Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

BOM "Filename" file extension

12 REPLIES 12
Reply
Message 1 of 13
gatnact
2920 Views, 12 Replies

BOM "Filename" file extension

I would like to know if there is a way to remove the file extension (.ipt, .iam) from the "Filename" column for a B.O.M.?

 

Also, if you have the "Material" column active when editing the B.O.M. and would like to change a material type, is there a way to have the selector look at a different library, i.e. Favorites or a custom library? I attached a picture of what I am asking for.

 

And in the end...
12 REPLIES 12
Message 2 of 13
karthur1
in reply to: gatnact

I don't know of a way to remove the extension from the filename like you are asking, but rather than displaying the filename, can you display the partnumber instead?  If your partnumber and filename are the same name (that is the way I do it), then the partnumber will not have the extension.

 

Kirk

 

2014-04-23_1217.png

Message 3 of 13
gatnact
in reply to: karthur1

This would only work if our company here always used the same part name as the file name all the time. Sometimes we will get a customer drawing and the part number has to be different than our numbering structure but the customer will need there part number and our shop will need ours.

And in the end...
Message 4 of 13
karthur1
in reply to: gatnact

Just curious what you are having to do with the BOM at the assembly level?  If you are exporting it to excel, then maybe edit it in excel and remove with the  "Find and Replace" tool.

 

Most of the time, I never export to excel the BOM from the assembly, but rather I export the parts list from my idw.

 

Not telling you how to do it, just how I do it.

 

Kirk

Message 5 of 13
gatnact
in reply to: karthur1

I am not exporting to excel. I want to make a drawing, create a parts list for an assembly, have the column that says file name without .ipt or .iam. This is the part number I use for the shop drawings.

 

 

The file name is the name I put in upon creation of the parts and assemblies. The part number I type in after the new part or Assemblies is created and saved with the file name.

 

I want to use the file name without the file extension so I don't have to type that number in twice. Once when saving the part/aassembly and then once in the BOM editor and/or iProperties.

 

Picture attached

And in the end...
Message 6 of 13
brendan.henderson
in reply to: gatnact

I'm pretty sure it can't be done, and I don't understand why you want it that way. Each to their own I guess.

 

From your picture "b.o.m. question2.PNG" it appears that the Part Number and the Filename are the same, but Part Number loses the extension of course. So from your picture you could use Part Number instead of Filename. Although the picture supplied is probably only a small example of a typically larger BOM where the Part Number and Filename may actually be different?

 

You probably already know this, but by default when you save an Inventor file the Part Number gets filled in with the Filename, less the extension. This is the way the software was built to be used.

Brendan Henderson
CAD Manager


New Blog | Old Blog | Google+ | Twitter


Inventor 2016 PDSU Build 236, Release 2016.2.2, Vault Professional 2016 Update 1, Win 7 64 bit


Please use "Accept as Solution" & give "Kudos" if this response helped you.

Message 7 of 13
Paul-Mason
in reply to: gatnact

Would it not be better and easier to use the parts list as this has a selectable addable and removable columns for separate file names, parts number etc, then you could have one column for your in house stock number and one column for customer number use in the one idw

 

The Customer Pt No is added by using the "NEW PROPERTY" in the part list edit that can then either be filled in manually, or it can be added as a custom iprorpety at ipt level if your saving each customers project separately

 

PM screen shot001.png

 

The permutations and location of columns using this method is just about limitless. Best of all it can be made to fit your own requirements.

 

It's the way I prefer to do it then for billing/ordering export to excel and add any other columns required

 

Also if you want a small graphic of the part the is a small add in "Thumbnail Parts List" that will reporoduce the parts list with a small representation of the part in a Word doc or docx format, I've attached this in win zip format, its  good little program.

==============
Inventor 2023 Pro
HP Z420 workstation
Xeon 3.7Ghz CPU 8 Cores, 64 GB Ram
64bit (The Garbage known as) Windows 10 Pro
AMD FirePro V3900 (ATI FireGL) (1GB RAM)
=================
Ashington Northumberland (UK) ~ Home to the WORLD FAMOUS Pitman Painters Group
Message 8 of 13
jddickson
in reply to: gatnact

This should do what you want. You will just have to use a custom iProperties.

 

    File_Name = ThisDoc.FileName(True)
    
    File_Split = Split(File_Name, ".")(0)

    iProperties.Value("Custom", "File" ) = "=" & File_Split

 

I hope this helps

Message 9 of 13
mcgyvr
in reply to: jddickson

What about using the "Stock Number" field or the "Project" field" or the "vendor" field or any of the others that aren't being used..

Simply use another.. filename includes the suffix or the ilogic code to populate a custom field. 

 



-------------------------------------------------------------------------------------------
Inventor 2023 - Dell Precision 5570

Did you find this reply helpful ? If so please use the Accept Solution button below.
Maybe buy me a beer through Venmo @mcgyvr1269
Message 10 of 13
jddickson
in reply to: gatnact

I tried to edit my post from before but it would not let me for some reason. You should be able to use this code to get what you want. 

 

 

    File_Name = ThisDoc.FileName(True)
    
    iProperties.Value("Custom", "File Name" ) = Split(File_Name, ".")(0)

 

 

pic 1.jpg

 

I hope this helps

Message 11 of 13
gatnact
in reply to: brendan.henderson

Thank you for this reply. 

I would like to use the part number instead of the file name. I guess the picture is a bad example. The picture I am showing, show the two numbers matching but the part number was missing some of the number from the file name and some were different, I am guessing from a previous saved part and from contenet center parts. The pictured list shows the list that I have already done edited.

And in the end...
Message 12 of 13
jddickson
in reply to: gatnact

This should do it.

 

 File_Name = iProperties.Value("Project", "Part Number")
    
 iProperties.Value("Custom", "File Name" ) = Split(File_Name, ".")(0)
Message 13 of 13
antti
in reply to: brendan.henderson

Hi,

I just found this quite relevant issue.

I faced this on case liked this.

You'll add new part to your assembly. This new part will be a profile from Content Center. There will be some machining for that profile (like holes) and by your company policy this means that it must have "real" file name (not that DIN blaa blaa blaa..). So we named (and saved) that new part like "12345".

On Your assembly tree it does show like "12345", fine.

On your drawing in BOM it will be liked "DIN blaa blaa blaa", if you are using "Part Number" - field.

 

So the main issue is that when you insert profile from Content Center and on Save dialog will save it with new name it won't make any change to "Part Number" - field, which is quite logical (there is still information of the the profile), but then you can't used the "Part Number" on your BOM.

 

The best work-around for this could be using "File name" on BOM (instead of "Part Number"), but then there is the file extension.

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report