Using parameters as my description

[Yashasvi23481]

Hi All,

   I am back to designing and drafting after 3 years and i vaguely remember a way to create my geometry as parameters during build say L=90mm and W=12MM and extrude using T=16mm and then link them to derive description of product. This is done so that if you change thickness or geometry, you dont have to update description its linked with equation in description like = (L) x (W) x (T). I cant recollect exactly. Can somebody let me know how to do this ? This was in 2018 and i am using 2024. My client likes his BOM and description as Raw Materials instead of work description. 

Any help will be appreciated. Thanks in Advance. 

Regards,

Yash

[mojtaba77f · Accepted solution]

Hi there!

In the "Parameters" tab, create the parameters you need. For example, you mentioned Length (L), Width (W), and Thickness (T). You can do this by clicking on the "Create" button in the "Parameters" panel. then Use these parameters to create sketches and features in your part. For instance, you can create a sketch and use the L and W parameters to define the rectangle's dimensions then Use the parameter-driven sketches to create extrusions and other features. For the extrusion depth, you can again use the parameter "T" instead of a fixed value. then To link these parameters to your description and BOM, you can use equations. In the "Equations" dialog (usually located under the "Manage" tab), you can define custom equations. For example, your description equation could be something like:
Description = "Raw Material: " & L & "mm x " & W & "mm x " & T & "mm"

When you generate a Bill of Materials (BOM), you can include the parameters you've created. In the BOM template, choose the parameters you want to display alongside your components.

If you need to make changes to the dimensions, you can directly edit the parameters in the "Parameters" tab. This will automatically update the model, sketch, features, and descriptions linked to those parameters.

[SBix26 · Accepted solution]

One additional detail: after creating the parameters Lg, Wd, and Th (I found that Inventor won't let you use W alone because it's already in use as a unit [Watts]), check the Export Parameter box for each one-- this makes them Custom iProperties for use in the description.  Then right click on each one and set up the formatting for that custom iProperty so it shows up in the Description as you want.

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Sam B

Inventor Pro 2024.1 | Windows 10 Home 22H2

[Yashasvi23481]

@SBix26 & @mojtaba77f Thanks for solution so i was unable to select W for width because its used for Watt and will remember to use 2 letters in parameters and export parameter is what i was missing/forgot. Thank you. I have marked both as accepted solution.