NAA P-51D Mustang: Project Cad Technote; iParts

NAA P-51D Mustang: Project Cad Technote; iParts

When it comes to organising standard parts using a Cad system like Inventor there are various ways to achieve this. Initially I considered a custom content library or even an iLogic expression linked to a parameter spreadsheet but I settled on using iParts.

The main reason for this is due to the fact that I already have a plethora of data contained in many spreadsheets for everything from ordinates to document registers and at any one time one or more of these spreadsheets is usually open for reference. Therefore the iparts seemed to be the ideal choice by maintaining all the relevant data in a single Cad part file.


A simple example of this would be for the AN960 standard washers. I could have done something really clever here as the actual part number contains references to the physical sizes and properties of the washers and I had thought it would be great to link the naming convention to the parameters.

However there is no real benefit to be gained from this and would have added a level of complexity that’s quite frankly unnecessary for this type of component.

We have 3 dimensions that define the washer; the Outside Diameter (OD), Inside Diameter (ID) and the Thickness (Thk). We also have a material type but the Cad library will need to be updated to include the specifics of the materials for a P-51 mustang, which is another custom job; so I have ignored it for now!

The above sketch shows the expressions of the parameters defining the relationship of the values as declared in the parameters dialogue; this is where it gets interesting.

2015-07-15_22-55-47I should note that the template and default units for this model is millimeters. The standard units for the washers is inches.

This image on the left is the parameters dialogue box to which I first added some user parameters (1) set to “inch” units. I then created the cad model dimensional parameters (2) and linked those to the user parameters (1) with the units set to “mm” (3). The wonderful thing about this is that Inventor will adjust the values based on the unit type automatically; so just by changing the unit type the value will change accordingly, which is verified in the nominal value column (4)…great stuff!
This is the iPart creation dialogue, showing the table of values, input from the standard catalogs in “inches”.

Its very important that the original values are retained as “inch” units so that it is easier to check and verify the correctness of the information and traceability.

Tip: If I already had these values set-out in exactly the same format in excel I could just copy and paste the spreadsheet directly into the iPart table.

At some stage I will add the material values to the end of this table for each of the components listed. Some examples of iparts include the Locking Stud and Clevis Fork; colour coded to differentiate size..

Locking Stud Clevis Fork

The notion of working with different units is made so much easier by the capabilities of these cad systems. Essentially when inputting the dimensions in a model sketch the value of the dimensions will change if you select either inches or millimeters according to the default template units setup for the cad model; it will even work with fractions.

For example if you type in “3/4 in” for a dimension in a sketch based on the “mm” unit template then the actual value for the dimension will be “19.05 mm”.

Another example; 12 23/64″; for this you type in 12 leave a space then 23/64 followed by “in”…”12 23/64 in” gives us “313.928 mm”.

About Hugh

BIM & Cad Manager/Strategist, 3D/4D, multi-discipline cad workflows, integration. Interests include photography and historical aviation.
This entry was posted in 3d Cad, 3d cad modelling, Aviation, Inventor, P-51 Mustang and tagged , . Bookmark the permalink.

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