Camtastic is quirky CAM software that comes with Altium (formally know as
Protel). It's useful for importing Gerber files, making minor changes to them,
and for panelizing.
Unfortunately, the software has terrible documentation. Doesn't use the same user
interface or philosophy as the other Altium tools, and is buggy. I suspect
they bought this program from another company and they did a half baked job of
integrating it into Altium.
We will try to give some tips on how to use this software and ultimately how to
panalize different board into a single panel.
The first important thing to know about Camtastic is that you select the operator
first, and then you select the objects that you want to operate upon. This
is opposite of how nearly every other user interface in the universe works. So
if you want to delete something, you select "Cut" from the menu, then you draw a
box around the items you want to delete, then right click to complete the
Another interesting "feature" is that the mouse works differently if you drag
from left to right and right to left. This is extreemly frustrating when
you don't know why the mouse has stopped acting normally.
Panelizing Different Boards
First thing to know is that their OBD step thing is incomprehensible, and poorly
documented and should be ignored.
To panelize different board types do the following steps:
- Create a new Camtastic document.
- Use gerber quickload to open the gerber set, including the NC drill file.
If it imports funny, make sure that the units are correct - english or metric.
- Move the board that you just imported away from its current location. The
reason is that when you import the second board, they will overlap, and you wont
be able to separate them. Select Move under the Edit menu. Select the
board with the mouse, by drawing a box around it, and then right click, then
drag with the left mouse key to the position where you want it.
- Import the second board now.
- Use the panelize function to create arrays of each board type. Select
Panelize PCB under the Tools menu. Select the board with the mouse, and
right click when done. A dialog pops up. Fill out the info.
- Panelize the second board.
- Note that you can not use the Copy command from the Edit menu. I don't
know why, other than it doesn't work. Instead if you want to copy a board use
the Copy of Field command. You can copy and place any number of boards
that you like using this command.
- Note you can delete the boundaries that were created around each panel.
- Do not delete the vent layer that it creates, it will cause a major freakout
when you export the gerbers.
- To create the gerbers, export them. Make sure that the RS-274-X option is
selected, otherwise the apperatures wont be saved, and you wont be able to
import the file again.
- Explicitly export the drill file. Camtastic creates a txt drill file, but
it doesn't import again. The file name of this will be .drl. You can
rename it to .txt again if you like.
- To check your work. Create a new Camtastic document, and do a gerber
quickload on the files you just created. Everything should import including the
drill file. If it does, you've successfully created a panel.
- Lastly make sure you are consistent with gerber units of inch and mm.
Daycounter specializes in contract
electronics design. Do you need some help on your project? Contact
us to get a quote.
Salt Lake City, UT, USA
Disclaimer: Daycounter, Inc. doesn't guarantee the accuracy of any of it's content. Use at your own risk.
© Copyright 2016 Daycounter, Inc. All rights Reserved.