Pro/rNGINEER Wildfire Tips & Tutorial (Pro/E Wildfire 4.0, Wildfire 3.0, Wildfire 2.0 and 2001)

TUTORIAL: Create BOM Table in Pro/E Detailing

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. 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

Pro/E insert table

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

Pro/E insert table

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.

pro/E create BOM table

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.

pro/E BOM table text

pro/E note properties dialog box

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

pro/E BOM table - ITEM

pro/E drawing BOM table

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

What is Repeat Region in Pro/E?

Repeat Region is dynamic report table cells which are based on the principle of "smart" table in Pro/E. Repeat regions can expand or contract by accommodating the amount of data that the associated model currently possesses.

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

pro/E repeat region

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

 Pro/E repeat region

 Pro/E repeat region

 Pro/E repeat region

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

 Pro/E repeat region

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

 Pro/E repeat region Report Parameter

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

 Pro/E repeat region Report Parameter

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

 Pro/E repeat region Report Parameter

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

 Pro/E save BOM table

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. is an independent website providing tips and tutorials for Pro/ENGINEER users.
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