[SOLVED] What are the files required to the PCB manufacturer

[pal114525]

Hi,

I am new in PCB design.
I have designed a layout (manually) from schematic using DipTrace. I have also generated gerbers and drill files.
Can anybody tell me what are the files required for the manufacturers to manufacture a PCB.

Thanks & Regards.

 

[KlausST]

Hi,

You can use a forum search.
Or you can use the "similar threads" at the bottom of this page.

I've answered about the same question just some days ago..

https://www.edaboard.com/threads/345177/

Klaus

 

[Linda.guo]

Hello ,

To PCB manufaturer, they just need the files you want PCB like.
normally, you need to output below files:
1. circuit layers, such as GTL,GBL for outer layer, if it is multilayer PCB , you should also output all inner circuit layers, such as GND, vcc, inner layer 1, inner layer 2 and so on.
2. solder mask layer: Such as GTS,GBS
3. components marks/ silkscreen layer, such as GTO, GBO
4. Drill holes : such as drill
5. drill drawing
6. if you need carbon or peelable mask to be printed on PCB , you also need to outgoing carbon or peelable mask layer.
Any questions related to PCB manufacturing process , you can ask me.

hoping my words above can help you out .

 

[pal114525]

Hello ,

To PCB manufaturer, they just need the files you want PCB like.
normally, you need to output below files:
1. circuit layers, such as GTL,GBL for outer layer, if it is multilayer PCB , you should also output all inner circuit layers, such as GND, vcc, inner layer 1, inner layer 2 and so on.
2. solder mask layer: Such as GTS,GBS
3. components marks/ silkscreen layer, such as GTO, GBO
4. Drill holes : such as drill
5. drill drawing
6. if you need carbon or peelable mask to be printed on PCB , you also need to outgoing carbon or peelable mask layer.
Any questions related to PCB manufacturing process , you can ask me.

hoping my words above can help you out .

Hi,

Thanks for your valuable feedback.
I have generated the following output files for PCB manufacturing:

1. Board.gbr
2.BoardOutline.gbr
3.Bottom.gbr
4.BottomAssy.gbr
5.BottomDimenasion.gbr
6.BottomMask.gbr
7.BottomPaste.gbr
8.BottomSilk.gbr
9.Top.gbr
10.TopAssy.gbr
11.TopDimension.gbr
12.TopMask.gbr
13.TopPaste.gbr
14.TopSilk.gbr
and 15. Drill.drl

Please let me know what else is required?

Thanks & Regards.

 

[FvM]

Minimal required is top/bottom copper (3/9), mask (6/12), board outline (2) and drills(15). Silkscreen (6/14) if actually printed, paste (7/13) if the board manufacturer is also making solder stencils. Other files are for assembly and service purposes.

But there's no problem to send the complete file set to the board manufacturer. The job details should be clearly specified anyway.

 

[Linda.guo]

Hi,

yes, they are enough for PCB manufaturer to produce your PCB.

Good Luck !

 

[Mattylad]

Can you also make an IPC-D-356 netlist?

 

[Linda.guo]

Sorry, i am not professional in generate Netlist.
i think you can find how to generate Netlist from below link:
https://www.diptrace.com
hope it can help you !

 

[pal114525]

Can you also make an IPC-D-356 netlist?

Hi,

Would you please tell me why this format is required?

Thanks & Regards.

 

[FvM]

An IPC S-365 file contains a design netlist that can be checked against the gerber files to identify possible post process faults and also used for an electrical test of the finished PCB.

Presently most PCB manufacturers are extracting the netlist for an electrical test (if performed at all) from the gerber data. So it can recognize PCB manufacturing faults, e.g. trace shorts and discontinuities or defective vias, but not gerber faults.

It seems to me that even if you provide an IPC D-365 file, it's not necessarily used by the PCB manufacturer. But performing a gerber check yourself with respective full featured gerber tools might safe you from dumping PCB lots to the trashcan. In so far it's worth to mention the option. Recent PCB tools should have an option to generate IPC D-365 netlists. Cheap semiprofessional tools possibly don't have a built-in D-356 option, but might be still able to generate the netlist format by macro or script programming means.

 

[marce]

If you have the option use ODB++

 

[jennygcl]

1. Printed Circuit Board Data:

Circuit Board data can consist of the traditional data package which must include the following:

Gerber Data in the following formats:
274D including separate aperture list with all apertures defined.
274X - Preferred
Gerber files with aperture lists
DXF can be used requires an approval prior to production
ODB++ format
Drill Data in the following formats:
Excellon 1
Excellon 2
Also acceptable is ODB++ data. ODB++ will be supplied as a single file, usually with the extension of .tgz. ODB++ contains all the required board and drill information.

Note: Any other data formats need to be reviewed and approved by Epec Engineering before the order can be placed.


2. Printed Circuit Board Fabrication Instructions:

The fabrication instructions should contain all relevant information required to tool and build the part including:

Hole sizes with tolerances, and plating information
Board outline detail with all required dimensions and tolerances
Hole or feature to edge dimensions
Finished Copper Weights
Finished Board thickness with tolerances, and measurement criteria
Surface finish preference
Soldermask requirements
Silkscreen requirements
Technical contact information
Any additional requirements (i.e. impedance, controlled dielectrics, plugged vias, etc.)

The fabrication instructions may be found:

Fabrication Drawing:
Adobe Acrobat (.pdf)
Gerber
RS274X
HPGL
AutoCAD (.dwg or .dxf)
Graphic file (.jpg, .gif, .tif, etc.)
ODB++
Array configurations – tab or scored preference

[link to commercial site deleted]

 

[FlapJack]

Some pcb shops have specific requirements for files. They tell you what files they need and they want you to use specific names for different layers and will tell you what format to use.