Printed Circuit Board Design Engineer Network - Click to return home

Vutrax Basic Training tutorial part 2, Libraries

Part 1> Part 2> Part3>

Useful notes before you start...

Set increments:
This is useful for quickly numbering pins & pads that can be numbered in sequence.
So before you start any numbering sequence, click the ++ icon on the toolbar & type in the number you’d like to start with (e.g 1), & set the incremental jump sequence (e.g 1).

Count Points:
Counts are the number of points & data points within a part. To query any count point use Esc to lock onto a point, then read the information from the command line.
You can use a command line letter M to move around any count sequence within a part. This is particularly useful when looking for Count 1 to place your Device name/Graphical name data point.
E.g, if you are querying count 27 & want to move to Count 1, simply type M-26. This will take you back 26 steps.
To query all counts & view as a list, goto, Footprint > Attributes > List Footprint Attributes.

Symbols:
Draw outline:
Use the 2D drawing tool, generally on Layer 2. Draw your pin storks first then the outline. Storks are usually placed 150 thou apart.

Combine outline:
Combined the structure before adding pins & attributes.
Goto, Symbol > Join all Inside. Drag a box around the outline to combined.

Add pins:
Set increment first, if required (as above).
Goto Symbol > Attributes > Required Pin / optional / tied. Give each pin a number or name. (Remember these names for later use, when you have to join this symbol to the footprint).

Add Device name:
Device name can only be placed on Count 1 of the outline. See Count Points above.
Goto Symbol > Attributes > Library name. Type in a name, click OK, then click on Count 1.
Now add Symbol Name, Goto Symbol > Attributes > Symbol name. Type in a name, click OK, then click anywhere on the outline.

Add Silk (Name XXX):
Add Silk Name reference by clicking on the XXX icon (2nd right). Move the cursor to your desired location & click.

Add Text description:
Goto the T icon (1st right), type in the text & place near the outline.
Finally, combine the outline & any other items like text to complete. These steps above are the minimum requirements to create a symbol.

Optional extras:
Symbols.
Part Value:
Should your part need value input from the schematic (e.g Resisters 10K) then goto, Symbol > Attributes > Part Value Mark.

Index information:
This information will be displayed in the Index Library window when searching for parts. A fuller description here will make finding parts more easy.
Goto, Symbol > Attributes > Index/General Text. Type in a full description, click OK & place the text within the outline.
Now this text does not needed to be seen on screen but only as a hidden attribute by Vutrax, so we now need to make it zero size & invisible.
Goto, Edit > Properties > Size > Text size. Type in 0, then click on the bottom left corner of the text.

Hardware information:
Goto, Symbol > Attributes > Hardware information. Type in a full description, click OK & place the text within the outline. You will then need to zero size this text.

Pin names/numbers:
Set increment first, if required (as above).
Goto, Symbol > Attributes > Pin numbers, type in your name/number, click OK & place next to your relevant pin or stork.

Protect:
This will protect your symbol in schematic mode from being accidentally pulled apart or corrupted. Goto, Symbol > Protect, & click on the outline.

Finally, combine your outline & any new attributes again using “Join all Inside”.

Footprints: (Land patterns)
Pad Table: 999 pads definable:
First check that you are using a common Pad Table, this will help avoid problems later.
Pad tables are an embedded database that’s sits in the background of a PCB or Library file. Note that different files can have the same pad number defined differently in each file.

Add Pads:
Goto Footprint > Place Pads > PTH component pad / SMT component pad.
Click & place the Pad down, then move the cursor out away from the pad a little to create a short stork to tag a pad number on there.

Pad Size:
Now go around each pad & give it a pad definition.
Goto Footprint > Place Pads > Pad Size. Click on each pad in turn to apply definition.

Pads numbering:
Set increment first, if required (as above).
Goto Footprint > Attributes > Pin Numbers. Click & apply a number to each Pad.

Combine Pads:
Goto, Symbol > Join all Inside. Drag a box around the Pads to combined.

Draw outline:
Use the 2D drawing tool to draw the component outline on Layer 7. You can create this outline to one side of the pads if it helps, then move it into position after. Make sure the width is no narrower than 8thou.

Add Silk (Name XXX):
Add Silk Name reference by clicking on the XXX icon (2nd right). Move the cursor to your desired location & click.

Add Text description:
Goto the T icon (1st right), type in the text & place near the outline.

Combine outline & Pads:
Combined the structure before adding pins & attributes.
Goto, Symbol > Join all Inside. Drag a box around the outline to combined.

Add name:
The name can only be placed on Count 1 of the outline. See Count Points above.
Goto Footprint > Attributes > Graphical Name. Type in a name, click OK, then click on Count 1.
Note: Vutrax will not allow a Library name to be placed on a Pad. If Count 1 happens to fall on a Pad, then you must create a Before corner. Goto, Footprint > Draw Outline > Corner Before. Click on Count 1, pull the banding out to create a short stork & click. Your name can now be added to the end of the stork. After naming make the stork invisible by using Width 0 & applying it to the line.

Joining the two together & finalising the new part:
Goto, Library > Footprint & Symbol. Pick a library file that you want the new part to sit in, or create a new library by typing in a new name.
Next, read the command line at the bottom of your screen, it is asking you to locate & click on your new Footprint (the one with the pads), then pull the banding out from the footprint & click on your new symbol.
A menu will then pop-up. Choose “Universal Device” Next> “Standard No-Connect” Next> “Number of Groups (1)” Next>
Now match up the Pin numbers to the Pad numbers on each part.
When done, click “Finish”. An AscII window will pop-up, just close it & click YES.
That’s it !

List Attributes:
To view an AscII file list of the part you’ve made goto, Footprint > List Footprint Attributes.

Part 3, PCB layout >

These tutorials assume that the user is familiar with basic PCB design knowledge.

Associated sites:
DCB Automation - Automatic Optical Inspection for PCB assemblies.

Vivace Lighting - Luminus Products Ltd. LED lighting for architectural, constructional applications, hospitality, commercial and outdoor market places.