Creating BOM (Bill Of Materials) Report from the PCB Editor only for the Top Layer

Hi,

Generate your report or export the placement, save out the report to disk. Within the report you should see a field called SYM_MIRROR. This field determines if a component is on the top of the board or mirrored indicating the component is on the bottom of the board.

Pull the file into Excel and sort the file by the SYM_MIRROR field. Anything that does not have an "M" for the component is on the top of the board.

There is probably a dedicated skill file that can do this, however I do not know of a way to parse a standard report based on the value of the SYM_MIRROR field. Natively I don't think it has ever been possible as a standard report. Perhaps others can chime in on that.

Best Regards.

Hi Rohit

I figured out an easy method to generate your report. It is working here so perhaps you can try it out and confirm it works.

To create your report you need a custom report. I created two simple reports to illustrate. Select each text below and save out as an individual .txt file to a folder on your drive.

I named these BOM_TOP-ONLY.txt and BOM_BOTTOM-ONLY.txt

#BOM TOP OF BOARD ONLY
COMPONENT
REFDES
SYM_NAME
SYM_MIRROR=NO
END

#BOM BOTTOM OF BOARD ONLY
COMPONENT
REFDES
SYM_NAME
SYM_MIRROR=YES
END

The value of SYM_MIRROR determines if a footprint is on the top or bottom of the board.

To use these reports go to Tools > Reports. This loads the reports interface. Verify Display Reports is checked. Next click on the browse button and navigate to where you saved the custom report files to load the report.

Click on the report button to run the report.

Give that a go at your end to see if it fits your needs.

Best Regards.

Hi Excellon,

Does this approach work for all board layouts, or are there specific situations where it might fail?

Escape Road

Hai Excellon1,

I have tried the suggested steps, and I am able to create the BOM for the top layer.

However, there were some properties that were not visible in the BOM.

Like Part Number, Part Type.

In the schematic design, I am placing the schematic symbols from the CIS database, which is configured using the Excel format database.

We place the symbols from the CIS database into the schematic design and sync them with the PCB layout.

Once done we tried to export the BOM on the top layer, some properties were seen in the BOM but properties like Part Name and Part type was not seen in the BOM.

The reason why I am using these properties is because, in the CIS Excel-based database, the properties are defined as the Part Name and Part Number.

What could be the reason for these properties not visible in the Bill of Materials 

Regards,

Rohit Rohan

its because if doing the BOM in the PCB editor you actually have to specify them. What I suggest is make a note of the properties you want to use then in the PCB editor do a custom Bom to print out the additional properties you need.

You could try the following for top only to see if it works.

COMPONENT
REFDES
REFDES_SORT
SYM_NAME
SYM_MIRROR=NO
PART NAME
PART NUMBER
END

You may want to verify part name and number is not really PART_NAME, PART_NUMBER instead.

Best regards