Adding Configuration to BOM Table

Pattabi_Kakumanu

Hi Everyone!

I’m working on a part in Onshape where I have a variable input for an extrude length defined in the Part Studio. I would like to specify this length in the assembly and have it automatically appear in the BOM table. My goal is to avoid having to create a drawing just to check the length of the extrude.

Does anyone know how I can add the length of the extrude as a configuration value or custom property so that it shows up in the BOM table directly? Any help or tips would be much appreciated!

Thanks in advance!

Adding Configuration to BOM Table.gif

jelte_steur814

you could use the Partname custom feature, and include the length in the partname:

https://cad.onshape.com/documents/f4d470584fdeef9603415532/v/7d0c0b30a8b73bbd6ed13b01/e/acddbbed81af3772a07adf21

Pattabi_Kakumanu

https://forum.onshape.com/discussion/comment/114969#Comment_114969

Thanks for the suggestion!

I intend to define the length at the Assembly level, not at the Part Studio level, because the aluminum extrude can be used in different sizes at the Assembly level, which I cannot know when creating it at the Part Studio. Otherwise, every time I need a different size, I would have to create a new configuration in the Part Studio, which I want to eliminate.

jelte_steur814

When defining the length at the assembly level, you'll be able to call in a configurable part studio (unlimited options if you use a configuration variable for the length). It will change the length, as well as the partname in one go since it will apply the variable to all features in the tree, not just the geometry.

rightclick to 'convert to expression' on the sting/text field and input your configuration variable there. using toSring(#variable)…

in the example you'll see I used toString(#Length/millimeter) (to make it unitless), and then added the units in the third string.

@EvanReese: is there a way to make a units option in the feature? so that it'll do that for you for all 'ValueWithUnit' types?

https://cad.onshape.com/documents/c440134b177eb7d0461c0b2b/w/d9e444e9085393c16f067af4/e/2f121e3a43ec7d0196864cd8

see below the assembly on the right (BOM showing) and configurable part studio on the left.

Pattabi_Kakumanu

@jelte_steur814 Thanks for the detailed explanation.

The concept you explained would not work if I wanted to have this many times in Assembly with different sizes. Below is an example of what I am looking for.

I have a Square Profile at the Part studio as a Purchase part now I want to use the part in an assembly with different sizes like 500 and 200 mm, and now how can I communicate the length through BOM? See the below images. I wanted to have the same Part Number and Name for both the parts.

jelte_steur814

if you insist on using a single part number for different length parts, be my guest.

there are 2 ways to approach this:

If you rock a pro or enterprise license, you could create a custom property, add it to the BOM and configure that in a similar custom feature as partname, but then adapted to configure the length.
else try and hack the partname feature to configure the description.

MichaelPascoe

You can set any part property with this feature:

Set Property
https://forum.onshape.com/discussion/24731/set-property-new-custom-feature…

.

Pattabi_Kakumanu

@MichaelPascoe Thanks, Micheal! This is exactly what I am looking for. Can you also please share the "Add to string" Feature script, it's not available online!