width (1 µm width = 1mm heigth). The line width determines the extrusion height. If you want some pins of your e.g. TQFP part shown in the 3D Model you will have to draw extra rectangular shapes for every pin.

57_TCAD
Layer 57: tCAD Polygons for Plastic Case and Pins

Be aware, that eagle connects lines which are close together, to a single polygon, therefore, parallel outline shape of pins and plastic case should not be connected since you will get errors when generating the idf-file. You can check if they are connected, by zooming in wide, or only moving the shapes a bit. You will see if they stick together immediately. To have no problems i move the conours by entering the numbers directly into the Info of a shape contour, so they will always be in a distance of more than 1µm. In the 3D Model you wont see that distance between feet and plastic case.

NOTE: Be sure that you draw something like the maximum outline dimensions, since big parts may have mm Tolerances and they might collide in your housing if you don’t consider that sometimes parts are bigger than the typ. size shown in the Datasheets!

50_PCBOutline
Layer 50: PCB Outline with PCB cutout

Next step is to generate a new layer in your .brd:
.brd Layer 50: for the PCB Outline (you may copy only the Dimension to that Layer). as in the Package.
The line width also determines the PCB Thickness, in the same way.

 

one simple PCB Outline with a breakthrough and three simple Parts placed
one simple PCB Outline with a breakthrough and three simple Parts placed

If you want some cutouts or breaktroughs in your Board, you can do so by defining a Polygon with line width set to 0.0µm. When you are done with the Layout, here in my tiny example i only put one Resistor and another Capacitor onto the Board, it may look something like this.

After that you will have to generate the 3D idf Data with a eagle ulp Program called generate-3d-idf-data.ulp.

3D_test
step file generated with idf-stepper (idf and idb file as Input)

There will be 2 files generated. On is the named *.idf and it contains the information of the whole polygons. idf-stepper will generate a step file for every single polygon and store it in the root folder. The *.idb file contains the Information how the polygons are oriented to the Board origin. idf-stepper will take all the generated step files, put them in place to one big step assembly. In windows idf-stepper works with drag&drop the *.idf and *.idb files simply onto the executable and you are done!

When you are using your simple rectangular shapes like me in my little example you will then get a generated step file looking something like this. For most Mechanical Engineers this generated step Information is all what they need to place the parts in a mechanical assemly and check collisions and correctness of mounting points.

But idf-stepper also can also deal with advanced very complex step models. Exactly this function gives you the most powerful capability:


By only using the *.idb file you can take every very advanced 3D Model as Input source to the idf stepper. Only take a short look at the naming convention, take your advanced model, give it the right orientation and you can use it immediately by replacing the generated step file of this part generated by idf-stepper. If you deliver the idf-stepper only the *.idb file as Input, the existing step files wont be overwritten.


 In another Project i used more advanced 3D Models for the LEDs, once you have rotated the advanded LED-Models into the right angles, you can use them every time again:

3D_advancedLED_Models
included advanced step files for LEDs

One addiotional highly useful and powerful feature: Since FreeCAD has the Ability to save the step file as *.html (every modern Browser can use WebGL) you can send your 3D Model as html-file to everyone, still if he has no CAD Viewer, he will be able to rotate the model, zoom in/out within the browser. The only thing you might have to adjust by your own with a simple text editor is, to set the camera Position far enough from your board, since if the standard Position is (0.0, 0.0, 1.0), which means the camera is set in the PCB, so by default you do not see any parts. I like to use something like that camera.position.set( 100.0, 100.0, 200.0 );

This last sample i provided here, outgoing from an with idf-stepper generated step-file, opened with FreeCAD and saved as html(webGL) file.

Where PCB Perfection starts – Part2

The Schematic Editor

Most electronic desings start with the schematic editor, placing some parts and changing their values. Not every designer is thinking about concrete parts (Manufacturer Product Number – MPN), their physical case dimensions, and the availability when designing the schematic.

What you really have to consider is, what component technologies you might want to use, in order to meet your assembly requirements. Threrefore you might have to look for TSSOP Cases instead of no-leaded QFN packages. Most active parts you will get in different cases directly from the distributor, only take a look into the Datasheet, all possible packages of one part are clearly shown, often with dimensions and order codes (Maufacturer Part Number). As an Exaple you might take a look into that Datasheet of a DAC. You could freely choose between TSSOP or QFN Package, the costs and the availability at the distributor is nearly the same.

When using parts in the schematic it makes clearly sense to think about what concrete part, also what passive components like resistors and capacitors, you will place in your layout, especially if some cases may have long lead times.

So when you already know what parts you want to use its time to set up your CAD Library properly.

 

Where PCB Perfection starts – Part1

The CAD Program

There are several tools existing, and many work well. But in my opinion E.A.G.L.E Layout editor is one of the, compared with others, cheapest editors you might can get. If you are only using two layers in Layout and only need euro-card sized PCB’s its free. As far i know most other Editors are organized in a similar way.

The Schematic Editor uses the parts Symbols.
The Layout Editor uses the parts Packages.
The Part Library connects Symbol Pins with physical Package Pins.

One Symbol can be connected to different Packages e.g. one Resistor Symbol can be realized as case size 0603 or 0805 as Package.

In my upcoming posts i will show you some details you have to consider when generating part libraries by your own. I am working with E.A.G.L.E so some tips are only useful if you are using Eagle, but especially for designing Part Libraries on your own, all Information given here might be helpful to you.

Innovative Electronic Design – pushing the limits