I have used dxf imports before in Layout 15.7 and we had a simple way to use layers for the basic designs and then import a v12 dxf.
But when I try to develop a basic board outline for Allegro 16.3 or 16.5, there does not appear to be a way of importing the plated and non-plated holes into a PCB. What is the class and subclass for the hole imformation?
The impossible we do straight away. Miracles take a little longer.
In reply to LEAS:
LEASHi.The Drill Chart TOP to BOTTOM is in Class Manufacturing/Subclass Nclegend 1-2 (for 2 faces) and Nclegend 1-4 (for 4 faces)For the board outline who does not appear, verify in Artwork Control Film the "Undefined line width" is not at 0. ( i configure at 0.254)
Drill Chart? Does this control the actual holes? How does it distinguish between plated and unplated holes?
In reply to tmd63:
Drill chart?? No way... You need a Padstack with a drill to make a hole in the board - or a Keepout / Ouline and so on. The DXF is going to give you the location for the hole, then you need to snap the mechanical part to it. The "best" way is to layer the DXF data so that the Outline is on one DXF layer and the "hole targets" on another. The outline might not be closed so import it to a temporary layer like Board Geometry Assembly Detail, the use Shape>Compose Shape to close the shape to the required Board Geometry Outline layer. For the Mounting holes, Place Manually, set the "Library" option in Advanced Settings, select Mechanical Symbols from the drop-down in Placement List, select the Mechanical Symbol in the list, "Hide" the form and the hole will be on the cursor, locate and hover over the target location and use the right-click>Snap To menu to snap to the location. The holes will show up in the Drill Legend when it gets created.
In reply to oldmouldy:
In Layout 15.7, all I had to do was place a circle of the correct size on a special layer and the dxf import would create a hole with the correct hole size and pads of the same size on all layers automatically. All that would be needed afterwards, was to change the padstack to increase the etch pads to a siutable size for clearances etc.
Surely, the more advance Allegro package can do this simple task??