'lbmass' How can I change this?

One of the little quirks that urks me in Inventor is its inability to change the unit display on weight (MASS) in drawing notes. One of my clients likes to have a total assembly weight below the Bill of Material (Parts List) on their drawings.

Now this isn't a difficult task as Inventor allows you to port physical iProperties like MASS into a block of text. The issue is that it populates the note with a unit string of 'lbmass' after the value. I have yet to meet anyone who uses this format of a unit string. There are a few cases in Inventor where adding certain physical properties result in units that are not desired and no option to override it.

Here is a quick work around to customize that trailing format on a weight note.

Start of by creating a User parameter and name it something like ‘Weight_lb.’ You can call it whatever you would like providing it conforms to the parameter naming rules. Set its unit type to ‘Unitless ul’ and modify its value to that reflects the unit type. (Example 1ul)

Export the parameter by putting a check in the Export column.

Next right click on the parameter and select ‘Custom Format Property.’ Select the desired precision and uncheck the ‘Unit String’ check box.

Next we will create an iLogic rule to pass the physical mass of the model to our User parameter / custom iProperty. In the iLogic browser right click on the model name and select ‘Add Rule’. (Alternately you can add this to an existing rule if you prefer.)

Enter the following snippet into the iLogic editor.

InventorVb.DocumentUpdate() Parameter("Weight_lb")=iProperties.Mass InventorVb.DocumentUpdate()

Now you can insert this new Custom iProperty into a string of text and add what ever unit descriptor you would like.

Now it's obvious that this deserves a permanent place in your model templates so it can be used in any ‘Sketched Symbols’ you may use in your drawing templates.

Let me know if you have any questions about this or any other topic and thanks for visiting.