Drill drawings for multilayer designs with blind/buried vias.

Many designers still produce drill drawings along with their Gerber files as Manufacturing Notes for various reasons and this is a how to for multi layer boards.
 
When you are designing a multi layer board that includes blind/buried vias you may want to provide a drill drawing per layer pair, to provide all the layer pairs on one drawing can confuse and enable mistakes to be made, let me explain how this can be done.

In order to make multiple drill drawings we need to understand a few things about recent releases of CADSTAR, the most important being that we no longer need to provide a "Drill Drawing" output, instead since V13.0 we have had drill letters and an automatic drill table available so it is now truly WYSIWYG so it should now be produced as an "Artwork".

Each different sized drill hole can be assigned a drill letter to be displayed on a drill layer of our choice, there is a table that will display the drill letter, size, count and slotted hole length and from V14.0 an additional comment per drill. The drill table is linked directly to the design and any changes will be automatically changed in the table. The table can either have a manually created tool table or an automatic one that requires no input from the designer.

It can also be set to display the drills for a specific layer pair, however we only have one table which can only be placed on a single layer so if we have a board with PTH, 2x Blind and 1 x buried via layer pairs making it that we want to produce 4 different drawings where each drawing has its own specific drawing number and other identifying text etc then we have to get constructive with how we manage the table etc.

For a completely PTH board it is not an issue as you only need a single drill drawing layer. Also when manually creating different drawings the tables layer can easily be changed, however when using the much preferred batch process output we cannot change the layer the table is on.

What I suggest for this drawing set is that we adopt a few layer specific practises, i.e the individual layer pair text etc would need to be on their own layers per layer pair, the drill table on its own layer and common items such as a drawing border, dimension lines etc on a common layer. Multi layer boards have a lot of layers and outputs so having a few more documentation layers is no great deal.

Set it up like this:

1) Create a documentation layer for common documentation items.
    (border, design identification text etc.)

2) Create a documentation layer for the drill table.

3) Create a documentation layer for the PTH drill information, text, drill letters etc.
    (Through Hole)

4) Create a documentation layer for the Layer pair 1 (Blind) drill information, text,
    drill letters etc. (LP1)

5) Create a documentation layer for the Layer pair 2 (Buried 1) drill information, text,
    drill letters etc. (LP2)

6) Create a documentation layer for the Layer pair 3 (Buried 2) drill information, text,
    drill letters etc. (LP3)

7) Create a colour file that displays layers 1, 2 & 3. (Drilldwg_PTH.col)
8) Create a colour file that displays layers 1, 2 & 4. (Drilldwg_LP1.col)
9) Create a colour file that displays layers 1, 2 & 5. (Drilldwg_LP2.col)
10) Create a colour file that displays layers 1, 2 & 6. (Drilldwg_LP3.col)

When preparing the design for the drawings follow these practises;
Add your document borders, manufacturing note symbols etc to layer #1.
Add the drill table to layer #2 and configure it, auto allocate seems to work well.
Add the PTH specific text to layer #3.
Add the blind and buried drawing identifying text to their specific layers #4 to #6.

Try each colour file and you will see the specific items for each layer with the exception of the drill letters in the PCB and table, this is controlled by changing the layer pair in the drill table properties. This can be saved in selections files that change the layer pair, however the selections files used in the drill table dialogue cannot be used for manufacturing output so we must create separate files for these.

Start the batch process and create 4 layers in addition to your usual Gerber layers.
These layers will be setup the same as the top/bottom/inner layer copper etc as an Artwork, Photo Plotter, rs274-x.usr and for each one in the selections file field type in the name of a new selections file for the specific layer pair:
Drill_PTH.sel
Drill_LP1.sel
Drill_LP2.sel
Drill_LP3.sel
If they do not exist you will be prompted to create them.
These should all be set the same, Auto Position, Origin, Drill Letter Association etc each with a different layer pair selected.

For each layer use the colour file created for it and when running the process it will change the layer pair for the table and drill letters and output the 4 different drawings as required.

Looking back at what I have just written it looks like a long complicated process but in reality it is not, its really rather simple and by doing it this way you can create your different drill drawings for any layer type with ease.

When you next update the PCB and change the number of drilled holes then this process can give you a much more accurate set of drawings than those produced the old way with a manually entered text filled table that does not update when the design does.

Try it for yourself, adjust it to suit the layer pairs you are using.