Standard Parts - File Properties in BOM 1

[beebo666]

i am still somewhat new to SE using V19. i am wondering how you all handle Standard Parts in the BOM. when the standard parts are created they are read only, so i can't change the file properties so i can display the info i want in the BOM. at my compnay they want to see a McMaster or MSC part number. i used to work i inventor and i could overwrite fields in the BOM. i don't see a way to do that in SE.

 

[KENAT]

I don't know of a way to overright most properties 'in the BOM', if someone knows one I'd be interested too.

There are some options in 'Occurance Properties' from the assembly feeding the BOM but I don't think enough for what you're trying to do.

What you need to work out is how modify the 'library' parts to have the information you need in their properties. This way they are there for the next person too. We had a little trouble with Standard Parts at our place but I think it's mostly due to our set up, not necessarily a problem with the function itself.

Can anyone help with this, I remember vague things from some training I had last year but not enough to help Bebo.

 

[beachcomber]

You can't overwrite fields in the bom.
The whole idea is that the model is the master and holds the information required to populate the bom fields.
Any property and most variables in the mdel can be accessed in the bom.
Select the bom in your draft file, then RMB and properties.
Click on the 'columns' tab and select the properties you require. You can set widths and headings etc here also.
If they are not there you will need to add them to your parts.
Unfortunately you WILL require write access to the part files to do this - it's a basic requirement for any file that you want to edit, not just SolidEdge.
To add them, I would suggest creating a part with the properties you require and the values. If the values are common enter it, otherwise use a "-". Then use Property manager to open this file and the others you want to add the properties to. To start proprty manager in this way start SolidEdge but before you epen a file go to Tools>Property Manager. You will be presented with a dialog box where you can select the files you want to open in property manager. Just highlight the ones you want and the click open.
Set the columns in property manager to show these new properties and fill in the properties for the parts that require them. You can use copy/paste, and also find/replace.

bc

 

[KENAT]

Thanks beachcomber, that was my understanding that you had to change it in the part (or for qty set up the part so it could be changed at the assy level) but I've been proven wrong before so didn't want to be too definitive.

Really emphasises that you need to get write access to your parts or find how to replace them. Are there any specific issues with standard parts here that anyone can help beebo with.

FYI you can add custom properties to parts on the custom tab for the initial part then as beach says, property manager is the way to go. If you have access you may want to set your template up with the additional custom properties, we did this to add cage code, manufacturer P/N & remarks.

 

[beebo666]

my solution was to make the standard parts folder wite instead of read only. i can now access and change the file properties as i need. thanks for the replies.

 

[sc1000]

Simple fix...In standards parts there is a open command instead of the place part command. Place the part in a directory you are working. for example.. a repository of parts and subassemblies that are destined for your final assembly.

Open the file in solidedge part and use the save as command and place it in the directory of your choice....done. now just fill in the properties and save it.

After that just place it in an assembly and it will populate the bom the way you have defined.