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ptc-7261111-Visitor
1-Visitor
April 19, 2012
Question

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

  • April 19, 2012
  • 7 replies
  • 3295 views
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

Chris3
Chris321-Topaz I
21-Topaz I
April 19, 2012
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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P
pdkoren1-Visitor
1-Visitor
April 19, 2012
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...
M
mjenkins10-Marble
10-Marble
April 19, 2012

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





M
mpeterson1-Visitor
1-Visitor
April 19, 2012
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
-

P
ptc-7261111-VisitorAuthor
1-Visitor
April 19, 2012

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

E
eslotty1-Visitor
1-Visitor
April 20, 2012
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
P
ptc-7261111-VisitorAuthor
1-Visitor
April 20, 2012

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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