House_Cat
Advanced Member level 4
altium logo
The information you need to provide to a fab is the same, regardless of what EDA program you use.
Gerber files are also called photoplot files. They are used to produce plots through which photosensitized panels are exposed to light. They contain no intelligence about the design except the exact location of lines and pads on whatever layer for which they are generated. To provide the rest of the information necessary to manufacture a board, you either have to create a mechanical layer containing the data, or provide a text file with the information. You also need the drill file to define the location of drilled holes.
1. Normally, you put all of the necessary mechanical information on the "Drill Drawing". In AD, this is a defined layer by that name. If you are going to have an assembly house assemble your board, you will need to provide other mechanical layers to them with information that helps locate all of the components.
2-3. You need to generate a Gerber file for each of the copper layers/planes in your board. You should also generate a Gerber file containing the board outline - this will be used by the fab for routing the board from their panel. You will also need the Drill Drawing Gerber layer upon which you have written all of your specifications for the board - material type, dimensions, stackup, and any other information you want used to produce your board exactly as you have designed it. Finally, you need the drill file so the fab can drill the vias and thru-hole pads.
4. It is a good idea to specify which Gerber file goes with which layer. Every EDA program does it differently. For example, Allegro produces files with the numerical sequence of the stackup in the name and the extension ".PHO". The numerical sequence starts with the top silkscreen, and continues down through the solder mask, top, inner layer 1, etc. Your fab may not necessarily be used to the way your EDA software names the files - it's best to tell them to be sure.
5. The "CAM" file produced by CAMTASTIC in AD6.7 is a summary file that is readable ONLY by CAMTASTIC. Every cam editor has its own proprietary file format for storing a summary (composite). Your fab would have to have the same CAM editor you use in order to open that file. It is NOT intended to be a fabrication file. Stick with Gerbers and Drill files, or ODB++ (an alternative fabrication file).
6. Where you set your user origin doesn't matter. When you generate your Gerber files, you are given the choice of having the Gerber reference the relative or absolute origin.
7. The IPC Standard your fab is talking about is probably IPC-2221 "Generic Standard on Printed Board Design". I think the section to which they are referring is: "When conductors of melting metal have a width larger than 1.3 mm, the design of the conductor shall provide a relief through the metal to the base laminate substrate. The relief should be at least 6.45 mm2 in size and located on a grid no greater than 6.35 mm. When conductor areas of melting metal are to be left uncovered, the design for all class boards shall provide that the solder resist shall not overlap the melting metal by more than 1.0 mm."
Note that unless your board needs to pass some sort of acceptance testing as a commercial product, the above standard is optional. Nothing says you MUST follow the standard.
8. You should do the tenting in your original PCB file. It can be done in CAMTASTIC, but it's a lot of manual work. The solder mask Gerber is a negative image - in other words, mask is applied everywhere there is not an object on the plot. You would have to remove all of the objects corresponding to mask openings in order to tent from the Gerber file. In the PCB Editor, tenting is a simple instruction in the pad or via dialog, and can be generated globally.
The information you need to provide to a fab is the same, regardless of what EDA program you use.
Gerber files are also called photoplot files. They are used to produce plots through which photosensitized panels are exposed to light. They contain no intelligence about the design except the exact location of lines and pads on whatever layer for which they are generated. To provide the rest of the information necessary to manufacture a board, you either have to create a mechanical layer containing the data, or provide a text file with the information. You also need the drill file to define the location of drilled holes.
1. Normally, you put all of the necessary mechanical information on the "Drill Drawing". In AD, this is a defined layer by that name. If you are going to have an assembly house assemble your board, you will need to provide other mechanical layers to them with information that helps locate all of the components.
2-3. You need to generate a Gerber file for each of the copper layers/planes in your board. You should also generate a Gerber file containing the board outline - this will be used by the fab for routing the board from their panel. You will also need the Drill Drawing Gerber layer upon which you have written all of your specifications for the board - material type, dimensions, stackup, and any other information you want used to produce your board exactly as you have designed it. Finally, you need the drill file so the fab can drill the vias and thru-hole pads.
4. It is a good idea to specify which Gerber file goes with which layer. Every EDA program does it differently. For example, Allegro produces files with the numerical sequence of the stackup in the name and the extension ".PHO". The numerical sequence starts with the top silkscreen, and continues down through the solder mask, top, inner layer 1, etc. Your fab may not necessarily be used to the way your EDA software names the files - it's best to tell them to be sure.
5. The "CAM" file produced by CAMTASTIC in AD6.7 is a summary file that is readable ONLY by CAMTASTIC. Every cam editor has its own proprietary file format for storing a summary (composite). Your fab would have to have the same CAM editor you use in order to open that file. It is NOT intended to be a fabrication file. Stick with Gerbers and Drill files, or ODB++ (an alternative fabrication file).
6. Where you set your user origin doesn't matter. When you generate your Gerber files, you are given the choice of having the Gerber reference the relative or absolute origin.
7. The IPC Standard your fab is talking about is probably IPC-2221 "Generic Standard on Printed Board Design". I think the section to which they are referring is: "When conductors of melting metal have a width larger than 1.3 mm, the design of the conductor shall provide a relief through the metal to the base laminate substrate. The relief should be at least 6.45 mm2 in size and located on a grid no greater than 6.35 mm. When conductor areas of melting metal are to be left uncovered, the design for all class boards shall provide that the solder resist shall not overlap the melting metal by more than 1.0 mm."
Note that unless your board needs to pass some sort of acceptance testing as a commercial product, the above standard is optional. Nothing says you MUST follow the standard.
8. You should do the tenting in your original PCB file. It can be done in CAMTASTIC, but it's a lot of manual work. The solder mask Gerber is a negative image - in other words, mask is applied everywhere there is not an object on the plot. You would have to remove all of the objects corresponding to mask openings in order to tent from the Gerber file. In the PCB Editor, tenting is a simple instruction in the pad or via dialog, and can be generated globally.
