altium print outline problem

[parasbhanot]

hello everyone ,

I am trying to print Pcb  for home etching in altium 16 by File > fabrication output > Final. But the only problem is that in my output pdf file outline of IC-atmega 32 is appearing . Since i have used polygon pour ,So every pin of  this ic is getting short. Is there any way to remove this outline ?

i have attached my output pdf file.

Thanks in advance

[Christe4nM]

If you use  File > fabrication output > Final Altium prints the layers form a pre-selected set. This apparently includes the layer with your IC's outline.

Instead do as follows:
- File->New->Output Job File
- In the new file you have a table where you can specify what you want. Now look for the line that says "Documentation Outputs" and click below on the line that says "[Add New Documentation Output]"

- From the drop-down menu select "PCB prints"->"your_file_name.PcbDoc". A new line is created for you PCB prints.
- Right click on this new line and select "Page Setup". A pop-up window opens. Make sure the top right corner says Scale Mode: "Scaled Print" and Scale: 1.00. Adjust other parameters to your liking. - click close

- Right click on the "PCB prints" line again, now select "configure". A pop-up window opens. This is where you can specify which sets of layers you want to be put into your PDF's pages. There are a number of sets of layers. Each one has a title in a grey block. Below that grey block the layers that are printed are specified. Each set is printed on a single page.
- In your case: Right-click on one of the 'grey blocks' and select "Delete". Do this for every single one except Top Layer and/or Bottom Layer (depending on which ones you need)
- In the remaining sets: remove all but Multi-layer, Top Layer (if it's the Top Layer set) or Bottom Layer (if it's the Bottom Layer set)
- If you use the Bottom Layer set, make sure the 4th box (Mirror) is ticked.
- Click OK

- To the right of the screen there is a PDF output container (as Altium calles it). Click in it to select it.
- In the line with your PCB prints output, all the way to the right is a circle (Enable column). Click that to link it to the PDF output
- In the PDF output container, click "Change".
- In the pop-up window, click "Advanced" (lower right corner)
- Check in the bottom-left section that the line that says "PCB page size and orientation source" is set to "Page setup dialog"

- If desired specify a folder where you want to PDF to be placed in. Other wise, you find it in your project folder, in a sub-folder called something like "project_name outputs"

- In the PDF output container, click "generate content"

Done


Edit: Altium is very powerfull and lets you make it work as you want it to. Yet you need to take a few steps to tell it how you want it. Once you get the hang of the output job files it's quite simple.

[parasbhanot]

Problem Solved

Thank you very much.