Originally Published 10/16/2013
|Typical Flanged Connection with Stud Fasteners|
Most of the work that I do involves using Autodesk ® Inventor’s Tube & Pipe feature. That means a lot of flanged connections. In our industry, most flanged connections are held together with studs, nuts and washers of various materials. Inventor’s Bolted Connection wizard on the Design Accelerator does not have the ability to include studs in a connection, nor are there very many stud families in the Content Center. For sure there are no ANSI standard studs. This tip gives a workaround that allows you to use Bolted Connections with studs. The trick? Make Inventor think your studs are actually hex head bolts!
To get started on this, I first opened a Hex Head bolt form the Content Center, as custom, and saved it into my playing around folder. My intent was to deconstruct it and see how it had been authored and published. You can view the way a Contrent Center part is authored by re-authoring it. For a fastener this command is on the Manage Tab of the ribbon, in the Author panel.
|Component Authoring Command Tool|
The Component Authoring command window has two tabs, the first of which shows the physical layout of the authoring. Here you designate the Placement Edge, Cylinder Axis, and then an Orientation Plane for placement. These three create iMates on the part which are used when the bolt is placed either manually form the Content Center, by using the CC’s Auto Drop feature, or from Inventor’s Bolted Connection interface.
|Component Authoring Layout Tab|
The next tab on this window is the Parameter Mapping tab. Here part or user parameters are mapped to required authoring parameters. This tab gave me a list of the required parameters for authoring an item as Hex Head bolt…. regardless of what it looked like.
|Component Authoring Parameter Mapping Tab|
With this information handy, I set about creating my stud part. The geometry was extremely simple. I was more concerned about making sure I had all the right information for those required mappings. Nominal Length and Nominal Diameter were easy, I used model parameters for these, as well as the thread information. For Head Height and Grip Length, I created user parameters that I could easily tabulate in the Content Center.
|Once I had the model created and saved, I used the Author tool on it. Under category I selected Hex Head and selected the three iMate locations.|
|Authoring Tool – Layout|
Next I mapped the required Hex Head parameters to those in my model that I had created. As long as everything is assigned, this part will successfully Publish as a Hex Head, and will be recognized by Bolted Connections.
Since I did not create this part as an iPart, there was only the one size available when I published the part to the Content Center. But that’s ok, I didn’t feel like manually adding all of those different diameter and length combinations. So, once the part was in the CC, I opened up the Family Tab;e of a Hex Head bolt, and edited it using Microsoft Excel ®.
|Hex Head Family Table w Excel ® Edit Button|
With the Family Table open in Excel ®, I saved the file out to a working location, so I could edit it without harming the Hex Head family. I closed this editing session without saving any changes, and proceeded to edit the new spreadsheet I had saved. I removed any columns form the table that did not apply to my stud part model, and added a few for iproperties that I am mapping to and from Vault. Then, back in Inventor I edited the family table of the stud part and opened it using Excel ®.
With both tables open in separate sessions of Excel ®, I copied the contents of the former Hex Head table into the more recent Stud table. I saved it and closed, returning me to the Family Table editor in Inventor, with all of the sizes and lengths that were in the original hex head table. Once I added all of my part numbers and other custom information, I was able to save and had a full table of useable studs. I can now take this family and copy it as many times as I need for different materials and specs.
|Completed Stud Family Table|
It occurred to me last night that I did not explain how I got the leading edge of the stud to protrude from the nut and washer as shown in that first image. My apologies! It’s really quite simple. During the authoring stage, when the iMates are placed on the stud, but before you publish the part to the Content Center, one of the iMates needs to be modified. the insert iMate which defines the insertion point of the fastener. Find this in the list of iMates in your model browser, right click and select Properties. Add an offset value as shown below, this may vary depending on how much of the fastener you want protruding. I chose a simple 1/2″, but it needs to be a negative to have it protrude away form the insertion point. The protrusion on the opposite end will be determined in the Bolted Connection process. Now you’re ready to publish. Sorry for any confusion this caused!
|iMate Offset for Protrusion|
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