TUTORIAL: Create BOM Table in Pro/E Detailing

Version: Pro/E 2001, Wildfire, Wildfire2.0, Wildfire3.0
 
Pro/ENGINEER doesn’t provide any BOM table by default. Users may create your own BOM table or download from internet. This has caused inconvenient especially to the new Pro/E users. BOM table / parts list should be a standard item in MCAD 3D modeling software now days.

Proengineertips.com provides you with both of the options. You can learn how to create a BOM table from this tutorial and also you can also download BOM table here.

Below is a short tutorial for creating a BOM table in Pro/E Detailing (Drawing).

1. In Pro/E drawing mode, clicks Table > Insert > Table from the drop down menu

2. Menu manager appears, click on the screen to draw a table. For this tutorial, we are creating table by Number of Characters

3. After the 1st clicks, there are some numbers appears towards the right. These numbers basically represent number of characters. For the 1st column, I would like to have 4 characters. Move your mouse pointer to the spacing between 4 & 5 and click. Next, continue to create another 3 columns using the same method.

When you are done with the columns, hit MMB to define the rows. For BOM table in Pro/E, only 2 rows are required.

4. We are going to enter some text in a cell. Double clicks the cell and the Note Properties dialog box appears and type in the desired note. Say: ITEM and hit the OK button.

5. The table cell should now fill with text - ITEM. After that, continue to enter notes to the rest of the cells in the same row – DESCRIPTION,  NAME, QTY

6. Next, we are going to create a repeat region in the table.

To create repeat region, clicks Table > Repeat Region from the drop down menu

7. Next, clicks Add in the menu manager and clicks the table cell (from –to) as shown in the following images.

You should notice that the selected cells’ boundary turn to orange color. This is indicating the repeat region.

8. Select the cell as shown below, press and hold RMB. Choose Report Parameter from the context sensitive menu.

Report Symbol dialog box appears. Pick the desired symbol for the cell.

I. rpt.index
II. asm.mbr.description (user defined)
III. asm.mbr.name
IV. rpt.qty

9. After regenerate, your parts list will appears in the table. You can save the BOM table as a *.tbl file to use it in another Pro/E drawing.

Select any cell in the table, clicks Table > Save Table > As Table File from the drop down menu

Download: Pro/E BOM table file *.tbl (Top – Down: Downwards)
Download: Pro/E BOM table file *.tbl (Bottom – Up: Upwards)

 To insert BOM table using the downloaded files in Pro/E, clicks Table > Insert > Table From File from the drop down menu. You may need to customise the BOM table to fit your company requirement.

TIPS: Report Parameter in Pro/E (coming soon)