Can I reduce the number of similar part files?

[roknjohn]

I've been playing around with Inventor and managed to model everything we've built so far. I'm very impressed with the software. There is one area, though, that I may be doing the hard way.

Suppose you have an assembly made of several pieces of 2x4 aluminum of various lengths. Up to now, I've had to create a separate part file for each extrusion length, then assemble them together. Is there a quicker way? For example, while working in the assembly, can I place a part and then specify its length?

In other words, if my assembly uses 10 pieces of 2x4 aluminum, each of different lengths, will I need 10 separate part files?

Thanks for the help.

John

[Madison]

Originally posted by roknjohn
Suppose you have an assembly made of several pieces of 2x4 aluminum of various lengths. Up to now, I've had to create a separate part file for each extrusion length, then assemble them together. Is there a quicker way? For example, while working in the assembly, can I place a part and then specify its length?


Yes, you can. Unfortunately, I don't yet know how to do it. I'm sure Ed Sparks will come along to share the details, however ;)

Essentially, you need to create the profile you want extruded to different lengths and save it as an iPart file. These files contain data, in a spreadsheet, for several variations of a part. Similarly, you can include a length variable in your iPart, and each time you insert it into an assembly, you'll be prompted to enter a part length.

I haven't played around enough with iParts to walk you through creating them, however. Sorry.

Check here (http://www.cbliss.com/inventor/Parts/Structural/structural_shapes.htm), though. They have a rectangular tube iPart already created that uses custom lengths. That may be what you're looking for.

[Ed Sparks]

roknjohn ......

The short answer is Yes. Inventor requires a seperate .ipt file for each unique length of aluminum.

The good news is, as M. Krass points out, that you can take advantage of iParts to make generation of these files somewhat automated.

An iPart is really an association of some graphics and a spreadsheet table. Take a shaft collar for example. They all look alike but are available in different sizes so we set up a table with each row containing the values of the dimensions that make up each version of shaft collar available.

The result of all this is that when the user inserts this part into an assembly, a dialog box pops up and asks which version of the part you want to insert. Once the user makes a selection, an Inventor part (.ipt) file is generated and stored in the current project space. If the iPart has a "filename" column defined, the text in that cell is used as the name of the generated .ipt file else the file is stored as "Part1, Part2, Part3 ..... etc."

Now, A really cool thing about all of this is that a column of values can be declared as a "Custom Parameter" which means that the dimension associated with this cell can be defined through that dialog box I talked about earlier.

So, you can see that you could define an iPart of Angle Aluminum for example that has a row of data for each size available and a custom parameter that allows you to define the length when the part is inserted into an assembly. In this case I would not define the filenames (your given a chance to name the file when it's generated).

You can even suppress part features that may not exist in some configurations of a part. For example my iSprocket gives you the ability to generate sprocket .ipt files with or without hubs, and/or keyways. This is a good example of an iPart that you can dissect to see how things work.

Hope this helps .....

First Cad Library (http://www.firstcadlibrary.com)