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BOM export (w/ sub-levels) to Excel w/o PDM

ptc-726111
1-Newbie

BOM export (w/ sub-levels) to Excel w/o PDM

Hello,

I am wondering how to export a complete assembly in Pro-E WF 4.0 to Excel containing the complete BOM and each sub-assembly level. Here are the steps I am using so far:

If not using a PDM system:

1) insert a BOM table into the drawing,

2) select the table, then

3) Table > Save Table > As txt file,

4) then switch over to Excel & open the .txt file

This works fine but it does not include the each sub-assembly level with all its components. I am guessing I need to change the BOM table in Pro-E to do this properly, and would appreciate any advice on how to do this.

Chris
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7 REPLIES 7
Chris3
20-Turquoise
(To:ptc-726111)

Just change the repeat region to be Recursive.

Table -> Repeat Region -> Attributes -> Recursive

FYI you can also set No Dup/Level which changes it so that there is only one row per part. Ie the same part isn't listed multiple times.

In my table I have an @ in between every column and then I delimit in Excel on the @ symbol. This way if you have a column with titles that have commas it doesn't throw off the import.

Chris

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In wf3, and I think in 4 too, just open assembly andINFO - BILL OF MATERIAL...select TOP ASSY in the popup, then it will open a window with both a list of the top level assembly, AND a list of the contents of the subassemblies AND a list of ALL parts in the assembly along with quantities... You can just FILE-SAVE AS to a .txt file and then read that into EXCEL...
mjenkins
5-Regular Member
(To:ptc-726111)

Try inserting this table:

In Reply to Christopher Thompson:


Hello,

I am wondering how to export a complete assembly in Pro-E WF 4.0 to Excel containing the complete BOM and each sub-assembly level. Here are the steps I am using so far:

If not using a PDM system:

1) insert a BOM table into the drawing,

2) select the table, then

3) Table > Save Table > As txt file,

4) then switch over to Excel & open the .txt file

This works fine but it does not include the each sub-assembly level with all its components. I am guessing I need to change the BOM table in Pro-E to do this properly, and would appreciate any advice on how to do this.

Chris





Chris,

That is the general approach I have used for a while, but to get the desired
results I adjust the BOM in Pro/E to show what I want whether its sub-assy's or
hinding parts or what ever. Get the Pro/E BOM as you want it and then Save As
the TXT file. When you open in Excel use the delimited option in Step 1 of the
import wizard. In Step 2 uncheck the Tab box and check the Comma box and then
continue and finish. Then your Excel BOM should be divided into the same columns
as your Pro/E BOM.

Mark A. Peterson
Sr Design Engineer
Igloo Product Corp
-

Thanks for the replies. I received this suggestion from Tech support:



The functionality of exporting a bill of materials directly to Excel is not a current functionality of Pro/Engineer, However as an alternative you can follow these steps to open the BOM file in Excel:



  1. Set the config.pro option 'info_output_format' to 'text'

  2. Create a BOM file by #Info> #Bill of Materials and save the Information window by #File> #Save as and save the BOM file as a .bom file

  3. Open this file in Excel, this can be done by choosing #File> #Open and selecting #All file types.

  4. Choose #Delimited #Next, check the #Space option, and select #Finish from the File import wizard dialog box.

This worked great, except it was missing the part / assembly description. So I was referred to this link for creating a custom BOM


It requires setting-up a *.fmt file containing the following information that is accessed by the config.pro file:


To add parameters in the text of the BOM, use the following formatting characters:


<dd>%$ - a percent sign followed by a dollar sign indicates that the next word is one of the three system-supplied attributes: name, type, or quantity </dd><dd>% - any word preceded by a percent sign is a user defined parameter
</dd>


I do not yet know if it will work as this will be a first time setting it up.


Chris

A BOM table with a comma column between the data fields works nice...
it's not visible on drawings but when saved as a TXT file, the comma
delimiter separates the data...



Have a great weekend...



GE Healthcare Technologies

Clinical Systems

Monitoring Solutions

Eric R. Slotty

Mechanical Designer

8200 W. Tower Avenue

Milwaukee, WI 53223

Okay, so far the best results seem to be this advice below. Just add columns to the BOM table in the drawing as needed: description, rev level, material, etc. and I find that it is easier to adjust then trying to generate a BOM directly from the assembly model.


Part of the reason I was having issues is these Pro-E models were generated by another company and they used parameters that our BOM tables did not recognize until I modified the tables. I am considered to be the SolidWorks expert at this company I am working for as a contractor and now they want me to be a Pro-E expert as well (I had not touched Pro-E for a few years until late 2011).


Thanks for all the helpful advice.


Chris



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