Creating a positive or negative print for use with photoresist coated board

When you wish to create a positive or negative printed image of the copper layers this can be achieved as follows.

1. In Windows set your default printer to a PDF printer. The Windows 10 "Microsoft Print to PDF" is suitable or select your preferred PDF printer.

2. From the menu bar select Output - Manufacturing Plots, shortcut Shift + P

3. Select the "Auto-Gen Plots" button and a window will launch where you can select the Windows output option which in our case will be the PDF printer.

DO NOT select the PDF option as this is for the photo plotter PDF which does require and hence does not support negative image generation.

4. Selecting the "Windows" option will open a further window allowing you to select the required plots to be produced. For this example we assume a double sided PCB, but you can configure for any layers required. Select the options as shown in the tick boxes in green.
You may also find the drill file useful to assist with the drilling, so 

 5. The files to be plotted are then listed in the left hand column under "Plots".

The two in the green box are required, the Drill Ident is optional.
The selected plot (left mouse click) and highlighted in blue then has all the options for that plot in the right hand panel identified by the grey box. These settings can be configured as required and ONLY affect the highlighted plot.

 It is suggested that the copper layers also include the board outline (click to toggle from N to Y) to enable the printed mask to be aligned with the PCB edge or to show where the PCB needs to be cropped after etching.

6. In the "Settings" tab you can decide whether to have pad holes shown. If they are not checked as "filled" a hole will be etched, this may allow easier drill alignment, but if the drilled hole is not central the copper pad will not reach the edge of the holes.

Checking the filled drill holes will give a better result regarding copper reaching the hole edges.

On this tab we also have the important option as to whether we produce a positive or negative print, select what is required for your photo sensitive PCB.

7. The final tab is the "Position" tab. Use this to set the position of the PCB image on the print. In this case we illustrate a one inch offset from the corner.
No other setting should require changing.

8. Now select the Plot "Bottom Copper" and repeat any required changes to the options in each tab for this plot.

Note: The preview window is just an indication of the plot with some of the PCB layer features shown. It does not indicate the final print out and for example does not reflect the positive/negative plot.

9. With the plots now set up you can click the "Run" button to generate the PDF file. As you are using a PDF printer, this device will provide the option of where to save the PDF file. It is suggested you use the project folder for the destination.

Below are the top and bottom copper plots with the above settings.

 The above completes the required printed artwork, the following tips can also assist with your production steps. 

Drilling

10. Once you have etched the PCB you will then have the task of drilling the board. Some form of aid to assist identifying the drill hole size would be useful and here the "Drill Ident Drawing" will prove useful. 

The Drill Ident Drawing from this design together with the drill table from the Plot Report is shown. Select your drill size to match as required to the designed hole size and complete the PCB.

 Note. In the "Plot Report" the drill ident table allows you to configure the shape and the size of the symbol (highlighted in orange) this can provide additional assistance in locating the holes on the PCB.

11. As it can be difficult to precisely drill the holes there is a technique commonly referred to as "drill spotting". A small hole is etched in the centre of the pad copper to align the drill precisely.

First produce the above drill ident drawing for reference of the required hole sizes and their location.
Next make a copy of your PCB file as you will be editing the pad hole sizes and the required hole sizes will be lost if you work on the original design file.

Open the new copy of the PCB file and launch the Design Technology - shortcut Shift+T and select the "Pad Styles" tab. Here the "Hole Size" column shows the required drill sizes.

Edit the entry for each to say 0.4 as shown below and apply to your design.

Next  produce the manufacturing files as detailed previously, but set the check boxes as shown below, i.e. we have selected not to have the drill holes filled.

Below shows the PDF negative image with the small opening in the copper pads for drill location.

Etching.

12. Add a copper pour over the PCB layer. This can provide electrical performance improvements, but more importantly reduces the amount of copper required to be etched. Below is the top copper with a copper pour showing a large reduction in the copper required to be etched.